The SolidWorks Blog

Discover and Fix Your Vibration Vulnerability with SolidWorks Simulation

When I go biking during the summer, I rely on the frame of my bicycle to withstand stresses such as vibration and impact. As I speed down the trail, I think about the engineers and their process of designing a product that adeptly serves the needs of their customers. How did they test out the bicycle to make sure it doesn’t fall apart if the path becomes rocky? If the bike falls over, how did they make sure that the pedals don’t fall off? How do the engineers evaluate which loads can highlight problems in the design?

As it is ridden over rough ground the bicycle frame has to withstand not only the loads from the pedals and the weight of the rider but also the vibrational loads from the suspension system.  The danger is, if the vibrational loads are at the same frequency as the products natural modes of vibration, resonance can occur and the bicycle could literally shake itself apart.

Some design issues are hard to detect because you can’t see them visually. The SolidWorks Failure Mode Analysis video series will allow you to figure out some of the ways to detect hidden flaws in your designs using SolidWorks Simulation so that you can avoid product recalls and save time and money. The video on Vibration vulnerabilities will show you how you can use SolidWorks Simulation to fix your vibration vulnerability by allowing you calculate resonant frequencies, visualize natural vibration modes and dynamically test for vibrational stresses as you model product operation.

Whether you design complex machinery, hi-tech, or consumer products, Simulation helps every engineer vanquish their own design demons.

With its easy to use, powerful capabilities SolidWorks Simulation is the ideal tool to ensure your designs avoid this complex failure mode. SolidWorks Simulation allows you to easily calculate resonant frequencies and visualize the natural modes of your product design. 

To learn more about how you can revise and enhance your product design, such as a bike frame, for optimal service, watch the video.

5 SolidWorks Tips You May Have Never Seen Before

Chances are if you’ve been around SolidWorks for any significant amount of time, you may have seen some of these before, but I’ll be surprised if more than a handful of seasoned SolidWorks users have seen all 5 of these tips and tricks. While I’ve shown countless tips and tricks for SolidWorks in my time, these 5 are some of my personal favorites.

#5 Selecting an Edge and Starting a Sketch

This particular feature simply does several things with minimal input... a SolidWorks trademark. Simply select any Edge of any solid body and click INSERT | SKETCH.

A Sketch Plane is created automatically, Normal to the Edge Selected, with the Origin Coincident to the End Point nearest to where the Edge was selected.

This operation supports any Edge type from Linear and Prismatic to completely Organic and Lofted. You could also use INSERT | Reference Geometry to add a Plane Perpendicular to a Curve, but this takes care of all those steps AND starts a new Sketch.

#4 Loop Select

Do you like using Convert Entities but wonder why it only converts the exterior edges of a face? Tired of manually selecting each and every edge of that inside loop? I’ve got your answer in 2 clicks!!!

After you’ve started a new sketch, just select the same old face you would normally use to Convert Entities, but use the CTRL key to add one more selection to that set... 1 Inside Edge!

This is called a LOOP Select and will take the ‘focus’ of the selected face from the Outside Loop (default) to the Inside Loop.

Normal Face Select | CONVERT ENTITIES gets Outside Loop (Default)

CTRL Select Face and 1 Inside Edge | CONVERT ENTITIES gets Inside Loop

**Loop Select BONUS**

This tip also works for Loop Selection of the Inside Loop if you want to add a Fillet or Chamfer to the Inside Loop but not the Outside Loop.

It has an added bonus that if you were to change the sketch that affects the inside cut shown above, your Fillet or Chamfer would NOT error out with the addition or removal of edges to the cut profile.

You WOULD, however, get a Fillet or Chamfer error if you had discretely selected all the Inside Edges and there was a change that affected the edge count of the cut profile. It would take an Edit of the applied feature to resolve the Missing or Added edge.

#3 Explode Direction Control

Like SEVERAL other functions in SolidWorks, Control of the Triad orientation can be modified using the ALT key along with a Drag and Drop of the Triad.

Simply start the Explode Command, or edit an existing Exploded View and begin a new Explode Step.

The triad always mimics the triad orientation of the part or assembly.

