Welcome to the Onshape forum! Ask questions and join in the discussions about everything Onshape.

First time visiting? Here are some places to start:

  1. Looking for a certain topic? Check out the categories filter or use Search (upper right).
  2. Need support? Ask a question to our Community Support category.
  3. Please submit support tickets for bugs but you can request improvements in the Product Feedback category.
  4. Be respectful, on topic and if you see a problem, Flag it.

If you would like to contact our Community Manager personally, feel free to send a private message or an email.

Using point pattern in asemblies

Hi,
I need to use @cody_armstrong 's point pattern in an assembly to replicate parts.
Did anyone figure out how to?

Comments

  • MBartlett21MBartlett21 Member Posts: 1,554 EDU
    @Benjamin_Dellal
    You can't use it in an assembly. You can vote up this improvement request for custom features in assemblies:
    https://forum.onshape.com/discussion/9663/featurescript-for-assembly#latest
    MB - I make FeatureScripts: view FS (My FS's have "Official" beside them)
  • cody_armstrongcody_armstrong Moderator, Onshape Employees, Developers Posts: 188
    @Benjamin_Dellal As @mbartlett21 mentioned FeatureScript features cannot be used in the assembly. If you post an example or give us more details we may be able to help find an alternative.

    Have you tried the replicate command in the assembly?
  • Benjamin_DellalBenjamin_Dellal Member Posts: 8 PRO
    My problem is the following:
    I have an assembly that is using 100x the same part. I am currently in the process of migrating our CAD model from our Catia platform to Onshape.
    In Catia, I am cheating: I made a single part, in a single body and used "user pattern" to replicate it based on a point cloud that sets their positions. I manually correct this on the BOM later. 

    I can not find any good way to do the same in onshape. 
    • I cannot import my sketch containing the points. Points just do not show up. So, I cannot use point pattern in Onshape.
    • Importing the catia model as is, Onshape just makes 100 different parts out of the 1 original part

  • tim_hess427tim_hess427 Member Posts: 119 PRO
    When you've tried to import the sketch - is that using the DXF/DWG import tool in the sketch environment? It seems odd to me that the points wouldn't show up. Maybe its a bug?
  • TimRiceTimRice Member, Moderator, Onshape Employees Posts: 204
    edited November 2018
    What format are you attempting to bring the sketch into Onshape? Only dxfs can import sketch geometry. If you can export just the unique part from Catia as well as the points in a dxf this should be a simple job to setup in an Onshape assembly. The BOM would be correct as well.

    Workflow: Import catia part into part studio. Import dxf into a second part studio, add a mate connector at each point. Bring the sketch into an assembly and mate part to mate connector at each sketch point.
    Tim Rice | User Experience | Support 
    Onshape, Inc.
  • Benjamin_DellalBenjamin_Dellal Member Posts: 8 PRO
    Thanks guys.
    I found a decent work around for now:
    The part that mates to all 100 parts has locating holes for these. After constraining one instance, I can use the replicate command as if my parts were screws. 

    But, I still need to find a better way and using the point pattern in as assembly would be ideal.
  • TimRiceTimRice Member, Moderator, Onshape Employees Posts: 204
    Currently FeatureScript cannot be used in assemblies and only in part studios
    Tim Rice | User Experience | Support 
    Onshape, Inc.
  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 2,197
    @Benjamin_Dellal depending upon how you mate your first part, you should be able to select “all edges on face” (or similar) in Replicate to do it all in one go. 
    Neil Cooke, Director of Technical Marketing, Onshape Inc.
Sign In or Register to comment.