SOLIDWORKS Tech Blog http://blogs.solidworks.com/tech Sat, 24 Jun 2017 15:00:04 +0000 en-US hourly 1 SOLIDWORKS Hidden Gem: The Delete Face Tool http://blogs.solidworks.com/tech/2017/06/solidworks-hidden-gem-delete-face-tool.html http://blogs.solidworks.com/tech/2017/06/solidworks-hidden-gem-delete-face-tool.html#respond Sat, 24 Jun 2017 15:00:04 +0000 http://blogs.solidworks.com/tech/?p=17287 SOLIDWORKS contains a lot of features, but most users only use a small selection of them. In this tech blog I want to reveal a feature, which is relatively unknown to many users, but yet very powerful: Delete Face. It

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CAD2M

CAD2M is certified reseller of SOLIDWORKS, SolidCAM, DriveWorks and our private label dddrop 3D printer. The CAD2M approach integrates this range of products into an all-in-one solution that covers the complete product development process. Take the full advantage of working in 3D with our advice, training and expertise. For more information, visit www.cad2m.nl.

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SOLIDWORKS contains a lot of features, but most users only use a small selection of them. In this tech blog I want to reveal a feature, which is relatively unknown to many users, but yet very powerful: Delete Face. It is a feature which I use often on day to day basis to solve some customer issues.

Where to find it?

You can find Delete Face  on the Surfaces toolbar (CommandManager), or Insert > Face > Delete.

What can it do?

The main target of Delete Face is to delete faces, as you probably already could tell based on the name of the feature. The command itself has three options to choose from:

  • Delete
    Deletes a face from a surface body, or deletes one or more faces from a solid body to create surfaces.
  • Delete and Patch
    Deletes a face from a surface body or solid body and automatically patches and trims the body.
  • Delete and Fill
    Deletes faces and generates a single face to close any gap.

Example of Delete and Patch

Let’s take a look at an example of an imported sheet metal part. In this case you can use the Insert Bends feature, so you can generate the flat pattern of this imported file. But the problem is that you cannot change the bend radius which is already defined in the imported body. So here Delete Face can help you out.

In the image below you can see that all the bend faces are selected in the Delete Face PropertyManager.

With the Delete and Patch option, these faces are deleted, and the adjoining faces will extend to form an unbroken surface. Now the Insert Bends feature can be used and any bend radius can be entered without any problem. The images below show the result of this action.

Example of Delete and Fill

Another example is about a fillet feature which created a lot of small faces. Also here Delete Face is the solution. In this case the option Delete and Fill will be used.

In the image below you can see that all the unwanted faces are selected in the Delete Face PropertyManager.

With the Delete and Fill option, these faces are deleted, and are filled by a single unbroken surface. The Tangent fill option is used to create tangent transitions between the new face and the rest of the part. The image below shows the result of this action.

Conclusion

We have seen how the Delete Face tool can easily solve some issues with your SOLIDWORKS models. Note that Delete Face is also very helpful to delete unwanted details from downloaded library parts, so these are better to handle in a large assembly. It can even help to delete a simple hole, without having the risk of ruining your design intent.

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CAD2M
CAD2M is certified reseller of SOLIDWORKS, SolidCAM, DriveWorks and our private label dddrop 3D printer. The CAD2M approach integrates this range of products into an all-in-one solution that covers the complete product development process. Take the full advantage of working in 3D with our advice, training and expertise. For more information, visit www.cad2m.nl.

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SOLIDWORKS Rocket Hacking Tutorial – Part 1 http://blogs.solidworks.com/tech/2017/06/solidworks-rocket-hacking-tutorial-part-1.html http://blogs.solidworks.com/tech/2017/06/solidworks-rocket-hacking-tutorial-part-1.html#respond Fri, 23 Jun 2017 21:00:46 +0000 http://blogs.solidworks.com/tech/?p=17321 Hey SOLIDWORKS users, Happy 4th of July! So to celebrate the holiday we are taking an off-the-shelf model rocket and making it our own with the help of SOLIDWORKS, 3D printing, and a little elbow grease. So let’s get started

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SOLIDWORKS

Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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Hey SOLIDWORKS users, Happy 4th of July! So to celebrate the holiday we are taking an off-the-shelf model rocket and making it our own with the help of SOLIDWORKS, 3D printing, and a little elbow grease. So let’s get started with our 3 part series.

SOLIDWORKS Rocket Hacking Tutorial - Final Product
In part 1 of the series, we’ll begin modeling a new nose cone and a new tail piece for our model rocket using mostly essential modeling tools.

Can’t wait to watch the next video? View all of the tutorials on the playlist here.

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SOLIDWORKS
Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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Design Re-use http://blogs.solidworks.com/tech/2017/06/design-re-use.html http://blogs.solidworks.com/tech/2017/06/design-re-use.html#respond Thu, 22 Jun 2017 15:00:22 +0000 http://blogs.solidworks.com/tech/?p=17258 “I know that part’s here somewhere… I think I saved it in the XXX project folder…  We designed a similar assembly last year…” Sound familiar? If you’ve ever spent time hunting for previous designs or recreated the same content multiple

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TPM

TPM, Inc. is the Carolina’s largest 3D CAD provider and a leading technology company proud of its reputation of providing cutting-edge solutions to the engineering and design community for the past 40 years. Founded in 1973, TPM Inc. serves more than 3,000 customers across the Southeast each year. Inspired by our founder, Jerry Cooper, we are committed to offering our clients the best: 3D Design Software, 3D Printing and Scanning Options, Data and Document Management Solutions, Large-Format Graphics, Wide-Format Plotters and Office Equipment, and Reprographics.

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“I know that part’s here somewhere… I think I saved it in the XXX project folder…  We designed a similar assembly last year…” Sound familiar? If you’ve ever spent time hunting for previous designs or recreated the same content multiple times, you’re not alone. Fortunately, SOLIDWORKS includes powerful capabilities that minimize this pain and help you get your job done fast.

Here’s a short video, maybe you can relate.

That was a ton of information, let’s recap and expand:

Design Library

  • Includes out of the box standard mechanical design content (like o-ring grooves, keyways, sheet metal punches, etc.)
  • Windows folder structure – easy to organize and share with co-workers
  • Easily add content you re-use (like drawing notes, feature sets, purchased parts and assemblies, company logos, welding symbols, start parts, and much more)

SOLIDWORKS Toolbox

  • Included with SOLIDWORKS professional and premium (turn on the add-in)
  • Thousands of standard hardware components (o-rings, nuts, bolts, washers, gears, retaining rings, bearings, pins, and much more)
  • Fully configured with all standard sizes and lengths
  • Autosize to your corresponding features
  • Can add BOM details and custom components using the “Configure Toolbox” wizard

Integrated SOLIDWORKS Search

  • Setup all locations you want to index
  • Tools > Options > System Options > File Locations > Search Paths
  • Set options like when to index and whether to show 3DCC results
  • Tools > Options > System Options > Search
  • Use keyboard shortcut “I” to activate the search

3D Content Central

  • Free online resource
  • Thousands of vendors with configurable and downloadable 3D files, and tons of user uploaded content too
  • Preview 3D files right in browser
  • Use integrated SOLIDWORKS search (if 3DCC set to show in results)
  • Drop right into SOLIDWORKS

Mate References

  • Add to any part or assembly you will re-use and want to snap into position
  • Use a circular edge between a cylindrical and planar face to get both concentric and coincident mates added.
  • Add up to 3 references and name the mate reference to get it to find mating components automatically. Just use the same name for the mate reference in the mating part.  Put into an assembly and they will snap together like magic.

Smart Components

  • Allow you to insert features, parts, or both. Think mounting holes and hardware for example.
  • Features can include full tolerances that will carry over.
  • Use a simple setup assembly when creating the smart component (I store them in my design library).
  • Create: edit the part in the context of the setup assembly and use Tools > Make Smart Component.
  • Use: insert and position the part in your assembly. Click the smart component icon in the graphics or right click the part > Insert Smart Features.  Select what to include and any references needed.

Give them a try today and fuel your blazing fast skills!


Want more tips? Check out this 3-part series on mating! 

  • Part 1 covers getting parts inserted and mated quickly,
  • Part 2 covers three of the most powerful everyday mates; Profile Center, Width, and Slot
  • Part 3 covers automation for frequently used components.  Mate References, Magnetic Mates, and Smart Components

Check out Part 1 of the series below:

 


By: Mike Staples • Elite Application Engineer • TPM

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TPM
TPM, Inc. is the Carolina’s largest 3D CAD provider and a leading technology company proud of its reputation of providing cutting-edge solutions to the engineering and design community for the past 40 years. Founded in 1973, TPM Inc. serves more than 3,000 customers across the Southeast each year. Inspired by our founder, Jerry Cooper, we are committed to offering our clients the best: 3D Design Software, 3D Printing and Scanning Options, Data and Document Management Solutions, Large-Format Graphics, Wide-Format Plotters and Office Equipment, and Reprographics.

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SOLIDWORKS Harry Potter’s Golden Snitch Tutorial – Part 3 http://blogs.solidworks.com/tech/2017/06/solidworks-harry-potters-golden-snitch-tutorial-3.html http://blogs.solidworks.com/tech/2017/06/solidworks-harry-potters-golden-snitch-tutorial-3.html#respond Mon, 19 Jun 2017 21:00:02 +0000 http://blogs.solidworks.com/tech/?p=17067 It’s safe to say that Quidditch is Harry Potter’s favorite wizarding pastime. As Hagrid would say, a wizard’s passion for Quidditch is the equivalent to a muggle’s passion for football. This year marks the 20th anniversary of the first publication

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SOLIDWORKS

Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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It’s safe to say that Quidditch is Harry Potter’s favorite wizarding pastime. As Hagrid would say, a wizard’s passion for Quidditch is the equivalent to a muggle’s passion for football. This year marks the 20th anniversary of the first publication in the series, Harry Potter and the Sorcerer’s Stone. To celebrate, we are showing SOLIDWORKS users how to model the Golden Snitch – the little ball that Harry loves to hate. So hop on your Nimbus 2000 and let’s get started flying through our four part series.

SOLIDWORKS Harry Potter's Golden Snitch Tutorial

Welcome back SOLIDWORKS wizards to our 4-part series where we are building the Golden Snitch to celebrate the anniversary of the start of the Harry Potter world. We’ve completed adding the outer detail to the Snitch’s body in the previous videos, now in part 3 of the series, we are going to begin building the wings using some unique tools, including the sketch on sketch Projected Curve option, the Flex tool, and the Curve Driven Pattern tool.

Wizards and muggles alike can learn something new from our Golden Snitch tutorial series! Can’t wait to watch the next video? View all of the tutorials on the playlist here.

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SOLIDWORKS
Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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SOLIDWORKS Simulation – Define Shell Elements by Selected Faces http://blogs.solidworks.com/tech/2017/06/solidworks-simulation-define-shell-elements-selected-faces.html http://blogs.solidworks.com/tech/2017/06/solidworks-simulation-define-shell-elements-selected-faces.html#respond Mon, 19 Jun 2017 15:00:54 +0000 http://blogs.solidworks.com/tech/?p=17145 SOLIDWORKS Simulation When simulating large, thin objects it is much more simple, computationally, to define these types of objects as shell elements rather than solid elements. The problem is that most beginner simulation users are not comfortable with this element

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GoEngineer

GoEngineer delivers software, technology and expertise that enable companies to unlock design innovation and deliver better products faster. With more than 30 years experience and thousands of customers in high tech, medical, machine design, energy and other industries, GoEngineer provides best-in-class design solutions from SOLIDWORKS, Stratasys, CAMWorks, Altium and Product Lifecycle Management (PLM). For more information, visit goengineer.com.

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SOLIDWORKS Simulation

When simulating large, thin objects it is much more simple, computationally, to define these types of objects as shell elements rather than solid elements. The problem is that most beginner simulation users are not comfortable with this element type because they do not know how to define a shell element mesh or how to connect it to the rest of the parts in the analysis once it is defined. In this post, I will show you how to define a shell element using the Shell Definition tool and then how to define Loads, Mesh Controls, Fixtures, and Contact Sets to that shell element once it has been defined. Lastly, we will briefly go over what a fully meshed shell element mesh looks like.

How to define a Shell Element Manually

First, find a part that is large in one plain, but comparatively thin through its thickness. For example, a sheet metal piece. The bracket you see below is an example of this sort of geometry.

Figure 1: Example of what a shell element should look like.

Next, click on the object in the graphics window to see it highlighted in the simulation tree.

Figure 2: Simulation feature highlighted after clicking on part file in the graphical window

 

After right clicking on the part file in the simulation tree, you will see the Define Shell by Selected Faces command in the popup window.

Figure 3: “Define Shell by Selected Faces” Command highlighted

 

After clicking on this tool next click on the faces of the large thin object that you wish to treat as a shell element mesh instead of a solid element mesh. Now set the shell thickness to the actual thickness of the object.

Figure 4: Shell Definition Command Manager

 

Lastly, make sure that the offset parameter is correct based on the face that was used to define the shell element. In the image below, the top surface choice has been selected and this puts the offset that the Simulation program uses to calculate the stresses and displacements through the sheet metal part in the opposite direction then it actually is.

Figure 5: Incorrect shell offset option for the selected face

 

In the image you see below, the Bottom Surface Offset option has been selected and can be seen to be the correct direction to cover the thickness of this sheet metal part. It should be observed that a green side is on one side of the thickness and an orange side is on the other side of the thickness.

Figure 6: Correct shell offset option for the selected face

 

Now that you have defined a shell by its selected face, make sure that you use that same face or faces when defining the studies Loads, Mesh Controls, Fixtures, and Contact Sets. Otherwise, the program will not know what you mean and will throw errors when the study is running and will fail to finish.

If the Simulation study has a lot of shell elements in it, it can be very difficult to remember which faces were used to define the shell element to use to apply Loads, Mesh Controls, Fixtures, and Contact Sets. An easy way to visually see the selected faces that define a shell element is to click on the object in the graphics window to see it highlighted in the simulation tree. Then expand the shell manager folder to view all of the shell definitions for the part below it. Now, just click on the shell definition of interest and the faces that were used to define the shell element will be highlighted in blue as you can see below.

Figure 7: Defined shell face highlighted by clicking the feature for that shell element in the simulation feature tree.

 

Now, simply apply the conditions that you wish to apply to this highlighted face. After doing so, this shell element simulation part should be fully defined and you can move onto fully defining the next one.

What a fully meshed shell element mesh looks like

After the entire model has been set up properly in the simulation, it is now time to mesh. Shell elements have no thickness so be prepared for the geometry to look different than it did when it was a thin but solid part file.

Figure 8: What a shell element looks like meshed

 

As can be seen in the screen shot above the meshed shell element is infinitely thin and shows a gap now between the shell part and solid part. This is to be expected and will not affect the analysis if the simulation was set up correctly. Because shell elements are infinitely thin, SOLIDWORKS Simulation uses a color coding system to distinguish one side of the shell element from the other. The Orange color corresponds to the bottom surface of the shell element while the gray corresponds to the top surface of the shell element.


Author: Taran Packer

Taran is a SOLIDWORKS Simulation Technical Support Specialist at GoEngineer. He has a Bachelor’s degree in Biomedical Engineering from the University of Utah. Taran enjoys learning about different tools in SOLIDWORKS Simulation, Flow Simulation, and Plastics.

 

 

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GoEngineer
GoEngineer delivers software, technology and expertise that enable companies to unlock design innovation and deliver better products faster. With more than 30 years experience and thousands of customers in high tech, medical, machine design, energy and other industries, GoEngineer provides best-in-class design solutions from SOLIDWORKS, Stratasys, CAMWorks, Altium and Product Lifecycle Management (PLM). For more information, visit goengineer.com.

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SOLIDWORKS Tech Tip: Surfacing Techniques Made Easy http://blogs.solidworks.com/tech/2017/06/solidworks-tech-tip-surfacing-techniques-made-easy.html http://blogs.solidworks.com/tech/2017/06/solidworks-tech-tip-surfacing-techniques-made-easy.html#respond Sun, 18 Jun 2017 21:00:00 +0000 http://blogs.solidworks.com/tech/?p=17255 Many high quality designs are created using Surfacing commands in SOLIDWORKS. These commands can seem daunting to use if you’re not too experienced, however many of them are a lot simpler than you may think! For example, many thin-walled bodies

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SOLIDWORKS

Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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Many high quality designs are created using Surfacing commands in SOLIDWORKS. These commands can seem daunting to use if you’re not too experienced, however many of them are a lot simpler than you may think! For example, many thin-walled bodies are created from just a couple features. Often times, Surface Bodies are created to be oversized and incorporate twist and curvature, then they’re trimmed back to refine the shape. From there, the thin walled body can be created from thickening the surface. Check out the video below to learn more!

Want to see more SOLIDWORKS Tech Tips? Check out our playlist on YouTube to catch up on past videos or you can even jump ahead to the next video!

Do you have a suggestion for the next Tech Tip? Tell us in the comments; we’d love to hear your ideas!

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SOLIDWORKS
Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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SOLIDWORKS Part Reviewer: Bowling Pin Tutorial http://blogs.solidworks.com/tech/2017/06/solidworks-part-reviewer-bowling-pin-tutorial.html http://blogs.solidworks.com/tech/2017/06/solidworks-part-reviewer-bowling-pin-tutorial.html#respond Sat, 17 Jun 2017 21:00:45 +0000 http://blogs.solidworks.com/tech/?p=17189 Bowling Pin: This model shows how to use split line curves. It also has newer SOLIDWORKS functionality using circular profile sweeps. The circular profile sweep eliminates the need for an additional sketch with a circle on it to create the

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SOLIDWORKS

Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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Bowling Pin: This model shows how to use split line curves. It also has newer SOLIDWORKS functionality using circular profile sweeps. The circular profile sweep eliminates the need for an additional sketch with a circle on it to create the sweep.

There is an example of 3D sketch and different display states. The features used in the bowling pin include: revolves, sweeps, split line curves, extrude surfaces and a circular pattern. The model includes three different configurations and has some display states to toggle the colors of the crown or neck bands.

Download this file to learn about split line curves and display states and also to learn about bowling pin construction.

Download: Bowling Pin 
Complexity: Moderate
Features: Curve Driven Pattern, Revolve, Split Line Curve, Sweep, Extrude Surface, 3D Sketch, Circular Profile Sweep

View all the Part Reviewer Tutorials here.

DraftSight Download: In conjunction with DraftSight, Dassault Systèmes’ 2D CAD product, the 2D drawing(.dwg) file of the Bowling Pin tutorial is now available for download here.

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SOLIDWORKS
Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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Using SOLIDWORKS 3D Interconnect With Sheet Metal Parts http://blogs.solidworks.com/tech/2017/06/using-solidworks-3d-interconnect-sheet-metal-parts.html http://blogs.solidworks.com/tech/2017/06/using-solidworks-3d-interconnect-sheet-metal-parts.html#respond Fri, 16 Jun 2017 15:00:59 +0000 http://blogs.solidworks.com/tech/?p=17213 The new 3D Interconnect functionality introduced in SOLIDWORKS 2017 is useful when working with a variety of native non-SOLIDWORKS files, including parts that are sheet metal in nature. A Note On Methodology There are a few ways to add sheet metal

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GSC

GSC fuels customer success with 3D engineering solutions for design, simulation, data management, technical documentation, and 3D printing, as well as the most comprehensive consulting, technical support, and training in the industry. As a leading provider of SOLIDWORKS solutions and Stratasys 3D printing technologies, GSC’s world-class team of dedicated professionals have helped numerous companies innovate and increase productivity by leveraging advanced technologies to drive 3D business success. Founded in 1989, GSC is headquartered in Germantown, WI. For more information about GSC, please visit www.gsc-3d.com.

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The new 3D Interconnect functionality introduced in SOLIDWORKS 2017 is useful when working with a variety of native non-SOLIDWORKS files, including parts that are sheet metal in nature.

3D Interconnect Sheet Metal Example

A Note On Methodology

There are a few ways to add sheet metal information to a part referencing an external file. The trick when using 3D Interconnect is to add bends specifically using the Convert To Sheet Metal feature. Yes, the Add Bends feature will work initially. However, if a new version of the part comes along that changes more than the part thickness, the update will not work.

Now that we have the preliminaries out of the way, I present the method I’ve discovered to use SOLIDWORKS 3D Interconnect with sheet metal parts. If you try it, I’d love to hear how this method worked out for you.

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GSC
GSC fuels customer success with 3D engineering solutions for design, simulation, data management, technical documentation, and 3D printing, as well as the most comprehensive consulting, technical support, and training in the industry. As a leading provider of SOLIDWORKS solutions and Stratasys 3D printing technologies, GSC’s world-class team of dedicated professionals have helped numerous companies innovate and increase productivity by leveraging advanced technologies to drive 3D business success. Founded in 1989, GSC is headquartered in Germantown, WI. For more information about GSC, please visit www.gsc-3d.com.

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A Complete Guide to Using SOLIDWORKS Rx http://blogs.solidworks.com/tech/2017/06/complete-guide-using-solidworks-rx.html http://blogs.solidworks.com/tech/2017/06/complete-guide-using-solidworks-rx.html#respond Thu, 15 Jun 2017 15:00:18 +0000 http://blogs.solidworks.com/tech/?p=17200 The SOLIDWORKS Rx tool allows you to easily capture video and diagnostic information for troubleshooting problems, checking your system performance, and updating your video card driver. It also allows you to run tests and compare your results with fellow SOLIDWORKS

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Alignex, Inc.

Alignex, Inc. is the premier provider of SOLIDWORKS software and partner products to the mechanical engineering industry in Minnesota, Wisconsin, Iowa, North Dakota, South Dakota, Colorado and Wyoming. With more than 25 years of technical experience, Alignex offers consulting services, training and support for SOLIDWORKS as well as support for partner products. For more information, visit alignex.com.

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The SOLIDWORKS Rx tool allows you to easily capture video and diagnostic information for troubleshooting problems, checking your system performance, and updating your video card driver. It also allows you to run tests and compare your results with fellow SOLIDWORKS users.

By familiarizing yourself with how to use the SOLIDWORKS Rx tool, you’ll have the diagnostic tools to communicate and solve any problems you come across.

How do I open SOLIDWORKS Rx?

SOLIDWORKS Rx can be opened from the Windows start menu or from the SOLIDWORKS task pane under the SOLIDWORKS Tools.

SOLIDWORKS Rx Guide

In Windows 7 and older you will find the SOLIDWORKS Rx tool by following this path:

Windows Start > Programs > SOLIDWORKS 20xx > SOLIDWORKS Tools folder

On the newer Windows platform you can either search type in the name, if you are using Cortana, or you can manual scroll through the apps.

SOLIDWORKS Rx Guide

Why use SOLIDWORKS Rx?

SOLIDWORKS Rx is a valuable tool that can help you monitor and test your computer and SOLIDWORKS performance.

When you open SOLIDWORKS Rx you will see this window.

SOLIDWORKS Rx Guide Programs

Next, you will see a listing of tabs at the top of your window. These are also listed in the first inset window as hyperlinks for faster access.

There is another inset beneath the first.

SOLIDWORKS Rx Guide Tabs

This has two tools that you can use for testing purposes.

  1. The ‘Click here to Launch SOLIDWORKS in OpenGL mode’ will open a session of SOLIDWORKS that will not use on CAD video card. This can be helpful test to see if the graphic issue in SOLIDWORKS has to do with your graphics card or graphics card firmware or software.
  2. The other tool you will see is ‘Click here to launch SOLIDWORKS while bypassing the Tools/Options settings’. Click here to launch your SOLIDWORKS. Since this tool bypasses your SOLIDWORKS Tools and System Options, you might use this as a test to verify the SOLIDWORKS issue you are seeing is related to something you have customized in your options or something that is not functioning correctly.

SOLIDWORKS Rx Diagnostics Tab

This will list your current hardware and system settings that affect SOLIDWORKS.

Most important is the graphics card information on the very top.

You should always go to the SOLIDWORKS video card tested website and filter through the options to get a tested SOLIDWORKS video card driver for your system.

SOLIDWORKS Rx Diagnostics Guide

An out-of-date driver can lead to instability and strange graphical behaviors.

If your graphics card is out of date, you may need to update your graphics by going to the video card testing website.

You can also see a diagnostic test warning about our Toolbox.

SOLIDWORKS Rx Troubleshoot Tab

This will need a login to your SOLIDWORKS Customer Portal for full access. You can see by the list there are 12 areas you can explore to fix information in the SOLIDWORKS Knowledge Base (KB).

SOLIDWORKS Rx Guide

SOLIDWORKS Rx Guide

System Maintenance 

This allows several optional automated tasks with a single click.

  • Clean SOLIDWORKS backup directory
  • Clean SOLIDWORKS temporary directory
  • Clean Windows temporary directory
  • Clean temporary internet files
  • Cleaning temporary files in SOLIDWORKS data folders
  • Run Checkdisk
  • Run Windows Defragmenter

SOLIDWORKS Rx Guide

SOLIDWORKS Rx Problem Capture Tab

SOLIDWORKS may or may not be running in the background when you run the tool. If an issue starts to occur during your SOLIDWORKS session, for example, you can start Rx and begin recording a video of what you are seeing. This information is invaluable when troubleshooting issues. This information can capture the process flow to create an issue you are seeing in your SOLIDWORKS as well as gathering important operating system information. There are three steps to a Problem Capture.

STEP 1: Record

SOLIDWORKS Rx Guide

After clicking on start capture you will see this screen.

SOLIDWORKS Rx Guide

In most cases you will select ‘Use Current Session’.  If you are going to start a new session of SOLIDWORKS and demonstrate the issue in its entirety, then choose ‘Restart SOLIDWORKS Now’.

Click on the ‘Start Recording’ button.

SOLIDWORKS Rx Guide

Note: if you have dual monitors and the SOLIDWORKS menus do not appear inside the SOLIDWORKS graphics window, then these windows will not be recorded.

Click the record, move the record menu window aside so we can capture and access all of SOLIDWORKS as we record this issue. When done recording, click on ‘Finish Recording’.

SOLIDWORKS Rx Guide

Next, you will be prompted to close SOLIDWORKS to complete the next steps of the problem capture.

SOLIDWORKS Rx Guide

STEP 2: Package Files

Be sure to add your SOLIDWORKS files using ‘Add More Files to Zip’ if necessary and make sure you select a location, to save this information so you do not have to search for after the Problem Capture creation is complete.

SOLIDWORKS Rx Guide

SOLIDWORKS Rx Guide

SOLIDWORKS Rx Guide

Next, select Continue to Step 3’.

SOLIDWORKS Rx Guide

STEP 3: Description You will need to completely fill out the Problem Capture Details form.

SOLIDWORKS Rx Guide

Once you click ‘OK’ your RX package will be saved. The resulting zip folder will need to be sent to Alignex. If the zip folder is larger than 10MB, please upload it to our FTP server.

SOLIDWORKS Rx Guide

SOLIDWORKS Rx Reliability Tab

The Reliability tab provides you with information on sessions that have been terminated in the past 60 days. To use this tab you can review the daily summary to see different color icons.

  • Blue is a normal termination
  • Orange is terminated by user

Red indicates terminated unexpectedly

SOLIDWORKS Rx Guide

For sessions terminated by the user or terminated unexpectedly, the Session Ending section lists Windows events. This includes events like driver crashes or network failures.

For sessions that terminate unexpectedly, the Reliability tab displays a call stack.

Click on the number in the session with the same stack to display the list. This data can help communicate important information about what might be causing SOLIDWORKS to terminate.

Windows and installation events shows us windows drivers and patches.

(When you create the Problem Capture, all this information is collected into a zipped file folder.)

SOLIDWORKS Rx Benchmark Tab

The SOLIDWORKS Performance Benchmark Test is used to run tests and compare results with other SOLIDWORKS users.

www.solidworks.com/benchmarks

Before running a Benchmark, note the following:

  • Reboot your computer before starting
  • This test can take 30 minutes or more depending on your computer configuration
  • Do not use your computer for other applications during this test

SOLIDWORKS Rx Guide



Written By: Matthew Kusz , Application Engineer at Alignex, Inc. Matthew is a regular contributor to the Alignex Blog. Find more tech tips on the Alignex Blog and
 subscribe to get content like this delivered straight to your inbox.

