SolidWorks BOM Showing Incorrect Information

I recently had a technical support call from a customer who was trying to copy an existing project of assembly files and part files to make another project that was similar but different.  They had renamed the files with new part file and assembly file names, but the BOM information which was to show these new part names wasn't.  It was showing the old file names instead.  So after some head scratching, I checked to see if these files had configurations in them.  They in fact did and were set at the configuration property level to show a 'user specified name' instead of the file or configuration name.  This is why file name 102-12345 was showing as 102-xxxxx instead of the correct file name.  Once we set these configuration properties to show the file name, all was well.  So if you encounter this same behavior on your system, remember that the configurations each have their own properties and verify that they are listing what they should be listing in your BOM.

So hopefully if this issue ever comes up in your work flow, you will remember this simple tip.  Thank you.

Brian Reel
CATI 

Computer Aided Technology, Inc. Team raising money and awareness for men's health.

Over the last few years November has received a face lift, changing its name to Movember. The staffs at CATI, customers, and partners are working together to not only to raise money but to raise awareness on health issue. So if you are a mother, father, brother, sister or even a grandson or granddaughter you can impact the futures of your loved ones.

So visit Movember today, donate, learn and care about what matters most; people.

http://us.movember.com/team/443309

Thank you for your consideration.

Bob McGaughey, CSWE

CATI

Adding same size hole wizard hole to other faces

Have you ever come across an issue where you need to add an additional hole to a sheet metal part?  The issue is, if you have a hole wizard hole on a face of a sheet metal part.  If you later need to add the same size hole to another face you cannot just edit the hole wizard feature and place on another face because you lose the 3D sketch option when you edit feature (if 3d sketch was not used).  If you just add another hole wizard feature on the other face, the hole callout command will only list the one hole and will not show the 2X qty as you would expect.  You have a few options to correct this issue so let’s take a look.

Option 1:

You can always delete the original hole wizard feature and recreate it so you have the 3D Sketch option.

Option 2:

You can add an additional hole feature on the other face and use the hole table in the drawing to label the holes.

Option 3:

You can roll back your part before the hole wizard hole and use the unfold command to unfold the bends.  At that point, you can roll forward past the hole wizard hole and edit the feature and place the hole.  You don’t need the 3D Sketch option because the part is flat now.  Once the hole is added you just need to fold the part back and you are done.

Realistic load transfer in SolidWorks motion simulation

    When setting up a motion study in SolidWorks, the interactions between the different components of your part will be dictated by how the mates are set up.  This is because the mates will tie up respective degrees of freedom relative to the two components being mated.  This means that transfer of the loading from one component to another will depend on the mate.  In other words, how one part moves another based on the load it is under is controlled by how those two components are mated.

    SolidWorks mates do a great job in defining the degrees of freedom.  Any combination of motions is easily achievable by chosing the appropriate mates.  Load transfer, however, involves more than just direction and magnitude (freedom) of the motion.  Load transfer is also concerned with the stiffnesses of the part under loading.  This is because materials have the ability to deform both plastically and elastically. Simply creating the mate does not account for this flexibility.

    To deal with this inherent rigidity, SolidWorks has a utility that allows us to define a bushing in the mate. Right inside the mate command, there is an analysis tab that helps us set up such parameters like the flexibility of the mate.

This means that our study will reflect the real world that much more accurately as we are able to account for the deflection that occurs in the component before the load is transfered to the next component.

Brian Adika, CSWP
Applications Engineer, CATI

How to Set up Mouse Gestures in SolidWorks

Short little video on "How to" set up your SolidWorks interface.

 

Todd Werginz

Computer Aided Technology, Inc.

Customizing SolidWorks Flyout Toolbars

CATI's monthly contribution to the SolidWorks Blog was posted last week. This month I chose to write about how to customize the SolidWorks Flyout Toolbars. The article is based  upon a problem I ran into when watching a video on some of the new SolidWorks 2013 features and details the steps it takes to add, remove or reorder the buttons in your Flyout Toolbars.

