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.

Is it possible to keep the original orientation of a patterned feature during a Circular Pattern?

StephenG
StephenG Member Posts: 384 ✭✭✭
in Community Support
I have a linear slot feature that I want to pattern around a hole and maintain the orientation of patterned feature.

Here is what OS allows me to do....

But what this is what I desire...

I do not see an option within Circular Pattern feature control panel to effect it.
Tagged:

Best Answer

Answers

  • StephenG
    StephenG Member Posts: 384 ✭✭✭
    Yep, the Curve Pattern feature w/Keep Orientation option did the trick. 


    Now if I could only suppress individual occurrences of the pattern I would be one happy clam.

    Thanks!
  • mahir
    mahir Member, Developers Posts: 1,324 ✭✭✭✭✭
    StephenG said:

    Now if I could only suppress individual occurrences of the pattern I would be one happy clam.

    Thanks!
    You can also use the Point Pattern featurescript. It would let you place points wherever you want. And if you want to skip an instance, just don't place a point there.

    Point Pattern FS
  • StephenG
    StephenG Member Posts: 384 ✭✭✭
    The "Point Pattern" Feature Script I found (Cody Armstrong's) appears to be a work-in-progress; it is only capable of patterning part entities. It should be capable of patterning feature, surface, plane, and mate connector entities.

    Yes, I could have used it by...
    •  Creating the slot feature as a cutting tool part volume
    •  Creating a circular pattern of 8 points
    •  Use "Point Pattern" selecting just the desired points (locations)
    •  Use Boolean "Subtract" to create the slot features in the target part  
    but this a lot more work than just "suppressing" specific instances of a patterned entity (part, feature, surface, etc) within a "Circular Pattern" feature. Instance suppression within a pattern is something I have seen/used in other CAD products.

    Thanks for making me aware of this Feature Script. 
  • MBartlett21
    MBartlett21 Member, OS Professional, Developers Posts: 2,064 ✭✭✭✭✭
    You can use delete face or delete part to get rid of the instances you don't want
    mb - draftsman - also FS author: View FeatureScripts
    IR for AS/NZS 1100
  • StephenG
    StephenG Member Posts: 384 ✭✭✭
    Yes, using "Delete faces" is also a good suggestion to accomplish the result. I like this approach because it makes it easier to interpret/see design intent in the Feature list. I can rename the "Delete face N" feature name to "Remove unwanted pattern instances".  

    (Use "Create selection" w/"Tangent Connected" to speed the face section process for the slots to be removed.)

Categories