The SolidWorks Blog

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.

Free SolidWorks Certification for Subscription Service Customers

Are you looking for a way to test your skills in SolidWorks or maybe you are in the hunt for a new job and want to make yourself more marketable, then trying one of the SolidWorks Certification Exams is a good way to do that. SolidWorks has been certifying their users since the product first came to the market and has continued to add a variety of different certifications over the years. What many people do not know is that one of the advantages to keeping your license active on Subscription Service is that SolidWorks put out a codes that will allow you to take the test for free.

The best way to access the codes for the free SolidWorks certification is to go to the SolidWorks Customer Portal this can also be found by going to http://www.solidworks.com and selecting Login in the upper right hand side of the site. Once you log into the Customer Portal you can go to Certification in the Community section.

 

Note: If this is your first time logging into the SolidWorks Customer Portal and there are locks on many of the links you need to go to the Register My Products and enter in your SolidWorks Serial Number.

Once you select the Certification link it will take you to the SolidWorks Website and the you need to select the link for Certification Offers for Subscription Service Customers.

At the bottom of the page it will list all of the current offers and when the codes will expire. Make sure you read all of the notes at the bottom of the page.

You want to check the site on a regular basis for any new codes or offers that might be going on.

Good luck with your certifications

Josh Altergott, CATI Support Manager

 

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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.

You can learn more about SolidWorks certification programs and SolidWorks Subscription Services on the SolidWorks website

Allowing SolidWorks to Perform

For the 4th year in a row Adrian Fanjoy and I have done one of our favorite SolidWorks World presentations, "Allowing SolidWorks to Perform".  The presentation was well received and we thought it would be a good idea to share the information with more than just the SolidWorks World attendees.

We will be publishing our presentation thru a series of blog articles so check back often to see what we have added to the series. We have also included a set of links at the bottom of this article that will take you to all past and future articles.

To get the series started we are starting with Who, What, When, Where, Why and How of putting together this information.

Introduction

From the standpoint of performance in a SolidWorks modeling environment; large assembly modeling is the most strenuous endeavor. As users of any CAD software can understand large assemblies can easily take a workstation to the limits of its capability. In working with several customers and from our past testing Adrian and I have determined many different means of improving performance for SolidWorks. This year we structured our testing a little differently so we could quantify the improvement and determine what improvement is worth the investment.

Our testing was different this year in that we were given a large assembly from Racine Railroad that we are now able to show. We also moved away from our benchmark macro to a custom built API that runs the model through many aspects of SolidWorks measuring our performance in a manner that has never before been done. In our tests we isolate individual changes in our hardware and modeling environment and measure the time difference of running the API against a Typical, Practical, and Optimal system. This allowed us to measure the effect of a single change and then compare that to other changes to determine where to invest time and resources to improve SolidWorks performance.

Please realize that the results that we are presenting in this document are specific to our environment, models, and tasks performed. While we are certain that you can expect similar results when making such changes, the magnitude of your performance increase will definitely be different than ours. When working with large assemblies the benefits that you realize may be more or less than ours. Overall you should see an improvement but realize that we cannot determine what other environments may hold, thus we will not guarantee the effect these changes will have in any environment other than ours.

Tests

To determine what changes make the most significant difference in hardware and modeling performance we ran our model through a custom SolidWorks API created by Bob Hanson (CATI/InFlow) that performed operations common in a typical designers day (ie. modeling, rotations, rebuilds, opens, closes, saves, etc...). We tested many specific aspects in the categories of hardware, system configuration, and modeling methodology.