Author information

Alignex, Inc.
Alignex, Inc. is the premier provider of SOLIDWORKS software and partner products to the mechanical engineering industry in Minnesota, Wisconsin, Iowa, North Dakota, South Dakota, Colorado and Wyoming. With more than 25 years of technical experience, Alignex offers consulting services, training and support for SOLIDWORKS as well as support for partner products. For more information, visit alignex.com.

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No More Disappearing Menu Boxes with this Trick http://blogs.solidworks.com/tech/2017/06/no-disappearing-menu-boxes-trick.html http://blogs.solidworks.com/tech/2017/06/no-disappearing-menu-boxes-trick.html#respond Wed, 14 Jun 2017 15:00:15 +0000 http://blogs.solidworks.com/tech/?p=17150 When it comes to designing, speed and efficiency definitely matter most. In SOLIDWORKS, the best way to do something usually turns out to be the quickest or most efficient way. One of the most best ways to focus on your

Author information

Stephen Petrock

Since 1998, TriMech has helped our clients design better products by partnering with them and offering, not only CAD, CAE, PDM, FEA, CAM software products, but also by engineering solutions involving full-time and temporary staffing, contract design, analysis and drafting services, rapid prototyping, custom programming and implementation services. TriMech is a value-added reseller of SOLIDWORKS and Stratasys 3D Printers in the Mid-Atlantic and South-East including New Jersey, Pennsylvania, Delaware, Maryland, West Virginia, Virginia, North Carolina, South Carolina, Tennessee, South Carolina, Georgia, Florida, Alabama, Mississippi, Oklahoma, Arkansas and Louisiana.

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When it comes to designing, speed and efficiency definitely matter most. In SOLIDWORKS, the best way to do something usually turns out to be the quickest or most efficient way. One of the most best ways to focus on your designs and model quicker is to take advantage of the context menus that appear as you click on an item. These are those boxes that appear offering you quick access to things like sketch relations or mates.

SOLIDWORKS Menu BoxesClick on an entity and a box appears; but move your mouse anywhere but directly to it and it will disappear. This may seem passive aggressive at first but really it makes sense. If you don’t immediately need or use the functionality it disappears so it won’t come between you  and your model. But what  if you want to use that functionality? How do you get these context boxes to appear again? 

It’s easy! Just move your mouse to the area where the box was press the control key. This will bring the box back, giving you access to that quick and direct modeling functionality.

Author information

Stephen Petrock
Since 1998, TriMech has helped our clients design better products by partnering with them and offering, not only CAD, CAE, PDM, FEA, CAM software products, but also by engineering solutions involving full-time and temporary staffing, contract design, analysis and drafting services, rapid prototyping, custom programming and implementation services. TriMech is a value-added reseller of SOLIDWORKS and Stratasys 3D Printers in the Mid-Atlantic and South-East including New Jersey, Pennsylvania, Delaware, Maryland, West Virginia, Virginia, North Carolina, South Carolina, Tennessee, South Carolina, Georgia, Florida, Alabama, Mississippi, Oklahoma, Arkansas and Louisiana.

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SOLIDWORKS Support Monthly News – June 2017 http://blogs.solidworks.com/tech/2017/06/solidworks-support-monthly-news-june-2017.html http://blogs.solidworks.com/tech/2017/06/solidworks-support-monthly-news-june-2017.html#respond Wed, 14 Jun 2017 08:17:12 +0000 http://blogs.solidworks.com/tech/?p=16936 Hello to all, Welcome to this new edition of the SOLIDWORKS Support Monthly News, coauthored by members of the SOLIDWORKS Technical Support teams worldwide. It’s SOLIDWORKS Knowledge Base Month! OK, that’s not really true: Every month is SOLIDWORKS Knowledge Base

Author information

Julien Boissat

Sr. Technical Customer Support Engineer, SolidWorks, EMEA at DS SolidWorks Corp.

I have been a Tech Support engineer for Simulation products since 2002. I was previously a product manager at SRAC, the original makers of COSMOS for those who remember that time! ;-). I am currently in charge of the content of the certification exams for simulation products. I also initiated and still author the Simulation Knowledge Base and participate as much as possible in the expansion and evolution of the SolidWorks Knowledge Base. Finally, I handle the SolidWorks Support Monthly News blog.

The post SOLIDWORKS Support Monthly News – June 2017 appeared first on SOLIDWORKS Tech Blog.

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Hello to all,

Welcome to this new edition of the SOLIDWORKS Support Monthly News, coauthored by members of the SOLIDWORKS Technical Support teams worldwide.

It’s SOLIDWORKS Knowledge Base Month!

OK, that’s not really true: Every month is SOLIDWORKS Knowledge Base Month! Do you count yourself among the thousands of SOLIDWORKS professionals who search the Knowledge Base (KB) each month to find answers to questions and solutions to problems? There is a good chance that there is a solution already available that will answer your support question. If so, a KB Search can save you valuable time.

Key indicators:

  • More than 30,000 Solutions published to users
  • Solution with most views has more than 34,000 of them
  • 4,500 Solutions reviewed and updated in the last 12 months

 

As you can imagine, much activity takes place to ensure we are delivering useful and actionable information in the Knowledge Base, and our KB users play an important role in helping us define and deliver high value KB content. As an example, we actively review the information you submit in the Submit Feedback form on the KB Search web page (see the screen capture to the left); we use your feedback to identify areas of need and topics that we can improve and refresh. If you are unhappy with a Solution, please give us a hint in the Comments field about the nature of your dissatisfaction (Solution may be obsolete, duplicate or incomplete for instance).
There’s nothing so obvious that a short comment won’t help clarify.

 

SOLIDWORKS 2018 Beta – looking back 10 years ago

While we eagerly wait for the beginning of this year’s Beta program (around the end of June) to discover and test all the new features in version 2018, let’s take a look back at what shook the world of SOLIDWORKS ten years ago, in version 2008. It is really amusing to see how what we now take for granted once made the big headlines in the What’s New pages of the documentation!

SOLIDWORKS

  • Instant3d!  – you can now grab any face or feature and graphically drag to resize the geometry!  Turn cuts into extrudes and vice versa!
  • Fun fact! When version 2008 was released, it shipped in bigger boxes than version 2007: two DVDs (for the x32 and the x64 editions) were included, whereas in version 2007 both editions could fit on a single DVD.
  • S Key shortcut menu – the S key launches a context sensitive toolbar next to the cursor – this is huge time-saver when modeling.
  • RealView. Check out these scenes!
  • Let’s not forget the UI overhaul, now with a CommandManager
  • … and an expandable menu bar

  • New tools:

    • DimXpert for parts is a set of tools that applies dimensions and tolerances to parts according to the requirements of the ASME Y14.41-2003 standard.

    • TolAnalyst is a tolerance analysis application that determines the effects that dimensions and tolerances have on parts and assemblies

    • DFMXpress checks your designs for manufacturability.You can identify areas that are difficult, expensive, or impossible to machine early in the design process.

    • DriveWorksXpress is a design automation tool you can use to automatically generate parts, assemblies, and drawings based on predefined design information.

SOLIDWORKS Simulation

  • New study types
    • Pressure Vessel
    • Linear Dynamic: Modal time History, Random Vibrations, Harmonic
    • Nonlinear Dynamic
  • You can mix beams, shells, and solids in a mixed mesh study

SOLIDWORKS Motion

  • Motion Studies now use the MotionManager (adapted from SOLIDWORKS Animator).

SOLIDWORKS Flow Simulation

  • Project is saved to model. Now the created project is saved together with the model’s geometry in the same CAD file, eliminating the need to have the separate project file. You do not need to worry about the project file (the .fwp file) anymore when copying or moving the model files.
  • New types of fans. The Axial and Radial fans

  • Automatic correction of invalid contacts and Highlighting of invalid contacts remaining in the model.

  • Real gases

If you liked that time travel session, check out the May 2014, June 2014 and May 2015 editions of the SOLIDWORKS Support Monthly News for a reminder of the best enhancements in versions 2004, 2005 and 2001 respectively.

Understanding sheet metal sketches, transformed sketches and how they behave

By Mario Iocco

Sheet metal parts can have sketches in the folded and in the flat pattern state (Fig. 1)

Sketches created in the folded state can have an equivalent “transformed” sketch in the flat pattern state.

All sheet metal parts have a fixed face. The fixed face is the one that remains in the same position when unsuppressing the flat pattern. (Fig. 2)

Sketches created in fixed faces will not be transformed. The sketches created in non-fixed faces will be transformed when viewed in the flat pattern. (Fig. 3)

The circular sketch was created in the flat pattern fixed face., it does not need to be transformed. The square sketch was not created on a fixed face, it was transformed when unsuppressing the flat pattern feature (Fig. 4)

The transformed sketches will be visible in the flat pattern feature, under the “Sketch Transformation” folder. The sketches that has been transformed will be hidden in the folded state (Fig. 5.)

The non-transformed sketches will remain visible in the folded state (Fig. 6.)

The transformed folder does not exist when the flat pattern is suppressed (Fig. 7.)

 

The transformed folder is created only when unsuppressing the flat pattern feature (Fig. 8.)

Sketches in the Flat Pattern Drawing View

When you create a flat pattern drawing view, the system creates a flatten derived configuration. After the creation of the flat pattern drawing view, the sketches in the flatten derived configuration and drawing become independent from each other. That is, if you want to see the transformed sketches being displayed in the flat pattern drawing view, you must expand the drawing view feature tree and manually show those sketches (Fig. 9)

 

Simulation Step-Up Series

Last month, Omar discussed the topic of Basic failure analysis. This month, Reza discusses the topic of Accuracy and Convergence.

Next month, Ramesh will come back and discuss the topic of Viewing results (Parts 1 & 2).

Noteworthy Solutions from the SOLIDWORKS Knowledge Base

icon - SW After installing SOLIDWORKS® 2017, why does the ‘Pack and Go’ feature not preserve the full folder path?
‘Pack and Go’ now uses short, relative folder paths.
In versions prior to SOLIDWORKS® 2017, the entire path was used, causing problems with the Windows® 256 character limit.
For more information about this, see this What’s New topic.
In response to customer feedback, SOLIDWORKS Development now offers a solution to restore the previous functionality with a modification to the registry keys.
For more detailed information, see Solution Id: S-073053.

Icon - EPDM Using SOLIDWORKS® Enterprise PDM 2015 or later versions, how do I manually install the 64-bit version of the Autodesk® AutoCAD® add-in?
When you install the SOLIDWORKS® Enterprise PDM CAD Editor client on a system that has a 64-bit version of the Autodesk® AutoCAD® software installed, you can select to install the AutoCAD add-in. If SOLIDWORKS PDM client installer does not detect the AutoCAD software, or if you install AutoCAD after finishing the SOLIDWORKS PDM client installation, you can install the add-in manually.
For more detailed information, see Solution Id: S-072975.

How do I manually calculate the ‘Acoustic Power’ and ‘Acoustic Power Level’ to validate the values given by SOLIDWORKS® Flow Simulation?
The foundation to such a hand calculation is to follow the explanation and equations given in the “Noise Prediction” topic of the Online Help.
Attachments to Solution Id: S-072876 provide:
• A sample calculator in an Excel spreadsheet
• A sample part model
• A screen capture of ‘Acoustic Power’ and ‘Acoustic Power Level’ results

Is there a limit to the number of ‘Injection Locations’ I can place on a SOLIDWORKS® Plastics mesh?
The limit to the number of ‘Injection Locations’ you can place on a SOLIDWORKS® Plastics mesh is equal to the number of nodes comprising your mesh.
For more detailed information, see Solution Id: S-072792.
In the SOLIDWORKS® Simulation software, why do I receive the error ‘Cyclic symmetry is not supported by Frequency [or Buckling] Analysis…’?
Effective with the release of SOLIDWORKS Simulation 2017 SP3.0, the option to use Cyclic Symmetry fixtures has been removed from frequency and buckling studies. Starting with that release, you must suppress or remove ‘Cyclic Symmetry’ fixtures in frequency and buckling studies.
For more detailed information, see Solution Id: S-072834.


That’s it for this month. Thanks for reading this edition of SOLIDWORKS Support News. If you need additional help with these issues or any others, please contact your SOLIDWORKS Value Added Reseller.

Also, comments and suggestions are welcome. You can enter them below.

 

Author information

Julien Boissat
Sr. Technical Customer Support Engineer, SolidWorks, EMEA at DS SolidWorks Corp.
I have been a Tech Support engineer for Simulation products since 2002. I was previously a product manager at SRAC, the original makers of COSMOS for those who remember that time! ;-). I am currently in charge of the content of the certification exams for simulation products. I also initiated and still author the Simulation Knowledge Base and participate as much as possible in the expansion and evolution of the SolidWorks Knowledge Base. Finally, I handle the SolidWorks Support Monthly News blog.

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SOLIDWORKS Harry Potter’s Golden Snitch Tutorial – Part 2 http://blogs.solidworks.com/tech/2017/06/solidworks-harry-potters-golden-snitch-tutorial-part-2.html http://blogs.solidworks.com/tech/2017/06/solidworks-harry-potters-golden-snitch-tutorial-part-2.html#respond Tue, 13 Jun 2017 21:00:41 +0000 http://blogs.solidworks.com/tech/?p=17058 It’s safe to say that Quidditch is Harry Potter’s favorite wizarding pastime. As Hagrid would say, a wizard’s passion for Quidditch is the equivalent to a muggle’s passion for football. This year marks the 20th anniversary of the first publication

Author information

SOLIDWORKS

Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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It’s safe to say that Quidditch is Harry Potter’s favorite wizarding pastime. As Hagrid would say, a wizard’s passion for Quidditch is the equivalent to a muggle’s passion for football. This year marks the 20th anniversary of the first publication in the series, Harry Potter and the Sorcerer’s Stone. To celebrate, we are showing SOLIDWORKS users how to model the Golden Snitch – the little ball that Harry loves to hate. So hop on your Nimbus 2000 and let’s get started flying through our four part series.

SOLIDWORKS Harry Potter's Golden Snitch Tutorial

Welcome to part 2 of our 4-part series where we are celebrating the anniversary of the release of the first Harry Potter book, by modeling arguably the cutest, yet most frustrating object from the wizarding world, the Golden Snitch. We began laying out the Snitch’s body in part 1 of the series, now, in part 2, we will finish up adding the detail to the outside of the body using a few more projected curves and sweeps, plus we’ll prep the body for mirroring using the Split tool.

Wizards and muggles alike can learn something new from our Golden Snitch tutorial series! Can’t wait to watch the next video? View all of the tutorials on the playlist here.

Author information

SOLIDWORKS
Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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7 Insider Secrets to Create Amazing Illustrated Manuals with SOLIDWORKS Composer http://blogs.solidworks.com/tech/2017/06/7-insider-secrets-to-create-amazing-illustrated-manuals-with-solidworks-composer.html http://blogs.solidworks.com/tech/2017/06/7-insider-secrets-to-create-amazing-illustrated-manuals-with-solidworks-composer.html#respond Sun, 11 Jun 2017 21:00:49 +0000 http://blogs.solidworks.com/tech/?p=16960 By Ferry Vermeulen and Vadim Rybakov You have spent months, or even years, on the development of your super user-friendly product, but the user manual still sucks. You don’t want your user to have a bad customer experience due to

Author information

Ferry Vermeulen

Ferry Vermeulen
Director at INSTRKTIV

I am director at Berlin and Amsterdam based INSTRKTIV GmbH. INSTRKTIV helps brands to create compliant and user-friendly user instructions.

The post 7 Insider Secrets to Create Amazing Illustrated Manuals with SOLIDWORKS Composer appeared first on SOLIDWORKS Tech Blog.

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By Ferry Vermeulen and Vadim Rybakov

You have spent months, or even years, on the development of your super user-friendly product, but the user manual still sucks.

You don’t want your user to have a bad customer experience due to struggling with your manual. Ideally, you would like to have an easy to understand, comprehensible and well-illustrated manual…. Or even better. But just how do manual designers produce comprehensible manuals? Do you ever wonder what their secret is when creating a user friendly manual?

In this post, we will reveal the untapped secrets of the best manual designers for creating awesome instructions and will give you clear instructions on how you can do exactly the same using SOLIDWORKS Composer.

1. Do not illustrate your manual

There is one major thing that should be mentioned that really distinguishes good manuals from the rest, and it takes the number one position in this post: good manuals are incredibly continuous.

This cannot be achieved by illustrating the drawings based on photos or free drawing techniques. Awesome illustrations are mostly created with the original 3D technical drawings.

In order to create comprehensible drawings, make sure you have 3D models of your product available. If you don’t have them, maybe because you simply imported the product, you can easily have them created using freelancers on platforms like Upwork.

To help create a 3D model, make sure you send your freelancer very clear photos of all the details and moving parts that are needed to explain the use of your product in the user manual.

When your 3D model is ready, use SOLIDWORKS Composer to create comprehensive illustrations for technical communication.

Clear manuals usually always have the same perspective and view. With SOLIDWORKS Composer, you can set the desired perspective and view and use it for every illustration, over and over again.

Designers take pains to render each successive picture from a single, unchanging point-of-view (mimicking that of the customer), so that confusing rotations or perspective changes are minimized. The customer can stay oriented more easily as he or she moves back and forth between the booklet and the parts.

To create illustrations with the same perspective and view using SOLIDWORKS Composer:

  1. Select File>Open.
    The Open dialog appears.
  2. Select the file you want to open and click Open.
  3. Click on the arrow of the Align Camera icon in the Home Select one of the ¾ views from the list. Usually, these four views will be sufficient to create all you illustrations. By choosing one of them, you will always get the same view of your product.


  1. Select File>Preferences.
    The Application Preferences dialog appears.
  2. Select Camera. Set the Default perspective to 20 degrees.
  3. Click OK.

Explanation:

Fig. 1 – The same product view but with different perspectives.

Fig. 2 – Three different products but with the same view and perspective.

Figure 2 shows the same view but with different perspective angles. The larger the angle, the bigger the distortions will be. By using a ¾ views and by setting the perspective angle, you will always get the same view and perspective for all of your products.

2. Make use of distinctive colors

Although most manuals have a black and white appearance, smart manual designers work closely with product designers to use color-coding in their products.

When colors play an important role for being able to install the product correctly, smart product designers make sure a colored image is not necessary by coding the color in their products.

For example, with products that require electrical installation, it’s pretty important that you know exactly how to connect electrical wires. Where the wires of many products are a uniform brown, blue or black, as a manufacturer you could add an extra coding, like a black line or a spiral-shaped design. By doing this, the colored wires can easily be distinguished, even in a black and white user manual.

To create illustrations with color coding:

  1. Click on the Technical Illustration icon in the Home The Technical Illustration pane appears.
  2. Uncheck the Color Regions checkbox from the Workshops pane.

 

    1. Click Save As… to save the file as a SVG file on your computer.

 

  1. Open the saved filed in Adobe Illustrator. Add the color coding.

3. Add text to the user manual

An image does not need to be translated and an image says more than 1000 words. Those are the main reasons why many brands limit the text in their user manuals. However, not using text isn’t always possible. Often times, text isn’t always necessary when only the installation of a product needs to be described (and not the use of a product). For some products however, describing the use is a must.

Text can also increase the safety level when there are installation steps that contain a higher level of risk, for example during electrical installation. Also, any other warnings against residual risks during the complete product life cycle can be added in text.

Where installation steps can only be explained fully with illustrations, explaining the use of a more complex product may still need some textual support.

To add text to illustrations using SOLIDWORKS Composer:

  1. Click on the Text 2D icon in the Author

  1. Click in the middle pane on the location where you want to add text. Type your text.

  1. Edit the font, background color, shadow, etc. from the Properties

  1. You can add another text field or you can move the product image or text.

4. Avoid a comic-book kind of approach

Although many well illustrated manuals very much look like a comic book, telling a story with a user manual should be completely avoided; think in topics when creating your user manual! Topic based communication in technical manuals uses a modular approach for content creation. With this approach, all content is structured around topics.

A topic always has a well-defined beginning and ending. At the end of a topic, a particular task has been completed. This has huge advantages. By structuring around topics, (parts of) topics can be mixed and reused in different contexts. The opposite of topic-based authoring is narrative content, written in the same type of linear structure as written books. One example of a topic-based approach would be the way the following task is described:

  • Use a screw driver to attach all 14 screws (article number 118331).

By using a topic based approached, illustrations can be reused throughout the manual, or even throughout manuals about other products, especially if you use the same views all the time.

5. Use the right tools

With the right 3D software you can create comprehensive illustrations. With these tools you can set your perspective and views to create consistent illustrations and ensure consistency for all future publications.

I think SOLIDWORKS Composer is by far the best tool to use to achieve the desired level of branding in your company’s instructions. But, whatever software you use, make sure to export your drawings as vector images.

 

Fig. 3 – An illustration made with SOLIDWORKS Composer

 

6. Begin with a promise

Consider beginning you manual with a promise: the end result. This has a HUGE psychological effect. When buying a product or DIY product, you often dedicate your evening or Saturday afternoon to build your recent purchase. By directly visualizing the end result at the beginning, the user is confident that he will complete his task successfully.

To start with a promise:

  1. In SOLIDWORKS Composer, make sure you have chosen the same view and perspective as the rest of the drawings (see step 1).
  2. Create an illustration of the fully assembled product.
  3. Add this illustration as the first picture in the user manual

7. Use corporate guidelines

Consistent illustrations determine for a large part the look and feel of your manual. However, in order to create ultimate consistent manuals, you should use corporate guidelines for your instructions.

These guidelines include elements for the brand design, logo and a specific font and colors. When using text, also consider to use guidelines for the language (American English or British English?), the tone of voice, the system of measurement, how do different types of information look like (e.g. warnings, instructions, tips) or when to use various types of highlighting (e.g., bold or italics type).

To choose specific (line) colors in SOLIDWORKS Composer:

  1. Click on the Technical Illustration icon in the Home The Technical Illustration pane appears.
  2. Click on the arrow from the Show visible lines dropdown menu.

  1. Select More Colors…
  2. Choose the required color.

  1. Select the Preview button to see how your illustration will look like.

 

To use your company’s font:

    1. Click on the Text 2D icon in the Author

 

    1. Click in the middle pane on the location where you want to add text. Type your text.
    2. Make sure your text is selected.
    3. In the Text field of the Properties pane, click on the button with the three dots behind the font. The font window appears.
    4. Select the font you need.

To add your company logo:

  1. Click on the Image 2D icon in the Author Select Image 2D.

    1. Click in the middle pane and create a logo place holder by dragging your computer mouse.

 

  1. Make sure the logo field is selected. In the Texture field of the Properties pane, click on the button with the three dots behind Map Path. Browse to your logo, select it and click OK. Your logo is placed. Notice: added 2D images will not appear in the technical illustration preview. To see your logo, save the file as as SVG or EPS file.

  1. In the Placement field of the Properties Pane, make sure that Keep Aspect Ratio is checked to avoid distortions of your image.
  2. In the Border field of the Properties Pane, make sure that the checkbox is unchecked.
  3. In the Shadow field of the Properties Pane, make sure that the checkbox is unchecked.

Conclusion

Your user deserves a great user experience at every stage of their customer journey and after spending all that time creating a great product, you also want to give your customer a good experience when consulting the user instructions.

Imagine a user being able to install or use your product without any help from customer support.

Imagine a user manual that contributes to a better user experience.

You can achieve this!

In order to do so, follow the steps as described in this post and your users will as excited when installing or using your product with your stunning user manual as you want them to be!


Vadim Rybakov
Freelance Technical Illustrator
I have over six years of experience with Solidworks Composer. What started as a hobby evolved to helping dozens of companies in creating professional technical illustrations. Take a look at my works on Behance and Linkedin.

Author information

Ferry Vermeulen
Ferry Vermeulen
Director at INSTRKTIV
I am director at Berlin and Amsterdam based INSTRKTIV GmbH. INSTRKTIV helps brands to create compliant and user-friendly user instructions.

The post 7 Insider Secrets to Create Amazing Illustrated Manuals with SOLIDWORKS Composer appeared first on SOLIDWORKS Tech Blog.

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SOLIDWORKS PDM Forms Series Part 3: XML as Forms http://blogs.solidworks.com/tech/2017/06/solidworks-pdm-forms-series-part-3-xml-as-forms.html http://blogs.solidworks.com/tech/2017/06/solidworks-pdm-forms-series-part-3-xml-as-forms.html#respond Sun, 11 Jun 2017 15:00:14 +0000 http://blogs.solidworks.com/tech/?p=17053 Written by: Bryce Hooper, Application Engineer at DASI Solutions In case you missed the earlier parts, check out Part 1 on Excel and Part 2 on Word. To conclude the series on PDM and EC forms, we’ll discuss something that

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DASI Solutions

DASI Solutions

DASI Solutions is dedicated to service and support. As one of a handful of original, charter value-added resellers (VAR) in the SolidWorks Community, DASI Solutions has built partnerships and success stories with many of our customers. We are very pleased to bring you SolidWorks 3D CAD design engineering software and 3D printing services.

The post SOLIDWORKS PDM Forms Series Part 3: XML as Forms appeared first on SOLIDWORKS Tech Blog.

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SOLIDWORKS PDM Tech Tip

Written by: Bryce Hooper, Application Engineer at DASI Solutions

In case you missed the earlier parts, check out Part 1 on Excel and Part 2 on Word.

To conclude the series on PDM and EC forms, we’ll discuss something that not everyone is familiar with and most aren’t quite sure what it does. XML, or the Extensible Markup Language, can be used to store data. What does XML do exactly? Well, according to the source for web standards, W3 Schools, XML does nothing. That’s right. It does nothing.  However, it does store and allows us to organize data. For example, we can look at my EC form.

This form in the end will look very similar to the forms used in the first and second installments of this blog series. But to start, we have this:


<?xml version=”1.0″ encoding=”UTF-8″?>
<EC_Form>
                <EC_Number>17020006</EC_Number>
                <EC_Part_Number>A0004</EC_Part_Number>
                <EC_Notice_Date>2017-02-18</EC_Notice_Date>
                <EC_Department>Painting</EC_Department>
                <EC_Old_Rev>A</EC_Old_Rev>
                <EC_New_Rev>B</EC_New_Rev>
                <EC_Description_of_Change>Change paint color to blue</EC_Description_of_Change>
                <EC_Reason_for_Change>Green no longer attainable</EC_Reason_for_Change>
                <EC_Effected_Parts>A0004</EC_Effected_Parts>
                <Signatures>
                                <Creator>BKH</Creator>
                                <Created_Date>2017-02-18</Created_Date>
                                <EC_Approval_ENG></EC_Approval_ENG>
                                <EC_Approval_ENG_Date></EC_Approval_ENG_Date>
                                <EC_Approval_MFG></EC_Approval_MFG>
                                <EC_Approval_MFG_Date></EC_Approval_MFG_Date>
                                <EC_Approval_QUAL></EC_Approval_QUAL>
                                <EC_Approval_QUAL_Date></EC_Approval_QUAL_Date>      </Signatures>
</EC_Form>

So what do we have here? Well, we can see with the starting tag that we have an EC form. Everything within that tag is data for that EC Form. Going down the line we find the same information that we had in the previous forms, just with a different look. It’s still readable, but it isn’t necessarily pretty. There are a few things to understand about this data.

According to W3schools.com:

  • XML was designed to be read and understood by both machine and human.
  • XML was designed to store and transport data.
  • XML was designed to be self-descriptive

These things seem to make sense when we look at our data. Our tags aren’t difficult to read, they seem to be labeled to make sense. And clearly this is storing data. It even does so in a very small format. (This file is about 920 bytes, as opposed to a 26 kilobytes file in Word. Not a huge file either way, but the difference is still large.)

W3 Schools also goes on to mention that XML is designed to be a similar markup language as HTML. As we all should know, webpages are made of HTML and allow us to make nice looking forms and pages. There must be a way to combine the two… but we’ll get to that later.

It is important to know, that XML does not have any pre-defined tags.  The tags shown in my examples are made up by me, and are nothing you have to stick with.

With that in mind, we will continue by setting up the variables inside of PDM.

Edit Variable in SOLIDWORKS PDM

 

The block name for this file type is quite simple. It is just XML. Same for the file type. The Attribute names can get a little… tricky. The SOLIDWORKS help goes more into what is possible, but I will start here with what I have in this image. We’ve already looked at the structure of my XML document. We saw that an EC_Form tag encompasses the whole form. From there we have children tags. This is reflected in the Attribute name. We start at the root level, and add the child levels after a slash (“/”). For this case it is “EC_Form/EC_Old_Rev”. My example above also has some tags buried 3 levels deep. These will look similar to this “EC_Form/Signatures/EC_Approval_ENG”.

