Boolean operation on solid failed?
Boolean operation on solid failed?
(OP)
Hi all, I've been trying to use the inter-part copy from my assembly to remove one object from another. I kep getting an error that reads "boolean operation on solid failed" Any ideas as to why?
By the way, this post started here for reference:
http://www .eng-tips. com/viewth read.cfm?q id=218570& amp;page=1
By the way, this post started here for reference:
http://www





RE: Boolean operation on solid failed?
First, you do want the inter-part copy to be surface geometry. if it wasn't, then the solids would join into a single part and you wouldn't have any surfaces (or body geometry) to subtract. You would end up having to figure out a way to to a cut feature. That's not what you're after.
Look closely at your geometry. Do you have a cylindrical surface mating up with a planar surface between the two bodies? When you subtract this type of geometry out, you end up with a line-to-line contact. That contact is neither solid, nor surface, and therefore SE can't figure out what to do with it but give you an error.
Also, when dealing with surfaces in SE, surfaces whos open edges are in intimate contact with a solid body, or are slightly below the body (don't extent through), often result in an error because SE doesn't know how to remove solid geometry from the surface. If you have a closed surface body, this shouldn't be an issue. This only occurs with surfaces that have open edges (non-stitched). If you have this condition, use the surfacing tools to extent the open edge of the surface past the solid body.
If your surface body has hollows in it, then you also run in to a multi-body part error because SE doesn't want to leave material floating inside of another solid during a Boolean operation. You may need to prep your surface body to get rid of any hollows or voids.
--Scott
http://wertel.eng.pro
RE: Boolean operation on solid failed?
bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.
RE: Boolean operation on solid failed?
RE: Boolean operation on solid failed?
I had to post it on my personal site. For some reason Engineering.com wouldn't work.
Here is the link: www.mrdeadman.com/tire_mold.zip, Just copy and post it into your browser.
Version 18 or 19 will do.
Thanks
RE: Boolean operation on solid failed?
no problems neither with V19/Sp11 nor V18/Sp12. Just
open the out then insert the tire as construction and
finally boolean subtract tire from outer -- that's it.
Maybe you V18 needs an upgrade your current patch is
SP3. attached file is V18 and features rolled back, just
place it in same folder along with the tire
dy
RE: Boolean operation on solid failed?
RE: Boolean operation on solid failed?
Here is a link to the file. It's pretty big (around 20mb).
http://www.mrdeadman.com//main_assy.zip
I think it has something to do with the conversion. The file was originally ProE and the gave it to me as a .sat.
Thanks again.
RE: Boolean operation on solid failed?
RE: Boolean operation on solid failed?
When you open the Pro/E or Sat file, does it come in as a single solid body feature, or is it a surface feature (or a bunch of features)? I have a feeling that the translated geometry has some import errors making it a surface body and that results in an error during the Boolean operation. You'll have to interrogate the translated geometry and look for any errors.
--Scott
http://wertel.eng.pro
RE: Boolean operation on solid failed?
SE is able to read native Pro/E files (part/asm) V19 up to
WF2 (V20 WF3). When that's not possible ask for a STEP file
as it's more reliable than a .sat which is also version dependend.
I once, however got a STEP file that could not be converted
due to the internal accuracy. The accuracy was decreased to
0.002mm and then I was able to convert it. Don't ask where
and when in Pro/E this has to be done (general or for export
only ??)
dy
RE: Boolean operation on solid failed?
www.mrdeadman.com/main.zip
Hopefully that one works... Let's just say its off a little bit like dy said. How can I fix that?
Thanks again guys.
RE: Boolean operation on solid failed?
RE: Boolean operation on solid failed?
I tried taking the inner curved profile out of the revolved solid on the outer part. When I did this the boolean worked OK. Sectioning the model showed that the tyre surface and the sketch for the inner profile are coincident.
bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.
RE: Boolean operation on solid failed?
http:
Second Image -
http:
Third image -
http:
bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.
RE: Boolean operation on solid failed?
Thanks again.
RE: Boolean operation on solid failed?
bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.
RE: Boolean operation on solid failed?
Only problem now is that this part file is upwards of 60mb. Anyway to compress that a bit by removing some feature without actually losing them?
Thanks for everyones help on this!
RE: Boolean operation on solid failed?
(I did wonder if the problem was that you weren't spelling "tyre" correctly
bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.
RE: Boolean operation on solid failed?
Tyre? Isn't it "tire" or did I miss something?
RE: Boolean operation on solid failed?
The other "tire" is what happens to you as you work hard.
Did you follow my method ? - it could make a difference on file size.
bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.
RE: Boolean operation on solid failed?
RE: Boolean operation on solid failed?
As far as I'm concerned this is now a closed issue, thank you all for your help. Hopefully this thread will help others in the future.