Environment

To run tests of this nature and insure that the integrity of the testing was maintained we needed a system that was extremely adaptable. BOXX Technologies provided that workstation. The 3D BOXX 4920 Extreme Workstation gave us the ability to test a wide range of configurations without jumping from one workstation to another which would have made maintaining consistency in our configuration almost impossible. This ability to adapt allowed us to run tests that ranged from:

• 1 core to 6 cores
• 3.42GHz to 4.43GHz processor speeds
• 2GB to 32GB of RAM
• 5 different Nvidia graphics cards
• 5 different hard drive types

Model

Our model was given to us this year by Racine Railroad Products and was the ideal assembly to use for performance testing. It is a combination over 10,000 components with many layers of subassemblies that gave us the flexibility to perform all of our testing. The model, as seen below, is their Safelok Applicator & Remover, A.K.A. SAR Machine. The machine both applies or removes the Safelok clip used mostly in concrete railroad tie scenarios; although there are wood tie applications as well.

The stats for this assembly are:

• 10559 total components
• 9693 parts
• 866 sub-assemblies
• 1292 top level mates
• 15093 bodies

In total the dataset takes up 1.92GB of disk space and has 4854 files.

Baseline or Typical Machine

For our baseline test we chose to run the API in a manner that we felt was consistent with typical environments that we see with customers and this will be referred to as our Typical Machine in all of our testing.

The core aspects (These never change)

• SolidWorks 2013 SP0
• WIN7 64bit OS

Hardware

• 1 - i7 processor with 2 cores @ 3.4GHz
• 8GB RAM
• OS and assembly storage on the same 7200RPM hard drive

Configuration

• SolidWorks options set to defaults
• Files are stored locally
• Several Add-Ins are turned on
• Operating system visual settings are set to default

Modeling methods

• Image quality set optimally
• High level of detail in some components
• Large number of top level mates
• Assembly is fully resolved

With our environment configured as above our benchmark ran in 4:43:44. Most of the comparisons that follow in our blog articles will be compared to this Typical machine.

In the subsequent articles in this series we are going to explore each test that we did. We will put the tests in no particular order with the exception of we will be posting all of our hardware tests followed by modeling tests. We will finish with 2 optimal configurations to see what the effect can be when you combine all of the improvements together into the same environment and model set.  Occasionally we will veer off track and discuss a side topic here and there as well.

I hope you find these articles informative and helpful. Please check back to the CATI blog as we will continue posting our series of articles that goes further into the details of each of our tests. All of these articles will be stored in the category of Free SolidWorks from Performance Constraints and links to each with their release date are listed below:

• FSWPC-13-#1 Introduction (3/19/13)
• FSWPC-13-#2 RAM (3/21/13)
• FSWPC-13-#3 Processor Cores (3/26/13)
• FSWPC-13-#4 Processor Cores for Simulation and PhotoView360 (3/28/13)
• FSWPC-13-#5 Processor Clock Speed (4/2/13)
• FSWPC-13-#6 Hard Drives (4/4/13)
• FSWPC-13-#7a Graphics Cards-SolidWorks Functionality (4/9/13)
• FSWPC-13-#7b Graphics Cards-Hardware Comparison (4/11/13)
• FSWPC-13-#7c Graphics Cards-Model Complexity (4/16/13)
• FSWPC-13-#8 Files stored in an older version (4/18/13)
• FSWPC-13-#9 OS Visual and User Settings (4/23/13)
• FSWPC-13-#10 SolidWorks Options (4/25/13)
• FSWPC-13-#11 SolidWorks Image Quality (4/30/13)
• FSWPC-13-#12 SolidWorks RealView Graphics (5/2/13)
• FSWPC-13-#13 SolidWorks  Level of Detail (5/7/13)
• FSWPC-13-#14 SolidWorks Mates and Flexible Subassemblies (5/9/13)
• FSWPC-13-#15 SolidWorks Defeature (5/14/13)
• FSWPC-13-#16 SolidWorks Envelope (5/16/13)
• FSWPC-13-#17 SolidWorks Large Design Review (5/21/13)
• FSWPC-13-#18 SolidWorks SpeedPak (5/23/13)
• FSWPC-13-#19 SolidWorks Save as Part (5/28/13)
• FSWPC-13-#20 SolidWorks Large Assembly Mode (5/30/13)
• FSWPC-13-#21 Optimal Configuration and Conclusion (6/4/13)

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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.