Note: We cannot have any spaces in the names of our attributes in XML. The spaces cause issues interpreting the files.

Since we have this mapped, we will need a base template before the data card will automatically enter our data.

What is important, is that we create any root tags so that their children tags and be given values and that we have our most important header tag.


<?xml version=”1.0″ encoding=”UTF-8″?>
<EC_Form></EC_Form>

With this little bit of information, PDM can write the rest.

So… this looks nothing like a form. We can’t present this to anyone. What more can we do?  Similar to HTML, which has CSS to stylize; XML has XSL. This is the eXtensible Stylesheet Language. With this, and an additional tag, we can convince our XML document to look presentable.

Here we can write a little bit of HTML and CSS in an XSL format to help us display our data. My form isn’t too complicated, just a simple table and some formatting. I won’t go too in depth on how to write this as the focus on this is the XML as a form. However, I will provide my sample code.


<?xml version=”1.0″ encoding=”UTF-8″?>
<xsl:stylesheet version=”1.0″ xmlns:xsl=”http://www.w3.org/1999/XSL/Transform”>
                <xsl:template match=”/”>
                  <html>
                                <style>
                                p.title
                                {
                                                text-align:center;
                                                font-size:28.0pt;
                                                line-height:107%;
                                                margin-top:0in;
                                                margin-right:0in;
                                                margin-bottom:8.0pt;
                                                margin-left:0in;
                                                line-height:107%;
                                                font-family:”Calibri”;
                                }
                                td.label
                                {
                                                background-color:black;
                                                color:white;
                                                border:solid windowtext 1.0pt;
                                                padding:0in 5.4pt 0in 5.4pt
                                                valign:middle;
                                                align:center;
                                                font-family:”Calibri”;
                                }
                                td.value
                                {
                                                background-color:white;
                                                color:black;
                                                font-family:”Calibri”;
                                }
                                </style>
                                <body>
                                                <xsl:for-each select=”EC_Form”>
                                                                <p class=”title” align=”center”><img width=”166″ height=”84″ src=”../../Templates/DASILogoJan30.png”/>Engineering Change Notice</p>
                                                                <table border=”1″ cellspacing=”0″ cellpadding=”0″ align=”center”>                                                                <tr>
                                                                  <td class=”label” width=”120″>Part Number:</td><td class=”value” width=”150″><xsl:value-of select=”EC_Part_Number”/></td>
                                                                  <td class=”label” width=”120″>Old Rev:</td><td class=”value” width=”150″><xsl:value-of select=”EC_Old_Rev”/></td>
                                                                </tr>

                                                                <tr>
                                                                  <td class=”label” width=”120″>Date of Notice:</td><td class=”value” width=”150″><xsl:value-of select=”EC_Date_of_Notice”/></td>
                                                                  <td class=”label” width=”120″>New Rev:</td><td class=”value” width=”150″><xsl:value-of select=”EC_New_Rev”/></td>
                                                                </tr>

                                                                <tr>
                                                                                <td class=”label” width=”270″ colspan=”2″>Description of Change:</td>
                                                                                <td class=”label” width=”120″>Department:</td><td class=”value” width=”150″><xsl:value-of select=”EC_Department”/></td>
                                                                </tr>

                                                                <tr>
                                                                                <td class=”value” width=”540″ height=”100″ colspan=”4″ valign=”top”><xsl:value-of select=”EC_Description_of_Change”/></td>

                                                                </tr>

                                                                <tr>
                                                                                <td class=”label” width=”540″ colspan=”4″>Reason for Change:</td>
                                                                </tr>

                                                                <tr>
                                                                                <td class=”value” width=”540″ height=”100″ colspan=”4″ valign=”top”><xsl:value-of select=”EC_Reason_for_Change”/></td>
                                                                </tr>

                                                                <tr>
                                                                                <td class=”label” width=”540″ colspan=”4″>Effected Parts:</td>
                                                                </tr>

                                                                <tr>
                                                                                <td class=”value” width=”540″ height=”100″ colspan=”4″ valign=”top”><xsl:value-of select=”EC_Effected_Parts”/></td>
                                                                </tr>

                                                                <tr>
                                                                                <td class=”label” width=”120″>Creator:</td><td class=”value” width=”150″><xsl:value-of select=”Signatures/Creator”/></td>
                                                                                <td class=”label” width=”120″>Created Date:</td><td class=”value” width=”150″><xsl:value-of select=”Signatures/Created_Date”/></td>
                                                                </tr>

                                                                <tr>
                                                                                <td class=”label” width=”120″>Engineering Approval:</td><td class=”value” width=”150″><xsl:value-of select=”Signatures/EC_Approval_ENG”/></td>
                                                                                <td class=”label” width=”120″>Approved Date:</td><td class=”value” width=”150″><xsl:value-of select=”Signatures/EC_Approval_ENG_Date”/></td>
                                                                </tr>

                                                                <tr>
                                                                                <td class=”label” width=”120″>Mfg Approval:</td><td class=”value” width=”150″><xsl:value-of select=”Signatures/EC_Approval_MFG”/></td>
                                                                                <td class=”label” width=”120″>Approved Date:</td><td class=”value” width=”150″><xsl:value-of select=”Signatures/EC_Approval_MFG_Date”/></td>
                                                                </tr>

                                                                <tr>
                                                                                <td class=”label” width=”120″>Quality Approval:</td><td class=”value” width=”150″><xsl:value-of select=”Signatures/EC_Approval_QUAL”/></td>
                                                                                <td class=”label” width=”120″>Approved Date:</td><td class=”value” width=”150″><xsl:value-of select=”Signatures/EC_Approval_QUAL_Date”/></td>
                                                                </tr>
                                                </table>
                                                </xsl:for-each>
                                </body>
                  </html>
                </xsl:template>
</xsl:stylesheet>


This code, will result in a form that looks roughly like this:

SOLIDWORKS PDM Forms - Engineering Change Notice - Created with XML

Note that the values of the XML tags are displayed in this form through a special tag. This tag <xsl:value-of select=”Signatures/EC_Approval_MFG”/> retrieves the value specified in the select statement. Now that we have a stylesheet defined, we need to tie it into our XML document. This is another easy tag across the top that looks like this:


<?xml-stylesheet type=”text/xsl” href=”../../Templates/ECN.XSL”?>

The href tag is the path to the XSL file. In order for this to work, we either need to put this in a central location and reference it in an XML template, or copy it each time. For the best benefit of an XML form, I recommend putting it in a central location. My location is 2 levels above where my EC forms will reside, in the templates folder.

From here, we can take our standard approach to creating templates. Create a template card to capture inputs and fill in a serialized EC number. And, of course, we can create workflow actions to fill in values along the way.

As with any method, there are some pros and cons to this. As with the other methods I’ve discussed in this series, I’ll break down some of what I see.

Pros:

  • Previews update without opening and re-saving the file
  • Forms require no software beyond a web browser to be able to view or print
  • Once a format is set, a change can be cascaded to all existing forms by altering the XSL*
  • No known issues with variable types

Cons:

  • Requires that someone know HTML/CSS to write
  • Requires a folder structure to allow consistent reference paths if keeping the XSL in a central location
  • Likely to be a new concept, so would require converting existing forms

 

*Changing the format of all existing forms can be avoided by creating a second stylesheet, leaving the first in place for old documents.

Author information

DASI Solutions
DASI Solutions
DASI Solutions is dedicated to service and support. As one of a handful of original, charter value-added resellers (VAR) in the SolidWorks Community, DASI Solutions has built partnerships and success stories with many of our customers. We are very pleased to bring you SolidWorks 3D CAD design engineering software and 3D printing services.

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SOLIDWORKS Modeling Challenge – Measuring Imported Fillets http://blogs.solidworks.com/tech/2017/06/solidworks-modeling-challenge-measuring-imported-fillets.html http://blogs.solidworks.com/tech/2017/06/solidworks-modeling-challenge-measuring-imported-fillets.html#comments Fri, 09 Jun 2017 21:00:45 +0000 http://blogs.solidworks.com/tech/?p=17131 * This is one of a series of modeling challenges you can use to test your SOLIDWORKS skills.  First, read the challenge and try to figure out a solution on your own.  Then, compare your solution with my good, better,

Author information

Jordan Tadic

Territory Technical Manager - NA East at SOLIDWORKS

Certified Elite Application Engineer. Provide technical sales support for all SOLIDWORKS products to OH, KY, and PA.

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* This is one of a series of modeling challenges you can use to test your SOLIDWORKS skills.  First, read the challenge and try to figure out a solution on your own.  Then, compare your solution with my good, better, and best recommendations.  As always, feel free to share even more tips and tricks in the comments below.

Modeling, measuring, and modifying native SOLIDWORKS files is easy.  Most of the really fun modeling challenges arise when working with imported geometry.  All you’re typically given to start off with is what we call a “dumb solid” – just a hunk of digital mass with no intelligence (i.e. parametric feature history).  Sometimes you’re even left at the mercy of another CAD system’s inferior export quality.  This can be troublesome, because what one CAD system may consider cylindrical, SOLIDWORKS may not.

For example, imagine importing what looks like a simple sheet metal part file, using the Convert to Sheet Metal tool to flatten it, and then realizing it won’t work because the bent faces aren’t perfectly cylindrical.  The only workaround is to replace the filleted faces with true cylindrical faces.  Here’s how to do it:

  1. Use Copy Surface (Offset Surface with an offset value of 0) to copy the flat faces
  2. Use Delete Body to delete the original imported solid
    Expand the solid body folder, select the body, and click the delete key to quickly activate this tool
  3. Use Extend Surface to fill the gaps of the removed filleted faces
  4. Use Face Fillet to bridge between the surface bodies with a perfectly tangent transition
  5. Use Convert to Sheet Metal to convert the surface body to a sheet metal solid body
  6. Now you can use the Flatten command to display the flat pattern

So that’s a pretty cool tip, but that’s not the modeling challenge for this post.  I skipped a step between #3 and #4.  First you need to know the size of the fillet before you can model it.  Since imported models don’t have feature dimensions, the challenge is – how do we measure imported fillets?

Status Bar

Most of us know you can use the Status Bar (the informational text shown in the bottom right hand corner of the SOLIDWORKS interface) to display measurements of select edges and faces.  Most of us also know if you select a circular edge, the Status Bar will report a radius.  This can help in situations as shown on the left end of the model below.  The problem is that when selecting an edge that isn’t perfectly normal to the direction of the circular profile, all the Status Bar will report is an Arc Length – no help when trying to measure a fillet.  So what do we do when neither edge of a cylindrical face is normal to the profile of the fillet?  SOLIDWORKS solved this problem in 2015 when we added the ability to display a radius value when selecting a cylindrical face.  It’s a pretty simple solution that you definitely want to be aware of!

Normal Profile Sketch

The last solution works for cylindrical faces, but what about fillets that are applied to a curved edge (i.e. fillets that aren’t cylindrical)?  In these cases, we’ll need to create a circular profile to measure.  Here’s an easy way to do so:

  1. Select the vertex and the edge of the fillet and then create a sketch
    By preselecting a vertex and an edge before creating a sketch, SOLIDWORKS automatically generates a plane coincident to the vertex and normal to the edge and activates a new sketch on that plane all in a single step
  2. Select the filleted face and then create an Intersection Curve
    And Intersection Curve will generate a sketch entity at the intersection of the selected face and the active sketch plane which will create a circular arc normal to the profile of the fillet
  3. Select the resultant arc to display the measured radius in the Status Bar

Curvature Evaluation

Even with those nifty shortcuts, that last tip still took too many steps for me.  It also wouldn’t have helped us with our original imported sheet metal example that didn’t contain fillets with exact radii.  That leads us to our final solution.  It’s actually way too easy, but it’s also commonly overlooked and neglected, which is why I felt compelled to write this post.  To measure any fillet in any condition, all you have to do it fire up the Curvature Evaluation tool and hover over the filleted face.  SOLIDWORKS will display a live measurement of the curvature directly under your mouse.  That’s all there is to it!

If you create models with a ton of different sized fillets, this is also a great way to make a quick final inspection to make sure all of your fillets were applied correctly.  Enjoy!

Author information

Jordan Tadic
Territory Technical Manager - NA East at SOLIDWORKS
Certified Elite Application Engineer. Provide technical sales support for all SOLIDWORKS products to OH, KY, and PA.

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Dimensioning in Style (with SOLIDWORKS Dimension Styles) http://blogs.solidworks.com/tech/2017/06/dimensioning-style-solidworks-dimension-styles.html http://blogs.solidworks.com/tech/2017/06/dimensioning-style-solidworks-dimension-styles.html#respond Fri, 09 Jun 2017 15:00:15 +0000 http://blogs.solidworks.com/tech/?p=17092 Author: Jim Peltier, CSWE, Javelin Technologies  Often times, SOLIDWORKS Dimension Styles are passed without notice because it is quite easy to get the job done without using them. However, they can be used for dimensions that have very common notes

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Javelin Technologies

Javelin Technologies is a provider of technology solutions since 1997. We are experts in 3D design and have helped thousands of companies with solutions for mechanical design, electrical design and 3D printing.

Large or small, we have the skills, experience, and services to propel your organization to new heights so you can aim high.

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Author: Jim Peltier, CSWE, Javelin Technologies 

Often times, SOLIDWORKS Dimension Styles are passed without notice because it is quite easy to get the job done without using them. However, they can be used for dimensions that have very common notes attached to them. For instance, when I used to design automated machinery, often times, we would add text to a dimension such as “BTS” (Build To Suit), or “DRILL AND REAM” or “TRANSFER AT ASSEMBLY” among others. I’ve created a simple example below:

SOLIDWORKS Dimension Styles Example

SOLIDWORKS Dimension Style Examples

As you can see, I am doing a few different things with my dimensions on this part. My 100.0 dimension at the top includes a note that says “Build To Suit,” indicating that it will be whatever length the shop floor deems appropriate, hence why the 100.0 is to 1 decimal place and in parentheses. So, I’ve done 3 things to this dimension and I do these 3 things often enough that I want a better way.

I will use SOLIDWORKS Dimension Styles to make my life easier…

Adding a SOLIDWORKS Dimension Style

I start by selecting the dimension, then I go over to the left-hand side:

Update a Style

Update a Style

Once on the left side, I click the “Add or Update a Style” button (star with a + sign). Then a dialogue window appears and I give it a meaningful name (such as BTS). On this drawing, I can pick any dimension, and from the drop down menu below the “Add or Update a Style) button, I can choose BTS and it will change the 3 things on it. I’ve just created and tested my Dimension Style and it works great. Then I create a new drawing and am dismayed to find that BTS doesn’t appear in the drop down of the new drawing:

Style Selection

Style Selection

How do I copy Dimension Styles from one drawing into another?

I then go back to the drawing that has my Dimension Styles. I need to do one more thing to them so I can access them: I need to save them out as an external file.

Save Style

To do this, I simply go back to the left and click on the Save Style button. I then save it to an external file (.sldstl). I repeat for each of the Dimension Styles I have created. Then I switch back to my other drawing and use the Load Style button and select the Dimension Styles I want to bring into the new drawing:

Open a Style

Open a Style

Then I have access to the SOLIDWORKS Dimension Styles in the new drawing. I am able to select it from the drop down and apply it to the dimensions in this drawing as well:

Style selection available

Style selection available

Apply styles to a template

Of course, I don’t want to have to do this every time I want to use SOLIDWORKS Dimension Styles from a previous drawing. So, there’s one other thing I need to do.

I’m going to create a new, blank drawing, then load my Dimension Styles as described before, then I’m going to save my drawing as a Drawing Template, overwriting the old template. Now every new drawing I create (with this template) will have all my Dimension Styles available!

Author information

Javelin Technologies
Javelin Technologies is a provider of technology solutions since 1997. We are experts in 3D design and have helped thousands of companies with solutions for mechanical design, electrical design and 3D printing. Large or small, we have the skills, experience, and services to propel your organization to new heights so you can aim high.

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Creating a Fidget Spinner in SOLIDWORKS http://blogs.solidworks.com/tech/2017/06/creating-fidget-spinner-solidworks.html http://blogs.solidworks.com/tech/2017/06/creating-fidget-spinner-solidworks.html#respond Thu, 08 Jun 2017 15:00:26 +0000 http://blogs.solidworks.com/tech/?p=17083 Getting our kids into STEM has always been a priority for our family. What better tool to jumpstart their love for engineering than SOLIDWORKS? When our trip to several stores to buy the latest toy craze left us empty-handed, I

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CADimensions

We are an authorized SOLIDWORKS and Stratasys reseller with certified training & support centers located in New York and Pennsylvania, USA. We are 100% focused on living a CADLIFE and have our vendor's unconditional endorsement in the sales and support of their products.

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Getting our kids into STEM has always been a priority for our family. What better tool to jumpstart their love for engineering than SOLIDWORKS? When our trip to several stores to buy the latest toy craze left us empty-handed, I was able to turn it into a “teachable moment.” I was able to teach them about patience and more importantly, if you can’t buy something… design and build it!
Using basic design processes, we “napkin sketched” out a few ideas for their own Fidget Spinners. Using SOLIDWORKS, I was able to visually show them the concepts of moment of inertia and center of mass.


Once we finalized our design, they asked how we were going to get one (or two). That’s where I was able to introduce them to the world of 3D printing. They knew that CADimensions sold 3D Printers, and that it could make cool “things,” but up until that moment, they didn’t connect that we could print something that was useful to them!
Some quick disassembling of my old rollerblades for the bearings and a couple of hours of print time later, viola – custom fidget spinners!


Check out this video for a more detailed explanation of my process:

The down-side? Now they want to design EVERYTHING in SOLIDWORKS. I also made the mistake of showing them SOLIDWORKS SIMULATION. I have effectively lost any free-time I had at home and now teach them SOLIDWORKS every day! I guess that’s not that big of a down side. As I mentioned before, I will always jump at an opportunity to get kids interested in engineering and science, they are the future.
As always, thanks for reading, and Happy Engineering!

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CADimensions
We are an authorized SOLIDWORKS and Stratasys reseller with certified training & support centers located in New York and Pennsylvania, USA. We are 100% focused on living a CADLIFE and have our vendor's unconditional endorsement in the sales and support of their products.

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SOLIDWORKS Harry Potter’s Golden Snitch Tutorial – Part 1 http://blogs.solidworks.com/tech/2017/06/solidworks-harry-potters-golden-snitch-tutorial-part-1.html http://blogs.solidworks.com/tech/2017/06/solidworks-harry-potters-golden-snitch-tutorial-part-1.html#respond Mon, 05 Jun 2017 21:00:39 +0000 http://blogs.solidworks.com/tech/?p=17036 It’s safe to say that Quidditch is Harry Potter’s favorite wizarding pastime. As Hagrid would say, a wizard’s passion for Quidditch is the equivalent to a muggle’s passion for football. This year marks the 20th anniversary of the first publication

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SOLIDWORKS

Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

The post SOLIDWORKS Harry Potter’s Golden Snitch Tutorial – Part 1 appeared first on SOLIDWORKS Tech Blog.

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It’s safe to say that Quidditch is Harry Potter’s favorite wizarding pastime. As Hagrid would say, a wizard’s passion for Quidditch is the equivalent to a muggle’s passion for football. This year marks the 20th anniversary of the first publication in the series, Harry Potter and the Sorcerer’s Stone. To celebrate, we are showing SOLIDWORKS users how to model the Golden Snitch – the little ball that Harry loves to hate. So hop on your Nimbus 2000 and let’s get started flying through our four part series.

SOLIDWORKS Harry Potter's Golden Snitch Tutorial

In part 1 of the series, we’ll begin modeling the body of the Snitch using the Revolved Boss tool and a series of projected curves. We’ll also introduce you to the circular profile option in the Swept Boss tool.

Can’t wait to watch the next video? View all of the tutorials on the playlist here.

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SOLIDWORKS
Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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SOLIDCRAFT – Using SOLIDWORKS API for Fun and Games http://blogs.solidworks.com/tech/2017/06/solidcraft-using-solidworks-api-fun-games.html http://blogs.solidworks.com/tech/2017/06/solidcraft-using-solidworks-api-fun-games.html#comments Mon, 05 Jun 2017 15:00:33 +0000 http://blogs.solidworks.com/tech/?p=16782 What is SOLIDWORKS API? SOLIDWORKS API is a gateway to automating your design process and data management. Using .NET compatible languages (VB, C#, C++) one can write small macros or build full-blown add-ins for modelling, routine edits and feeding data

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Solid Solutions Technical Team

Solid Solutions commenced business as a SolidWorks Training and SolidWorks Support provider in 1998 and has consistently achieved strong growth year-on-year to become the UK’s leading SolidWorks 3D CAD reseller. Growth has been completely organic and has been consistently driven by a focus on recruiting the best from academia and industry and by delivering high quality services to more than 4,000 customers.

Our customers range widely in size and are drawn from a broad spectrum of industry sectors. SolidWorks software is used by over 2 million engineers and designers across the world. As a company we are dedicated and focused at providing first class training and support to help you realise the best return on your investment.

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SOLIDWORKS-Minecraft-Blog-SolidSolutions

What is SOLIDWORKS API?

SOLIDWORKS API is a gateway to automating your design process and data management. Using .NET compatible languages (VB, C#, C++) one can write small macros or build full-blown add-ins for modelling, routine edits and feeding data from one software package to another.

We at Solid Solutions offer bespoke coding on a consultancy basis. Be it a one-page input form, a PDM Pro custom task or a multiplatform app that talks to SOLIDWORKS – we have a team of automation specialists able to tackle a wide range of challenges.

But what can be done with API outside of office hours, just for fun? Well, it’s not very hard to implement some basic MINECRAFT functionality with a couple of macros. Let’s have a look at the process and some results!

Creating a Macro

  1. We start with a small 10x10x10mm cube model (could be any other size).
  2. Start recording a macro (Tools->Macro->Record).
  3. Perform the following steps by hand:
    • Select any face on the cube surface and start a new Sketch.
    • Use the Sketch -> Convert Entities command.
    • Boss extrude 10mm Blind without merging the result. Actual extrusion depth depends on the size of your initial cube.
    • Stop recording the macro, save it into a separate folder.

SOLIDWORKS-Minecraft-Blog-SolidSolutions

You will need to edit the code behind your macro to remove the selection part. This is done through Tools -> Macro -> Edit. Your macro code will look similar to one below:

SOLIDWORKS-Minecraft-Blog-SolidSolutions

This macro allows you to ‘draw’ cubes on top/below/next to other cubes. If bound to a keyboard shortcut or a spare mouse button this can be done very quickly.

But all of these cubes are grey, where are the Minecraft textures?!

Okay, this is where things get tricky. You will need some SOLIDWORKS API and VBA programming knowledge from here onward. I created some textured appearances and saved them as .p2m files in a sub folder next to my macro file. Then we add some bits of intelligence to the already existing macro:

SOLIDWORKS-Minecraft-Blog-SolidSolutions

I created two macros for ‘bark’ and ‘leaves. Now we can ‘draw’ some vegetation:

With some time and effort we can grow trees even:

SOLIDWORKS-Minecraft-Blog-SolidSolutions

 

SOLIDWORKS-Minecraft-Blog-SolidSolutions

In Conclusion

Here we have barely scratched the surface of what SOLIDWORKS API is capable of… Minecraft within SOLIDWORKS!

Now show this to the young people you know, maybe they will become SOLIDCRAFT Engineers one day.

Rodion Radchenko
Elite Applications Engineer

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Solid Solutions Technical Team
Solid Solutions commenced business as a SolidWorks Training and SolidWorks Support provider in 1998 and has consistently achieved strong growth year-on-year to become the UK’s leading SolidWorks 3D CAD reseller. Growth has been completely organic and has been consistently driven by a focus on recruiting the best from academia and industry and by delivering high quality services to more than 4,000 customers. Our customers range widely in size and are drawn from a broad spectrum of industry sectors. SolidWorks software is used by over 2 million engineers and designers across the world. As a company we are dedicated and focused at providing first class training and support to help you realise the best return on your investment.

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Getting Started with SOLIDWORKS Plastics http://blogs.solidworks.com/tech/2017/06/getting-started-with-solidworks-plastics.html http://blogs.solidworks.com/tech/2017/06/getting-started-with-solidworks-plastics.html#respond Sun, 04 Jun 2017 15:00:59 +0000 http://blogs.solidworks.com/tech/?p=17023 Simulating the process of injection molding a plastic part is easy with SOLIDWORKS Plastics, crazy easy in fact.  Here is a run-down of the simple steps you’ll follow to get started. Step 1: Create a 3D model, which you were

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MLC CAD Systems

Celebrating Three Decades of Unbeatable Service!
MLC CAD System's mission is to help design and manufacturing companies, entrepreneurs, creative individuals, research institutions and other organizations put their ideas and products into production using the industry's best software technologies including SOLIDWORKS 3D CAD, Mastercam, 3D Systems' & Markforged 3D printers well as other leading CAD and CAM technologies.

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Simulating the process of injection molding a plastic part is easy with SOLIDWORKS Plastics, crazy easy in fact.  Here is a run-down of the simple steps you’ll follow to get started.

Step 1: Create a 3D model, which you were going to do anyways. SOLIDWORKS has powerful tools for creating intricate geometry and validating the design for manufacturability.  Analysis tools measure draft angles, wall thickness, undercut, even automatically finding and creating the parting line and the parting surfaces.  Powerful mold design tools make it easy to build mold geometry but that won’t be necessary to get started with Plastics.

Step 2: Show the Plastics tab and create a Solid or Surface mesh. Tip: Use Solid mesh when the thickness varies widely or when accuracy is important, use a surface mesh for faster results and especially for parts with uniform wall thickness.  Automatic mode will give you a good starting mesh, and manual mode will allow for simple refinement and feedback on mesh quality.

Step 3: Choose your polymer; thousands of material models come preloaded and are organized by material type and supplier, but you can modify or enter new data to suit your specific needs or choose a generic material if the final formula is TBD.

Step 4: Set the injection location. Again, an automatic option makes this one-click simple, but you will want to make sure the injection location is on a parting line or a hidden face to keep the visible geometry clean and smooth. Flow pattern prediction gives you a quick check to make sure you’re choosing a location that will give appropriate results.

Step 5: Solve it! Double click the Flow icon to see the part fill before your eyes. Results are displayed as the part fills so you can monitor progress. The Results Adviser gives you a summary of the results when the solution is done.

Plastics operates inside the SOLIDWORKS user interface as a native program so you can quickly adjust the design and verify the fill without swapping windows or transferring files.  Although Plastics will automate the process parameters for injection molding based on manufacturer recommendations and industry best practices, it can be completely customized and adjusted to accommodate the most challenging real-world scenarios.  From a simple check for short-shots to a final check for residual stresses or measuring directional warp, SOLIDWORKS Plastics is a powerful tool to improve manufacturability and predict the outcome of an injection molded part design.

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MLC CAD Systems
Celebrating Three Decades of Unbeatable Service! MLC CAD System's mission is to help design and manufacturing companies, entrepreneurs, creative individuals, research institutions and other organizations put their ideas and products into production using the industry's best software technologies including SOLIDWORKS 3D CAD, Mastercam, 3D Systems' & Markforged 3D printers well as other leading CAD and CAM technologies.

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SOLIDWORKS Wonder Woman Tutorial Series – Part 1 http://blogs.solidworks.com/tech/2017/06/solidworks-wonder-woman-tutorial-series-part-1.html http://blogs.solidworks.com/tech/2017/06/solidworks-wonder-woman-tutorial-series-part-1.html#respond Fri, 02 Jun 2017 21:00:16 +0000 http://blogs.solidworks.com/tech/?p=17044 Welcome to our mini-series where we are honoring The Amazon Princess, Wonder Woman, by modeling her iconic invisible jet in SOLIDWORKS! … On second thought, maybe we should provide you a series on how to model something a little more…tangible.

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SOLIDWORKS

Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

The post SOLIDWORKS Wonder Woman Tutorial Series – Part 1 appeared first on SOLIDWORKS Tech Blog.

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Welcome to our mini-series where we are honoring The Amazon Princess, Wonder Woman, by modeling her iconic invisible jet in SOLIDWORKS!