To view the article use the link below.

http://blogs.solidworks.com/solidworksblog/2012/10/customizing-solidworks-flyout-toolbars.html

Before Customizing                                   After Customizing

 

Josh Altergott

CATI Support Manager

Why Automate Your Designs With DriveWorks?

There are several good reasons why companies want to
automate what they do:

• Reduce the cost of custom
  designs


• Respond quickly to sales
  enquiries


• Enhance product quality


• Reduce repetitive tasks 

The Benefits of DriveWorks

• DriveWorks lets you capture and
  re-use knowledge and rules to specify, design and engineer to order


• It allows you to respond
  quickly to sales enquiries


• DriveWorks can capture and protect
  individual's knowledge


• It reduces cost of custom
  design repetitive tasks


• DriveWorks can enhance the
  product quality/audit trail by elminating human error


• It bridges the gap between the
  engineering and sales departments


• DriveWorks offers a scalable
  solution all the way to 3D configuration on the web!

Jim TeDesco
Marketing Manager
Computer Aided Technology, Inc. 

How to: Set an Admin Image Path in SolidWorks – How long is too long?

Advanced assembly cut

When working with parts in an assembly you are limited to extruded cuts and revolved cuts through multiple pieces. If you would like to create a more advanced assembly cut (Cut Sweep, Cut Loft) we need to get creative. One way of accomplishing this is to create a new part in your assembly model. Design your cut feature as a solid part. Edit the first part that needs to be cut and use the cavity command. This will remove material from your part where the part we created overlaps in volume. Repeat these steps for all parts that intersect your cutting body. In this example I am going to put two blocks into an assembly, add a new part, and then use that part to remove material from the two blocks.

The assembly of two blocks and new part of have been generated. These are the two sketches that define the sweep for my cavity part. Be careful not to add in context relations to sketches used for cutting. After you cut the model they will be broken.

The sweep part has been created and now we can use it as a cavity feature.

Edit the first part in context to the model. Use the cavity feature located under "Insert -> Features -> Cavity". Choose the swept part as the design component. Accept the feature and the overlapping swept body will be removed from the first block in the assembly.

Repeat that process until all parts have been cut. The swept body has been hidden for illustrative purposes.

Thanks,

Jordan Nardick, CSWE
Technical Analyst
Computer Aided Technology, INC.

 

How to Rename a Project in DriveWorks Solo

This is how to rename a DriveWorks Solo project.
Renaming the project does not affect any of the models used by the project.

A DriveWorks Solo project consists of three
files, all of which have the name name but a different file extension. The name
of each fule is the name of the project, and the extensions are:
".driveproj", ".drivegroup" and ".drivemaster".

By default, Windows XP and later don't display file
extensions.

To rename the project, simply change the name of each
file to be the new project name, and leave the entensions as they are.

For example, if a project is called "Trailer
Body" in a folder called "C:\Trailer Project", then the project
files will be called

1. C:\Trailer Project\Trailer Body.driveproj

2. C:\Trailer Project\Trailer Body.drivegroup

3. C:\Trailer Project\Trailer Body.drivemaster

To rename the project to "Trailer Body Model
2", the files need to be renamed to be:

1. C:\Trailer Project\Trailer Body Model
2.driveproj

2. C:\Trailer Project\Trailer Body Model
2.drivegroup

3. C:\Trailer Project\Trailer Body Model
2.drivemaster

 

Jim TeDesco
Marketing Manager
Computer Aided Technology, Inc. 

DriveWorks Pro Concept: File Naming

File
naming is an important consideration when planning an implementation, and
DriveWorks affords complete flexibility in how files are named. This article
describes how files get named in DriveWorks, and how the names you choose
interact with the concept of alternatives and driven alternatives so that you
can build up libraries of parts that can be used again and again without
needing to be generated for each specification that is generated.