SolidWorks Dismissed Warning and Error Messages

One call that we get on a regular basis on the support line is a question of "I used to get this warning message when I did.... and now thing are not happening the way they did before--why?" More often than not we find the answer in the SolidWorks System Options in the Messages/Errors/Warnings, as this is where dismissed error messages go when we check the box on a dialog that say "Don't Show Again." While there are cases where this is a good thing more often than not we forget that we dismissed the message and find ourselves trying to find it again.

It is important to know what the messages mean and what the consequence is when we check the box for Don't show again. For example warning below come up when we open an assembly and SolidWorks cannot find a part or assembly file in the location it was once in or if the name changed. If we choose the option of Suppress and Don't show again then for all other files we open that cannot find a referenced file then they will automatically be suppressed.

There are also other things that can happen when we check the option for Don't show again. For example if we set an option to Prompt and then when we are prompted and check the Don't show again box the System Option will change according what we set when we are prompted.

The last messages to watch out for are the ones that apply to a specific assembly or session of SolidWorks meaning that on the next file you open or the next time you close and restart SolidWorks you will be prompted once again for the same thing we were once before.

A good rule is to set yourself a reminder to go in once a month and check your system options to make sure that there is nothing that has been dismissed and that all of your settings are set to where you want them to be.

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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.

Be sure to check out the SolidWorks Support FAQ every month for more answers to common questions--directly from the SolidWorks support team.

Snapshots of PhotoView 360: Appearances

Read the entire series: (Part One: The Basics, Part Two: Appearances)

Appearances are usually one of the first properties added to produce a rendered image. They can add a color, texture, or illumination settings to an assembly, component, face, feature, body, or part. Applying appearances works in a hierarchy; assembly appearances will always override component appearances, and component appearances will override face appearances, and it continues down the list.

TIP: Adding appearances does NOT add mechanical properties.

When dragging and dropping appearances onto a part from the task pane, pressing ALT while dragging and dropping will enable the property manager for that appearance. This gives you the option of choosing your settings without having to edit the appearance to enable the property manager of that appearance.

Creating Drawings for SolidWorks Multi-body Parts

When you have a multi-body part in SolidWorks the question that comes into play at some point is how do I make a drawing for each of the different bodies "parts". The answer to this is like many items in SolidWorks is open ended and has many different solutions and I am going to run you thru a few of these options.

Option 1 - Insert into New Part

This option creates a new derived part that contains a reference back to the parent part. Each new part contains a single feature named Stock- <parent part name> - n ->.

If you change the geometry of the original part, the new parts also change. The software updates the existing derived parts, preserving parent-child relations.

The items I see that can be a downfall to this method is that you now have an additional part that you need to maintain as well as a part the has no dimensions when you go to create a drawing of the part.

Option 2 - Save Bodies

This works much like Option 1 but does give you a few more items that you can control such as the file name, creating an assembly of all the different solid bodies, and part template choice.

Overall it is up to you which of these options will work best for your application.

Option 3 - Creating Configurations

You can always create a configuration(s) to represent the different bodies and their features.

For our example all we needed to do was create a new configuration called Steel Rule and suppress all of the features that were not related to our "target body". One warning is you have to make sure that when doing this you check all Parent/Child Relations to make sure when you suppress one feature it does not take out others you do not want suppressed.

The benefit to this is that you now have a configuration you can reference on the drawing or for an assembly later and you have dimensions that you can easily show on your drawing. The downside to this is you have to be aware of changes that you make to the file and managing all of the features.

Option 4 - Select Bodies (Model View)

The last option we have is Select Bodies which allows us to choose which body we want to create a drawing view of. The one item to consider is if your body is not oriented in a standard drawing view you will need to create a new named view to use in the drawing.

The downfall to this method is when inserting dimensions it brings in the dimensions for the entire model and not just the solid body.

I hope this helps everyone as they create different drawings.

Also a special thanks to Ken Zirbel from Fox Valley Tool & Die Inc. for letting my use his models for this example.

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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.