SOLIDWORKS Wonder Woman Tutorial - Invisible Jet

… On second thought, maybe we should provide you a series on how to model something a little more…tangible. So, instead, let’s walk through a 4-part series on how to model Wonder Woman’s Tiara and Indestructible Bracelets. These models will become available to you at the end of the series so stay tuned for instructions on how to download them. I could definitely see some of you female warrior engineers 3D printing these artifacts in time for Halloween.

SOLIDWORKS Wonder Woman Tutorial Series - Tiara

In part 1 of the series we’ll begin modeling the central portion of Wonder Woman’s Tiara. Within this part of the series we’ll run through creating and working off of a few reference surfaces, and running through various options within the Extruded Boss/Base tool.

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SOLIDWORKS
Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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SOLIDWORKS Visualize: D Cube Design Ltd Q&A http://blogs.solidworks.com/tech/2017/06/solidworks-visualize-d-cube-design-ltd-qa.html http://blogs.solidworks.com/tech/2017/06/solidworks-visualize-d-cube-design-ltd-qa.html#respond Fri, 02 Jun 2017 15:00:40 +0000 http://blogs.solidworks.com/tech/?p=16991 SOLIDWORKS Visualize provides a suite of standalone software tools that combine industry-leading rendering capabilities with design-oriented features and workflows that enable easy and fast creation of visual content for designers, engineers, marketing, and other content creators. One such user is Josh Fear,

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Innova Systems Experts in SOLIDWORKS Training & Support

We specialise in the supply, consultancy and training of SOLIDWORKS software. Based in Cambridge we have a central location to service a UK wide customer base. We offer the skills and experience to help you develop new products using SOLIDWORKS - empowering smarter, faster and more cost effective design.

We've been recognised by SOLIDWORKS Corporation for providing the highest rated customer support in Northern Europe in 2014, 2015 and 2016.

Email: info@innova-systems.co.uk / Telephone: 01223 200690.

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SOLIDWORKS Visualize provides a suite of standalone software tools that combine industry-leading rendering capabilities with design-oriented features and workflows that enable easy and fast creation of visual content for designers, engineers, marketing, and other content creators. One such user is Josh Fear, Managing Director of D Cube Design Ltd in Leicester, England, who provide a high quality CGI rendering service for manufacturers. We sat down with Josh to find out a little more about how he uses SOLIDWORKS Visualize to create the renders you see here.

InnovaHi Josh, tell us a little bit about yourself and how long you’ve been using SOLIDWORKS.

Josh: I’ve been using SOLIDWORKS for about four or five years now. I’ve always been fascinated with engineering and started playing around with the SOLIDWORKS Student edition when I was 16, learning how the software worked, making stuff for my own enjoyment, just random stuff.

When I left school, I went on to a company that specializes in the design and manufacture of polyethylene tanks for agricultural, industrial and residential applications.

Innova: What kind of stuff were you doing there?

Josh: I was their Technical Sales Manager, so I provided technical support and advice on a large range of products and services. I also worked with clients on projects, providing technical drawings and rendered images as necessary. The company wasn’t actually using SOLIDWORKS at the time, so I had to convince them it was the way to go. We got a free trial from Innova Systems, which soon turned into a full license of SOLIDWORKS Premium when my employer saw what could be achieved.

D-Cube-Design-Ltd-SolidWorks-Visualize-Desk

Innova: So that was your first experience of using SOLIDWORKS Visualize?

Josh: No it wasn’t, actually! I’d heard about the SOLIDWORKS Visualize beta program and contacted Innova Systems who set me up with early-access. Coming from SOLIDWORKS, I picked it up extremely quickly and when it came to the full release, I was all set, because SOLIDWORKS Visualize Standard is included with a Premium license of SOLIDWORKS.

Innova: What sort of stuff were you using SOLIDWORKS Visualize for?

Josh: I did a lot of high quality product renders for marketing materials and the product pages on the company’s website. I used to use Photoview 360, which produced quick, “nice-enough” visuals, but Visualize enabled me to take things a step further and them make incredibly lifelike, “sellable” images of products that hadn’t yet been produced, or didn’t look too good when photographed.

Ultimately, Visualize saved the company time and money – Whereas they would previously have had to manufacture the product, hire a professional photographer and then Photoshop the images to get them looking right, I could now produce consistent, great looking, lifelike renders from SOLIDWORKS models in a fraction of the time. It proved to deliver a very rapid return on investment which is vital for any small company.

Innova: Tell us about your new company, D Cube Design Ltd.

Josh: D Cube Design Ltd specializes in rendering for small manufacturing companies that don’t have the ability or resources to create renders in-house.

The company is really taking off now, with excellent resource and specialist CAD operatives across the globe. We’ve done many different renders from tank level indicators, watches, office furniture and also architectural work – all completed in SOLIDWORKS Premium and SOLIDWORKS Visualize Professional.

Over the next 2-5 years, we have some rapid growth plans which include expanding our core in-house team, and becoming increasingly specialist in the manufacturing industry.  We are very clear about the value and benefits we bring to our clientele, and are actively looking to increase our client database.

SolidWorks-Visualize-Supercharger-Render-Motion-Blur-Innova-Systems-D Cube Design-Ltd

Innova: How would you describe your usual design process?

Josh: Working with different clients means things are never exactly the same, but it usually starts with a briefing session, where we iron out what is required for the project: “I want this tank rendered in front of this greenhouse at this time of day”, for example.

I usually have a technical drawing or a model to work from, so I’ll load SOLIDWORKS to do some initial tweaks like applying materials, textures etc. I’ll then use Visualize to create low resolution renders for client approval. Once any changes are made and the client is happy, I’ll set up and export a high quality rendering for final use.

Innova: What are your top 3 Visualize features?

Josh: Firstly, I’d have to say the output functionality. So thing’s like like VR, Photos, and Animations. It’s so slick and lets you present your product designs in the best way possible.

Being able to customize the colors, scenes, lighting, textures and camera angles and then set it everything up as a reusable template. This means I can save time by reusing my settings and everything follows the same look and feel. Great for brand-sensitive projects where the colors have to be just right, for example.

Lastly, when creating an explode animation (see video below), the autoframe functionality is superb. You set your start and end points for each part of your model and Visualize does the rest. Again, a great time saver and produces fantastic effects with little effort.

Actually, can I have a fourth favorite feature? I’m a keen photographer in my spare time and Visualize really is like having a camera inside SOLIDWORKS. You’ve got things like depth of field and shutter speeds, which really give you great control as if you were there with your Canon.

Innova: How does SOLIDWORKS Visualize help companies like D Cube Design Ltd?

Josh: It’s a tough, competitive world, so being able to show your products in the best possible light, before committing to manufacture will help companies to outpace their competitors, ultimately winning their business. SOLIDWORKS helps you to quickly converge on the right solution, so you’ll be able to delight your customers much earlier in the process.

D-Cube-Design-Ltd-SolidWorks-Visualize-Innova-Systems

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Innova Systems Experts in SOLIDWORKS Training & Support
We specialise in the supply, consultancy and training of SOLIDWORKS software. Based in Cambridge we have a central location to service a UK wide customer base. We offer the skills and experience to help you develop new products using SOLIDWORKS - empowering smarter, faster and more cost effective design. We've been recognised by SOLIDWORKS Corporation for providing the highest rated customer support in Northern Europe in 2014, 2015 and 2016. Email: info@innova-systems.co.uk / Telephone: 01223 200690.

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Modelling a Drill Bit with a Compound Swept Cut in SOLIDWORKS http://blogs.solidworks.com/tech/2017/06/modelling-drill-bit-compound-swept-cut-solidworks.html http://blogs.solidworks.com/tech/2017/06/modelling-drill-bit-compound-swept-cut-solidworks.html#comments Thu, 01 Jun 2017 15:00:57 +0000 http://blogs.solidworks.com/tech/?p=16962 Can you model a drill bit? Picturing a drill bit you might be inclined to give a resounding yes, but not so fast! What about those organic compound cuts that neatly taper off, how do you tackle these in the geometric

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TMS CADCentre

TMS CADCentre - is a SOLIDWORKS Reseller based in Scotland providing 3D CAD Design Software, analysis software & product data management software. The company was formed in 1981 and now pleased to be celebrating 35 years in business. TMS CADCentre is the only UK SOLIDWORKS Reseller based and funded within Scotland and have been providing SOLIDWORKS software, training and support since 1996 when the product was first launched in the UK.

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Can you model a drill bit? Picturing a drill bit you might be inclined to give a resounding yes, but not so fast! What about those organic compound cuts that neatly taper off, how do you tackle these in the geometric favoring CAD world?

Modelling a Drill Bit with a Compound Swept Cut

 

It starts like this: create a solid body to represent your cutting tool and position it at the start of your Compound Curve:

Now for the trickier bit… Think about what a Compound Curve is. It’s a curve which bends in two planer directions at once, whilst this sounds like the plot to a CAD horror movie the SOLIDWORKS Projected Curve actually makes it very easy.

Here’s how: Create your curves on two separate planes, in my example below you can see these as sketch lines. The blue line is my projected curve (found under Features/Curves/Projected Curves). The intention here is to use the resulting projected curve as the path whilst the solid body forms our profile.
Compound Swept Cut
Finally, use a Swept Cut to form the cut. A Circular Pattern can also be used in the case of a drill bit to give us the multiples instances usually seen around the head of a drill bit.

And there you have it! The Projected Curve tool is a great utility for lots of applications; it’s not limited to creating Cuts, it can be used for Sweeps and even creating the edges of complex Compound Surfaces. For this reason it stays firmly pinned on my SOLIDWORKS toolbar!


Grant Davidson is a Senior Applications Engineer at TMS CADCentre, a SOLIDWORKS Value Added Reseller in Scotland.  You can read more from Grant on the TMS CADCentre blog

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TMS CADCentre
TMS CADCentre - is a SOLIDWORKS Reseller based in Scotland providing 3D CAD Design Software, analysis software & product data management software. The company was formed in 1981 and now pleased to be celebrating 35 years in business. TMS CADCentre is the only UK SOLIDWORKS Reseller based and funded within Scotland and have been providing SOLIDWORKS software, training and support since 1996 when the product was first launched in the UK.

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Understanding Sheet Metal and Transformed Sketches and How They Behave http://blogs.solidworks.com/tech/2017/05/understanding-sheet-metal-and-transformed-sketches-and-how-they-behave.html http://blogs.solidworks.com/tech/2017/05/understanding-sheet-metal-and-transformed-sketches-and-how-they-behave.html#respond Wed, 31 May 2017 15:00:05 +0000 http://blogs.solidworks.com/tech/?p=16897 Sheet metal parts can have sketches in the Folded and the Flat Pattern states (Fig. 1) Sketches created in the folded state can have an equivalent “transformed” sketch in the Flat Pattern state. All sheet metal parts have a fixed face.

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Mario Iocco

Mario Iocco
Sr. Technical Customer Support Engineer, SolidWorks, Americas.

Mario Iocco is a veteran CAD user.
He started as a Mechanical Engineer first working in 2D with AutoCAD, moving on to 3D using  both SW and some  of the other CAD software on the market.
He began his career with SolidWorks over 15 years ago. He started in R&D working on many of the new functionalities developed at the time -eDrawings, Sheet Metal, Weldments, etc.
In the last few years, he moved to TS., working closely with VARs,
Mario wrote the sheet metal functionality best practice manual, as well as creating hundreds of Sheet Metal Knowledge Base articles. He has presented webinars  on "Sheet Metal Tips and Tricks" and "Sheet Metal Bend Tables".

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Sheet metal parts can have sketches in the Folded and the Flat Pattern states (Fig. 1) Sketches created in the folded state can have an equivalent “transformed” sketch in the Flat Pattern state.

All sheet metal parts have a fixed face. The fixed face is the one that remains in the same position when unsuppressing the Flat Pattern. (Fig. 2)

Sketches created in fixed faces will not be transformed. The sketches created in non-fixed faces will be transformed when viewed in the Flat Pattern. (Fig. 3)

The circular sketch was created in the Flat Pattern fixed face, it does not need to be transformed. The square sketch was not created on a fixed face, it was transformed when unsuppressing the Flat Pattern feature (Fig. 4)

The transformed sketches will be visible in the Flat Pattern feature, under the “Sketch Transformation” folder. The sketches that has been transformed will be hidden in the Folded state (Fig. 5.)

The non-transformed sketches will remain visible in the Folded state (Fig. 6.)

The transformed folder does not exist when the Flat Pattern is suppressed (Fig. 7.)

 

The transformed folder is created only when unsuppressing the Flat Pattern feature (Fig. 8.)

Sketches in the Flat Pattern Drawing View

When you create a Flat Pattern drawing view, the system creates a flatten derived configuration. After the creation, the sketches in the flatten derived configuration and drawing become independent from each other. That is, if you want to see the transformed sketches being displayed in the Flat Pattern drawing view, you must expand the drawing view Feature Tree and manually show those sketches (Fig. 9)

Author information

Mario Iocco
Mario Iocco
Sr. Technical Customer Support Engineer, SolidWorks, Americas.
Mario Iocco is a veteran CAD user. He started as a Mechanical Engineer first working in 2D with AutoCAD, moving on to 3D using  both SW and some  of the other CAD software on the market. He began his career with SolidWorks over 15 years ago. He started in R&D working on many of the new functionalities developed at the time -eDrawings, Sheet Metal, Weldments, etc. In the last few years, he moved to TS., working closely with VARs, Mario wrote the sheet metal functionality best practice manual, as well as creating hundreds of Sheet Metal Knowledge Base articles. He has presented webinars  on "Sheet Metal Tips and Tricks" and "Sheet Metal Bend Tables".

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Create Your Own Customized Color Swatch in SOLIDWORKS http://blogs.solidworks.com/tech/2017/05/create-your-own-customized-color-swatch-in-solidworks.html http://blogs.solidworks.com/tech/2017/05/create-your-own-customized-color-swatch-in-solidworks.html#respond Sat, 27 May 2017 15:00:11 +0000 http://blogs.solidworks.com/tech/?p=16824 When you add colors to your SOLIDWORKS files, you can select colors from a standard color palette like this one: But quite often users want to add their own custom colors. This could be company specific colors or colors based

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CAD2M

CAD2M is certified reseller of SOLIDWORKS, SolidCAM, DriveWorks and our private label dddrop 3D printer. The CAD2M approach integrates this range of products into an all-in-one solution that covers the complete product development process. Take the full advantage of working in 3D with our advice, training and expertise. For more information, visit www.cad2m.nl.

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When you add colors to your SOLIDWORKS files, you can select colors from a standard color palette like this one:

Color_swatch

But quite often users want to add their own custom colors. This could be company specific colors or colors based on the international color standard RAL. In the case of RAL it is quite easy to find RGB color codes, which can be entered in SOLIDWORKS to define the desired RAL color. As long as you do not create a custom color swatch it could be a time-consuming task to define your color each time. So, in this tech blog I want to show you how to create your own custom color swatch, which will save you a lot of time when adding color to your parts.

Step-by-step process

1. In the Color PropertyManager, select Create New Swatch Color swatch.

2. Enter a name for your custom color swatch and click Save.

Tip: you can change the file location for your color swatches in Tools-Options-File Locations.

3. Next you will see that the color swatch is added and that the swatch is empty.

color swatch

4. Now we can start to fill our color swatch. Just choose a color or enter a RGB code. After that you select Add Current Color to Swatch .

5. Repeat step 4 until your color swatch is complete. In case you want to remove a color from your swatch, just select Remove Selected Swatch Color .

Conclusion

Now you know how to create your own custom color swatches in SOLIDWORKS, you will be able to color your parts fast and in the right color. Also, the possibility to share one color swatch with all your colleagues is a big advantage to meet your company standards.

Written by Martijn Visser

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CAD2M
CAD2M is certified reseller of SOLIDWORKS, SolidCAM, DriveWorks and our private label dddrop 3D printer. The CAD2M approach integrates this range of products into an all-in-one solution that covers the complete product development process. Take the full advantage of working in 3D with our advice, training and expertise. For more information, visit www.cad2m.nl.

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SOLIDWORKS Tech Tip: Compare Documents Command http://blogs.solidworks.com/tech/2017/05/solidworks-tech-tip-compare-documents-command.html http://blogs.solidworks.com/tech/2017/05/solidworks-tech-tip-compare-documents-command.html#respond Fri, 26 May 2017 21:00:15 +0000 http://blogs.solidworks.com/tech/?p=16916 Often times parts vary slightly in design, which can result in different geometry. The Compare Documents command is used to compare the document properties, the features used, the geometry itself, or a bill of materials between two documents in SOLIDWORKS.

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SOLIDWORKS

Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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Often times parts vary slightly in design, which can result in different geometry. The Compare Documents command is used to compare the document properties, the features used, the geometry itself, or a bill of materials between two documents in SOLIDWORKS. Because the documents can be so closely compared, it helps identify areas that may cause mechanical issues based on differences in the design geometry. This is an especially great tool for comparing imported geometry to a repaired or modified version of a design. Check out the video below to learn more!

 

Want to see more SOLIDWORKS Tech Tips? Check out our playlist on YouTube to catch up on past videos or you can even jump ahead to the next video!

Do you have a suggestion for the next Tech Tip? Tell us in the comments; we’d love to hear your ideas!

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SOLIDWORKS
Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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“Fix” Your Fixtures http://blogs.solidworks.com/tech/2017/05/fix-your-fixtures.html http://blogs.solidworks.com/tech/2017/05/fix-your-fixtures.html#comments Thu, 25 May 2017 15:00:51 +0000 http://blogs.solidworks.com/tech/?p=16859 Since its infancy, CAD has been a tool for engineers and designers alike. Analogous to going to your tool box and getting something to remove a bolt, you will usually have several options to choose from. Will a ratchet be

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TPM

TPM, Inc. is the Carolina’s largest 3D CAD provider and a leading technology company proud of its reputation of providing cutting-edge solutions to the engineering and design community for the past 40 years. Founded in 1973, TPM Inc. serves more than 3,000 customers across the Southeast each year. Inspired by our founder, Jerry Cooper, we are committed to offering our clients the best: 3D Design Software, 3D Printing and Scanning Options, Data and Document Management Solutions, Large-Format Graphics, Wide-Format Plotters and Office Equipment, and Reprographics.

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Since its infancy, CAD has been a tool for engineers and designers alike. Analogous to going to your tool box and getting something to remove a bolt, you will usually have several options to choose from. Will a ratchet be best for this situation? Maybe a pair of pliers? Each condition and the environment in which the bolt is in will determine the best solution… Sometimes, we just need to reach for the torch and sledge hammer!

This being the case, I thought I’d share a few methods I’ve uncovered over the past 25 years utilizing 3D parametric CAD, specifically to design jigs and fixtures.

Method 1- 3D Printed Parts

Most of us have access to either a 3D printer and/or a 2.5 axis CNC router. These machines are priceless when it comes to taking something that is virtual in SOLIDWORKS and making them in reality. This is by far the most common practice we see today to achieve this. In a few short hours, very precise and custom fixturing can be brought to life with a simple click of a print button. SOLIDWORKS has many features available to assist in creating these very important components. My personal favorites are listed below:

Creating Multibody Part in Preparation

Following the Combine Operation, Offset Surface can be used to adjust the fixture as necessary.

Method 2- Templates

Complex Bend-Steel Tubing

Route Check fixture on CNC.

MDF/Plywood usually works fine. I’ve even used high density foam, and HTPE. Basically, whatever you have available will suffice. Note: Be sure the surface won’t catch fire!!! Wood and red hot steel don’t work well together.

What about those insane junctions on welded frames? Fisheye cuts, not a problem!

Insane Junction

Individual tube derived to generate dxf or full scale drawing

Full Scale drawing

Simply cut this template out with scissors, and wrap around your tube. Trace curves with a Sharpe. Remove material with tool of your choosing. Repeat for back side of tube. Small hash marks can be embossed on the tube to aide in clocking angles in the event one side is rotated relative to the first cut.

Method 3- Purchased Fixturing Systems

My third method is a little heavier on the pocket books, but is a great solution for professional applications. I have firsthand experience using these systems. They can be used early on the design process to fabricate prototypes, and on the backside as a quality control check fixture. You can tear em down….and build them back the same way 2 years later. Think of the possibilities, not to mention the floor space you can save by getting rid of all those versions of fixture templates!

The concept is simple. Create a library of 3D components, that reflect what the shop has available. A precise 3D model of the fixturing table usually provides mounting holes, or a common coordinate system between a scanner, SOLIDWORKS, and the fixturing table in the shop will do the job as well.

You ultimately decide how to get the information from a virtual environment, to a real one. Traditional drawings can be used to locate the items. However, MBD remains top on my list of next generation graphical communication for engineering.

Bluco, the manufacturer of the system I used, is a common option when looking to purchase these types of items.

Bluco Fixturing system

And after all this… YOU STILL BETTER HAVE ONE HECK OF A WELDER!

For those of you readers that have additional ideas, I’d love for you to share them. I believe the more creative we think in these respects, the more powerful the technology we have access to will become.


By: Rob Stoklosa • SOLIDWORKS Application Engineer • TPM

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TPM
TPM, Inc. is the Carolina’s largest 3D CAD provider and a leading technology company proud of its reputation of providing cutting-edge solutions to the engineering and design community for the past 40 years. Founded in 1973, TPM Inc. serves more than 3,000 customers across the Southeast each year. Inspired by our founder, Jerry Cooper, we are committed to offering our clients the best: 3D Design Software, 3D Printing and Scanning Options, Data and Document Management Solutions, Large-Format Graphics, Wide-Format Plotters and Office Equipment, and Reprographics.

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WARNING: SOLIDWORKS Resources Running Low http://blogs.solidworks.com/tech/2017/05/warning-solidworks-resources-running-low.html http://blogs.solidworks.com/tech/2017/05/warning-solidworks-resources-running-low.html#respond Wed, 24 May 2017 15:00:25 +0000 http://blogs.solidworks.com/tech/?p=16660 Warning: SOLIDWORKS System Resources Running Low This blog is for those unlucky individuals working in SOLIDWORKS are persistently annoyed by this message. You check the Task Manager, only to find that there are still plenty of RAM left; not even

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NCCS Australia

N C CAD CAM SYSTEMS, Authorised SOLIDWORKS Reseller in Victoria, Australia. Over 20 years, we have offered CAD/CAM and manufacturing solutions to thousands of Australian and New Zealand companies.

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Warning: SOLIDWORKS System Resources Running Low

This blog is for those unlucky individuals working in SOLIDWORKS are persistently annoyed by this message.

You check the Task Manager, only to find that there are still plenty of RAM left; not even at 50% capacity. Most of the time, you are likely to ignore or dismiss this message and just continue working. However, if this message turns into “Available system memory is Critically Low” then we are at a risk of the application crashing.

In this article, couple of suggestions will be made which will help prevent these messages from appearing, and hopefully avoid the inevitable crashes due to insufficient system memory. The resource monitor does not pin point what’s causing the lack of memory/resource. It could be any of or combination of GDI Objects, RAM and VRAM shortage.

WARNING: SOLIDWORKS Resources Running Low

1. GDI Objects Limit

GDI Objects (Graphics Device Interface) is a core windows component responsible for representing graphical objects and outputting them to devices such as printers or monitors.

For every window or application that is open, it uses up GDI Objects. The problem arises when there are too many objects are in use and causes unresponsive program behavior. This is also what may trigger the lack of system resources. For Windows 8 and later, the system wide GDI Objects are limited to max out at 65,536; and the maximum  single process is 16,384.

The default limit set by Windows for any single process is 10,000 GDI objects. If your application GDI Objects exceeds this amount, that process is likely to crash.

SOLIDWORKS should not require more than the default limit of 10,000.  If you observe over 10,000 GDI objects after following the below steps to monitor GDI usage, contact your local Value Added Reseller (VAR) for assistance troubleshooting this and reporting to SOLIDWORKS Support.

You can monitor this through the Task Manager.

  1. Open Task Manager (right click on start bar > Task Manager OR through CTRL+ALT+DEL)
  2. Click on ‘Details’ Tab
  3. Right click on one of the columns and click on ‘Select Columns’
  4. Tick the GDI objects

WARNING: SOLIDWORKS Resources Running Low
Suggested Solution:

This solution will involve editing the Windows Registry.

Disclaimer: Modifying the registry can cause serious problems that may require you to reinstall your operating system. We cannot guarantee that problems resulting from modifications to the registry can be solved. Use the information provided at your own risk.

As mentioned before, the windows by default sets the GDI Objects limit for a single process to be 10,000. However the maximum allowed is 16,384. By increasing this limit in the registry, it will give any given application more room to breathe.

  1. Open Regedit (via Run > type ‘regedit’)
  2. Locate to the key: HKEY_LOCAL_MACHINE\SOFTWARE\Microsoft\Windows NT\CurrentVersion\Windows\GDIProcessHandleQuota
  3. Right click on the ‘GDIProcessHandleQuota’ and click ‘Edit’.
  4. Change the registry key to the maximum process limit 16,384; set the BASE to DECIMAL.

WARNING: SOLIDWORKS Resources Running Low
2. Virtual Memory

Another major cause for insufficient system memory could be due to virtual memory of Windows.

Virtual memory, also known as Page File is a memory combination of RAM and a portion of your hard drive disk. Whenever your system runs out of physical RAM, Windows will make use of the Page File to temporarily store files and swap back to the physical RAM when it is freed.

By default, your virtual memory (page file) managed by windows. Custom Size allows you to set the size of the page file. As a general guide, the maximum size of the paging file should be 2 times the amount of physical RAM installed on the machine.

How to set custom sized virtual memory:

WARNING: SOLIDWORKS Resources Running Low

  1. System > Advanced System Settings > Advanced (Tab) > Settings..
  2. Advanced (Tab) > Change..
  3. Untick ‘automatically manage paging file size for all drives
  4. Choose the Drive you would like to utilize Virtual Memory on. (eg. My workstation only had C:\ which is the SSD)
  5. Choose Custom size button
  6. Enter the Initial size value of 2 times the amount of physical RAM installed in your system (eg. If you have 16GB, type in 32000MB.)
  7. Enter Maximum size value same as the initial size.
  8. Press ‘Set’
  9. Restart your workstation.

WARNING: SOLIDWORKS Resources Running Low

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NCCS Australia
N C CAD CAM SYSTEMS, Authorised SOLIDWORKS Reseller in Victoria, Australia. Over 20 years, we have offered CAD/CAM and manufacturing solutions to thousands of Australian and New Zealand companies.

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SOLIDWORKS Time-Lapse Tutorial: Useless Box http://blogs.solidworks.com/tech/2017/05/solidworks-time-lapse-tutorial-useless-box.html http://blogs.solidworks.com/tech/2017/05/solidworks-time-lapse-tutorial-useless-box.html#respond Tue, 23 May 2017 21:00:03 +0000 http://blogs.solidworks.com/tech/?p=16875 Looking for the perfect gift but don’t want to buy anything new? In this guide we will show you how we took an old useless box and use SOLIDWORKS and 3D printing and turned it into something new. Now this

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SOLIDWORKS

Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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Looking for the perfect gift but don’t want to buy anything new? In this guide we will show you how we took an old useless box and use SOLIDWORKS and 3D printing and turned it into something new.

Now this box isn’t all that useless, it serves a purpose. That purpose is to do nothing so, in turn, it is a useless box. Confusing right? We will give you a minute to process. So this is an old kit we got a little while back, but the acrylic and metal look got a little dull after some time so we decided to use SOLIDWORKS and 3D printing to bring it back to life.

Useless Box
The design process for this was simple; first replicate, then create. We started by reproducing a simple version of the PCB by just highlighting the important element. This saves time rather than recreating every element. Then, the original body was generated around the PCB which created a perfect skeleton to work from.

We then began create the new box around the old one. We used the old box as a reference for the scale and for the placement of splits, which are needed for the lids. We gave it a more shapely body with rounded edges, making it softer. Now, you could go ahead and add more details and extravagant markings but, we chose this shape to serve not as a final product but as an inspiration for your own projects.

Once all three parts were complete, we separated them and prepared them to print. We were lucky for this project as we didn’t run into any troubles with the printing process. With the design, we kept each overhang above 45 degrees to the bed. This allowed all parts printed with no support so they came off the bed clean and ready. This is the ideal scenario for any 3D printing project.

