united extrude using sketch which touches the body in one point

[bataattila]

Hi,

I have to reproduce a model formerly made in Pro/E. I got stuck at one point, the picture says it all. The error message is simply 'unable to perform boolean'.

Is there a workaround for this NX limitation?

Thanks in advance:

Attila

 

[MickyV007]

Try a tolerance of 0.1 instead of 0.0254. Or is there a blend involved on some of the corners?

Best regards,

Michaël.

NX7.5.4.4 + TC Unified 8.3
Win 7 64 bit

 

[bataattila]

Unfortunately changing the tolerance didnt't help. This must be a common NX limitation, i've tried the operation on a sample body too, resulting the same error.

NX6

 

[cowski]

Try giving it a small negative start value so your tool solid has a small interference with the main solid.

http://www.nxjournaling.com

 

[bataattila]

I've tried that too with no success.
Thanks anyway!

NX6

 

[Walterke]

I must say that I have to agree with NX here. What you're asking is physically impossible.
Only workaround I would see is to leave a .0001mm gap on the line contact.

NX 7.5
Teamcenter 8

 

[cowski]

Offset the front face so you don't have that line to line contact, then use replace face to match the existing face.

http://www.nxjournaling.com

 

[bataattila]

I can see that, but in proE this method was used, so my modell will not be identical with the original.
maybe that much difference wont be a trouble; but then again, I thought there is a known workaround.

NX6

 

[MickyV007]

Maybe a strange a solution, but instead of Unite Boolean that piece, try Subtract the other side?

Best regards,

Michaël.

NX7.5.4.4 + TC Unified 8.3
Win 7 64 bit

 

[bataattila]

That's not strange at all, i was expecting solutions like you mentioned, but that is not working either. the problem is the same, no matter it is unite or subtract.

NX6

 

[wackolacko]

I was able to do similar with just using offset face.

John Lackowski
NX Support
Win 7 64bit NX 7.5.4.4 TC 8.3.1.1

 

[ewh]

Have you tried synchronous modeling, such as Pulled Face? I don't think this is an impossible situation for NX, just not as obvious as it could be.

Technically, the glass is always full.

 

[JohnRBaker]

These are classic 'non-manifold' conditions, which are considered as invalid solids. And if a CAD systems allows them to be created, without any sort of warning, this could prove to be problematic as they will never be able to be manufactured. Their existence would be as hypothetical models at best.

BTW, what makes them non-manifold is attempting to create a model where more then two faces share the same edge. The simplest example of this is taking a rectangular pad 100mm square and then creating two 50mm square blocks placed on the top of the original pad and then attempt to Boolean unite the first block to the pad and then the second 50mm blocks, as shown below:

This Boolean will fail.

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

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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

 

[Walterke]

John,
Say I want to create the part in your image, but with an edge blend where the model is now false. Is there a possibility to temporarily create this false part and "un-falsify" it by adding the edge blends?

Or do I have to start from a blended sketch and extrude that?

NX 7.5
Teamcenter 8

 

[bataattila]

@Walterke: excellent question!

of course the goal is not that the part to be impossible to manufacture. There are steps after that, so that edge disappears in the end. To be honest, I was trying to make my life easy when I decided to follow the steps as they are in the the ProE version of the model.
I'm sure there are other ways to achieve the final geometry, I'm just new to modeling, and need to know what can be, and what can't be done.
Thanks for all of your help, have a nice day!

(still interested in John's answer though)

NX6

 

[JohnRBaker]

There are a couple of a approaches, but certainly a 'blended' sketch would be one of the more obvious ones.

Note that there has been discussions over the years about providing a temporary non-manifold state which could be used in a situation like above where the next step was to add a blend thus resolving the invalid state, but we have not done anything yet, but it's still on the table.

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

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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