 

Related articles

Make A Single Body with Multiple Open Contours in SolidWorks 2013

Why are some of my dimensions grey and others black?

Using SolidWorks to Create a Helical Pattern

Something Intersecting in SolidWorks 2013: Join Your Parts to Find Volumes

SolidWorks Materials: Manage & Customize

Managing SolidWorks Favorite Materials: Add, remove or rearrange your favorite list

You can add materials you often use to your SolidWorks favorite list for faster access. This option is oftentimes overlooked, even though it resides in a window you probably use frequently. To access the window, just right-click on material in the feature manager tree, shown below. Customizing your list will make adding material to every 3D CAD model you have much simpler.

 

To manage your favorite list, click on "Manage Favorites." A new window titled "Material" opens, shown below. To add a material to the list, simply click on the material you want to add from the list to the left and click "add." Once you have added your favorite materials, you can rearrange their order in the list by clicking on the "Up" or "Down" buttons in the window. Furthermore, you can remove them using the "Remove" button.

Creating SolidWorks Custom Materials: Adding custom materials with mechanical properties

To create your own custom material in SolidWorks, click on Edit material. If you right-click on the custom material folder, you have the option to create a new library folder or just add a new category. The category can be Steel, Iron, Carbon Fiber, "ACME Material," etc.

You can now simply right-click to copy one of the materials under SolidWorks materials and paste it in the appropriate category.

Once a material is added to your custom library, you can then rename and manage it just like any other material in the list by right-clicking on the material itself. Furthermore, you can input the mechanical properties of this material - such as the elastic modulus, density, tensile or compressive strength, etc. An example is shown below.

 

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Nady Osmat is a SolidWorks Sales 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.

SolidWorks Enterprise Licensing Made Simple

You’ve anticipated installing a newer version of SolidWorks Enterprise PDM for the last month. You’ve let everyone know of the impending update. You’ve downloaded the latest service pack from www.SolidWorks.com. You’ve made backups of your SQL databases. You’ve ensured the archive folders have been backed up. You performed the upgrade procedures from the Installation guide PDF to the ‘T’ (pg. 92). After the upgrade is completed, you test your first client to the upgraded server and you see:

No licenses available!

If you see this, we might need to review the installation procedures one last time. On the bottom of page 92 under the heading ‘Client Licenses’, there are two brief paragraphs explaining what might have happened:

A database upgrade to a new major version resets the license count to 0 users. After the upgrade, you must install a valid license for multiple users to log in.

When upgrading from an older service pack, for example Enterprise PDM 2009 SP1 to Enterprise PDM 2009 SP2, your existing license code is still valid. The license file must have been missed.

As stated above, you must have a new license file for every major release (i.e. 2012 to 2013) but it is not required for upgrades within a release (2012 SP0 to 2012 SP4). If you do receive the above message, it is advised that you retrieve your license file as quickly as possible. You can do this immediately with your company login to www.solidworks.com. It does not require a technical support ticket through your local reseller.

To obtain your license, follow these steps:

1. Go to www.solidworks.com and select ‘Login’.
   
   
   
   
2. Click the icon for customer portal and provide your customer log in information.
   
   
3. Select ‘My Products’ for a listing of your registered products. Note: If you have not registered your SolidWorks Enterprise PDM software yet, you must do so before retrieving your license file by clicking the ‘Register My Products’ link.
   
4. Select the licenses file for the product you are installing (step 1). In this image below, the 2012 product is selected. Then click ‘Get License’ (step 2). You should next see a message indicating that the license file is being sent to your email.
   
5. Within a few minutes, you should receive an email with your license file attached. Save this to a location on your machine for easy access in the next step.
   
   
6. The last step is to load the license file into SolidWorks Enterprise PDM. To do this, we launch the SolidWorks Enterprise PDM Administration tool, log into our vault, double click the ‘License’ node(step 1). When the ‘Set License’ window appears, click the ellipsis button and browse to the text file from the email (step 2). Click ‘OK’ to apply and double click the ‘License’ node. You should now see licenses available in the bottom list (step 3).
   