Simple File Names (Suffixed)

DriveWorks
decides file names for models in a very simple way, for example, if we have the
following assembly stucture and file name rules:

• MyAssembly [=DWSpecificationId]
  
  
  
  • MyPart1 [=DWSpecificationId]
  
  
  • MyPart2 [=DWSpecificationId]
  
  
  
  

Then
DriveWorks will generate a new assembly and parts for a specification numbered
8, as follows:

• MyAssembly8
  
  
  
  • MyPart1 8
  
  
  • MyPart2 8
  
  
  
  

Absolute File Names

It is
also possible to tell DriveWorks not to use the original file name at all, for
example:

• MyAssembly [="*A-"
  & DWSpecificationId]
  
  
  
  • MyPart1 [="*P1-"
    & DWSpecificationId]
  
  
  • MyPart2 [="*P2-"
    & DWSpecificationId]
  
  
  
  

Would
create the following for a specification numbered 8:

• A-8
  
  
  
  • P1-8
  
  
  • P2-8
  
  
  
  

Prefixed File Names

The
other possibility is to tell DriveWorks to use the result of the rule as a
prefix, for example:

• MyAssembly [="*"
  & DWSpecificationId & "*"]
  
  
  
  • MyPart1 [="*" &
    DWSpecificationId & "*"]
  
  
  • MyPart2 [="*" &
    DWSpecificationId & "*"]
  
  
  
  

Would
create the following for a specification numbered 8:

• 8 MyAssembly
  
  
  
  • 8 MyPart
  
  
  • 8 MyPart
  
  
  
  

If you
have any questions about this process, or need any further assistance in
accessing your license keys - just visit the DriveWorks Pro Helpfile
or email us and we will be able to help you out! 

Jim TeDesco
Marketing Manager
Computer Aided Technology, Inc. 

SolidWorks Then and Now: 2d to 3d

In SolidWorks 2001 plus we introduced 2d to 3d functionality. Here is a quick run through on how it works. The following is an updated version of the “what’s new” document from September 2001.

 The 2D to 3D tools facilitate converting a single sketch into a set of separate sketches, each positioned and oriented as required to create a 3D model. The tools fold up the 2D sketch as if it were a piece of paper. When you import a drawing for conversion, you specify which portions of the drawing are the sketches for the front view, right view, and so on. You can also create auxiliary sketches that are not parallel to the principal view planes. Hidden lines, which are dashed lines in an imported drawing, are construction lines.

You use the 2D to 3D tools to align sketches with each other, with edges and vertices of a part, or with the origin. You can align sketches before you use them to create a part, or you can align sketches during the part construction process. The following tools are used to convert a single flat sketch into separate sketches in their correct position and orientation. For example, you select all the sketch segments that belong to the top view and click the Top tool to create a new sketch in the top view orientation.

1.Go to File, Open.

2.Change the file type to DWG or DXF

3.Click Open

4.Select the Import to a new part as 2D Sketch

5.Set Units of import accordingly

6.Customize layer import, turn off unneeded detail

7.Click finish

8.Set the origin for the sketch by selecting a single point on the sketch and clicking on align sketch icon.

9.Remove the detail view by box selecting around it and pressing the delete key on your keyboard.

10.Now it’s time to split out the views. Box select the front view and click the front view icon on the 2d to 3d toolbar

11.Now repeat this process for the Top and Right side views.

12.Now that views are folded we will do a little alignment with the align command on the 2d to 3d toolbar.

13.You will first select the line segment that will be moving from the top view. Second you will select a segment on the front view so you can align the top view segment to it. Then click the align sketch icon.

14.Repeat this procedure for the Right view sketch and front plane. Select an segment on the right view sketch first followed by the front view sketch.

15.Now extrude the front view sketch.

16.Change the End Condition to the up to vertex option and select a vertex on top value that corresponds to the depth you need.

17.(optional) Click in the selected contours dialog and add the selections for the pivot hole and slot to remove them from the extruded area.

18.Let’s remove the finger tips by using the right view sketch as a cutting tool. Start the cut extrude command and change the End Condition to Through All, and finish the command.

