Boolean operation on solid failed?

[Superslinky]

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/viewthread.cfm?qid=218570&page=1

 

[swertel]

My guess is non-manifold solid geometry.

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

 

[beachcomber]

Could you post the 2 part files here ?

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

 

[Superslinky]

I will try, the one part is something like 30mb...

 

[Superslinky]

Ok, here are the two parts. If you line up the coordinates you'll see how it should intersect with one another. I want the outer ring to remain and the tire to be subtracted.

I had to post it on my personal site. For some reason Engineering.com wouldn't work.

Here is the link:

http://www.mrdeadman.com/tire_mold.zip,

Just copy and post it into your browser.

Version 18 or 19 will do.

Thanks

 

[donyoung]

Hi,

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

 

[Superslinky]

I did exactly what you said and it worked fine. I don't know what I was doing before that I kept getting failures but this time was a charm. Thank you for your help.

 

[Superslinky]

Ok, here's another problem. When I use the tire provided to me by the customer I still can't do it.

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.

 

[Superslinky]

Sorry, post is at

http://www.mrdeadman.com/Main_Assy.zip

 

[swertel]

I tired downloading the zip file. It comes across as invalid or corrupt.

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

 

[donyoung]

Hi,

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

 

[Superslinky]

Hey guys, the original file was a step and when brought into SE it is a single body feature. I though SE was compatible with ProE complete with a translator and everything if needed. For whatever reason it was unalbe to read the file. Maybe there is something wrong with the original. Where either of you able to open the other link I left up there? I posted another one at the same place but created it new in case the other was corrupted.

http://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.

 

[Superslinky]

Here is the original file. Let me know if either of them are good or not. Thanks again.

 

[beachcomber]

I've had a look at the files and I think the problem is coincident faces.
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.

 

[beachcomber]

First image -

http://files.engineering.com/getfil...7-02eb-4014-b52b-aacd2454944d&file=image1.jpg

Second Image -

http://files.engineering.com/getfil...e-89d0-42c5-9ab6-2623f48314eb&file=image2.jpg

Third image -

http://files.engineering.com/getfil...9-1ade-4ec4-85d1-0d0f185699a6&file=image3.jpg

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

 

[Superslinky]

I had a feeling it was that and even tried to move that inner curve a little bit in both directions to see if it would work. Right now I'm attempting to remove it entirely so that my outer profile become one big piece without the cutout in the middle. Seems to be working so far but we'll see. Once I get a solution I will come back and post it.

Thanks again.

 

[beachcomber]

Just beat you with my post - you are on the right track !

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

 

[Superslinky]

Well it worked. I first created the same profile I was looking for without the inside cutout. I then part copyied the tire in and boolean subracted it. I then used my original sketch and created a cutout of the inner profile leaving me with exactly what I needed.

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!

 

[beachcomber]

My version of "mold_upper_outer_fin.par" in V20 is 33.5MB
(I did wonder if the problem was that you weren't spelling "tyre" correctly )

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

 

[Superslinky]

Yeah, mine (V18) is huge. I need to put 2 halfs of these together in an assembly that has a ton of stuff already going on. Don't know if this little computer will be able to handle it... I thought about exporting it as a step or something similar and then re-opening it to drop some of the feature and still be able to edit the existing one if need be. That should drop around 20mb or so (I think).

Tyre? Isn't it "tire" or did I miss something?