lofting from a sketch gets screwed up by other sketches on the same plane

Comments

• eric_pesty Member Posts: 1,836 PRO

  April 18

  Can you expand the "face of sketch1" selection the loft, I wonder if you somehow ended up with the face of the solid in there as well...

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• _anton Member, Onshape Employees Posts: 395

  April 18 edited April 18

  The problem (or at least one of them) is that loft doesn't support faces with inner loops (mouse over the red feature dialog header), and the red shapes are those loops.

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• stuart_robinson Member Posts: 37 ✭✭

  April 18

  @eric_pesty when i tried that earlier it didn't seem to show anything useful. just said "Face of Sketch 1" again i think

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• eric_pesty Member Posts: 1,836 PRO

  April 18

  @_anton
  He's saying he only selected sketch1 which doesn't have any internal regions. But the red preview does suggest there is a face of the solid selected in there somehow.
  
  You also only have one selection for the loft, did you try picking another profile for the loft to see if it solves it? It could just be a graphical glitch (refreshing should also clear that if that's the case).
  
  We might be able to figure what's going on if you share a link to your doc...
   

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• stuart_robinson Member Posts: 37 ✭✭

  April 18

  ok i think i figured out what's happening.  example here
  
  when you create a "New sketch" from the surface of a Part, this new sketch becomes cursed forever by the ghost of the Part's perimeter in that plane
  
  i'm worried that this is a Feature since i could imagine it could be useful at times if someone is aware of the behavior, but it's caused headaches for me before, and seems distinctly bad.  since i feel like you should be able to see that something is a Sketch, and understand everything about the Sketch from the Sketch itself.  without needing to remember hidden artifacts lingering around as side effects from the specific way that Sketch happened to be created.
  
  for example, here i have two sketches.  Sketch 1 is clearly a circle, and Sketch 2 is clearly a rectangle
  
  
  
  now i'd like to loft my rectangle:
  
  
  but i cant.  because there's an undead circle hiding inside it that i cant get rid of,
  
  because of how the rectangle was created. (by creating a "New sketch" from the other end of an extrusion of the circle sketch)
  
  
  
  
  
  https://cad.onshape.com/documents/a82f03eed8bf29ae67e2de8e/w/2e833e275c987e44d42fc3d0/e/d854c39f0f00246eaa8f19d4
  

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• stuart_robinson Member Posts: 37 ✭✭

  April 18

  so actually now that i understand how this works, i've been able to use it to solve a lot of other problems and it's really powerful and useful.  but i do still think it's a bad design.  unintuitive/cryptic 

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• eric_pesty Member Posts: 1,836 PRO

  April 18

  stuart_robinson said:

  so actually now that i understand how this works, i've been able to use it to solve a lot of other problems and it's really powerful and useful.  but i do still think it's a bad design.  unintuitive/cryptic 

  You can also turn it off in the sketch dialogue using the "disable imprinting" checkbox...

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• stuart_robinson Member Posts: 37 ✭✭

  May 2

  oh wow TIL "imprinting", thank you @eric_pesty!

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• nick_papageorge073 Member, csevp Posts: 804 PRO

  May 2 edited May 2

  Disable imprinting should be clicked on by default. My very strong opinion:) I've purposely wanted it maybe 2 times in 3 years. Every single other time I have to click that checkbox. And when my co-workers don't click that box, it becomes a mess.
  

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• glen_dewsbury Member Posts: 757 ✭✭✭

  May 2

  nick_papageorge073 said:

  Disable imprinting should be clicked on by default. My very strong opinion:) I've purposely wanted it maybe 2 times in 3 years. Every single other time I have to click that checkbox. And when my co-workers don't click that box, it becomes a mess.
  

  Cast a vote here.
  https://forum.onshape.com/discussion/comment/101644#Comment_101644
  

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