For assembly, we disassembled the old useless box, then put the battery box and PCB in place. We then glued the static lid in place and clipped on the moving lid. The hinge was a little stiff, so it was trimmed with a scalpel and used a lubricant to loosen it up. This made the hand press the switch and the lid went down went with it.

This project is great if you are bored with something and wish to change it up, or if you need a quick gift for someone and don’t have the time to go out and buy something. 3D printing is excellent for these any little project like this, and is an easy way to start your journey in the wonderful world of 3D printing. We hope you learned a lot from this tutorial and use this knowledge to brighten up your own home or someone’s day.

Check out our YouTube playlist for more SOLIDWORKS Time-Lapse tutorials!

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SOLIDWORKS
Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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SOLIDWORKS Drift Trike – Frame Design http://blogs.solidworks.com/tech/2017/05/solidworks-drift-trike-frame-design.html http://blogs.solidworks.com/tech/2017/05/solidworks-drift-trike-frame-design.html#respond Tue, 23 May 2017 15:00:47 +0000 http://blogs.solidworks.com/tech/?p=16430 In our latest SOLIDWORKS tutorial series, Cadtek Systems’ Stuart Wortley combines his passion for the outdoors to guide you through creating your very own Drift Trike. This latest gravity sport is rising in popularity both in the US and in the

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Cadtek Systems UK - Elite SOLIDWORKS Training & Support

Cadtek has been established for over 27 years. Based in the UK, we have unrivalled experience in providing design solutions for designers and engineers. We work across all disciplines and multiple industries.

An award winning Elite Reseller we can help you understand and choose the right 3D CAD solution. Call 0800 804 7766 to speak to an account manager. For more information, visit cadtek.com.

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In our latest SOLIDWORKS tutorial series, Cadtek Systems’ Stuart Wortley combines his passion for the outdoors to guide you through creating your very own Drift Trike. This latest gravity sport is rising in popularity both in the US and in the UK. It comprises of a single wheel at the front with two, often Nylon, wheels at the rear to allow “drift”. The 3D modelling techniques in this series cover a wide range of skills useful to any SOLIDWORKS user.

Frame Design

The first of a four part series Stuart will guide you through frame design in SOLIDWORKS 3D CAD. Not only is a frame the most important structural member it is also the biggest part and shapes the feel of the Trike. This video tutorial contains the step by step process for creating the frame and structure of the whole Trike. Using a layout sketch to drive all the features, your model will be smart in relation to other components. This makes it very easy to update and make changes if you need to in the future.

The topics covered in this part of the series include:

  • Introduction to the series
  • Layout Sketches
  • Multi Body Design
  • Lofts
  • Sweep Feature
  • Sheet Metal
  • Using End Conditions and References

See Cadtek’s original article here. Look out for the second part in this series in the coming weeks covering fork design. This will go into Layout Sketches, Lofts, Sweeps and Complex features, other skills that every SOLIDWORKS user should have under their belt. For more hints, tips and content head over to our Twitter page or our YouTube channel.


Cadtek Designer Profile – Stuart Wortley

Cadtek Application Engineer

Stuart has been with Cadtek Systems for 18 years and is key part of our application team. His passion for the outdoors, his VW Camper-van and SolidWorks is clear. It has seen him produce some great, easy to follow SOLIDWORKS tutorials around Paddle Boarding, Cabinet Design and now Drift Trikes! This year saw Stuart achieve the accolade of Elite Application Engineer at SOLIDWORKS World 2017 in LA, the highest level achievable.

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Cadtek Systems UK - Elite SOLIDWORKS Training & Support
Cadtek has been established for over 27 years. Based in the UK, we have unrivalled experience in providing design solutions for designers and engineers. We work across all disciplines and multiple industries. An award winning Elite Reseller we can help you understand and choose the right 3D CAD solution. Call 0800 804 7766 to speak to an account manager. For more information, visit cadtek.com.

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Everyday Problems: Creating an Enclosure for Raspberry Pis http://blogs.solidworks.com/tech/2017/05/everyday-problems.html http://blogs.solidworks.com/tech/2017/05/everyday-problems.html#respond Mon, 22 May 2017 15:00:39 +0000 http://blogs.solidworks.com/tech/?p=16850 My name is Rob and as anyone that knows me well will tell you, I have a problem with Raspberry Pis. They are my uncontrollable addiction and I cannot get enough. I currently have six of them with plans for

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CADimensions

We are an authorized SOLIDWORKS and Stratasys reseller with certified training & support centers located in New York and Pennsylvania, USA. We are 100% focused on living a CADLIFE and have our vendor's unconditional endorsement in the sales and support of their products.

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My name is Rob and as anyone that knows me well will tell you, I have a problem with Raspberry Pis. They are my uncontrollable addiction and I cannot get enough. I currently have six of them with plans for more in the near future; if I see a used one for sale, I have to have it. I use them for a variety of things such as, media centers, game emulators, home security systems, and various servers.

One of my latest projects was using an Arduino to control the temperature and water level in one of my saltwater fish tanks. The Arduino measures the water temperature and checks the water level via some external sensors. It then displays information about the tank to an LCD display, and sends serial data to a Raspberry Pi that stores the information in a database which can be queried and plotted through a web interface. Everything works flawlessly, but I didn’t have anywhere to put all of the components which would keep everything together and neatly organized. This is where SOLIDWORKS comes in.

I knew I wanted a simple enclosure to contain all of the components, but I didn’t know exactly what the enclosure would look like or how the components would be oriented. At this point, I went to the internet and found some CAD models for a Raspberry Pi, an Arduino, a breadboard, and an LCD display. With these 3D models now in a SOLIDWORKS assembly, I was able to align them how I wanted them to sit and use top down design methods to create an enclosure to house them.

Raspberry Pis

Using the “Insert New Part” function I was able to start creating a new part that would become the lower portion of the enclosure. This was done very simply by extruding the four sides and bottom, a small ledge for the Arduino to rest on, and then using cuts where things would get plugged into the Pi and Arduino. I threw in a few fillets, and the lower part of my enclosure was now exactly what I needed.

This ability to design around existing components is part of what makes top down design so powerful. I didn’t know exactly what the enclosure was going to look like and where holes would be located, but by putting the lower level parts into the assembly and then designing around them I was able to get exactly what I needed.

Now that I had the lower portion of the enclosure completed I needed to make a top to keep any water from getting splashed on the electronics. Again using top down methods I was able to insert a new part and create some very simple extrusions from a convert entity that was performed on the top edge of the lower enclosure. After this was extruded I capped off the top, inserted some fillets, and cut out the area where the display would be located.

Now that I had a model that looked like it would work with my components, I decided to head on over to the 3D Printer and create the enclosure. I came in the next morning to my printed components which neatly accommodated my electronics with the use of some double sided tape.

This small project really encompasses everything I love about SOLIDWORKS. I was able to download some files online and import them into SOLIDWORKS, then design around those parts, export STL files to use on the 3D printer, and then create those parts in a matter of hours. SOLIDWORKS provides the ability to solve extremely complex problems, but it can also be used for simple everyday issues that each of us may encounter even at home.

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CADimensions
We are an authorized SOLIDWORKS and Stratasys reseller with certified training & support centers located in New York and Pennsylvania, USA. We are 100% focused on living a CADLIFE and have our vendor's unconditional endorsement in the sales and support of their products.

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SOLIDWORKS Lindbergh’s Spirit of St. Louis Tutorial – Part 5 http://blogs.solidworks.com/tech/2017/05/solidworks-lindberghs-spirit-of-st-louis-tutorial-part-5.html http://blogs.solidworks.com/tech/2017/05/solidworks-lindberghs-spirit-of-st-louis-tutorial-part-5.html#respond Sun, 21 May 2017 21:00:25 +0000 http://blogs.solidworks.com/tech/?p=15502 On May 20th and 21st, 1927 Charles Lindbergh, aka “Lucky Lindy”, made history by completing the first solo, nonstop, transatlantic flight; piloting his monoplane, the Spirit of St. Louis, from Long Island, New York to Paris, France. To celebrate the

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SOLIDWORKS

Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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On May 20th and 21st, 1927 Charles Lindbergh, aka “Lucky Lindy”, made history by completing the first solo, nonstop, transatlantic flight; piloting his monoplane, the Spirit of St. Louis, from Long Island, New York to Paris, France. To celebrate the anniversary of Lindy’s achievement we’re showing SOLIDWORKS users how to model a 30” wingspan version of his iconic aircraft. Throughout this series, we’ll fly through lessons on how to work off imported images, and we’ll use a series of extrusions, lofts, and sweeps to model the Spirit of St. Louis.

Welcome to the final part of our 5 Part series where we are celebrating the anniversary of Charles Lindbergh’s historic feat by modeling his Spirit of St. Louis monoplane. We’ll pick up where we left off in part 4 with a nearly completed half of the aircraft and we’ll begin adding some of the aircraft’s details using some essential modeling techniques, as well as a few advanced techniques like the Circular Pattern command.  We will wrap up this part of the series by flying through how to add custom appearances and decals to your model.

Whether you’re an aviation enthusiast or are just looking for a new SOLIDWORKS challenge, the Lindbergh’s Spirit of St. Louis tutorial series is for you!

Can’t wait to watch the next video? View all of the tutorials on the playlist here.

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SOLIDWORKS
Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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Stump the Chump: How Can I make My Cam Follower “Roll” on the Cam Surface? http://blogs.solidworks.com/tech/2017/05/stump-chump-can-make-cam-follower-roll-cam-surface.html http://blogs.solidworks.com/tech/2017/05/stump-chump-can-make-cam-follower-roll-cam-surface.html#respond Fri, 19 May 2017 21:00:58 +0000 http://blogs.solidworks.com/tech/?p=16843 This blog explains how to make a cam follower roll on a cam surface using SOLIDWORKS.

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Barbara Schmitz

Barbara Schmitz
Senior Brand Introduction Manager at SolidWorks

Loyal dog owner, travel bum, cool mom, and lover of hoppy IPAs, alternative music and cool tech.

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This is the second installment of our new Stump the Chump blog series here at SOLIDWORKS. In this series we will delve into common SOLIDWORKS questions and/or problems that our users have on a day-by-day basis and will present various ways in which they can solve them. While we have a large team of seasoned CAD users at SOLIDWORKS available to answer user questions, we also have the most passionate and best CAD community in the world. So in this blog series, we are going to share advice, tips and suggestions from actual users.

We are scouring the SOLIDWORKS User Forums for questions and/or problems that we feel are probably pretty common among our users. If after reading this Stump the Chump post, you have an alternative answer or simply have an additional question, please feel free to add it to the comment section below.
So without further ado, here is the question:

Question: How can I make my cam follower “roll” on a cam surface?
User answer: I tried some things out, and I don’t think that it is possible using ONLY mates. I tried a combination of cam and RACK AND PINION mates, and it works, but only on the straight areas of the cam, if there are any.   But once the cam follower went around a corner, the rolling ceased and sliding started.

Stump the Chump

SOLIDWORKS Expert Weigh-in: Yes, it is possible to make the cam follower roll on the cam surface.  I created a video and attached the models showing two ways to approach this solution.

There are two ways to accomplish this. If you want to make something that looks good in a design review or video, you can accomplish it with a Gear Mate, and set the ratio to be close to the average diameter of cam. This will make the follower appear to roll on the surface of the cam. This works well visually, but if you are looking for the angular velocity of the cam follower, you will need to use SOLIDWORKS Motion, and choose a Motion Analysis study as opposed to an Animation study.

Since the Cam Mate does not account for friction as does some of the basic mates, you will want to use curve contact to define the contact and set the coefficient of friction between the cam and follower to be 1, or very sticky. Apply a motor to the cam, and gravity so that the follower does not fly off the cam, and run the motion study. This will give you the precise angular velocity of the follower if that is the information that you are looking for.

 

Thank you to John Bryjak for the question and to Dan Pihlaja for providing solutions in the SOLIDWORKS User Forum. If you have a question that you would like to pose to the greater SOLIDWORKS user community or to provide tips and tricks to your peers, our User Forums are a great resource. Access the SOLIDWORKS User Forums here.

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Barbara Schmitz
Barbara Schmitz
Senior Brand Introduction Manager at SolidWorks
Loyal dog owner, travel bum, cool mom, and lover of hoppy IPAs, alternative music and cool tech.

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SOLIDWORKS Simulation Quick Tip: Prescribed Displacements http://blogs.solidworks.com/tech/2017/05/solidworks-simulation-quick-tip-prescribed-displacements.html http://blogs.solidworks.com/tech/2017/05/solidworks-simulation-quick-tip-prescribed-displacements.html#respond Fri, 19 May 2017 15:00:30 +0000 http://blogs.solidworks.com/tech/?p=16820 When setting up an analysis in SOLIDWORKS Simulation, we typically think of applying forces or other loads and calculating the resulting stresses and displacements as our outputs. However, in situations where the forces may not be known, an expected displacement

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Hawk Ridge Systems

From design to production, Hawk Ridge Systems delivers best-in-class solutions in 3D design, CAM software, and 3D printing.

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When setting up an analysis in SOLIDWORKS Simulation, we typically think of applying forces or other loads and calculating the resulting stresses and displacements as our outputs. However, in situations where the forces may not be known, an expected displacement can effectively be used as the “load” input to the analysis.

This is known as a Prescribed Displacement and is available under the External Loads drop-down.

SOLIDWORKS Simulation Quick Tip: Prescribed Displacements - Part 1image001
Note that launching the Prescribed Displacement command actually brings the user to a type of advanced fixture, where a direction for the displacement must be specified. Then, the amount and direction of the prescribed translation or rotation are specified.

SOLIDWORKS Simulation Quick Tip: Prescribed Displacements - Part 1image003
As a result, the force required to achieve the prescribed displacement can be backed out by using the option List Result Force and of course the resulting stresses can be calculated.

If it is ever necessary to apply both a translation and rotation, then an alternate method is to use the Remote Load/Mass feature under the External Loads pulldown. Within the Remote Load/Mass is the option to apply a Displacement.

SOLIDWORKS Simulation Quick Tip: Prescribed Displacements - Part 2image001
This requires slightly more setup work since it is typically recommended to create a Coordinate System at the location where the displacement will be applied, as can be seen below. Once setup, however, it provides an easy way to prescribe both Translations and Rotations about this point in space.

SOLIDWORKS Simulation Quick Tip: Prescribed Displacements - Part 2image003
It’s also worth noting that the Remote Load/Mass can effectively be used as a type of advanced fixture when used with this “Displacement” option. In fact, an important consideration whenever using a Prescribed Displacement is that it is placing additional constraints on the system.  If a displacement is applied, then that displacement will never be exceeded no matter how much force is applied elsewhere in the model.


For additional details on how this process can be performed, please check out our YouTube channel or contact Hawk Ridge Systems today. Thanks for reading!

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Hawk Ridge Systems
From design to production, Hawk Ridge Systems delivers best-in-class solutions in 3D design, CAM software, and 3D printing.

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Adjusting Virtual Memory (Windows Pagefile) for increased SOLIDWORKS Performance http://blogs.solidworks.com/tech/2017/05/adjusting-virtual-memory-windows-pagefile-for-increased-solidworks-performance.html http://blogs.solidworks.com/tech/2017/05/adjusting-virtual-memory-windows-pagefile-for-increased-solidworks-performance.html#comments Tue, 16 May 2017 15:00:28 +0000 http://blogs.solidworks.com/tech/?p=16806 Author: Chris Briand, CSWE, Javelin Technologies A kin to the article that our teammate, Josh Carrier, wrote back in 2010, I thought it high time we review the process of how to increase virtual memory on your workstation. We use

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Javelin Technologies

Javelin Technologies is a provider of technology solutions since 1997. We are experts in 3D design and have helped thousands of companies with solutions for mechanical design, electrical design and 3D printing.

Large or small, we have the skills, experience, and services to propel your organization to new heights so you can aim high.

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Author: Chris Briand, CSWE, Javelin Technologies

A kin to the article that our teammate, Josh Carrier, wrote back in 2010, I thought it high time we review the process of how to increase virtual memory on your workstation.

We use this procedure a great deal when attempting to enhance the performance of systems where SOLIDWORKS is having difficulty with importing or exporting geometry, or handling larger assemblies. What we are essentially doing is raising the ceiling and giving the operating system the extra room it needs to maneuver if it runs out of physical memory.

One of the tidbits we have discovered over the years is that SOLIDWORKS typically throws the demand for more page file at the Operating System so quickly that it takes time for the operating system to allocate the needed amount of virtual memory, further slowing operations.

SSD or NOT?

One item to highlight, having grown in prominence these last few years, is the effect of a page file being located on an SSD drive, which may be acting as the host drive for your Operating system and installation of SOLIDWORKS.

Before SSD technology was readily available you would have placed the page file on the Root of the main drive (C:\), without jeopardizing the long term safety of your HDD drive. The trade off here is that writing operations to a page file located on the HDD would have slowed performance slightly as the HDD was much slower than RAM. This is still true today with SSD drives however there is an added danger, as SSD’s have a limited lifespan and can only handle so many writing cycles – it may be a better choice to locate a larger page file on a secondary spinning disk.

How much RAM?

To properly adjust your virtual memory values, you will need to know how much physical memory, or RAM, is on the system.  You can find this by navigating to the System Information Dialog

The System Info Dialog can be found by typing “System Info” in windows 10 and opening the System Info dialog (or Start > All Apps > Windows Administrative Tools > System Information)

IMPORTANT: One question to research before attempting the following procedure is: Do I have sufficient Disk Space to make a change to the page file size?

With Physical Memory (RAM) amounts of 4GB to 24 GB we suggest having a page file minimum size set to 2 times the amount of Physical Memory (RAM) in the system.

If you are lucky enough that you have more than 16 GB of RAM in the system, we suggest that the page file minimum be set between 1 and 1.5 times the amount of RAM.

Changing the Virtual Memory Values

  1. Within the Windows 10 Search type “Performance”
  2. This should bring up an entry that states: “Adjust the appearance and performance of Windows” (This is the same dialog that you would have accessed if you had navigated via the control panel: Control Panel > System > Advanced System Settings > Advanced Tab > Settings)

Adjusting Virtual Memory for SOLIDWORKS Performance

Accessing Virtual Memory

  1. Once you have arrived within the performance options dialog choose the Advanced Tab > and select the “Change” button located within the in the Virtual Memory section of the dialog.
  2. Uncheck the “Automatically manage paging file size for all drives” Option
  3. Select the drive where you have room or deem it appropriate to place the page file.
  4. Choose the “Custom Size” Radio Button.
  5. Enter a MINIMUM value of 1 to 2 times the amount of physical RAM you have in the system. (16GB would appear as 16000MB)
  6. Enter a MAXIMUM value of 2GB more than the MINIMUM value specified in the step above. (This will ensure that windows reporting and other diagnostic reports are correct)
  7. Choose the “Set” button
  8. Restart the Workstation to realize the changes to Virtual Memory.

 

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Javelin Technologies
Javelin Technologies is a provider of technology solutions since 1997. We are experts in 3D design and have helped thousands of companies with solutions for mechanical design, electrical design and 3D printing. Large or small, we have the skills, experience, and services to propel your organization to new heights so you can aim high.

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SOLIDWORKS Drawings – Automatically Create a Border http://blogs.solidworks.com/tech/2017/05/solidworks-drawings-automatically-create-border.html http://blogs.solidworks.com/tech/2017/05/solidworks-drawings-automatically-create-border.html#respond Mon, 15 May 2017 15:00:06 +0000 http://blogs.solidworks.com/tech/?p=16743 How to use the Automatic Border Feature The Automatic Border Feature quickly allows you to create a border in your sheet format. You can control every aspect of the border, including grid size and layout. When using the tool border,

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GoEngineer

GoEngineer delivers software, technology and expertise that enable companies to unlock design innovation and deliver better products faster. With more than 30 years experience and thousands of customers in high tech, medical, machine design, energy and other industries, GoEngineer provides best-in-class design solutions from SOLIDWORKS, Stratasys, CAMWorks, Altium and Product Lifecycle Management (PLM). For more information, visit goengineer.com.

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How to use the Automatic Border Feature

The Automatic Border Feature quickly allows you to create a border in your sheet format. You can control every aspect of the border, including grid size and layout. When using the tool border, zones automatically update. You can also add Margin Mask areas, where labels and dividers are not shown.

Let’s Get Started

To Start the Automatic Border Feature, go to – Open a drawing, then click the Sheet Format Tab. Select Edit Sheet and then Automatic Border.

Drawings
The first option you will see is the Delete list, you can select items that are already on your Sheet Format to be deleted. Select the arrow. You will want to delete any existing border, this prevents overlapping with the newly created border.

Drawings

Setting the Zone and More

The next step allows you to set the zone size, formatting, borders, and margins. You have two options for the zone formatting the “50mm from center” option creates zones every 50mm from the center or the “evenly sized” option creates rows and columns that are based on the paper size.

Drawings
The Margin options include left and right justifications, line size and adding a double border.

Drawings
If you want an odd number of rows and columns, the Center Zone Divider may overlap the center label.  If this is the case, you can specify the Outer Zone Divider Length to be zero.

Drawings

Margin Masks

The last step allows you to add margin masks.  Margin masks allow you to hide zone divider and labels in the margin. To create a margin mask, select plus button and position the rectangular mask over the area you want to hide. You can add multiple masks to the page.

Drawings
You have now created a parametrically linked border! Don’t forget to save it as a Sheet Format. To do so, save the sheet format, select File – Save As Sheet Format.

Drawings
And that’s a wrap on using the automatic border feature in SOLIDWORKS Drawings!


Author: Krystine Thoroughman
Krystine has been working with CAD for the past 10 years as a Designer and Technical Support Engineer. She became interested in the industry through working with her Dad, a machinist from Arizona. Krystine’s current focus is SOLIDWORKS PDM support and helping customers understand how different pieces of software can work together, to create a more efficient work environment!

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GoEngineer
GoEngineer delivers software, technology and expertise that enable companies to unlock design innovation and deliver better products faster. With more than 30 years experience and thousands of customers in high tech, medical, machine design, energy and other industries, GoEngineer provides best-in-class design solutions from SOLIDWORKS, Stratasys, CAMWorks, Altium and Product Lifecycle Management (PLM). For more information, visit goengineer.com.

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SOLIDWORKS Lindbergh’s Spirit of St. Louis Tutorial – Part 4 http://blogs.solidworks.com/tech/2017/05/solidworks-lindberghs-spirit-of-st-louis-tutorial-part-4.html http://blogs.solidworks.com/tech/2017/05/solidworks-lindberghs-spirit-of-st-louis-tutorial-part-4.html#respond Fri, 12 May 2017 21:00:04 +0000 http://blogs.solidworks.com/tech/?p=15500 On May 20th and 21st, 1927 Charles Lindbergh, aka “Lucky Lindy”, made history by completing the first solo, nonstop, transatlantic flight; piloting his monoplane, the Spirit of St. Louis, from Long Island, New York to Paris, France. To celebrate the

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SOLIDWORKS

Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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On May 20th and 21st, 1927 Charles Lindbergh, aka “Lucky Lindy”, made history by completing the first solo, nonstop, transatlantic flight; piloting his monoplane, the Spirit of St. Louis, from Long Island, New York to Paris, France. To celebrate the anniversary of Lindy’s achievement we’re showing SOLIDWORKS users how to model a 30” wingspan version of his iconic aircraft. Throughout this series, we’ll fly through lessons on how to work off imported images, and we’ll use a series of extrusions, lofts, and sweeps to model the Spirit of St. Louis.

Welcome to part 4 of our 5 -part series where we are modeling Lucky Lindy’s iconic Spirit of St. Louis monoplane. We have the basic components of the aircraft modeled and we are now ready to model in the unique landing gear and strut structures to the wing and tail. In this part of the series we will take a deep dive into the Sweep tool and we will touch on the Dome and Variable Size Fillet tools.

Whether you’re an aviation enthusiast or are just looking for a new SOLIDWORKS challenge, the Lindbergh’s Spirit of St. Louis tutorial series is for you!

Can’t wait to watch the next video? View all of the tutorials on the playlist here.

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SOLIDWORKS
Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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SOLIDWORKS PDM Forms Series Part 2: Word Documents as Forms http://blogs.solidworks.com/tech/2017/05/solidworks-pdm-forms-series-part-2-word-documents-as-forms.html http://blogs.solidworks.com/tech/2017/05/solidworks-pdm-forms-series-part-2-word-documents-as-forms.html#respond Fri, 12 May 2017 15:00:05 +0000 http://blogs.solidworks.com/tech/?p=16730 Written by: Bryce Hooper, Application Engineer, DASI Solutions Continuing our series on automating forms inside of SOLIDWORKS PDM, we’ll move along with an example in Microsoft Word. (See Part 1 on Excel docs as forms here.) Here is our example

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DASI Solutions

DASI Solutions

DASI Solutions is dedicated to service and support. As one of a handful of original, charter value-added resellers (VAR) in the SolidWorks Community, DASI Solutions has built partnerships and success stories with many of our customers. We are very pleased to bring you SolidWorks 3D CAD design engineering software and 3D printing services.

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SOLIDWORKS PDM Tech Tip

Written by: Bryce Hooper, Application Engineer, DASI Solutions

Continuing our series on automating forms inside of SOLIDWORKS PDM, we’ll move along with an example in Microsoft Word. (See Part 1 on Excel docs as forms here.)

Here is our example of an Engineering Change Notice form:Engineering Change Notice

Now, to map these properties to our file and our data card, we will need to start with the variable setup. For Microsoft Office documents, the setup is pretty simple. For each variable we are mapping we will want to use the attribute block CustomProperty. This should be familiar as it is the same that we would use for SOLIDWORKS documents and was also noted in our article about Excel forms.

Edit Variable

Set this to use the proper extensions that we are intending to use and the rest of the options can be set at your discretion.

It is then time to map the custom properties to those ranges. This is done by going to the file info inside of Word, then properties and Advanced properties.Microsoft Word Advanced Properties

In the dialog that shows we go to the Custom tab. Here we find a list of properties that are already defined. Any variables that have already been assigned a value inside of PDM will automatically be created. Any that haven’t we will create now. To do this, we give the property a name in the Name field and then give it a value in the Value field. A space will work for this value, but in the interest of seeing what we are setting up, it may be advantageous to give this a realistic value to get our formatting right.

Document Properties

Now that we’ve created the custom properties inside of Word, we can enter them into the body of our document. This is done by going to the Insert tab > Quick Parts > Field.

Insert Field - Microsoft Word

Do this with your cursor in the desired location, and the following dialog will help us add the right field.

SOLIDWORKS PDM Forms Series Part 2: Word Documents as Forms - Field Properties

To get to our custom properties, we need to scroll down to the Field Name “DocProperty”. This will give us the Field Property of our available custom properties (plus some file properties). Select the custom property that we need to enter and click “OK”. If we had filled in a value for the custom property, it will now show.

For Word, custom properties and the fields they are linked to do will not update automatically or open by themselves. We have two options in this case.

  1. Force an update each time we open by pressing Ctrl+A and then F9
  2. Add a macro to update the fields on each open

Here, I’ll give you the code to do number two on that list.

To start we’ll need to create a new macro in Word. To do this, we can press Alt+F8. We get the dialog shown below.

Create new macro in Microsoft Word

Click “Create” and paste in the following code snippet:

Sub AutoOpen()

    With Options

        .UpdateFieldsAtPrint = True

        .UpdateLinksAtPrint = True

    End With

    ActiveDocument.Fields.Update

End Sub

Save and close the VB editor. From now on, each time the file is opened the fields should update.

From here, we can make things even easier by creating a template to help us fill in values or serialize a naming convention. We can also create actions in our workflow transitions to automatically fill in names and dates for approvals.

There are, of course, some pros and cons to this technique. I’ll break them down a bit here. By no means is this an all-encompassing list.

Pros:

  • Your company’s forms are probably already in Word (or some other Office format), so the translation isn’t difficult.
  • If they aren’t already in Word, this is an easy program for anyone else to learn and create forms.
  • Setup for this is fairly simple and intuitive. The process works similarly for other office formats.

Cons:

  • The PDM Preview window does not update until the file has been checked out, opened, saved, and checked back in.
  • Requires Microsoft Office on any machine that would need to view/print it.
  • Does not handle changes down the line to the form/format with ease. I.E.: As your company uses the process and changes the formatting or logo, old forms will not update to the new format without manual updates.
  • As of this article, some variable types either don’t work (Yes/No) or don’t display correctly (Date)
  • Requires a macro to update correctly.