19.By checking on the Flip side to cut. And click OK. Enjoy you 3d model.

Bob McGaughey, CSWE

CATI

How to Find Your DriveWorks Solo License Keys

When you register for the DriveWorks Solo evaluation you are issued a temporary license code. This is sent to the email address you have supplied. Then, when you choose to purchase DriveWorks Solo a permanent code is also created and sent to the same email address. You can also view your license keys on the DriveWorks Solo website, this is how:

1. Go to www.driveworkssolo.com and click on the top left side of the home page to log onto your account.

2. Enter the details you supplied when the account was created in the Login to DriveWorks Solo sections (there are links to resend password or username if you have forgotten this)

3. Click Login,. Click View your license keys at the top right of the page.

4. All license keys assigned to you will be listed under the Your DriveWorks Solo License Keys section

5. If you have any questions about this process, or need any further assistance in accessing your license keys - just visit the DriveWorks Solo Helpfile or contact us.

 

Jim TeDesco
Marketing Manager
Computer Aided Technology, Inc. 

How to set 3DQPress Command Tabs in SolidWorks

Welcome to 3DQPress “how to setup”. The following blog will walk the new as well as current customers "How To" set up the SolidWorks Command Manager with 3DQPress Tabs. This blog is broke out in 2 sections, New Instalation and Update Instalation for ease of use.

New Installation

1. Start SolidWorks.

2. Select the Tools\Add-Insof SolidWorks.

3. At the bottom of the SolidWorks Add-Ins manager you will find the 3DQTools software that you have loaded, check both boxes so the software will auto-load when starting your next session of SolidWorks.

4. Close the Add-Ins manager.

5. 3DQPress will prompt “Do you have a Hardware Dongle”

a. “No” means you are running a TEMP code, continue by copy and paste the temp registration code that was sent to you by 3DQPress representative.

b. “Yes” means you have receive your hardware dongle, continue by plugging the dongle into one of your USB port, wait for the hardware to acknowledge the new dongle and download the driver software if needed. Copy and paste the serial number then select UPDATE tab, continue by copy and paste the registration code then select UPDATE tab, then close.

6. Once the software has loaded and the registry is complete you will see the 3DQPress Options menu, this shows the paths to the currently loaded files.

7. After selecting OK to complete the Add-Ins loading, the 3DQTools software has will be displayed in the SolidWorks top ribbon.

8. Close SolidWorks to find the Commands Manager Registry tab on your desktop.

9. Double click on “3DQP ComTabs.reg” and say “Yes” when asked to update the command manager tabs. Note: If a “3DQP ComTabs.reg” is not on your desk top skip to #12

10. Delete the “3DQP ComTabs.reg” Part and Assembly files from your desktop then start SolidWorks again, after opening a Part or Assembly file you will see the new 3DQPress Commands Manager Tabs.

11. If, when loading the software you are prompt “Unable to register the DLL/OCX: RegSvr32 failed with exit code 0x3” Windows denied the registration of 3DQP.

12. Contact your 3DQPress representative at 920.268.1721 or email Ronf@callsts.com .

Update Installation

1. Start SolidWorks.

2. Start a new Part file.

3. Right click on Command Manager Tabs and select Customize Command Manager.

4. Right click on the 3DQuickPress Command Manager tabs and select Delete to remove current 3DQPress Command Tabs.






5. Select File\Save the part file to your desktop.

6. Click OK to exit.

7. Start a new Assembly file.

8. Right click on Command Manager Tabs and select Customize Command Manager.

9. Right click on the 3DQuickPress Command Manager tabs and select Delete.

10. Select File\Save the Assembly file to your desktop.

11. Click OK to exit.

12. Close all documents and exit SolidWorks.

13. Double click on “3DQP ComTabs.reg” and say “Yes” when asked to update the command manager tabs. Delete the “3DQP ComTabs.reg” and Start SolidWorks again, you should see the new 3DQPress Commands Manager Tabs. Note: If a “3DQP ComTabs.reg” is not on your desk top skip to #16.