To move and re-orient the triad, simply hold ALT and pick and drag the triad using the blue sphere where the X,Y and Z axis meet... then drag it over other geometry. It will snap to Linear edges, Plainer faces and will align to the Axis of Holes or Cylindrical features. Then just drag the triad along the new direction and position your part.

ANYWHERE there is a triad in SolidWorks, consider this tip valid... Move/Copy Bodies... Move with Triad... etc.

#2 Copy Surfaces

Copying a surface from one part to another is a very useful tool when you want to build In Context relationships between parts, especially when you get an unruly imported file with thousands of surfaces... .but you only need to ‘touch’ just a few.

I also use it for operations where I may want to simulate a Coating or Tape application on a part. Just Copy the Surface and Thicken it as a new Body.

What you may be asking yourself is: "That sounds great, Darin, but there is NO ‘Copy Surface’ Command"... .and you’d be absolutely CORRECT!

Many users try to use the KNIT SURFACE command, but this doesn’t work unless the faces you select are adjacent to each other and can form a single, ‘knitted’ surface.

However, there is a simple trick to this one, and it lies in the OFFSET SURFACE COMMAND. Pick a face or faces, adjacent or disjointed, and select OFFSET SURFACES from the Surfaces Tab.

It will show the selection, and the title in the Property Manager will state “Offset Surface” until you set the distance to ZERO. Then the title changes to COPY SURFACE. That’s it! You can use this in context of an assembly, and while editing a part you can select faces of other parts and Copy the Surfaces. This will create Associative Surfaces in the part you are editing. This tool really has dozens of use cases.

#1 Move Sketches... EASILY

These features are presented in no particular order, but I do consider this one of the most hidden yet easy to use tools when you are unsatisfied with the location of your sketches relative to the origin or anything else.

Moving Sketches while in Edit Sketch mode is not always the easiest task, ESPECIALLY when they are Under Defined Sketches or those that are Copy/Pasted from DraftSight or other 2D applications.

Where most users run into trouble is that they feel, and I don’t disagree, that you should just be able to window select all the sketch entities and then just grab a point and drag the whole group. While this sounds logical, it has simply never been the case.

Then you could try the Move Entities command, but it doesn’t always snap to the final location as you might expect.

The following technique is completely effective and very easy to do, you just have to know the sequencing of the clicks.

First, Window select the sketch entities you wish to move.

Second, hold the CTRL key on your keyboard then Pick and Drag the selected entities from one of the points in the sketch.

CAREFUL NOW... The trick here is that a CTRL + Pick and Drag in Windows is a Copy... and that is ‘initially true’ here too. Note the Cursor with the little (+) next to it. If you let go of the Left Mouse Button FIRST, you will COPY the Sketch.

Instead, while in the middle of the ‘Copy Sketch’ operation, release the CTRL KEY while still holding your Cursor. The little (+) goes away and the entire operation turns into a MOVE command. Simply snap and release your cursor when your selected point is in the proper location, or snapped to the origin.

In summary, of the thousands of functions in the millions of lines of SolidWorks code, these are some of the more useful yet somewhat hidden functions I use frequently. I hope that you found something you didn’t know about that helps you improve your quality of designs, but most importantly saves you time and effort during your creative process.

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Darin Grosser is a SolidWorks Elite Application Engineer, Certified SolidWorks Expert and a senior member of the technical staff at DASI Solutions, a SolidWorks Value Added Reseller with locations throughout Michigan and Indiana. He is a regular contributor to the DASI Solutions Blog.

Want to see what's new in SolidWorks 2013? You can request a free SolidWorks trial on our website.

Want to see how SolidWorks can help you win new business and get to market faster? Request a  SolidWorks demo today.

Creating Section Views in SolidWorks 2013

One of the questions we have seen a lot in the Technical Support department today is about some of the new functionality that has been added in SolidWorks 2013. There are generally two questions that users ask and the first is "How do I use the new functionality?" and "Can I still use the tools that I have used for years past?"

Looking at one of the new tools in SolidWorks 2013 that we were given is a new Section View Property Manager. This is a great tool that now allows you to easily create an almost limitless amount of section view types.

To answer the first question, in this new tool we start by selecting the Section Cutting Line or Half Section type.