If you’re looking for other ways to create forms inside of PDM, you may also want to check out our blog on Microsoft Excel forms and watch for our upcoming third part in the series covering XML documents as forms in PDM.

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DASI Solutions
DASI Solutions
DASI Solutions is dedicated to service and support. As one of a handful of original, charter value-added resellers (VAR) in the SolidWorks Community, DASI Solutions has built partnerships and success stories with many of our customers. We are very pleased to bring you SolidWorks 3D CAD design engineering software and 3D printing services.

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Get Oriented – Tricks for Orienting Your 3D Model Views in SOLIDWORKS http://blogs.solidworks.com/tech/2017/05/get-oriented-tricks-for-orienting-3d-model-views.html http://blogs.solidworks.com/tech/2017/05/get-oriented-tricks-for-orienting-3d-model-views.html#comments Wed, 10 May 2017 15:00:22 +0000 http://blogs.solidworks.com/tech/?p=16733 It’s no secret that a 3D model makes conveying your concepts, ideas, or designs easier than ever but, navigating around the 3D space can sometimes prove tricky. It can even sometimes seem borderline impossible. So, here are a few tips that

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Stephen Petrock

Since 1998, TriMech has helped our clients design better products by partnering with them and offering, not only CAD, CAE, PDM, FEA, CAM software products, but also by engineering solutions involving full-time and temporary staffing, contract design, analysis and drafting services, rapid prototyping, custom programming and implementation services. TriMech is a value-added reseller of SOLIDWORKS and Stratasys 3D Printers in the Mid-Atlantic and South-East including New Jersey, Pennsylvania, Delaware, Maryland, West Virginia, Virginia, North Carolina, South Carolina, Tennessee, South Carolina, Georgia, Florida, Alabama, Mississippi, Oklahoma, Arkansas and Louisiana.

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It’s no secret that a 3D model makes conveying your concepts, ideas, or designs easier than ever but, navigating around the 3D space can sometimes prove tricky. It can even sometimes seem borderline impossible. So, here are a few tips that can help you orient your 3D models with ease. With these tricks you can save yourself from the tediousness of manipulating views and get back to conveying your concepts and designs.

Default hot keys 

Use the default hot keys for quick access to the standard views:

Get Oriented - Tricks for Orienting Your 3D Model Views in SOLIDWORKS

 

Normal to

  1. Press normal to a second time to flip the view 180 degrees
  2. Press normal to when not in a sketch and the view will orient to the closest orthogonal view
  3. Customize your “normal to” orientation by selecting a second face which will define the “up” direction

 

Use the Triad

  1. Clicking the triad will orient the view normal to the axis you select
  2. Rotate about the axis 15 degrees or 90 degrees using the shift or alt keys

 

Bonus

If you like a view, you can save it to your model or even “globally” to your SOLIDWORKS system

Author information

Stephen Petrock
Since 1998, TriMech has helped our clients design better products by partnering with them and offering, not only CAD, CAE, PDM, FEA, CAM software products, but also by engineering solutions involving full-time and temporary staffing, contract design, analysis and drafting services, rapid prototyping, custom programming and implementation services. TriMech is a value-added reseller of SOLIDWORKS and Stratasys 3D Printers in the Mid-Atlantic and South-East including New Jersey, Pennsylvania, Delaware, Maryland, West Virginia, Virginia, North Carolina, South Carolina, Tennessee, South Carolina, Georgia, Florida, Alabama, Mississippi, Oklahoma, Arkansas and Louisiana.

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SOLIDWORKS Support Monthly News – May 2017 http://blogs.solidworks.com/tech/2017/05/solidworks-support-monthly-news-may-2017.html http://blogs.solidworks.com/tech/2017/05/solidworks-support-monthly-news-may-2017.html#respond Wed, 10 May 2017 06:50:51 +0000 http://blogs.solidworks.com/tech/?p=16617 Hello to all, Welcome to this new edition of the SOLIDWORKS Support Monthly News, coauthored by members of the SOLIDWORKS Technical Support teams worldwide. NEW Functionality: Import SOLIDWORKS Bill of Materials into SOLIDWORKS Composer By Jennifer Tashiro With the latest

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Julien Boissat

Sr. Technical Customer Support Engineer, SolidWorks, EMEA at DS SolidWorks Corp.

I have been a Tech Support engineer for Simulation products since 2002. I was previously a product manager at SRAC, the original makers of COSMOS for those who remember that time! ;-). I am currently in charge of the content of the certification exams for simulation products. I also initiated and still author the Simulation Knowledge Base and participate as much as possible in the expansion and evolution of the SolidWorks Knowledge Base. Finally, I handle the SolidWorks Support Monthly News blog.

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Hello to all,

Welcome to this new edition of the SOLIDWORKS Support Monthly News, coauthored by members of the SOLIDWORKS Technical Support teams worldwide.

NEW Functionality: Import SOLIDWORKS Bill of Materials into SOLIDWORKS Composer

By Jennifer Tashiro

With the latest version of SOLIDWORKS Composer, you can now import SOLIDWORKS Bill of Materials (BOM) directly into SOLIDWORKS Composer.  This means that you can repurpose even more of your 3D CAD data and save more time when creating technical communication content.

To use the new Import SOLIDWORKS BOM functionality:

  1. In the ‘FILE’ > ‘Open’ dialog, select a SOLIDWORKS part or assembly which includes a Bill of Materials.
  2. Select the ‘SOLIDWORKS’ options, then select the ‘Import SOLIDWORKS BOM’ checkbox.


After the import, you can see that a BOM is automatically generated in SOLIDWORKS Composer.  The Composer BOM contains the same data as the SOLIDWORKS BOM.

The Import SOLIDWORKS BOM functionality is available in SOLIDWORKS Composer 2017 SP3 and later versions.  Other enhancements in SP3 include automatic import of SOLIDWORKS appearances and textures.

Augmented Reality with eDrawings

By Sagar Gokulchand AGRAWAL

Some of you have already been explosed to the Augmented Reality (AR) of the eDrawings app or have enjoyed product design using AR. But for the rest of us, just know that SOLIDWORKS 2017 enables you to experience 3D CAD data in virtual reality using either the eDrawings iOS app or the Android app.

So what is Augmented Reality?

In simple terms, Augmented reality (AR) is a live direct or indirect view of a physical, real-world environment whose elements are augmented (or supplemented) by computer-generated sensory input such as sound, video or graphics data.

What do you need to experience Augmented Reality with eDrawings?

Short answer: Google Cardboard & a smartphone in which eDrawings app is installed

Google Cardboard is the least expensive way to dip your toe into virtual reality. And Cardboard viewers are designed to work with nearly any smartphone.

How does it work?

Similar to other Cardboard apps, the AR function of eDrawings mobile generates two images of the object being viewed, with a slight offset to account for stereo vision, making the object appear three-dimensional.

Convex lenses in the Cardboard headset resolve the two images into one and make it appear farther than a few inches in front of your eyes. The accelerometers in the phone also track movement, so the object moves and rotates, changing your perspective as you move your head.

What is the procedure to view eDrawings with AR?

  1. Open a model in eDrawings

Launch eDrawings app on your Smartphone > select a model

  1. Start a VR mode

Once the model loaded in eDrawings > Select VR button from left menu bar

 

  1. Keep your phone in Google cardboard or any other VR devices

 

  1. Wear you device and gets ready to experience your CAD data in AR.

As an eDrawings user, you can able to view the model 360º by simply moving your head around.  Although I would advise some caution if using in conjunction with a swivel office chair and doing full 360º rotation!  It can bring on a little motion sickness!  J

Conclusion

Viewing a model in eDrawings virtual reality allows you to add an extra layer of immersive realism to your design, using the movement of your head, rather than your finger, to manipulate the model.

It would be very impressive to demo 3D models of products to clients, where they can interact with them in VR space. VR is available only with the professional version of the eDrawings app, for both Android and iOS systems.

Some of the most remarkable fields where AR in eDrawings can be applied are architecture, construction and furniture. In these cases, CAD images of a structure can be superimposed into a real life local view before constructing the physical building.

AR is also very helpful in industrial design because it can help designers experience products’ designs and operations before completion.

Simulation Step-Up Series

Last month, Reza discussed the topic of FEA with an Engineering View. This month, Omar discusses the topic of basic failure analysis.

Next month, Reza will come back and discuss the topic of Accuracy and Convergence.

Noteworthy Solutions from the SOLIDWORKS Knowledge Base

icon - SW Why is SOLIDWORKS graphical performance slow with Windows 10 after Windows Update?
Windows update might have automatically installed a new NVIDIA graphics driver on your Windows 10 system, the affected driver versions are 376.53 or 376.54.  Please verify the graphics driver version from System Information or Device Manager.
Until a fix is available from Windows/NVIDIA please roll back graphics driver then use this Microsoft tool to stop Windows from updating the driver: https://support.microsoft.com/en-us
From Solution Id: S-072912.

icon - SW General Hotfix for SOLIDWORKS® 2016 SP5 (SPR#1006822)
A hotfix is available for SOLIDWORKS® 2016 SP5 that addresses the following issue:
SPR#1006822 –  General Stability Hotfix to address crashes when CTRL+Q operation is performed on weldment assembly with weld beads.
The hotfix for this issue is included in the attachment of Solution Id: S-073024. This issue is addressed in SOLIDWORKS 2017 SP3.

icon - SW Is the SOLIDWORKS® software supported for use on Microsoft® Surface devices?
The SOLIDWORKS® software does not officially support the use of Microsoft® Surface devices because those devices do not include CAD system graphics.
However certification tests, showed the Surface Book run the SOLIDWORKS software capably.
For more detailed information, see Solution Id: S-072859.

Icon - EPDM In the SOLIDWORKS® PDM software, how do I control the number of pending tasks that a task host will process and place in ‘Starting up’ status?
By default, a SOLIDWORKS® PDM task host polls the file vault database every 30 seconds and starts processing all available tasks with the status ‘Waiting for host’.
In SOLIDWORKS PDM 2017 , too learn how to control how many pending tasks a task host can queue up when polling the vault database, follow the steps in Solution Id: S-072642.

How do I manually calculate the ‘Acoustic Power’ and ‘Acoustic Power Level’ to validate the values given by SOLIDWORKS® Flow Simulation?
The foundation to such a hand calculation is to follow the explanation and equations given in the “Noise Prediction” topic of the Online Help.
Attachments to Solution Id: S-072876 provide:
•    A sample calculator in an Excel spreadsheet
•    A sample part model
•    A screen capture of ‘Acoustic Power’ and ‘Acoustic Power Level’ results

When I enter an evaluation (EVAL) serial number in the SOLIDWORKS® Installation Manager, why do I see the error ‘Your serial number does not entitle you to SOLIDWORKS Plastics…’?
This error message indicates that the evaluation (EVAL) serial number you are using was issued as a SOLIDWORKS® Premium CAD serial number, with SOLIDWORKS Plastics as an Add-In asset. This means that you do not enter this EVAL serial number in the ‘Simulation’ section of the Installation Manager because it is a CAD serial number. Instead, you must enter this EVAL serial number in the ‘3D Design’ section for the ‘SOLIDWORKS Standard, Professional, Premium or SolidNetWork License’ option.
From Solution Id: S-072633.


That’s it for this month. Thanks for reading this edition of SOLIDWORKS Support News. If you need additional help with these issues or any others, please contact your SOLIDWORKS Value Added Reseller.

Also, comments and suggestions are welcome. You can enter them below.

 

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Julien Boissat
Sr. Technical Customer Support Engineer, SolidWorks, EMEA at DS SolidWorks Corp.
I have been a Tech Support engineer for Simulation products since 2002. I was previously a product manager at SRAC, the original makers of COSMOS for those who remember that time! ;-). I am currently in charge of the content of the certification exams for simulation products. I also initiated and still author the Simulation Knowledge Base and participate as much as possible in the expansion and evolution of the SolidWorks Knowledge Base. Finally, I handle the SolidWorks Support Monthly News blog.

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SOLIDWORKS Electrical 2017: Connection Dots http://blogs.solidworks.com/tech/2017/05/solidworks-electrical-2017-connection-dots.html http://blogs.solidworks.com/tech/2017/05/solidworks-electrical-2017-connection-dots.html#respond Tue, 09 May 2017 15:00:38 +0000 http://blogs.solidworks.com/tech/?p=16758 There’s no need to lament any further over missed connections thanks to the SOLIDWORKS Electrical 2017 Connection Dots feature. Missed Connections – Somewhere on Craigslist Prior to September 2016 Have you ever read those “missed connection” posts on Craigslist? I learned of them

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GSC

GSC fuels customer success with 3D engineering solutions for design, simulation, data management, technical documentation, and 3D printing, as well as the most comprehensive consulting, technical support, and training in the industry. As a leading provider of SOLIDWORKS solutions and Stratasys 3D printing technologies, GSC’s world-class team of dedicated professionals have helped numerous companies innovate and increase productivity by leveraging advanced technologies to drive 3D business success. Founded in 1989, GSC is headquartered in Germantown, WI. For more information about GSC, please visit www.gsc-3d.com.

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There’s no need to lament any further over missed connections thanks to the SOLIDWORKS Electrical 2017 Connection Dots feature.

Missed Connections – Somewhere on Craigslist Prior to September 2016

Missed SOLIDWORKS Electrical Connections - Somewhere on Craigslist prior to September 2016Have you ever read those “missed connection” posts on Craigslist? I learned of them from a radio morning show, where the on-air personalities would read these tragic (yet hilarious) tales of lost love and near misses. These posts always delivered the melodrama and were filled with regret. If only the individual had possessed the courage to make that connection, so their whole life could achieve its true meaning and purpose. Like I said, M-E-L-O-D-R-A-M-A-T-I-C. But, I digress.

So, How Do Missed Connections Tie into Electrical Design?

I was helping a new user who was experiencing the same regret… over missed connections of the electrical kind. He had created new symbols and built a schematic, but he had empty reports. At a glance, everything looked OK but zooming in very close revealed SNAP had been turned off when placing the symbols and wires on their schematics. That meant nothing was connected! Maybe not quite the melodramatics of a Craigslist missed connection, but frustrating nonetheless. Significant rework was needed to move and replace all of his symbol and wire work on the grid.

How do you know you’ve made a proper connection point, especially as a new user?

And, how do you spare yourself the regret of a missed connection? This may sound like a stretch (get it!?), but in SOLIDWORKS Electrical the connection is key. By missing the link between components, you miss out on the power of the automation and reports. With SOLIDWORKS Electrical 2017, we now have a great way to graphically verify if you’ve succeeded in making a proper connection. You are now guaranteed good results on all your reports!

SOLIDWORKS Electrical Missed Connection Example 1

You can always use the DRC for terminals not connected. Or, place connection labels.

But, how do you know on the fly if the new symbol you’ve created had the proper grid spacing for its connection points? And, how do you know if you had your SNAPS turned on and set properly when you drew in your wires? We have a new way of doing just that by using something that was already there!

No More “Close, But No Cigar” or Guesswork and Rework!

In previous versions of SOLIDWORKS Electrical, connection dots were just a graphical indication of where a symbol’s connection points were lining up. The connection dots could be shown or hidden based on the symbol settings. That all still applies, but now any symbol with Connection Dots enabled, an intelligent feature can show or hide depending on if a connection has been properly aligned.

Solidworks Electrical Display Connection Points

Not to mention that in SOLIDWORKS Electrical 2017 getting close now actually DOES count to make a connection! New users will also appreciate that confidence boost in their initial designs and the new symbols that follow key spacing rules (.25 inches or 5 mm) for wires and connection dots.

So, make use of those new functions in 2017, and steer clear of missed connection regret.

Author information

GSC
GSC fuels customer success with 3D engineering solutions for design, simulation, data management, technical documentation, and 3D printing, as well as the most comprehensive consulting, technical support, and training in the industry. As a leading provider of SOLIDWORKS solutions and Stratasys 3D printing technologies, GSC’s world-class team of dedicated professionals have helped numerous companies innovate and increase productivity by leveraging advanced technologies to drive 3D business success. Founded in 1989, GSC is headquartered in Germantown, WI. For more information about GSC, please visit www.gsc-3d.com.

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Multiple processor cores and FEA: Good or bad? http://blogs.solidworks.com/tech/2017/05/multiple-processor-cores-fea-good-bad.html http://blogs.solidworks.com/tech/2017/05/multiple-processor-cores-fea-good-bad.html#comments Mon, 08 May 2017 15:00:22 +0000 http://blogs.solidworks.com/tech/?p=16702 There’s a lot of information scattered around the net regarding the usefulness of multiple core processors for Finite Element Analysis (FEA) in SOLIDWORKS Simulation. So what exactly is the optimum number of cores for FEA? Good question! There are some areas

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Innova Systems Experts in SOLIDWORKS Training & Support

We specialise in the supply, consultancy and training of SOLIDWORKS software. Based in Cambridge we have a central location to service a UK wide customer base. We offer the skills and experience to help you develop new products using SOLIDWORKS - empowering smarter, faster and more cost effective design.

We've been recognised by SOLIDWORKS Corporation for providing the highest rated customer support in Northern Europe in 2014, 2015 and 2016.

Email: info@innova-systems.co.uk / Telephone: 01223 200690.

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There’s a lot of information scattered around the net regarding the usefulness of multiple core processors for Finite Element Analysis (FEA) in SOLIDWORKS Simulation.

So what exactly is the optimum number of cores for FEA?

Good question! There are some areas that do and do not benefit from utilizing multiple processor cores. Take a look at this table:

SolidWorks-Multi-Cores-FEA-Table

As you can see, not all areas of the software benefit from having multiple cores/processors. The areas that don’t benefit are linear processes only. There are some areas that do benefit, but there is a limit.

SolidWorks Simulation FEA Multi-core 1

Image 1 – Mutliple Cores/CPU’s vs. Solution time (numbers for illustration purposes only).

 

The graph above illustrates the convergence between the number of cores and the solution time of the study. This explains that, after a certain point, the number of cores has little or no significant impact on the solution time. This is due to the communication time between the individual cores; the more you have, the longer the time taken to communicate and therefore the longer the solution time. Please note that SOLIDWORKS Simulation doesn’t benefit from hyper-threading either.

In summary: For optimum hardware usage, limit the amount of processor cores to a maximum of 8.

Tip: A good rule of thumb when choosing hardware is to choose faster clock speed over quantity of cores!

Another technique you can use to utilize multi-core processors in SOLIDWORKS is to manually assign cores to the SOLIDWORKS process, as seen in the Image below. This can be done through the task manager, located on the ‘Details’ tab as seen in Image 2. Next, right-click on the SLDWRKS.exe and select ‘Set affinity’. This then presents you with a window where the number of cores required can be assigned to that process. After this has been done, ALL of the rest of the processes listed here need to be set accordingly to not use the cores that have been assigned to SOLIDWORKS. This then allows those cores to be solely used by SOLIDWORKS. By default each process will be assigned to all the available cores.

SolidWorks Simulation FEA Multi-Core 2

Image 2 – RMB>Set Affinity

 

SolidWorks Simulation FEA Multi-Core 3

Image 3 – Processor affinity window

We hope you found that useful.


Why not take a look at our blog archive where we have posted plenty of helpful tutorials and technical articles like this one. We also have a huge video library filled with easy-to-follow tutorial videos inspired by real customer enquiries. Don’t forget to follow Innova Systems on twitter for daily bite size SOLIDWORKS tips, tricks and videos!

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Innova Systems Experts in SOLIDWORKS Training & Support
We specialise in the supply, consultancy and training of SOLIDWORKS software. Based in Cambridge we have a central location to service a UK wide customer base. We offer the skills and experience to help you develop new products using SOLIDWORKS - empowering smarter, faster and more cost effective design. We've been recognised by SOLIDWORKS Corporation for providing the highest rated customer support in Northern Europe in 2014, 2015 and 2016. Email: info@innova-systems.co.uk / Telephone: 01223 200690.

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Creating Linked Views in SOLIDWORKS Composer http://blogs.solidworks.com/tech/2017/05/creating-linked-views-in-solidworks-composer.html http://blogs.solidworks.com/tech/2017/05/creating-linked-views-in-solidworks-composer.html#respond Sat, 06 May 2017 15:00:28 +0000 http://blogs.solidworks.com/tech/?p=16681 SOLIDWORKS Composer can enable users to transform 3D CAD data into technical communications that helps customers understand and retain product information effectively. One of Composer’s powerful functions is to “breathe life” into conventional 2D documentation and 3D interactive outputs with

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TMS CADCentre

TMS CADCentre - is a SOLIDWORKS Reseller based in Scotland providing 3D CAD Design Software, analysis software & product data management software. The company was formed in 1981 and now pleased to be celebrating 35 years in business. TMS CADCentre is the only UK SOLIDWORKS Reseller based and funded within Scotland and have been providing SOLIDWORKS software, training and support since 1996 when the product was first launched in the UK.

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SOLIDWORKS Composer can enable users to transform 3D CAD data into technical communications that helps customers understand and retain product information effectively. One of Composer’s powerful functions is to “breathe life” into conventional 2D documentation and 3D interactive outputs with dynamic hyperlinks and user-friendly navigation. By setting up a navigation structure ahead of time, the creation of the interactive content is reduced to a series of simple steps and the result is immediately apparent.

This example below shows the hierarchy of the parts catalog for a component. Each coloured box represents different areas which can be used for a website or an interactive document for example.

To create these links, both collaborative and geometric actor properties are configured to enable links to connect. There is a large variety of link types available in Composer and it is possible to hyperlink any actor to nearly any location, whether it be HTTP, FTP, a file on the network, or any point or portion of an animation in the Composer file.

This table has been compiled to list the available link types and their descriptions:

A common function is linking views throughout a document and this is demonstrated as follows:

Step 1: The relevant view is created (text box optional) and is pre-selected as the initial link

Step 2: In the Properties tab on the left-hand side, go to Event > Link > select the ‘…’ to open the URL options

Step 3: Under URL select view:// – From the drop down select the ‘View’ that is required to link and click OK.

Step 4: To validate the link – it is recommended to come out of the ‘design mode’ environment to simulate a user environment rather than editing the document. By clicking on the linked view, it should automatically switch to the designated view set earlier in steps 2 – 3.

Last step: Once all the links have been set up – an html file can be exported to publish to a website or alternatively, it can be used as an interactive assembly instruction guide in a workshop. The completed document can now be seamlessly navigated with ease.

Whether you’re new to SOLIDWORKS or a seasoned Composer user, I hope you’ve found this overview useful.


Andrew Tsim is an Applications Engineer at TMS CADCentre, a SOLIDWORKS Value Added Reseller in Scotland.  You can read more from Andrew on the TMS CADCentre blog

Author information

TMS CADCentre
TMS CADCentre - is a SOLIDWORKS Reseller based in Scotland providing 3D CAD Design Software, analysis software & product data management software. The company was formed in 1981 and now pleased to be celebrating 35 years in business. TMS CADCentre is the only UK SOLIDWORKS Reseller based and funded within Scotland and have been providing SOLIDWORKS software, training and support since 1996 when the product was first launched in the UK.

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SOLIDWORKS Lindbergh’s Spirit of St. Louis Tutorial – Part 3 http://blogs.solidworks.com/tech/2017/05/solidworks-lindberghs-spirit-of-st-louis-tutorial-part-3.html http://blogs.solidworks.com/tech/2017/05/solidworks-lindberghs-spirit-of-st-louis-tutorial-part-3.html#respond Fri, 05 May 2017 21:00:10 +0000 http://blogs.solidworks.com/tech/?p=15497 On May 20th and 21st, 1927 Charles Lindbergh, aka “Lucky Lindy”, made history by completing the first solo, nonstop, transatlantic flight; piloting his monoplane, the Spirit of St. Louis, from Long Island, New York to Paris, France. To celebrate the

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SOLIDWORKS

Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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On May 20th and 21st, 1927 Charles Lindbergh, aka “Lucky Lindy”, made history by completing the first solo, nonstop, transatlantic flight; piloting his monoplane, the Spirit of St. Louis, from Long Island, New York to Paris, France. To celebrate the anniversary of Lindy’s achievement we’re showing SOLIDWORKS users how to model a 30” wingspan version of his iconic aircraft. Throughout this series, we’ll fly through lessons on how to work off imported images, and we’ll use a series of extrusions, lofts, and sweeps to model the Spirit of St. Louis.

Welcome back to our 5-part series where we are celebrating the anniversary of Charles Lindbergh’s historic solo transatlantic flight by modeling his iconic Spirit of St. Louis monoplane. In part 3 of the series we are going to hollow out a portion of the fuselage using the shell tool, and we will run through a mix of essential and advanced functions to model the wing, horizontal stabilizer, and vertical stabilizer. You will walk away from this part of the series with knowledge of the Split command and Boundary command functionality.

Whether you’re an aviation enthusiast or are just looking for a new SOLIDWORKS challenge, the Lindbergh’s Spirit of St. Louis tutorial series is for you!

Can’t wait to watch the next video? View all of the tutorials on the playlist here.

Author information

SOLIDWORKS
Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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Good Vibrations: Reverse Engineering A Vintage Turntable Foot http://blogs.solidworks.com/tech/2017/05/good-vibrations-reverse-engineering-vintage-turntable-foot.html http://blogs.solidworks.com/tech/2017/05/good-vibrations-reverse-engineering-vintage-turntable-foot.html#comments Wed, 03 May 2017 15:00:11 +0000 http://blogs.solidworks.com/tech/?p=16622 Most audiophiles say that there is something warmer, richer, and better to the sound a vinyl record reproduces, especially compared to modern digital media. Not having listened to an album since I was young, I figured it was time to

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3DVision Technologies

Founded in 1995 in Cincinnati, Ohio 3DVision Technologies Corp. has enjoyed over 18 years of success as one of the finest SolidWorks providers in the Great Lakes Region. 3DVision Technologies is a team of experienced mechanical engineers that support the visions of engineers globally. With solutions for the design and manufacturing industries including 3D solid-modeling, computer aided analysis, product data management and 3D Printers our products solve engineers' most important product development goals: higher quality products, less time to market, lower development costs, better design communication, collaboration and review.

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Most audiophiles say that there is something warmer, richer, and better to the sound a vinyl record reproduces, especially compared to modern digital media. Not having listened to an album since I was young, I figured it was time to see what all the talk was about. I asked my father (long time high-end audio enthusiast) to get out his vintage 1973 JVC VL-5 turntable so we could give it a listen.

Note: This picture is post installation of the new feet.

After all these years in storage the turntable was in great shape.  Everything worked perfectly except for the vibration isolating rubber feet.  Out of the four feet, three had the material break down, leaving them brittle and cracking with large sections missing or crumbling. Obviously this was not good news as the turntable needs to sit level when in use.

I searched the internet for replacements but could not find any that were suitable.  The next step was to make our own.  Using SOLIDWORKS, my father reverse engineered a new set of feet for the turntable. After a few design iterations, the new feet were a little more stout than the originals. Thanks to SOLIDWORKS SImulation, the new feet exhibited the mechanical properties we desired.

We did not know the type of rubber used in the original foot.  This was not a problem as we used Simulation Premium and the Nonlinear material models to determine a relative stiffness.  By physically testing the original foot under a 2.5 lb. vertical load we measured a 0.1 in. displacement. Using Simulation and varying the material properties we found that a Shore Value of 70, gave a 0.095 in.corresponding vertical displacement.  Feeling confident in the design the next step was to test for vibrational characteristics.

The turntable operates at 33 1/3, and 45 RPM.  This equates to 0.556, and 0.75 Hz respectively.  SOLIDWORKS Simulation Professional made it possible to test the resonant frequency of the design.  The analysis results predicted the lowest resonant frequency at 16.32 Hz. This is well above the induced vibration due to the turning motor and drive mechanism, and lower than the 20,000-20 Hz most receivers output.

Next I turned to the Stratasys Polyjet line of printers that delivered an amazing print. The Polyjet printed a 70 Shore value model that behaved just like we expected. Not only did the print physically work, it looked great too.

reverse engineering

When you have access to SOLIDWORKS, Simulation, and Stratsys Printers no old turntable should be retired!


Robert Warren is a SOLIDWORKS Elite Application Engineer, Certified SOLIDWORKS Expert, and CAE Specialist at 3DVision Technologies, a SOLIDWORKS Value Added Reseller with locations throughout Ohio, Kentucky, and Indiana. He is a regular contributor to the 3DVision Blog.