14. Delete the “3DQP ComTabs.reg” Part and Assembly files from your desktop then start SolidWorks again, after opening a Part or Assembly file you will see the new 3DQPress Commands Manager Tabs.

15. If, when loading the software you are prompt “Unable to register the DLL/OCX: RegSvr32 failed with exit code 0x3” Windows denied the registration of 3DQP.

16. Contact your 3DQPress representative at 920.268.1721 or email Ronf@callsts.com .

How to Open SolidWorks 2013 Files in SolidWorks 2012 SP5

Throughout the years, almost all of our customers have asked at one time or another, "Can I open files from the newest version of SolidWorks into a previous version?" The answer has always been, "No. The latest version of SolidWorks uses newer technology that is not compatible with the older technology of previous versions of SolidWorks." As a result, customers have had to be careful when they upgrade to make sure that they stay compatible with their customers, suppliers, and internal teams. Well, the most asked for enhancement is finally here!

Starting with SolidWorks 2013, SolidWorks files are backwards compatible! With previous release interoperability, you can collaborate using a mix of SolidWorks 2013 and SolidWorks 2012 (SP5). Files can be opened directly and associativity is maintained. That's right. You do not have to export and import files!

HOWEVER... You Always Have to Read the Fine Print

Future version files appear in read-only mode when opened in the previous release. However, once you upgrade to the next version of SolidWorks, all the FeatureManager design tree data is available. SolidWorks 2013 files have reduced functionality in SolidWorks 2012 Service Pack 5. SolidWorks 2013 files will not have most FeatureManager design tree data when opened in SolidWorks 2012 Service Pack 5. Any actions that require FeatureManager design tree data cannot be performed with a SolidWorks 2013 document open in SolidWorks 2012 Service Pack 5.

You can open SolidWorks 2013 parts and assemblies using SolidWorks 2012 Service Pack 5. Although this is a great step forward, there are some limitations to be aware of. Starting with SolidWorks 2012 SP5, you will be able to open a future version file. This will be the same for future releases as well. For example, you will be able to open SolidWorks 2014 files in SolidWorks 2013 Service Pack 5. But... Backwards compatibility is only supported between consecutive releases. So, you will not be able to a SolidWorks 2014 file in SolidWorks 2012 SP5.

Further, here are some things that YOU CAN and CANNOT do in SolidWorks 2012 SP5:

1. Once a SolidWorks 2013 part or assembly file is open in SolidWorks 2012 SP5, YOU CAN view configurations, use the Measure tool, view Mass Properties and Custom Properties, and view Materials. YOU CANNOT edit the SolidWorks 2013 part or assembly in SolidWorks 2012.

2. YOU CAN work with SolidWorks 2013 parts and subassemblies in a SolidWorks 2012 assembly. YOU CANNOT edit mates or components in the SolidWorks 2013 subassembly.

But, in a SolidWorks 2012 assembly, YOU CAN:

• Mate the SolidWorks 2013 component or subassembly to SolidWorks 2012 or SolidWorks 2013 components.

• Add a Bill of Materials that includes SolidWorks 2012 and SolidWorks 2013 components.

• Suppress and unsuppress SolidWorks 2013 components.

• Create a drawing of the SolidWorks 2012 assembly that includes both SolidWorks 2012 and SolidWorks 2013 components.

• Use interference detection when mating SolidWorks 2013 and SolidWorks 2012 parts.

• Mirror and pattern components from SolidWorks 2013.

• See and reference default planes and origins of the SolidWorks 2013 part or subassembly.

There are new options in SolidWorks 2013 for part and assembly models that contain configurations. Because of these new options, you must rebuild and save data for each configuration that you want to be available in SolidWorks 2012 SP5.

