Revolve Cut

[crizzo]

Howdy,
I'm creating a model and attempting numerous revolve cut features. Some of my attempts result in the error:
"Unable to create this feature because it would result in zero-thickness geometry."

Some portions of the revolve cut would indeed be exiting the model, and essentially "cutting air". I want it to do that though! Any thoughts? I'm tinkering with a few work-arounds now....

 

[SBaugh]

If your using SW03 or 04 you can uncheck merge bodies and it might work.

If you have a tangency when the cut is being made, then that would create an error like that.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[pipsqueek]

I have had this error if the sketch is not closed or has badly shared endpoints.
Check the revolve sketch for errors.

 

[Theophilus]

Also, you may want to let the sketch profile cut through more air and not be so literal (just in case you have a sketch line that would sweep the cut right over a model edge as it goes around). This will bring your thickness down to zero and SW doesn't know what you really want to do with that.

So anything that would otherwise be an exact cut meeting a model edge should be expanded to catch a little air on the way around to avoid this error.




Jeff Mowry
Industrial Designhaus, LLC

http://www.industrialdesignhaus.com

 

[crizzo]

Thanks for the tips..I think my desired revolve cut might be sort of "riding an edge" of a solid, and possibly getting some ambiguity. What is frusturating though is seeing SW preview the revolve cut nicely, but then refuse to fully execute when I click the good ol' green check mark.
I resolved the revolve (slight pun) by doing a couple of sweep cuts, instead. They seem to plow thorough anything!

 

[TheTick]

Tech note:

When a feature like a revolved cut is previewed, it is done with an entity SW calls a "temporary body" in API terms. This is the body the feature makes before SW attempts the boolean operation that unites/subtracts the temporary body.

The temporary body generates fine in the preview, and the error isn't encountered until the boolean operation is attempted.

"Great ideas need landing gear as well as wings."--C. D. Jackson

http://www.EsoxRepublic.com

 

[JNR]

Sounds like either your cut is producing something that results in a sharp point in the middle of the model (imagine two cones point to point) or it is coming out tangent to a surface, then back in again slightly. Either case could be trying to creat zero thickness goemetry. It will make points at the edge of a part, but not in the middle. Ie. it can't go down to nothing and back out again. The amount of fresh air cut is irrelevant.

I was - and he did. So at least I didn't get coal.....