When we create a standard Section we are then given a popup that allows us to add one or several different offsets to the section view.

To answer the second question we also get asked if you can still create a section view the way you use to be able to by first drawing your section lines then choosing the Section View tool?

The simple answer is Yes but there is still some new functionality that you need to watch out for. You can create the lines or arcs that you want to use for your section and add in all the relations or dimensions to those sketch entities. When you are done you can use your Right Click selection on one of the lines and use the Select Chain option to easily grab all of the connected entities.

The new functionality comes in when you select the Section Line from the Command Manager and you are presented with the following options.

You will want to read this carefully and know that to get a "standard" section view that you are used to seeing you will want to choose the Foreshortened option. Also you want to be aware of the option in the lower left of the dialog for Don't show again. If you check this it will add this message to the Dismissed messages and the new default will be the option you choose when you dismissed the dialog box.

The only way to be offered the dialog box again is to make sure you clear out those dismissed messages.

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Josh Altergott is Support Manager at Computer Aided Technology, a SolidWorks Value Added Reseller with locations in Kentucky, Missouri, Kansas, Indiana, Wisconsin and Illinois. He is a regular contributor to the CATI Tech Notes blog.

Want to try out SolidWorks? You can request a free SolidWorks trial on our website.

Want to see how SolidWorks can help you win new business and get to market faster? Request a  SolidWorks demo today.

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Improve Your Oil and Gas Design Capabilities with SolidWorks

In honor of this week’s Offshore Technology Conference, which features offshore resources for drilling and exploration, SolidWorks has released a video that details how to improve your oil and gas design capabilities such as plant design. This video outlines tools you need to respond to mission-critical challenges such as design efficiency and cost-conscious design.

SolidWorks can automate piping and tubing design with ease, speed and accuracy. Features such as 2D – 3D integration, design documentation, design validation through simulation, optimization will allow you to explore the possibilities of your models.

For more videos on SolidWorks solutions such as SolidWorks Simulation and SolidWorks Costing, check out the SolidWorks Demo Library.

Simplify Your Models Using the Intersect Tool

Has this ever happened to you?

Imagine that you get this super complex model with a lot of intricate internal details from your customer or supplier. The file size is huge and the rebuild times are long, considering that you only need it for any one of these reasons:

• Use your customer’s model as a reference for modeling a nest in a fixture or tooling. You need to remove all the interior details.
• Use your customer’s model as a reference for modeling an enclosure around it. You need to keep only the external faces.
• Insert your supplier’s model as one item in your assembly and BOM. You need to remove as many details as possible,
• Just need to 3D Print it for your customer. You need to remove all the cavities (completely “fill” the model).

The first thing you will try is, of course, using the Defeature tool (introduced in SolidWorks 2011). But what can be done when defeature does not produce the expected results?

Starting with SolidWorks 2013 the answer is simple: use the magic of the new Intersect Tool to fill any internal cavities and also merge all the solid bodies that touch (on faces) or intersect each other.

Watch this video for a demonstration of this procedure:

  

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Alin Vargatu is an Elite Applications Engineer and CSWE at Javelin Technologies, a SolidWorks Value Added Reseller with locations in Ontario and Nova Scotia, Canada. He is a regular contributor to the Javelin blog.

Want to try out SolidWorks? You can request a free SolidWorks trial on our website.

Want to see how SolidWorks can help you win new business and get to market faster? Request a  SolidWorks demo today.

Trouble with the Curve? Not Anymore! How to Drive your SolidWorks Assembly Pattern with a Curve.

Have you ever experienced that SolidWorks moment when you'd like to see a part feature available in an assembly? Patterning is one such wish I've had and recently revisited when a customer asked me about creating a Curve Driven Pattern in an assembly.

Now, some users may spout off a quick 'No' to such a question, but those of us that spend our 20 hours of screen time per day torn between the rigors of supreme CAD functions and Call of Duty while consuming excessive amounts of energy drinks and cold pizza may have found a beacon of hope in the Feature Driven Component Pattern command.

So how does one achieve such magnificence in their SolidWorks Assembly?  Well, to be honest, it does require a little massaging from an underlying Part level Curve Driven Pattern Feature, but there are multiple ways this could be tackled.

