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stephen2501-Visitor
1-Visitor
February 14, 2019
Solved

Fail to extrude to a surface

  • February 14, 2019
  • 2 replies
  • 4694 views

I am trying to create a solid feature by extruding to a spherical surface. The spherical surface is created by revolving. I found it always says fail to regen if the origin is inside the extrude sketch pattern. I tried different patterns, circle, triangle, etc. As long as the origin is inside the pattern, it always fails to regen.

 

succeed when the origin's outside the patternsucceed when the origin's outside the patternfail to regen when the origin's inside the patternfail to regen when the origin's inside the pattern

So far the only scenario it can extrude is the pattern in the sketch is a circle and it's concentric to the spherical. But if the pattern is a square or something else. It still fails.

 

it can only be done when the circle is concentric to the spherical surfaceit can only be done when the circle is concentric to the spherical surfaceit fails with a squareit fails with a square

I told this to my friend who's using NX(UG) at work. He created the feature with the same way I did with CREO. i.e. revolving a spherical surface, thickening the surface, then extruding to the surface (inner or outer). He showed me it just works

 

NX.PNG

 

Could anyone please help me solve this problem? 

 

Best answer by Patriot_1776

Creo has, since the beginning, split surfaces like that in half.  If that spherical surface is part of a solid, copy those surfaces and try selecting it as a quilt instead of a surface where you only get half.  There's been times I've been able to copy those split surfaces, then merge them into 1 and that solved it, but dunno if it works in creo 3.

2 replies

Patriot_1776
Patriot_177622-Sapphire IIAnswer
22-Sapphire II
February 14, 2019

Creo has, since the beginning, split surfaces like that in half.  If that spherical surface is part of a solid, copy those surfaces and try selecting it as a quilt instead of a surface where you only get half.  There's been times I've been able to copy those split surfaces, then merge them into 1 and that solved it, but dunno if it works in creo 3.

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stephen2501-VisitorAuthor
1-Visitor
February 14, 2019

Thank you so much! I selected the two half surfaces as a quilt and copy/paste it as you suggest. Now I can extrude any pattern to the copied quilt now. Yeeyyyyyyyyyyyyy!

 

Capture.PNG

 

But, just out of curiosity, if this is a result of half surface of the solid feature, why the extruding works when the circle is concentric as I showed in the 3rd pic above? 

Patriot_1776
Patriot_177622-Sapphire II
22-Sapphire II
February 14, 2019

It's buggy?  Who knows....

 

Glad it worked for ya!

 

Edit:  Actually, I didn't look at your model tree before.  Looks like you could re-order your extrude and pattern BEFORE the thicken of the bowl, and select that quilt to extrude to, then thicken the bowl afterwards.  That'll save a couple features and clean up your model tree.

 

If that solves it, please mark the solution solved for the others.

 

Grazie!

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23-Emerald III
StephenW23-Emerald III
23-Emerald III
February 14, 2019

I can't open your part (I'm on Creo 4) but I did create my own version and it seems to just work for me no matter where I put the extrude.

Try starting a new part, new sketches. Sometimes software will just glitch and refuse to do something that should be easy. I usually restart the program or redo the part or whatever. 

 

sphere.jpg

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