I'll leave the title as repetitive and as generic as the stupid message that is showing up
There is this (typically unhelpful) SPR:
Also, the 'problem' is somewhere in the sketch itself. Specifically, the radii. If you remove all the radii, the revolve works:
If you add back any of the radii, it fails again.
If you make a surface revolve, it works:
You can even generate a planar surface at each end and then knit it all together as a solid:
The sketch continues to cause the same problem even if it is copy-pasted to a new document.
I simplified the sketch down to a few lines and still see the behavior. The sketch now looks like this:
If I increase the .21875 dimension by 0.000001, the feature fails. But the failure is also dependent on the other dimensions. If I decrease the 1.00 dimension to 0.5, the .21875 dimension can be made as large as I like. Removing the radius makes it behave no matter what the dimensions. If I recreate the above geometry from scratch in a new sketch, the problem doesn't happen. I suspect that the original sketch was imported from some other system and isn't quite right from SOLIDWORKS' perspective.
Lucas, how about a blind extrusion?
Thank you for the proposition
As presumable, a blind revolve certainly "works" ("bypasses" the bug)
But this plane is a restraint for this and many other features that come next
All of them must follow the plan, that might change
I got the same error message when I tried the same thing on SW2017.
An alternative method is to do a blind revolve at 45 deg. As also mentioned by John
I would believe because you're not revolving to a surface
This method always worked. Solidworks doesn't see difference between a face of a geometry and a datum, if both are planar
And I tried making a surface on that plane and revolving to this newly created plane. Nothing happens.
Is this what you are after?
I cannot open due to version difference, but tell me, how have you done it ?
Mike Lee (above) attempted the same on SW17 and stumped on the same issue
Lucas Silva wrote: Yes I cannot open due to version difference, but tell me, how have you done it ? Mike Lee (above) attempted the same on SW17 and stumped on the same issue
Lucas Silva wrote:
I have to wonder if something might have been "fixed" in 2018 . . .
I just popped it open, selected the sketch, selected Revolve, used the axis that was selected, changed to up to surface, selected the plane.
definitely weird . . .
how bout just create planar surface on the plane
thanks Todd didn't see that
I don't do Revolves much, but if you want it to look like the screenshot that Todd posted then don't you need to click on the "Change direction" icon? It looks like it's pointing the wrong way to get 45° of rotation. Or am I missing something?
It should work without reversing (the only difference would be a 315 degree turn).
But not even that happens...
Thank you for the input anyway
Lucas I tried this as well. "Should" be able to revolve to a plane, didn't work. I thought well maybe SW is not seeing the plane as a surface, so I created a surface on the plane, still didn't work. So I tried up to vertex and picked a corner of the new surface I created and that worked. I agree DOES NOT MAKE SENSE. Tom
I just tried this with a new part and was able to rotate to a surface with no problem, Go figure
Tom dunn wrote: I just tried this with a new part and was able to rotate to a surface with no problem, Go figure
Tom dunn wrote:
Now it is getting REALLY weird . . . there had to be an update to the code for this feature in 2018.
It IS a bug then !
Will try to mod the radii, as you suggest
It's probably the solution, since in past times I successfully created this same feature
You could link the Revolve angle to the plane angle through an equation.
Saves playing with the radius and everything is linked to the plane as intended.
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