    
   

At this point, you should be able to log into your client vault view and not receive the message regarding zero licenses available! A few considerations when updating:

• With the impending release of the new 2013 products, you are no doubt planning to update one or more product lines to the 2013 versions. In regards to SolidWorks and SolidWorks Enterprise PDM, SolidWorks Enterprise PDM must be at the same version or newer than SolidWorks. The SolidWorks Enterprise 2013 add-in will be compatible with SolidWorks 2011, 2012, and 2013. If you upgrade SolidWorks and not SolidWorks Enterprise PDM, SolidWorks 2013 files may not be compatible with SolidWorks Enterprise 2012 and is not supported in this setup.
• When updating a SolidWorks Enterprise environment, ALL clients and servers must be on the same year and servicepack release. As such, you must update all components simultaneously to prevent any outages in your environment and replicated sites. You will NOT be able to log into a vault view if the client differs in version from the server.
• When deploying large amounts of clients, you can use Group Policy to deploy the client to users. This can be found on page 57 of the Installation guide PDF.

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Royce Cole is a Certified SolidWorks Enterprise PDM Professional and Support Technician, and application engineer at DASI Solutions, a SolidWorks Value Added Reseller with locations throughout Michigan and Indiana. He is a regular contributor to the DASI Solutions Blog.

Customizing SolidWorks Flyout Toolbars

The other day while watching a video on some of the new SolidWorks 2013 features, I noticed that one of the Flyout Toolbars for Annotations had a command for Cosmetic Threads that I did not have in my Flyouts, so I set about going to find out how to make the same change. I looked in all of the standard places first, Help, Knowledge Base, etc. and found no real straight forward answer. So I resorted to my other bag of tricks, below is what I found and I think I will add this to my other collection of Redneck Workarounds.

So here is what we started with first we Customize the S key to add the Annotation Flyout Toolbar.

We can see that when we look at the Annotations Flyout that there is no Cosmetic Thread.

To get our Cosmetic Thread we will again go back to Customize, show the Annotation toolbar and add the Cosmetic Thread to the toolbar.

 Now we go back to our S key and you will see that we now have our Cosmetic Thread.

Note the location in the Flyout and it is the same location that we dropped the command into the toolbar in the earlier Customize.

We have tested this with several other Flyout Toolbars and we were able to add and or reorder buttons to several other toolbars with the same steps listed above.

Good Luck and I hope this helps in customizing SolidWorks. You can learn more about SolidWorks 2013 on the website (no registration required).

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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.

Increasing Performance in SolidWorks Patterns

I had a customer send me a file recently because they were having issues with the performance of their part file that had several pattern features in it. When you look at the file from the surface you do not see anything out of the ordinary but our Feature Statistics they tell a different story of a 108 second rebuild time and Linear Pattern8 & 9 taking a majority of that 108 seconds. Also if you try to edit one of these patterns you are met with a long wait time to Edit Feature or to check OK even if no changes have been made to the feature.

So the questions is what can we do to decrease the edit and rebuild time of these features. We can start with the Geometry Pattern option in each of the pattern features. The Geometry Pattern option allows SolidWorks to pattern features while not solving the end condition of those patterned features. This option was not applicable for this part so there was no benefit in using this option for our part.

Our next option is to look at the part in a different way and to do that we need to look at each group of features that needs to be patterned as its own solid body. So with some simple changes to uncheck the Merge Result option on some features and to be selective as to which bodies merge with each other in other features we are able to set out file up so that we can pattern Bodies vs. Features.

  
You can see the results below as we deleted the 2 problem patterns and replaced them with pattern features that utilized bodies and not features. This cut our rebuild time from 108 seconds to 12 seconds.

 

The only item we had to add after the patterns was a Combine of all the solid bodies and if you are going to do any modifications to the patterns you can easily use the Roll Back Bar to go above the combine.

Note: If we had not added the Combine feature our rebuild time would on been .75 seconds.

Enjoy

Josh Altergott

CATI Support Manager

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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.