3. YOU CANNOT open SolidWorks 2013 drawings in SolidWorks 2012 SP5.

YOU CAN create drawings of SolidWorks 2013 parts and assemblies in SolidWorks 2012 with some limitations. YOU CANNOT insert model items or access FeatureManager design tree data such as weldment cut lists and weld beads.

In conclusion, SolidWorks has tried very hard to provide the functionality that its customers request. SolidWorks 2013 does allow backwards compatibility with SolidWorks 2012. Because this new feature certainly has its limitations, it is still going to be up to the individual user and company to decide when the best time to upgrade is. Hopefully, though, this will help everyone decide to upgrade much sooner and take advantage of the latest and greatest version of SolidWorks.

Neil Bucalo

Technical Analyst

Computer Aided Technology, Inc.

Why are some of my drawing files so large?

You may notice sometimes you come across a drawing that is
very large in size, Sometimes larger than the part or assembly it is referencing.
What is the cause? The main reason I have found is due to views
being draft quality…But isn’t draft quality lower than high quality? – The answer
is actually no.

The high quality drawing view image is a vector
graphics image, also known as SVG format (Scalable Vector Graphics).  The
draft quality drawing view image is a raster graphics image, which is just like
a regular Bitmap.  The Bitmap files are much larger in size because the
image consists of pixels.  The vector graphics are smaller because the
image consists of lines.  The only downside of the vector graphics is that
those lines have to be calculated in order to produce an image.  That's
why it takes a longer time to calculate the high quality vector graphics
drawing view.

Shaded views also increase the file size because they have to be
represented by raster graphics.



Examples of an SVG and Bitmap of the same image are attached.  The SVG is
only 4.19 KB and the Bitmap is 2.53 MB (2,590 KB) so there is a very big
difference. 

How do you tell if your view is draft quality? – Cursor over your view,
you will see the draft quality icon appear.

So why do you have draft quality views? It can be a few reasons. First,
make sure you have your system options set to high quality views

The other reason you may have draft quality is that is actually may be
due to bad model geometry. Check
on the model or assembly that the drawing is referencing.

This can be accomplished under the tools/check menu.

 Once the geometry issues have been corrected this will allow you to switch back to high quality views.

SolidWorks 2013 SP0.0 is Now Available for Download

While working in the SolidWorks Customer Portal today the CATI Support Techs noticed that as of 10/9/2012 SolidWorks 2013 SP0.0 is available for download.

If you have an active Subscription Service for SolidWorks all you need to do is Login to the SolidWorks Customer Portal and proceed to the Downloads page and set the Version to 2013.

Enjoy working with 2013 and you can get more information on SolidWorks 2013 from CATI's website.

Josh Altergott

CATI Support Manager

Modeling beyond the limitations

 

Let’s take a look at moving around a modeling roadblock. We
have all had a feature for whatever reason doesn’t work even though there seems
to be no reason why not. Some times SolidWorks models may have issues that seem
to be trivial, in this example there is an overlapping cut sweep that won’t calculate.

This message from SW was not helpful in any means:

 

The underlying issue here is that at some point the profiles
overlap at an exact tangency. As many of you know that even putting two holes
into a part that touch at an exact point of tangency will have an error.
SolidWorks can’t decide if there should or should not be material at that very
point. The result is a geometry error as seen here:

 

 

 

 

 

Or attempting with selected contours give this more familiar message:

 

 

 

 

So in this example we have the profile section changing
position along a helix that is changing pitch. This at a spot along the curve
will result in a tangency issue. Although the error message doesn’t tell us
what the error is, there is at least one way to still make this work knowing
what we do about the software.

Here we take the initial helix and duplicate it.

 

Then we duplicate the profile as well and split it into two
profile sketches that deal with only part of the cut at a time. SolidWorks
allows each cut to be created as separate features.

 

Even though they still touch, SolidWorks doesn’t error because it is only dealing with
one cut at a time and doesn’t create a geometry calculation issue with
self-intersecting passes.

 

Finished results:

I am sure there are other solutions but this is not too painful to figure out.

John Van Engen
CATI Tech Support