Author information

3DVision Technologies
Founded in 1995 in Cincinnati, Ohio 3DVision Technologies Corp. has enjoyed over 18 years of success as one of the finest SolidWorks providers in the Great Lakes Region. 3DVision Technologies is a team of experienced mechanical engineers that support the visions of engineers globally. With solutions for the design and manufacturing industries including 3D solid-modeling, computer aided analysis, product data management and 3D Printers our products solve engineers' most important product development goals: higher quality products, less time to market, lower development costs, better design communication, collaboration and review.

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SOLIDWORKS Tech Tip: 3D Drawing View Mode http://blogs.solidworks.com/tech/2017/05/solidworks-tech-tip-3d-drawing-view-mode.html http://blogs.solidworks.com/tech/2017/05/solidworks-tech-tip-3d-drawing-view-mode.html#respond Tue, 02 May 2017 21:00:17 +0000 http://blogs.solidworks.com/tech/?p=16654 Creating and presenting drawings for parts and assemblies is an important step in any design process. In some cases, it may be made difficult to see specific areas of the model in that drawing view. This typically results from the

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SOLIDWORKS

Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

The post SOLIDWORKS Tech Tip: 3D Drawing View Mode appeared first on SOLIDWORKS Tech Blog.

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Creating and presenting drawings for parts and assemblies is an important step in any design process. In some cases, it may be made difficult to see specific areas of the model in that drawing view. This typically results from the model geometry getting in the way of seeing certain features based on the view angle. In any case, this problem can be easily solved using the 3D Drawing View mode. This mode allows you to rotate the drawing views out of their standard viewing plane in order to adjust the angle and view the area you’re looking for. Check out the SOLIDWORKS Tech Tip below to learn more!

 

Want to see more SOLIDWORKS Tech Tips? Check out our playlist on YouTube to catch up on past videos or you can even jump ahead to the next video!

Do you have a suggestion for the next Tech Tip? Tell us in the comments; we’d love to hear your ideas!

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SOLIDWORKS
Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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SOLIDWORKS Visualize Service Pack 2 is Here! http://blogs.solidworks.com/tech/2017/05/solidworks-visualize-service-pack-2.html http://blogs.solidworks.com/tech/2017/05/solidworks-visualize-service-pack-2.html#respond Mon, 01 May 2017 15:00:48 +0000 http://blogs.solidworks.com/tech/?p=16565 SOLIDWORKS Visualize is the fastest, most accurate and easiest to use rendering tool in the world. If SOLIDWORKS made rendering tools… oh wait we do! When SOLIDWORKS Visualize was brought out just over a year ago, we were amazed by how it took

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Solid Solutions Technical Team

Solid Solutions commenced business as a SolidWorks Training and SolidWorks Support provider in 1998 and has consistently achieved strong growth year-on-year to become the UK’s leading SolidWorks 3D CAD reseller. Growth has been completely organic and has been consistently driven by a focus on recruiting the best from academia and industry and by delivering high quality services to more than 4,000 customers.

Our customers range widely in size and are drawn from a broad spectrum of industry sectors. SolidWorks software is used by over 2 million engineers and designers across the world. As a company we are dedicated and focused at providing first class training and support to help you realise the best return on your investment.

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SOLIDWORKS Visualize is the fastest, most accurate and easiest to use rendering tool in the world.

If SOLIDWORKS made rendering tools… oh wait we do! When SOLIDWORKS Visualize was brought out just over a year ago, we were amazed by how it took the quality of our photorealistic images to a whole new level with very little effort.SOLIDWORKS Visualize Headphones

However for many images we were reaching for “Accurate” mode which while it does what it says on the tin in achieving amazing results it could take a bit longer to churn out those stunning images. Now almost like a birthday present to celebrate 1 Year of Visualize, we have the new improved “Fast Mode” in SOLIDWORKS Visualize 2017 SP2 in March.

This is now suited to most situations/ products, even those with lots of transparent appearances, scenes where light must bend and bounce to give a better representation of the product.

I’m going to let the results do the rest of the talking from here. All renders done at 1920×1080 using GPU mode on Dell Precision 7710 Laptop with NVIDIA Quadro M3000M

Example 1 – Engineering Product

Fast Mode – 2017 SP1 and Previous Versions

SOLIDWORKS Visualize

Render Time – 32 Seconds

Fast Mode – Quality 2017 SP2 Onwards

SOLIDWORKS Visualize

Now the main difference between Fast mode and Accurate is the light from the LEDs on the handle do not reflect off other objects. In fast mode emissive (light appearances) do not contribute light to the scene but will glow realistically.

Render Time – 26 Seconds

Accurate Mode – 1000 Passes

SOLIDWORKS Visualize

Render Time – 3 Mins 25 Seconds

Again, spot the difference vs Fast mode, the main difference being the lights, this could be compensated for in Visualize Professional using the Bloom post processing filter to blur the bright areas.

2017 SP2 Fast Mode – Speed

We even have a new option for “Speed” mode within options which makes “Fast” mode even quicker, albeit with some compromises

SOLIDWORKS Visualize - Click to Englarge

Render Time – 12 Seconds

Even this produces a passable result in a mere 12 seconds albeit with some additional shadowing that isn’t true to life.

SOLIDWORKS Visualize

Example 2 – Products with multiple transparent parts

Fast Mode – 2017 SP1 and Previous Versions

SOLIDWORKS Visualize

Render Time – 52 Seconds

Note the dark areas where light is not bending  to travel through the casing,

Fast Mode – 2017 SP2 Onwards

SOLIDWORKS Visualize

Some improvement over Fast quality however if you weren’t looking for the differences you may not spot them

Accurate Mode – 1000 Passes

SOLIDWORKS Visualize

Fast Mode – Speed 2017 SP2 Onwards

SOLIDWORKS Visualize

Clearly this new mode isn’t suited to complex items with lots of transparency the compromises in the bends and bounces of light mean this object isn’t lit correctly.

SOLIDWORKS Visualize

Example 3 – Product Design Render

Here is where you will see least difference, hard bodied plastic/painted and many metal products were just fine with Fast mode already. So I’ve chosen some a model with emissive appearances and reflective floors I know will show differences.

Fast Mode – Versions 2017 SP1 and Prior Versions

SOLIDWORKS Visualize

Render time – 60 Seconds

Fast Mode – Quality 2017 SP2 Onwards

SOLIDWORKS Visualize

Render Time – 55 Seconds

Accurate Mode – 1000 Passes

SOLIDWORKS Visualize

Render Time – 4 Mins 23 Seconds

Note how we get the LED emissive appearance bouncing off other objects giving a much more realistic effect and a better blurry reflection on the floor.

Fast Mode – Speed 2017 SP2 Onwards

SOLIDWORKS Visualize

Render Time – 23 Seconds

SOLIDWORKS Visualize

Example 4 – Interior Scene

Fast Mode – 2017 SP1 and Previous Versions

SOLIDWORKS Visualize

Render Time – 39 Seconds

Fast Mode – Quality 2017 SP2 Onwards

SOLIDWORKS Visualize

Render Time – 54 Seconds

Fast Mode – Speed 2017 SP2 onwards

SOLIDWORKS Visualize

Render Time – 25 Seconds

Clearly this is a less realistic representation however it is nice and bright, just lacking shadows and details to make things seem realistic. However could be useful for live presentations and when quick representations are required

Accurate Mode – 2000 Passes (interiors typically require 2000-5000 passes to reduce noise)

SOLIDWORKS Visualize

Render Time – 31 Mins 20 Seconds

SOLIDWORKS Visualize

Now clearly accurate mode still has its place for certain situations, such as interiors however now the results from fast mode are much improved these suit the vast majority of products especially when quick results are required, this is likely to only improve over time.

Other additions to 2017 SP2 include faster viewport interactions so your zooming, panning and rotating will be much smoother and improvements to the update system so that if a SOLIDWORKS model is updated SOLIDWORKS Visualize will prompt you the next time you open the file to see if your wish to update your Visualize Project also.

Alan Sweetenham
Elite Applications Engineer

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Solid Solutions Technical Team
Solid Solutions commenced business as a SolidWorks Training and SolidWorks Support provider in 1998 and has consistently achieved strong growth year-on-year to become the UK’s leading SolidWorks 3D CAD reseller. Growth has been completely organic and has been consistently driven by a focus on recruiting the best from academia and industry and by delivering high quality services to more than 4,000 customers. Our customers range widely in size and are drawn from a broad spectrum of industry sectors. SolidWorks software is used by over 2 million engineers and designers across the world. As a company we are dedicated and focused at providing first class training and support to help you realise the best return on your investment.

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SOLIDWORKS Lindbergh’s Spirit of St. Louis Tutorial – Part 2 http://blogs.solidworks.com/tech/2017/04/solidworks-lindberghs-spirit-of-st-louis-tutorial-part-2.html http://blogs.solidworks.com/tech/2017/04/solidworks-lindberghs-spirit-of-st-louis-tutorial-part-2.html#respond Fri, 28 Apr 2017 21:00:39 +0000 http://blogs.solidworks.com/tech/?p=15493 On May 20th and 21st, 1927 Charles Lindbergh, aka “Lucky Lindy”, made history by completing the first solo, nonstop, transatlantic flight; piloting his monoplane, the Spirit of St. Louis, from Long Island, New York to Paris, France. To celebrate the

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SOLIDWORKS

Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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On May 20th and 21st, 1927 Charles Lindbergh, aka “Lucky Lindy”, made history by completing the first solo, nonstop, transatlantic flight; piloting his monoplane, the Spirit of St. Louis, from Long Island, New York to Paris, France. To celebrate the anniversary of Lindy’s achievement we’re showing SOLIDWORKS users how to model a 30” wingspan version of his iconic aircraft. Throughout this series, we’ll fly through lessons on how to work off imported images, and we’ll use a series of extrusions, lofts, and sweeps to model the Spirit of St. Louis.

Welcome to part 2 of our series where we are modeling Lucky Lindy’s Spirit of St. Louis monoplane using a series of imported images to model around.  We left off in part 1 of the series with all our reference images imported including 3 main views and a few of the bulkhead shapes.  We also have our main side view outline sketched.  In part 2 of the series we will sketch in our various bulkhead profile shapes and guide curves to build the fuselage using a series of Lofts.

Whether you’re an aviation enthusiast or are just looking for a new SOLIDWORKS challenge, the Lindbergh’s Spirit of St. Louis tutorial series is for you!

Can’t wait to watch the next video? View all of the tutorials on the playlist here.

Author information

SOLIDWORKS
Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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Make It Move with SOLIDWORKS Part 3 – Motion Simulation http://blogs.solidworks.com/tech/2017/04/make-move-solidworks-part-3-motion-simulation.html http://blogs.solidworks.com/tech/2017/04/make-move-solidworks-part-3-motion-simulation.html#respond Thu, 27 Apr 2017 15:00:44 +0000 http://blogs.solidworks.com/tech/?p=16591 This is the final installment of the Make It Move with SOLIDWORKS series where we cover the last technique for making things move, Motion Simulation. Motion Simulation is the most powerful and detailed method of making your designs move in

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TPM

TPM, Inc. is the Carolina’s largest 3D CAD provider and a leading technology company proud of its reputation of providing cutting-edge solutions to the engineering and design community for the past 40 years. Founded in 1973, TPM Inc. serves more than 3,000 customers across the Southeast each year. Inspired by our founder, Jerry Cooper, we are committed to offering our clients the best: 3D Design Software, 3D Printing and Scanning Options, Data and Document Management Solutions, Large-Format Graphics, Wide-Format Plotters and Office Equipment, and Reprographics.

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This is the final installment of the Make It Move with SOLIDWORKS series where we cover the last technique for making things move, Motion Simulation. Motion Simulation is the most powerful and detailed method of making your designs move in SOLIDWORKS because you can simulate gravity, friction, and forces while getting useful outputs such as motor torque curves, motion profiles, sensors, and several other unique capabilities.

 

In this video, I use the same robot from FIRST Robotics Team 3506 YETI to fire a foam projectile into a target given a constant release angle, distance to the target, constant height of the target, and weight of the projectile.

You have all probably seen these equations before:

Kinematic motion is easy to calculate with enough time and patience to do it over and over for different angles of release and distances to the target but who has that kind of time?  I want to simply fire a ball and see if the robot scores or not and I want to know what speed to run the flywheels to get the ball to the goal at a given distance.  If the robot gets closer or farther from the target I can adjust the flywheel speed to score the perfect shot every time.  It sounds like a pain but it is actually pretty easy in SOLIDWORKS.  Just model the goal, the ground, and where you want the ball to start (in my case the exit point of the robot), give it a nice robot powered kick, and let gravity take over.  This technique should make that trebuchet in your back yard shoot farther than ever.  Wait, you don’t have one of those?

Since this is the last installment (or is it?) of the Make It Move with SOLIDWORKS series leave us some comments on the YouTube video posted below to see more content like this and check out our other installments on the TPM Solutions YouTube channel under our Three Minute Thursdays!


By: Robbie Hoyler • SOLIDWORKS Application Engineer • TPM

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TPM
TPM, Inc. is the Carolina’s largest 3D CAD provider and a leading technology company proud of its reputation of providing cutting-edge solutions to the engineering and design community for the past 40 years. Founded in 1973, TPM Inc. serves more than 3,000 customers across the Southeast each year. Inspired by our founder, Jerry Cooper, we are committed to offering our clients the best: 3D Design Software, 3D Printing and Scanning Options, Data and Document Management Solutions, Large-Format Graphics, Wide-Format Plotters and Office Equipment, and Reprographics.

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SOLIDWORKS Flow Simulation – Ski Jumping http://blogs.solidworks.com/tech/2017/04/solidworks-flow-simulation-ski-jumping.html http://blogs.solidworks.com/tech/2017/04/solidworks-flow-simulation-ski-jumping.html#comments Wed, 26 Apr 2017 15:00:16 +0000 http://blogs.solidworks.com/tech/?p=16570 Let’s find out the optimal forward lean angle for a Ski jumper in SOLIDWORKS Flow Simulation to help him get the longest jump in his life! In this article we will try to determine the value of a lift force

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SOLIDEXPERT

SOLIDEXPERT is an Authorised SOLIDWORKS Reseller in Poland that was established in 2002 in Cracow. During this time the company put much pressure on technical skills of it’s team. This help to build a good connection between SOLIDEXPERT and Customers, trust and confidence in the support and consulting that provides.

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Let’s find out the optimal forward lean angle for a Ski jumper in SOLIDWORKS Flow Simulation to help him get the longest jump in his life!

In this article we will try to determine the value of a lift force as a function of a forward lean angle (FLA) of Ski jumper. To find this characteristic, we tested four different body position. The body position in our studies are shown in the figures below:

   
Fig. 1a. Body position at forward lean angle equal to 20° Fig. 1b. Body position at forward lean angle equal to 30°
   
Fig. 1c. Body position at forward lean angle equal to 40° Fig. 1d. Body position at forward lean angle equal to 60°

 

Definition of case study

In the first step we will try to estimate the real velocity of ski jumper which depends on the forward lean angle. The most important is to find the drag force for each case. To do this, we define two goals: drag force and lift force on surface of a ski jumper’s body.

For all cases, we assume that horizontal velocity component of a Ski jumper is equal to 100 km/h.

After doing the necessary calculations, we know the value of Drag force for velocity of 100 km/h for each FLA. By including decreased velocity and increasing Drag force, the following equation will determine real velocity for Ski jumper:

Table 1. Estimated real velocity for Ski jumper assuming influence of a drag force

 

FLA

[°]

Velocity

[km/h]

Drag force

[N]

Real velocity

[km/h]

20 100 61.86 100.00
30 100 85.98 71.95
40 100 126.23 49.00
60 100 257.76 24.00

 

Results

Below we can observe the distribution of aerodynamic drag coefficient as a function of FLA:

   
Fig. 2a. Distribution of aerodynamic drag coefficient
(FLA of 20°)
Fig. 2b. Distribution of aerodynamic drag coefficient
(FLA of 30°)
   
Fig. 2c. Distribution of aerodynamic drag coefficient
(FLA of 40°)
Fig. 2d. Distribution of aerodynamic drag coefficient
(FLA of 60°)

 

In the first case, the biggest aerodynamic resistance appears on surface of head (fig. 2a). This resistance increases together with the increase of FLA and moves towards chest and shoulders (fig. 2b), forearms and abdomen (fig. 2c), to finally cover all front area of a ski jumper’s body (fig. 2d).

Figures 3. show the streamlines that are passing the ski jumper. For a low value of forward lean angle, we can observe a laminar flow. For a high value of forward lean angle, the airflow is separating.

   
Fig. 3a. Streamline flow passing a ski jumper
(FLA of 20°)
Fig. 3b. Streamline flow passing a ski jumper
(FLA of 30°)
   
Fig. 3c. Streamline flow passing a ski jumper
(FLA of 40°)
Fig. 3d. Streamline flow passing a ski jumper
(FLA of 60°)

 

Based on the simulation results, we can draw a graph that represents the lift force as a function of forward lean angle:

Fig. 4. Lift force as a function of forward lean angle

Conclusions

SOLIDWORKS Flow Simulation is very useful in getting the optimal parameters of body position to achieve better results in Ski jumping. It surely can be used as a supporting tool for athletes.

Thanks for all Guys from SOLIDEXPERT ~The Winner

Author:
Mateusz SZTANGRET
SOLIDWORKS and SOLIDWORKS Simulation Specialist at SOLIDEXPERT

Author information

SOLIDEXPERT
SOLIDEXPERT is an Authorised SOLIDWORKS Reseller in Poland that was established in 2002 in Cracow. During this time the company put much pressure on technical skills of it’s team. This help to build a good connection between SOLIDEXPERT and Customers, trust and confidence in the support and consulting that provides.

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SOLIDWORKS Lindbergh’s Spirit of St. Louis Tutorial – Part 1 http://blogs.solidworks.com/tech/2017/04/solidworks-lindberghs-spirit-of-st-louis-part-1.html http://blogs.solidworks.com/tech/2017/04/solidworks-lindberghs-spirit-of-st-louis-part-1.html#respond Fri, 21 Apr 2017 21:00:31 +0000 http://blogs.solidworks.com/tech/?p=15490 On May 20th and 21st, 1927 Charles Lindbergh, aka “Lucky Lindy”, made history by completing the first solo, nonstop, transatlantic flight; piloting his monoplane, the Spirit of St. Louis, from Long Island, New York to Paris, France. To celebrate the

Author information

SOLIDWORKS

Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

The post SOLIDWORKS Lindbergh’s Spirit of St. Louis Tutorial – Part 1 appeared first on SOLIDWORKS Tech Blog.

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On May 20th and 21st, 1927 Charles Lindbergh, aka “Lucky Lindy”, made history by completing the first solo, nonstop, transatlantic flight; piloting his monoplane, the Spirit of St. Louis, from Long Island, New York to Paris, France. To celebrate the anniversary of Lindy’s achievement we’re showing SOLIDWORKS users how to model a 30” wingspan version of his iconic aircraft. Throughout this series, we’ll fly through lessons on how to work off imported images, and we’ll use a series of extrusions, lofts, and sweeps to model the Spirit of St. Louis.

In part 1 of this series we’ll start importing and laying out several downloaded images to model around.  Keep this technique in mind when modeling any vehicle, be it an aircraft, boat, or car.

Whether you’re an aviation enthusiast or are just looking for a new SOLIDWORKS challenge, the Lindbergh’s Spirit of St. Louis tutorial series is for you!

Can’t wait to watch the next video? View all of the tutorials on the playlist here.

Author information

SOLIDWORKS
Dassault Systèmes SolidWorks Corp. offers complete 3D software tools that let you create, simulate, publish, and manage your data. SolidWorks products are easy to learn and use, and work together to help you design products better, faster, and more cost-effectively. The SolidWorks focus on ease-of-use allows more engineers, designers and other technology professionals than ever before to take advantage of 3D in bringing their designs to life.

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3D Interconnect – Say Adiós, Au Revoir and Goodbye to inter-CAD language barriers! http://blogs.solidworks.com/tech/2017/04/3d-interconnect-say-adios-au-revoir-and-goodbye-to-inter-cad-language-barriers.html http://blogs.solidworks.com/tech/2017/04/3d-interconnect-say-adios-au-revoir-and-goodbye-to-inter-cad-language-barriers.html#respond Fri, 21 Apr 2017 15:00:27 +0000 http://blogs.solidworks.com/tech/?p=16550 In this blog we are going to explore the bi-lingual capabilities of SOLIDWORKS 2017 through the powerful 3D Interconnect functionality. But first, let’s be clear about what we are talking about here, a quick google definition will help. “A device

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TMS CADCentre

TMS CADCentre - is a SOLIDWORKS Reseller based in Scotland providing 3D CAD Design Software, analysis software & product data management software. The company was formed in 1981 and now pleased to be celebrating 35 years in business. TMS CADCentre is the only UK SOLIDWORKS Reseller based and funded within Scotland and have been providing SOLIDWORKS software, training and support since 1996 when the product was first launched in the UK.

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In this blog we are going to explore the bi-lingual capabilities of SOLIDWORKS 2017 through the powerful 3D Interconnect functionality. But first, let’s be clear about what we are talking about here, a quick google definition will help. “A device used to connect two things together” that’s exactly what SOLIDWORKS 3D interconnect makes possible! The connecting of two completely different CAD packages!

Since the launch of SOLIDWORKS 2017 I can only imagine that international use of the word interconnect will have increased exponentially, considering the impact that 3D Interconnect has had on the world of inter-CAD collaboration. You’ll notice my predictive modification of the ‘Use over time chart’ to reflect my expectations.

The cool thing is that 3D Interconnect does not translate the proprietary data of other CAD systems into a language that SOLIDWORKS can understand, No! SOLIDWORKS 2017 is a computer aided polyglot! and already understands the languages of PTC® Creo®, Autodesk® Inventor®, Siemens® NX, SolidEdge®, and CATIA®
With SOLIDWORKS 2017 we can open proprietary CAD files right into SOLIDWORKS and treat them like native components without conversion or translation. What’s more! 3D interconnect can maintain or break the link to the original proprietary CAD file.

This means that changes made to the proprietary file when linked will associatively update directly within SOLIDWORKS and all downstream features will be maintained. If associativity is to be avoided then the link is easily broken.

You can turn on and turn off the 3D Interconnect functionality in the SOLIDWORKS software. It is turned on by default.
To turn 3D Interconnect on or off:

Click Tools > Options > System Options > Import.
In the dialog box, set File Format to Inventor/Catia V5/Creo/NX/Solid Edge.
Select or clear Enable 3D Interconnect.
Click OK.

3d interconnect

To quickly give an example of 3D interconnect in action, we have taken an Autodesk® Inventor® file and placed it into an existing SOLIDWORKS assembly. With 3D interconnect this operation is as simple as using the insert component tool within the open SOLIDWORKS assembly and browsing for the Inventor Assembly file extension. Once the file has been selected we can place it just like a regular SOLIDWORKS assembly file and mate it into position. The entire assembly structure from Inventor® will also come through and is visible in the feature tree.

If a design change is made to the Inventor® file and sent to us then it is a straightforward process to update that file within SOLIDWORKS. The newly updated design can be updated by overwriting the existing file location of the old design with the new files we received and the 3D interconnect ‘update’ function can be used within SOLIDWORKS. SOLIDWORKS will detect the new file we have pasted into our original file location and the update option will become available.

The update function is as simple as a right clicking the Inventor® assembly in the feature tree and selecting the update model option. The assembly file will then update and an in-context relationships and mates defined with the previous assembly file will all update seamlessly.

And that’s it! The process is so simple but extremely powerful. 3D interconnect is just one of the ways that SOLIDWORKS are providing solutions which make the day to day realities of inter-CAD collaboration that little bit more enjoyable.


Lewis Harvey is a Certified SOLIDWORKS Expert  and Applications Engineer at TMS CADCentre, a SOLIDWORKS Value Added Reseller in Scotland.  You can read more from Andrew on the TMS CADCentre blog

Author information

TMS CADCentre
TMS CADCentre - is a SOLIDWORKS Reseller based in Scotland providing 3D CAD Design Software, analysis software & product data management software. The company was formed in 1981 and now pleased to be celebrating 35 years in business. TMS CADCentre is the only UK SOLIDWORKS Reseller based and funded within Scotland and have been providing SOLIDWORKS software, training and support since 1996 when the product was first launched in the UK.

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15 Quick Steps to Setup a Design Library Feature http://blogs.solidworks.com/tech/2017/04/15-quick-steps-setup-design-library-feature.html http://blogs.solidworks.com/tech/2017/04/15-quick-steps-setup-design-library-feature.html#respond Thu, 20 Apr 2017 15:00:00 +0000 http://blogs.solidworks.com/tech/?p=16402 Are you finding yourself generating the same feature every time you create a new part? Would you like an easy way to stamp your company logo into your products? Then the SOLIDWORKS Library Feature is meant for you! Library features allow

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Alignex, Inc.

Alignex, Inc. is the premier provider of SOLIDWORKS software and partner products to the mechanical engineering industry in Minnesota, Wisconsin, Iowa, North Dakota, South Dakota, Colorado and Wyoming. With more than 25 years of technical experience, Alignex offers consulting services, training and support for SOLIDWORKS as well as support for partner products. For more information, visit alignex.com.

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Are you finding yourself generating the same feature every time you create a new part? Would you like an easy way to stamp your company logo into your products? Then the SOLIDWORKS Library Feature is meant for you!

Library features allow you easy access to commonly used features with all of the parameters and dimensions pre-defined to your specifications. Simply drag and drop onto your model and SOLIDWORKS takes care of the rest.

_Intro.gif

Let’s take a look at how this is done.

Before we get started, you’ll first want to create a custom Design Library directory to save everything into, whether on your personal hard drive or on a server to share with colleagues. You will reference this location in your settings [Tools > Options > File Locations > Design Library].

add-design-library.jpg

Now when you go to the Design Library tab in the Task Pane you will find a folder to the directory you linked. Right click on this and create a new folder.

2-Add-Folder-web.jpg

With the folder structure in place you are now ready to create your library feature.

Step 1: Create a Place Holder Extrusion

Begin by creating a place holder extrusion, similar to the geometry you plan on inserting this library feature onto. In this particular example I commonly create a vent sketch on rectangular faces so I will use this type of shape as my place holder.

3-Beginning-Shape-web.jpg

Step 2: Sketch the Geometry

Sketch the geometry you will be using with the library feature. As you create the sketch you should avoid creating relations tied to the origin of this place holder model, otherwise SOLIDWORKS will attempt to use this as a Reference when re-using the feature. You can either sketch off to the side or as you sketch hold the CTRL key on your keyboard to avoid creating a coincident relation to the origin.

4-Origin-No-Yes-zoomed.jpg

Step 3: Define Sizes of Sketch Entities

Next, fully define the sizes of your sketch entities if necessary. You want to make special considerations for the dimensions or relations controlling the geometry’s position in space. These References will be used when we turn this into a library feature in a few steps.

Because I typically dimension my vent off of edges of rectangular faces I will dimension the center position of my vent with this in mind. Note that even though the center is on top of the origin there is no coincident relation to it. As an alternative option if you would prefer to drop the feature onto any geometry regardless of its edge conditions you should not use these locating dimensions/relations and should instead leave the sketch under-defined. I often leave my sketch under-defined when creating a logo as shown in the final step of this article.

4-5-sketch-offset-locating-dimensions.jpg

Step 4: Create Features for Library Feature

From here you can create your cut or boss/base feature and any additional features you would like to incorporate into the library feature. You do not need to limit yourself to one sketch or one feature. How far you go is up to you. In my example the sketch is all I need.

Step 5: Drag Feature(s) into Folder within Design Library

When ready you will left click on the feature(s) to be used and drag them into the folder within your Design Library. In this step you do not want to include your place holder feature(s).

7-drag-and-drop-to-add.jpg

Step 6: Define Design Library Saving Preferences

The “Add to Library” PropertyManager should appear on the left allowing you to define what, where, and how you want to save into your Design Library. If you missed any features you can still add them to the list. For the File Type dropdown you will choose “Lib Feat Part (.sldlfp)”.

8-Add-To-Library-Property-Manager.jpg

Step 7: Open Library Feature Part

Once complete you will see the Library Feature Part in your Design Library. Save your original model if you wish, but you will want to close the original file and then open the Library Feature Part by double clicking it. You will notice there are some unique folders in the feature tree and all of the library features will have an “L” over their icons.