Let's use this conveyor example to show a few options. In this example, I want to pattern a Sub-Assembly that contains the leg and a foot plate part. My goal is to use a curve to pattern this Sub-Assembly around the curved conveyor rail within this Top Level Assembly.

 Exhibit A: Curve Driven Pattern in the Curved Rail part.

One way to do this is to create a Curve Driven Pattern in the Rail part. This can be something that may really exist in the part or may be a dummy feature that we fill in later using the power of feature order. Here I've established a curve for my pattern associated to the curved rail, and patterned a simple hole. Think of it as: wherever there is a hole, there will be a leg assembly aligned to that hole. Now if you don't need a hole in the rail, you could follow the Curve Driven Pattern feature up with some type of feature that will remove or fill in the holes (Extrude-Boss, Delete Face, etc.).

Back to the main assembly. Use the Feature Driven Component Pattern command to pattern the Sub-Assembly and your driving feature is the Curve Pattern from the Rail Part.  Done!

Exhibit B: Curve Driven Pattern in the Leg Part. Similar to exhibit A, here we are going to pattern the leg along a curve. In the leg part, capture the curve needed as a sketch (you may want to edit in context and Convert Entities from the Rail part or use a sketch you've drawn at the assembly level). Now use that sketch in the leg part to do a Curve Driven Pattern of the body. Again, we probably don't want the actual body instances left in the leg model, so you could follow that pattern feature with a Delete Bodies Feature that will remove all the instances created from the pattern.

Again, back to the main assembly. Feature Driven Component Pattern the Sub-Assembly needed and use the Curve Pattern from the Leg part as your driving feature. Done!

More flavors of these methods could be used as well. You could also use this for other patterns not available like Fill, Sketch, and Table.

I hope this was helpful, but if you're still thoroughly confused due to a buzz from your favorite energy drink, you can check out this little video I put together showing Exhibits A and B. Enjoy!

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Brian VanderPloeg is an Applications Engineer at Fisher/Unitech, a SolidWorks Value Added Reseller with locations across the Midwestern and Northeastern United States. He is a regular contributor to the Fisher/Unitech blog.

Want to try out SolidWorks? You can request a free SolidWorks trial on our website.

Want to see how SolidWorks can help you win new business and get to market faster? Request a  SolidWorks demo today.

 

Learn More About SolidWorks Using the Built-in Tutorials

I find that the best way to learn about the tools available in SolidWorks is by using them.

And one way that SolidWorks helps you to do this is by including an extensive selection of tutorials on a wide range of tools. These tutorials are fully incorporated into SolidWorks and are available in the SolidWorks resources tab of the task manager, or under the Help menu.

The tutorials are not only great examples of how to use the tools available to you in SolidWorks, they can also be used to try out some of the tools that you may not have used before such as Routing or Simulation. There is also a large section of tutorials for the newest additions to the software such as the new user interface for the Section Tool and Orientation Dialogue Box.

The tutorials are organised into easily navigated groups so that you can get straight to the relevant subject area.

By hovering your mouse cursor over the tutorial links, each of the tutorials will describe to you a rough timing for completion and also an overall description of what you will achieve upon completion. 

Then to open the tutorial, simply click on the one that you want. Each Tutorial will start with an overview describing the process to be followed.

 

The tutorials then describe exactly what the process is for the lesson, guiding you through step by step and helping you to understand not only what you are doing, but also describing why. There are clear instructions that include images of the process that is being carried out so that you can check your progress.

 

When opening the SolidWorks tutorials, your SolidWorks window automatically resizes to allow room for the tutorial window to be shown at the same time. And the interaction between SolidWorks and the tutorials doesn’t end there.

 

In the instructions for carrying out the tutorial, if you need to use a tool, both the name of the tool and what the button for that tool icon looks like in SolidWorks are given. If you are unsure at any point of where that tool is in SolidWorks, you can simply click on the button in the tutorial text and it will be highlighted in the SolidWorks user interface.

Also contained within the instructions are links to open SolidWorks models that can be used for the tutorial content.

All of this combines to make the tutorial set that is built in to SolidWorks a valuable knowledge resource for learning more about the software that you use.

