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Why is rotating sketch of 1/2 a part 360deg OK but the whole part 180deg is "self intersecting"?

paul_beltranipaul_beltrani Member Posts: 5

You can rotate a sketch of a semi-circle 360 degrees about its axis to make a sphere.  However, trying to rotate a full-circle 180 degrees about a diameter line results in "Revolve would create a self intersecting part."   The problem is the same for any other revolution about a mid-point within the item e.g. cylinder or disk from a rectangle.


I'm not asking how to do this.  I understand that one works and the other does not so just do it the way that works.

My question is, what's different about the two that one works and the other does not?  Are they not conceptually the same?  What's happening within the application that you can't do either method?

Best Answer

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    S1monS1mon Member Posts: 2,549 PRO
    Answer ✓
    Whenever you use revolve, I'm pretty sure the face that you're revolving needs to all be on one side of the axis of revolution. If you try to revolve this (a circle with the revolve axis through the center) it fails:

    Less than 180 you end up (theoretically at least) with two orange wedges joined at a line. Parasolid (the geometry kernel of Onshape and many other CAD tools) can't handle solids which join at a line or point. You could create each of these wedges as separate parts, but not as one part in a single operations.

    If you rotate more than 180, you are in effect, creating stuff twice - or self intersecting. Some tools, like shell, have special algorithms to handle some level of self intersection, but revolve and sweep do not.



    You can do funky things like have more than one face that's being revolved in a single feature (here creating two parts), and they don't necessarily need to be on the same side of the axis.


    You can also do less than 360 and this will also work:

Answers

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    S1monS1mon Member Posts: 2,549 PRO
    Answer ✓
    Whenever you use revolve, I'm pretty sure the face that you're revolving needs to all be on one side of the axis of revolution. If you try to revolve this (a circle with the revolve axis through the center) it fails:

    Less than 180 you end up (theoretically at least) with two orange wedges joined at a line. Parasolid (the geometry kernel of Onshape and many other CAD tools) can't handle solids which join at a line or point. You could create each of these wedges as separate parts, but not as one part in a single operations.

    If you rotate more than 180, you are in effect, creating stuff twice - or self intersecting. Some tools, like shell, have special algorithms to handle some level of self intersection, but revolve and sweep do not.



    You can do funky things like have more than one face that's being revolved in a single feature (here creating two parts), and they don't necessarily need to be on the same side of the axis.


    You can also do less than 360 and this will also work:

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    paul_beltranipaul_beltrani Member Posts: 5
    Fantastic answer, that's exactly the info I was looking. Thank you.

    FWIW, There's a simple work-around that lets me both have the full sketch and do the revolve.  Simply add a line along the axis and select half the sections.  I'm sure that's common knowledge to most people here but I'm including it for the next person searching for similar info.




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    John_vd_WerffJohn_vd_Werff Member Posts: 65 PRO
    Onshape does have a nice hidden feature to add diameter dimensions to a 'half' sketch. 
    You need to have a construction line at the rotation axis. Add dimensions from your contour to the construction line and place the dimension outside the area to be rotated (to the right of the construction line in the sketch below), the dimension will show the diameter of the intended rotated part:


    From my experience with parametric CAD I would suggest to add chamfers (and fillets) as separate features.



    This makes the model more robust for design changes.

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    paul_beltranipaul_beltrani Member Posts: 5
    Nice.  Thanks for the tip.

    Re chamfers/fillets.  Understood and thanks.  I did it that way for the next part in the assembly  and you're right, it's much easier.



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