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Issue: Sketch > Pattern tools only propagating some of the selected geometry

karl_mochelkarl_mochel Member Posts: 38 ✭✭
in Community Support
The selection...


The Linear Array tool is only propagating the top line, and there is no alert/message - Expect something like "Cannot work on all of the selected entities because..." so that I know how to fix the problem.



https://cad.onshape.com/documents/a84e4a5ca67dab8f05226f87/w/da2e02b1cfc363b6ee32f4f9/e/6c7d201699756e39298e6128?renderMode=0&uiState=65f77088dd73006b5a13900f

Answers

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    nick_papageorge073nick_papageorge073 Member, csevp Posts: 675 PRO
    It looks like OS cannot pattern a spline within sketch. I just tried it with several simple sketch splines. It looks like you found a workaround to pattern the solid instead. (that's usually preferred, anyway).
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    S1monS1mon Member Posts: 2,384 PRO
    edited March 18
    You can create a composite curve and pattern the curve “part”, but you can’t pattern a spline within a sketch.

    In this case, I agree with Nick, patterning a part is probably the most robust solution.
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    karl_mochelkarl_mochel Member Posts: 38 ✭✭
    I want to revolve the resulting profile, so I would have to extrude it, part pattern it, and then extract the profile I want to revolve. That is quite obtuse. Splines should be sketch patternable…
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    S1monS1mon Member Posts: 2,384 PRO
    How many copies do you want to pattern?

    What is the end goal shape you’re trying to achieve? 

    Do you need to be able to easily modify the number of copies parametrically? 

    There may be many other ways to approach this. 
  • Options
    eric_pestyeric_pesty Member Posts: 1,524 PRO
    karl_mochel said:
    I want to revolve the resulting profile, so I would have to extrude it, part pattern it, and then extract the profile I want to revolve. That is quite obtuse. Splines should be sketch patternable…
    I agree that sketch splines not being patternable isn't great... However you absolutely do not have to extrude anything if you want to revolve: just do one revolve with your sketch as-is and pattern the revolve feature... It's better practice to pattern features or parts than use sketch pattern anyway and in this case it isn't any more work... 

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    karl_mochelkarl_mochel Member Posts: 38 ✭✭
    This is what I am trying to create. This version of it cannot be thickened. While it is patterned it does not join and I believe it is causing Thicken to fail.

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    karl_mochelkarl_mochel Member Posts: 38 ✭✭
    S1mon said:
    How many copies do you want to pattern?

    What is the end goal shape you’re trying to achieve? 

    Do you need to be able to easily modify the number of copies parametrically? 

    There may be many other ways to approach this. 
    1) Variable depending on the size of the stock.
    2) See previous post - a wavy disk.
    3) Yes.
    4) OK... Figuring out one different then I thought up is the problem...
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    S1monS1mon Member Posts: 2,384 PRO
    edited March 27
    I was able to pattern the curve sketch along with a revolve of a single cycle of the wave, merging each instance of the pattern. This  created a single surface which can be used for a thicken or split operation. The trick is that I had to cheat in the center. I made a very small (0.001" radius) disc to which I then merged all the wave rings. This acts as a starter body to add to with the pattern, and it also seems to solve for a weird bug where I couldn't revolve and add a single wave in the center (I had tried to pattern from the outside in, using a flat ring as a starter body on the outside - that worked for all the waves except the center one. So I started the pattern from the microscopic disc in the center, and all is good).



    https://cad.onshape.com/documents/42789d61df0e6a7371d630f1/w/5bd04f8e1638ae8f16c1c293/e/a91ee328db610276a462c51a
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