8-9-Open-Library-Part-Feature.jpg

Step 8: Add Additional Features to Library Feature Part (Optional)

If you wish to add additional features to the Library Feature Part you can always right click on them in the tree and choose “Add to Library”. An “L” should appear over the feature’s icon.

Step 9: Move Dimensions into Locating Dimensions Folder

If you want an easy way to modify the Locating Dimensions when you use this library feature in a new part you will want to move the appropriate dimensions into the Locating Dimensions folder. These will be used later in step #13. The Internal Dimensions folder is further explained in step #14.

10-Move-Locating-Dimensions-web.jpg

Step 10: Drag and Drop from Design Library to Model

Save the changes and close the Library Feature Part. You are now ready to use your library feature in a new model. Simply drag and drop from the Design Library onto your model.

11-Inserting-Feature-Into-New-Part-web.jpg

Step 11: Define Face/Plane to Place Feature Onto

The Property Manager that appears will allow you to further define which face/plane you wish to place the feature onto. If the library feature has configurations you can choose it from the list. There is also a Link to library part option which will cause the feature to update in the future if the Library Feature Part is ever changed.

11-Configurations-and-Link-To-Part-web.jpg

Step 12: Select the New Edge to be Referenced in New Model

The References will list the geometries you used for positioning purposes (from step #3). Select each item and a small window will appear showing the original model. Within this model it will highlight the original edge referenced by the first dimension/relation. Within your new model you will need to select the new edge to be referenced. In my example I dimensioned to the edges of the rectangular face to control the vent position so I need to select the appropriate edges in my new model. If there were no references used in the original part there will be nothing listed here.

selecting-references-in-new-part.jpg

Step 13: Adjust Dimensions Further in ‘Locating Dimensions’ Folder

Because I placed dimensions into the ‘Locating Dimensions’ folder within the Library Feature Part (step #9) I can easily adjust them to further control the position of my feature.

13-Using-Licating-Dimensions-web.jpg

Step 14: Add Dimensions NOT to be Changed to ‘Internal Dimensions’ Folder

Under ‘Size Dimensions’ you can check the box to override the original dimension values. If there are any dimensions you do not want the ability to change you will want to add them to the “Internal Dimensions” folder referenced in step #9.

14-Overriding-Dimensions-web.jpg

Step 15: Confirm to Add Library Folder into FeatureTree

After you confirm the options you will see a Library Folder added into your FeatureTree. Within this folder will be the library features.

15-feature-tree-web.jpg

In my example only the sketch carried over but you can see in the example below we can incorporate as many features as we want when creating these Library Feature Parts. For additional examples to spark ideas on how you could apply this tool I would encourage you to look at the samples in the default Design Library which comes pre-installed with SOLIDWORKS. They are found within the ‘Features’ folder.

16-use-cases-web.jpg

You will notice above I created a Library Feature for the Alignex logo. If you wish to create your company logo in SOLIDWORKS you can find out how in our Smooth Sketching Using Splines in the SOLIDWORKS Sketcher article. Thanks for reading!


Written By: Jesse Butwinick, Application Engineer at Alignex, Inc. Jesse is a regular contributor to the Alignex Blog. Find more tech tips on the Alignex Blog and subscribe to get content like this delivered straight to your inbox.

Author information

Alignex, Inc.
Alignex, Inc. is the premier provider of SOLIDWORKS software and partner products to the mechanical engineering industry in Minnesota, Wisconsin, Iowa, North Dakota, South Dakota, Colorado and Wyoming. With more than 25 years of technical experience, Alignex offers consulting services, training and support for SOLIDWORKS as well as support for partner products. For more information, visit alignex.com.

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SOLIDWORKS: Bring Your Drawings to Life! http://blogs.solidworks.com/tech/2017/04/solidworks-bring-drawings-life.html http://blogs.solidworks.com/tech/2017/04/solidworks-bring-drawings-life.html#respond Tue, 18 Apr 2017 15:05:32 +0000 http://blogs.solidworks.com/tech/?p=16548 It’s easy to understand the range of motion of an assembly when you’re working with a 3D model. But how can one communicate this effectively in a 2D drawing environment? Well, the Alternate Position View makes quick work of this

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Hawk Ridge Systems

From design to production, Hawk Ridge Systems delivers best-in-class solutions in 3D design, CAM software, and 3D printing.

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It’s easy to understand the range of motion of an assembly when you’re working with a 3D model. But how can one communicate this effectively in a 2D drawing environment? Well, the Alternate Position View makes quick work of this by allowing you to indicate the range of motion of assembly components by showing them in different positions.

It utilizes configurations of your model to overlay one or more views on top of the original using phantom lines. You can either have these configurations created before inserting the view, or you have the option to create a new configuration when the view is created.

In this example, we’ll start with a drawing view of the assembly that shows the gripper in a closed configuration. Our goal is to superimpose a view of the assembly with the gripper in an open position.

SOLIDWORKS: Bring Your Drawings to Lifeimage001

 

To create this Alternate Position, we’ll select the view and click on Alternate Position View from the View Layout tab in the CommandManager. This will open the Alternate Position View PropertyManager where you’ll find two options: create a ‘New configuration’ or select an ‘Existing configuration.’ If we had a configuration of the gripper in the open position, we could select Existing configuration and choose it from the dropdown menu. Since we do not, we will select New configuration, and type in the new configuration name.

SOLIDWORKS: Bring Your Drawings to Lifeimage002

 

When you click OK, SOLIDWORKS will switch to the assembly model (or open it automatically) with the Move Component tool active. You can use the options in the PropertyManager to move/rotate components into the desired position. You can even use collision detection to achieve realistic motion/positions.

SOLIDWORKS: Bring Your Drawings to Lifeimage003

 

Once the assembly is oriented the way you want, click OK. SOLIDWORKS will switch back to the drawing and you’ll see that the outline of the new configuration (shown with phantom lines) has been added to the drawing view, which you can dimension as needed.

SOLIDWORKS: Bring Your Drawings to Lifeimage004

 

I hope you found this information useful. Be sure to check back often and also check out our YouTube channel for more great tips and tricks! Don’t forget to sign up for one of our Night Schools about drawings and detailing!

For a quote on SOLIDWORKS, check out our website or contact us at hawk@hawkridgesys.com today.

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Hawk Ridge Systems
From design to production, Hawk Ridge Systems delivers best-in-class solutions in 3D design, CAM software, and 3D printing.

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Technical Support FAQ: Share a Sketch, Stored Files and Saving Native Files http://blogs.solidworks.com/tech/2017/04/technical-support-faq-share-sketch-stored-files-saving-native-files.html http://blogs.solidworks.com/tech/2017/04/technical-support-faq-share-sketch-stored-files-saving-native-files.html#respond Mon, 17 Apr 2017 15:00:23 +0000 http://blogs.solidworks.com/tech/?p=16535 Can SOLIDWORKS share sketches between different part and assembly files? The easiest way to share a sketch is to create a Sketch Block.  A Sketch Block turns individual sketch entities into a group or block. Sketch Blocks can be saved

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GoEngineer

GoEngineer delivers software, technology and expertise that enable companies to unlock design innovation and deliver better products faster. With more than 30 years experience and thousands of customers in high tech, medical, machine design, energy and other industries, GoEngineer provides best-in-class design solutions from SOLIDWORKS, Stratasys, CAMWorks, Altium and Product Lifecycle Management (PLM). For more information, visit goengineer.com.

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Can SOLIDWORKS share sketches between different part and assembly files?

The easiest way to share a sketch is to create a Sketch Block.  A Sketch Block turns individual sketch entities into a group or block. Sketch Blocks can be saved and placed into the Design Library to be shared with multiple users or parts. Multiple sketch blocks can be used in a single part to layout a 2D part or assembly design.

To create a sketch block, simply create a sketch and right click and select block.  From the Design Tree, a Sketch Block can be edited, saved, exploded or added to the Design Library.

 

 

Why is performance so bad for files stored on Network Drives?

Optimal SOLIDWORKS Performance is dependent on many factors. Where the files are stored and how quickly those files travel through the network can greatly affect performance.  Slow performance may be due to indexing services, applications, anti-virus software and network bandwidth.

To test if the Network is causing poor performance, store files locally and then open the files.  If the files open quickly from the local hard drive, but not the network, then there is a problem with the network that needs to be addressed.

Can I save SOLIDWORKS files into native past version files?  Why not?

No, SOLIDWORKS files cannot be saved as a native past version file. Each version of SOLIDWORKS is packed full of new features, to make each of these features backward compatible is near impossible. As a workaround, SOLIDWORKS does allow users to save files as a native Parasolid, step, or IGES format.

To save a file as a Parasolid, step, or IGES format. Select File -> Save As. Any file format can then be chosen.


We hope you enjoyed this installation of the GoEngineer Technical Support FAQ. Let us know if you have a question we can address.


Author: Krystine Thoroughman
Krystine has been working with CAD for the past 10 years as a Designer and Technical Support Engineer. She became interested in the industry through working with her Dad, a machinist from Arizona. Krystine’s current focus is SOLIDWORKS PDM support and helping customers understand how different pieces of software can work together, to create a more efficient work environment!

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GoEngineer
GoEngineer delivers software, technology and expertise that enable companies to unlock design innovation and deliver better products faster. With more than 30 years experience and thousands of customers in high tech, medical, machine design, energy and other industries, GoEngineer provides best-in-class design solutions from SOLIDWORKS, Stratasys, CAMWorks, Altium and Product Lifecycle Management (PLM). For more information, visit goengineer.com.

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How Your Competition is Beating You Using SOLIDWORKS Smart Components http://blogs.solidworks.com/tech/2017/04/competition-beating-using-solidworks-smart-components.html http://blogs.solidworks.com/tech/2017/04/competition-beating-using-solidworks-smart-components.html#respond Sun, 16 Apr 2017 15:00:47 +0000 http://blogs.solidworks.com/tech/?p=16507 For those of you who haven’t noticed, SOLIDWORKS is really big on “data reuse.” That’s because recreating information is likely one of the largest contributors to lost time and designer frustration. I was recently on a call with a customer

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CADimensions

We are an authorized SOLIDWORKS and Stratasys reseller with certified training & support centers located in New York and Pennsylvania, USA. We are 100% focused on living a CADLIFE and have our vendor's unconditional endorsement in the sales and support of their products.

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For those of you who haven’t noticed, SOLIDWORKS is really big on “data reuse.” That’s because recreating information is likely one of the largest contributors to lost time and designer frustration.

I was recently on a call with a customer who was using the “Smart Components” feature in SOLIDWORKS in a really cool way. It is a neat example of file reuse. Here’s how it works:

Kevin Wilson at MAXPRO Technologies designs high pressure gas booster, liquid pump, and air amplifier systems, among other high pressure systems and components. Like any system, they use standard hardware and fittings to connect all their components.

Take this pressure regulator, downloaded from the manufacturer, for example:

For ease of use, Kevin was making sub-assemblies of this component, and its typical fittings. Easy, right?

Easy, until you have multiple instances of this regulator and a different fitting for each one. He was creating a different configuration of the assembly suppressing/unsuppressing each fitting.

Still not too bad, right?

That is, until you also have to change the angle at which that elbow is installed. When you change one instance, since it has been created using multiple instances of the same subassembly… they all change. This wreaks havoc on your mates and you end up spending time reattaching references. That has never happened to anyone, right?

Enter Smart Components. With a few simple clicks from a “dummy” subassembly, you can create this part with linked fittings and SOLIDWORKS will do the rest. If you want to learn how to create Smart Components, check out my tech tip on the topic here.

Once you set up your Smart Component, and add it to your assembly, the icon in the tree looks like this: , and when you highlight the component, it gets an icon like this:

When you click this icon in the graphics area, SOLIDWORKS opens a couple of windows, similar to when you insert a library feature (shameless plug for my library features webinar here).

Notice the graphics preview showing overlaid connectors. From the list on the left, just check the components you want. When you accept it, it automatically adds the components (AND THE MATES) to the assembly!

For those of you with keen eyes, notice that he even set up one of the connectors as a smart component. Now, with just a few clicks, he can repeat the process on the connector, and have everything update as needed while not affecting other instances of this “subassembly.”

This is a great method for reusing data and managing common components. In this particular instance, since all the components are purchased, revision control and part modification is not an issue. If you want to use Smart Components for your production parts, I would highly recommend some sort of data management solution.

There are many tools out there to help with this. An Enterprise solution like Dassault Systeme’s Exalead OnePart is the premiere option for tracking data. It parses everything in every file including CAD geometry and metadata (background file information) and provides incredible searching capabilities. Data management solutions like SOLIDWORKS Product Data Management (PDM) will help keep track of revisions and permissions, as well as walk your designs through workflows. Both options are great at what they do and I’m certain would come recommended by any professional in the field (myself included). However, they do require setup and administration to be effective.

I’d like to thank Kevin Wilson for allowing me to use his name and parts (and smarts) for this blog and tech tip! Kevin is a long-time SOLIDWORKS user and, from what I understand, quite the musician. If you were at SOLIDWORKS World 2015, I heard he stole the karaoke stage! Check out his Facebook Page.

As always, thanks for reading and Happy Modeling!

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CADimensions
We are an authorized SOLIDWORKS and Stratasys reseller with certified training & support centers located in New York and Pennsylvania, USA. We are 100% focused on living a CADLIFE and have our vendor's unconditional endorsement in the sales and support of their products.

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How to Hide/Show Dimensions in a SOLIDWORKS Drawing http://blogs.solidworks.com/tech/2017/04/how-to-hideshow-dimensions-in-a-solidworks-drawing.html http://blogs.solidworks.com/tech/2017/04/how-to-hideshow-dimensions-in-a-solidworks-drawing.html#respond Fri, 14 Apr 2017 15:00:22 +0000 http://blogs.solidworks.com/tech/?p=16518 In some cases instead of deleting a dimension, you might decide to hide SOLIDWORKS Drawing Dimensions. Now the question is how to make a hidden dimension visible again? This article demonstrates how to hide and then show dimensions in the drawing

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Javelin Technologies

Javelin Technologies is a provider of technology solutions since 1997. We are experts in 3D design and have helped thousands of companies with solutions for mechanical design, electrical design and 3D printing.

Large or small, we have the skills, experience, and services to propel your organization to new heights so you can aim high.

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In some cases instead of deleting a dimension, you might decide to hide SOLIDWORKS Drawing Dimensions. Now the question is how to make a hidden dimension visible again? This article demonstrates how to hide and then show dimensions in the drawing environment.

Step 1: Right-click on a dimension in a drawing view and select Hide from the shortcut menu:

Hide SOLIDWORKS Drawing Dimensions

Right-click on a dimension and select Hide.

The image below shows that two dimensions are hidden: “3” and “150”.

SOLIDWORKS Drawing Dimensions are hidden

Dimensions “3” and “150” are hidden.

Step 2: Activate Hide/Show Annotations. This is done through View > Hide/Show > Annotations (see below)

Activate the Hide/Show Annotation

Step 3: When the Hide/Show Annotations is active, the hidden dimensions appear in a gray colour. At this stage, the mouse cursor shape will change to an eye with a cross line on it. Now, clicking on any gray hidden dimension will display them in the drawing.  Also, clicking on a visible dimension will change it’s colour to gray meaning that when the Hide/Show Annotation selection is complete, the gray dimensions will be hidden from view.

By activating Hide/Show Annotation, the hidden dimensions would show in gray color.

Step 4: Deactivate the Hide/Show Annotations – If only dimension “3” is selected, it will show up after deactivating the Hide/Show Annotations and others would still be hidden. In the following image, dimension “3” is selected to show up, while dimension “150” is still hidden.

show dimensions

Dimension “3” has reappeared and dimension “150” is still hidden.

Hide or show Multiple Dimensions at Once

When Hide/Show Annotations is activated, all hidden and shown dimensions would be shown either in gray or black color. Selecting shown dimension would change their color to gray and vice versa. Therefore, if Hide/Show Annotations is activated as shown on Step 2, any numbers of dimensions could be set hidden or show hidden dimensions. The following image demonstrates how more dimensions are set to hidden.

Multiple dimensions could be set hide or show while Hide/Show Annotations is active.

Author: Mehdi Rezaei, CSWE, Javelin Technologies

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Javelin Technologies
Javelin Technologies is a provider of technology solutions since 1997. We are experts in 3D design and have helped thousands of companies with solutions for mechanical design, electrical design and 3D printing. Large or small, we have the skills, experience, and services to propel your organization to new heights so you can aim high.

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3 Ways to Make the Most of the Command Search in SOLIDWORKS http://blogs.solidworks.com/tech/2017/04/3-ways-to-make-the-most-of-the-command-search.html http://blogs.solidworks.com/tech/2017/04/3-ways-to-make-the-most-of-the-command-search.html#respond Wed, 12 Apr 2017 15:00:04 +0000 http://blogs.solidworks.com/tech/?p=16471 The Command Search function in SOLIDWORKS has to be my favorite feature. I find myself using it nearly every single day. What I love most about it is that any, and every, command is at my finger tips. Whether it’s

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Stephen Petrock

Since 1998, TriMech has helped our clients design better products by partnering with them and offering, not only CAD, CAE, PDM, FEA, CAM software products, but also by engineering solutions involving full-time and temporary staffing, contract design, analysis and drafting services, rapid prototyping, custom programming and implementation services. TriMech is a value-added reseller of SOLIDWORKS and Stratasys 3D Printers in the Mid-Atlantic and South-East including New Jersey, Pennsylvania, Delaware, Maryland, West Virginia, Virginia, North Carolina, South Carolina, Tennessee, South Carolina, Georgia, Florida, Alabama, Mississippi, Oklahoma, Arkansas and Louisiana.

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The Command Search function in SOLIDWORKS has to be my favorite feature. I find myself using it nearly every single day. What I love most about it is that any, and every, command is at my finger tips. Whether it’s a command I use once a quarter or once a decade, I can find it using this feature. But it doesn’t stop there, not only can you launch any command through this feature but you can also customize your interface and learn where a command is located through this tool. Here’s how:

3 Ways to make the most of the Command Search

 

  • Customize on the Fly: Drag a command from the search results to the command manager.

Search and Customize

  • Find a Command: Click on the “eye glasses” to have SOLIDWORKS automatically navigate through the menus. A big red arrow will show you where the command is located.

  • Launch a Command: Type in the search box and launch a command by clicking on it or scroll through with the arrow keys and press enter.command search tool

Author information

Stephen Petrock
Since 1998, TriMech has helped our clients design better products by partnering with them and offering, not only CAD, CAE, PDM, FEA, CAM software products, but also by engineering solutions involving full-time and temporary staffing, contract design, analysis and drafting services, rapid prototyping, custom programming and implementation services. TriMech is a value-added reseller of SOLIDWORKS and Stratasys 3D Printers in the Mid-Atlantic and South-East including New Jersey, Pennsylvania, Delaware, Maryland, West Virginia, Virginia, North Carolina, South Carolina, Tennessee, South Carolina, Georgia, Florida, Alabama, Mississippi, Oklahoma, Arkansas and Louisiana.

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SOLIDWORKS Support Monthly News – April 2017 http://blogs.solidworks.com/tech/2017/04/solidworks-support-monthly-news-april-2017.html http://blogs.solidworks.com/tech/2017/04/solidworks-support-monthly-news-april-2017.html#respond Wed, 12 Apr 2017 07:49:34 +0000 http://blogs.solidworks.com/tech/?p=16194 Hello to all, Welcome to this new edition of the SOLIDWORKS Support Monthly News, coauthored by members of the SOLIDWORKS Technical Support teams worldwide. Introducing NEW SOLIDWORKS Self-Paced eCourses on MySolidWorks.com By Joe Rousseau We all know that learning in

Author information

Julien Boissat

Sr. Technical Customer Support Engineer, SolidWorks, EMEA at DS SolidWorks Corp.

I have been a Tech Support engineer for Simulation products since 2002. I was previously a product manager at SRAC, the original makers of COSMOS for those who remember that time! ;-). I am currently in charge of the content of the certification exams for simulation products. I also initiated and still author the Simulation Knowledge Base and participate as much as possible in the expansion and evolution of the SolidWorks Knowledge Base. Finally, I handle the SolidWorks Support Monthly News blog.

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Hello to all,

Welcome to this new edition of the SOLIDWORKS Support Monthly News, coauthored by members of the SOLIDWORKS Technical Support teams worldwide.

Introducing NEW SOLIDWORKS Self-Paced eCourses on MySolidWorks.com

By Joe Rousseau

We all know that learning in a classroom is one of the best ways to learn SOLIDWORKS, but sometimes it’s not possible to attend a live class. You need the convenience to learn what you want, where you want. SOLIDWORKS is pleased to announce a library of self-paced, high quality, interactive eCourses that offer learning on your schedule.

The initial launch of this program includes eight eCourses:

  • Creating Animations Using SOLIDWORKS
  • Flow Simulation
  • Mold Design Using SOLIDWORKS
  • Routing: Piping & Tubing
  • Sheet Metal
  • SOLIDWORKS API Fundamentals
  • Surface Modeling
  • Weldments

You might be wondering what separates a SOLIDWORKS eCourse from other eLearning options. SOLIDWORKS eCourses include:

  • Everything from the SOLIDWORKS instructor-led training manual in a self-paced eLearning format
  • Background information and key concepts
  • Subject-matter expert videos and demonstrations
  • Interactive simulations that allow you to make the picks and clicks yourself
  • Offline exercises that allow independent study and further practice

SOLIDWORKS eCourses are hosted on My.SolidWorks.com and are available for purchase from your SOLIDWORKS reseller as a three month subscription.

For more information about the SOLIDWORKS eCourses and other training options, visit http://my.solidworks.com/training. To sign up for a SOLIDWORKS eCourse, please contact your reseller.

Proceedings of SOLIDWORKS World 2017 are available online

The SOLIDWORKS World 2017 Session Materials are available for viewing.

 

Spotlight of features: Noise Prediction in SOLIDWORKS Flow Simulation

by Lotfi Derbal

The Noise Prediction is available with SOLIDWORKS 2017 SP3. The acoustic Power Level is calculated with Proudman formulae, one of the known steady-state approach in CFD. The Proudman’s formula gives an approximate measure of the local contribution to total acoustic power per unit volume in a given turbulence field.

This can be used to estimate broadband noise generated by turbulence.

Available results include the Acoustic Power, in W/m^3 and the Acoustic Power Level, in decibel (dB).

Simulation Step-Up Series

Last month, Reza discussed the topic of Mixed Meshing. This month, he gives us an engineering view of FEA.

Next month, Omar will discuss the topic of basic failure analysis.

Noteworthy Solutions from the SOLIDWORKS Knowledge Base

icon - SW When using NVIDIA® GeForce® graphics cards with the SOLIDWORKS® software, what can cause extremely slow performance?
NVIDIA® GeForce® graphics cards have not been tested for use with the SOLIDWORKS software. For this reason, SOLIDWORKS does not officially support the use of these cards.
SOLIDWORKS Technical Support strongly recommends that you use a graphics card that the SOLIDWORKS software supports. For a list of supported graphics cards, follow the link.
It is possible that a recent Windows® or NVIDIA update installed graphics drivers that are causing this issue. If you continue to use a GeForce graphics card, you might be able to resolve the problem by installing a newer driver or by rolling back to an earlier driver version.
From Solution Id: S-072800.

Icon - EPDM In the SOLIDWORKS® PDM vault view, how do I refresh the thumbnail preview?
If SOLIDWORKS® files display the wrong thumbnails in the SOLIDWORKS PDM vault view, follow the steps in Solution Id: S-072536 to refresh the thumbnail preview so that the SOLIDWORKS PDM vault view works the same as the local Windows® Explorer view:.

Which level of the SOLIDWORKS® Plastics Add-In is active in my current session of SOLIDWORKS (Standard, Professional, or Premium)?
To determine which level of the SOLIDWORKS® Plastics Add-In is active in your current session of SOLIDWORKS, download and extract the  part file attached to Solution Id: S-072594. Then, compare the list of available analysis types to the images in attachment of the Solution.


That’s it for this month. Thanks for reading this edition of SOLIDWORKS Support News. If you need additional help with these issues or any others, please contact your SOLIDWORKS Value Added Reseller.

Also, comments and suggestions are welcome. You can enter them below.

 

Author information

Julien Boissat
Sr. Technical Customer Support Engineer, SolidWorks, EMEA at DS SolidWorks Corp.
I have been a Tech Support engineer for Simulation products since 2002. I was previously a product manager at SRAC, the original makers of COSMOS for those who remember that time! ;-). I am currently in charge of the content of the certification exams for simulation products. I also initiated and still author the Simulation Knowledge Base and participate as much as possible in the expansion and evolution of the SolidWorks Knowledge Base. Finally, I handle the SolidWorks Support Monthly News blog.

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Create Custom Cutting Threads in SOLIDWORKS http://blogs.solidworks.com/tech/2017/04/create-custom-cutting-threads-solidworks.html http://blogs.solidworks.com/tech/2017/04/create-custom-cutting-threads-solidworks.html#respond Tue, 11 Apr 2017 15:00:40 +0000 http://blogs.solidworks.com/tech/?p=16483 SOLIDWORKS 2016 introduced the Thread feature, which allows you to easily create standard threads as actual, fully-modeled geometry. What if you have non-standard threads you want to use? The answer is to create your own thread profiles. The process is

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GSC

GSC fuels customer success with 3D engineering solutions for design, simulation, data management, technical documentation, and 3D printing, as well as the most comprehensive consulting, technical support, and training in the industry. As a leading provider of SOLIDWORKS solutions and Stratasys 3D printing technologies, GSC’s world-class team of dedicated professionals have helped numerous companies innovate and increase productivity by leveraging advanced technologies to drive 3D business success. Founded in 1989, GSC is headquartered in Germantown, WI. For more information about GSC, please visit www.gsc-3d.com.

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SOLIDWORKS 2016 introduced the Thread feature, which allows you to easily create standard threads as actual, fully-modeled geometry. What if you have non-standard threads you want to use? The answer is to create your own thread profiles. The process is pretty straightforward and explained in the SOLIDWORKS Help.

One of the rules for custom thread profile creation clearly states that the pitch must be larger than the thread root, and this is understandable because we’re creating sweeps. If the pitch is smaller than the thread root, the sweep will intersect itself; of course, there is no such thread specification anyway, as it wouldn’t make sense.

But…What if you need to have the thread profile and pitch be the same?

This is something that, in the real world, you can achieve — but in SOLIDWORKS, such a sweep setup would result in zero-thickness geometry, which is an error condition.
Sharp vs. Standard threads in SOLIDWORKS

This quandary was presented to me by a prospective customer. I have to admit it took some experimentation to first discover a method that would give him what he was looking for, and then work through the available options to develop the easiest repeatable workflow.

Here’s the Secret…

In a nutshell, the secret is to realize that SOLIDWORKS is accurate to far more decimal places than typical manufacturing processes can discern. You can use this fact to get around the zero-thickness problem.

Say, for example, you wanted a thread profile that was 0.125″ high, but you also wanted a pitch of 8 threads per inch. You can define such a profile, but when using it with the Thread command, you’ll get an error. However, if you modify the pitch to be 0.125001, the feature works. For all intents and purposes, the pitch is 8 threads per inch, but geometrically, it’s just a tiny amount larger — enough for SOLIDWORKS make the sweep.
Sharp thread settings in SOLIDWORKS

While it would be nice to be able to put this pitch directly in the custom profile definition, my experience has shown it isn’t always reliable. However, when I make the modification in the Thread feature definition (overriding the built-in pitch), it has worked every time. Note also that, depending on the size of the sketch, adding 1 millionth of an inch may not be sufficient. But, I’ve never had to add more than 1/100,000 of an inch to get it to go.

That’s it! You now know the “secret” to create cutting threads in SOLIDWORKS 2016 and later.

Author information

GSC
GSC fuels customer success with 3D engineering solutions for design, simulation, data management, technical documentation, and 3D printing, as well as the most comprehensive consulting, technical support, and training in the industry. As a leading provider of SOLIDWORKS solutions and Stratasys 3D printing technologies, GSC’s world-class team of dedicated professionals have helped numerous companies innovate and increase productivity by leveraging advanced technologies to drive 3D business success. Founded in 1989, GSC is headquartered in Germantown, WI. For more information about GSC, please visit www.gsc-3d.com.

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