Subtract Problem 1

[jptooldie]

Hi

having a problem with the subtracting. trying to cut the green mother block by using the white cylinder. somehow it couldn't be cut until the diametre was reduced to 16 or less. but i do need 20mm diametre

attached is the file

thsnks

 

[cowski]

I changed the diameter of the white circle to 20 mm and it updated no problem. What type of error are you getting?

 

[jptooldie]

Unable to perform Boolean.


can you upload the updated part?

thanks

 

[JohnRBaker]

I tested this using NX 6.0.5.3 (no MP's) and it worked fine (edited the 'white' circle from 16 mm to 20 mm).

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[jptooldie]

I'm a bit frustrated here. Tried again. Still a no go. Can someone please upload the part after subtracting?

I made that diametre to 19. but failed at 19.5. And it became OK when I increased that diametre to 27.

Thanks

 

[JohnRBaker]

I would upload the part which I successfully edited the 'white' circle from 16 mm to 20 mm using NX 6.0.5.3. However, I'm working from a hotel in Minneapolis with a very slow WiFi connection which keeps timing-out before the upload is complete. I won't be able to upload the file until Monday when I get back into my office in SoCal.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[MARINA221171]

NX 7.5.1.5

Same problem "Unable to perform Boolean"

 

[jptooldie]

thanks John

 

[uwam2ie]

I have looked at the problem, it is not a nx problem,
it is a problem with the contour faces do a examine geometrie with 0.01 tolerance you wil find face problems on the contour face in the area you want to do the boolean

 

[jptooldie]

i had same problems in NX2 and NX4. but never had this kind of problem that I couldn't fix in NX6. And it happened a lot more frequently in NX6. yeah i know i had quite some complaint over NX6. This is ridiculous!!! It's supposed to make the design easier and quicker. The reality is after a few monthes on NX6 I'm still struggling.

Anyway is it possible to fix it in NX6? - this is the ultimate question.

 

[uwam2ie]

ok I have fixed the problem partially, I have done the workaround on two areas, look at it( tiny faces) , I think you should do this on the initial imported contour faces.

 

[uwam2ie]

another solution using heal geometrie with 0.03 tolerance on the linked body (exported the liked body-> heal geometry in the exported part-> copied result and replaced the linked feature)

 

[jptooldie]

Thanks. Can you please show me how to do the heal? I was looking for the command. But nowhere could i find it.

 

[uwam2ie]

look at file->export->Heal...

 

[cowski]

Here is the file that I edited. Note that I am currently running NX 6.0.3.6.

 

[JohnRBaker]

Here's my results:

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[jptooldie]

So John is there any easier way to fix this? (By the way feature 15 is the actual problematic one, not 14. That's why John and cowski didn't catch the right one. My fault. I turned the feature off).

Before NX6 this problem happened. But it's really easy to fix.

 

[JohnRBaker]

OK, now I see what the problem is. However the only way to fix this is to perform a 'Heal Geometry' which will remove all the parametrics, but at least we know why this is happening.

I ran an...

Analysis -> Examine Geometry...

...and noticed that there is a 'Consistency' problem with a face which is near where this subtraction is taking place. If the circle is set to around 19mm everything is fine, but as you get to around 19.2mm it starts to creap onto the face with the inconsistent topology and thus the Boolean failure occurs. So I ran your part through the 'Heal Geometry' utility and it fixed the model removing the inconsistency. I then recreated the tool body extruded from from 20mm dia arc and now it subtracts just fine.

Unfortunately I can't upload the new model until Wednesday as I'm currently out of the office and don't have access to a highspeed network.

However you can try this yourself. What you need to do is delete Extrude(15) but leave the 20mm arc in place. Now go to...

File -> Export -> Heal Geometry...

...and select the 'Select from Displayed Part' option and accept the default name (the system will create a new part file with the suffix '_hg' added to the current name). Once complete, open the new part file and using the existing 20mm arc create a new extrude feature and subtract it. It should now work fine.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[JohnRBaker]

as promised, now that I've got the band-width, here's that cleaned up model with the extrude.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.