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Duncan Crofts is an Applications Engineer & CSWE at TMS CAD Centre, a SolidWorks Value Added Reseller in Scotland. He is a regular contributor to the TMS CAD Centre blog.

Want to try out SolidWorks Premium? You can request a free trial on our website.

Want to see how SolidWorks can help you win new business and get to market faster? Request a  SolidWorks demo today.

Using SolidWorks Sub-Weldments

Something that has been confusing to students in my Weldments training classes is the proper way to create Sub-Weldments so that they retain all the work you have done creating properties for the cut-list items.

As of SolidWorks 2012 this is definitely possible but you have to do it in a specific way. The thing to remember with this is that the actual bodies do not store any properties, only the Cut-List Item folders do. So of course you have to do an “update” to your cut-list at least once before proceeding

Here are the steps for successfully creating a Sub-Weldment:

1. Create your weldment as normal.

2. Update the cut-list and add any additional properties to the folders.

3. Ctrl+Select the BODIES you want to make into a sub-weldment (either from tree or from screen with bodies filter).

4. Right+Click, CREATE SUB-WELDMENT.

5. Then update the cut-list again (this is important).  You will end up with three levels in the folder and the properties will be inherited into the Sub-Weldment.

This will even take the properties with the sub-weldment if you save it out to a separate part file (using right+click, "Insert into New Part" on the sub-weldment).  They will also be tied/related back to the original weldment file for updating!

Of course, as an alternative to actual “sub-weldments” done this way you can always just make a weldment, make another weldment, and then stick them into an assembly together.  The above method is nice because it keeps it all in one multi-body weldment part file rather than having to manage an assembly with multiple parts.

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Randy Simmons is an Application Engineer at 3DVision Technologies, a SolidWorks Value Added Reseller with locations across Ohio, Indiana, and Kentucky.  He is a regular contributor to 3DVision Technologies' Blog where you will find new ideas to improve your productivity with SolidWorks products.

Want to try out the weldment capabilities in SolidWorks Premium? You can request a free trial on our website.

Want to see how SolidWorks can help you win new business and get to market faster? Request a  SolidWorks demo today.

View and Annotate SolidWorks Files Anywhere with eDrawings Viewer

Imagine this scenario: you’re working from home and a team member asks to you to review their product designed in SolidWorks. You do not have access to your work computer, which has SolidWorks, but you need to provide feedback quickly to keep the design process moving. How do you view the file?

Thankfully, SolidWorks has a FREE solution to help you out. The eDrawings Viewer allows you to open eDrawings files, get dimensions, and collaborate with others by using the mark-up capability. This means you can annotate the design on the spot and share your thoughts with your team without worrying about working remotely.

The eDrawings Viewer is easy to download – you can find it on the SolidWorks homepage under the Products tab. Just click on Free CAD Tools: the second item on the page is the eDrawings Viewer. To download, just click “Download eDrawings Viewer FREE” and, presto, you’re done!

To see if the program installed correctly, check out some cool designs from our customers Donn McKinney and Teversham Engineering.

Breaking a sheet metal loft so it shows bend lines

Lofted bends are great way to create specialized sheet metal parts where you need a high degree of transition from one profile to another – think square to a circle duct work. 

The lofted bend requires two open contour profiles for it to work, with no guide curves or sharp corners, so there are limitations. 

 

The problem comes when you want to see the bend lines. SolidWorks has rules for the sketches in order to see bend lines. 

• The sketches must be parallel
• The sketches must have the same number of corresponding lines and curves

Looking at the previous image, we’re going from one sketch entity (an arc) to three (straight line - arc - straight line) = no bend lines.

How can you get around this problem? 

Easy--drop everything down to a single sketch entity via the Fit Spline and the straight line - arc - straight line are now a single spline entity.

Go back and edit the Lofted Bend feature and you now have the option to control the number of bend lines or Maximum Deviation.

And your flat pattern will now show the bend lines.

 

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Steve Ostrovsky is an Applications Engineer at TPM, a SolidWorks reseller with locations in North and South Carolina.

Want to try out the sheet metal capabilities in SolidWorks Premium? You can request a free trial on our website.

Want to see how SolidWorks can help you win new business and get to market faster? Request a  SolidWorks demo today.