Unite only specific adjacent faces on two solids; NX7.5

[MortenTN]

Hi, I need some help from some NX experts - looks like this is the right place.

I have two solids - two revolved halves of a ring. They are both revolved based on the same sketch and therefore have the exact same profile. At one end, the two revolves have 2 adjacent faces (Clean cut prodile and zero distance between faces). At the other end, the two bodies have a more complex structure, but still have a total of 4 adjacent faces (zero distance).

I need to unite the two bodies to one body, but only at the end where the two revolves meet in 2 adjacent faces. The remaining adjacent faces must not be joined.

Unite command will result in all adjacent faces being joined. Sew command will result in a hollow structure, even though Solid is selected and the profiles of the faces selected are exactly the same. I have tried many other commands with no luck.

Any help will be appreciated! Thanks!

Best regards,
Morten T Nielsen

 

[carlharr]

Hi,

Difficult without a pic, but I don't think this is possible because two "adjacent" faces can't be in the same physical space, either physically in the real world, or mathematically in CAD. CAD can't differentiate between two positions if they are the same.

If I'm understanding the part it's kind of like a split ring, in which case you'd be best just to model a (small) gap in I think.

http://www.jcb.com

NX 8.5 with TC 8.3

 

[MortenTN]

I will make a simple model to better illustrate the problem, but you are correct that it is just a split ring. The model needs to be divided in two bodies initially, in order to model the complex structure, where the ends meet.

The trick with the small gap is what we have used so far, but the zero gap is actually dimensioned on the final drawing, and therefore I would like to do without it.

 

[carlharr]

I'd stick with the small gap, as long as it's smaller than the number of DP on your drawing you'll be fine.

Or you could just model a solid ring and then draw the split on with curves.

http://www.jcb.com

NX 8.5 with TC 8.3

 

[KhimaniMohiki]

I think you could play a trick with the modelling tolerances to get the ends you want to unite other adjacent edge show a near zero gap. The problem is trying to avoid generating a non-manifold solid.

Khimani Mohiki
Design Engineer - Aston Martin
NX8.5

 

[MortenTN]

The attached picture shows the basic model, with just 2 adjacent faces at each end. Two bodies with more than 2 adjacent faces, and I only want to unite 2 of them.

I drawn split is also the kind of trickery I would like to avoid

 

[MortenTN]

Khimani, do you mean the general modeling tolerances under Preferences?

 

[KhimaniMohiki]

If its only for representation in the model and drawing then why not do a full revolve (to get a ring) and then divide the faces at the desired point with a surface, that way it will appear correct in the model and be dimensionable in the drawing.

Even if you did manage to find a way to unite just 2 of the adjacent faces, the other adjacent faces would never be visible or usable as far as I can see.

Khimani Mohiki
Design Engineer - Aston Martin
NX8.5

 

[MortenTN]

Sorry - the picture shows a simplified model. The open end of the ring has a slightly more complex shape than illustrated, but since this is work related, I didn't want to show too much.
Various roundings and chamfers are applied to the model at the open end, and therefore I can't just divide it by a surface.
It is a ring for sealing around a piston, and it is machined and then bend afterwards, which results in the complex shapes being adjacent.

I think this simply isn't possible.

Thanks anyway for the suggestions!

 

[cowski]

Apply a small offset to the faces that you do not want to merge, perform the unite operation, and finally offset the faces back out to where they should be. I know this work-around is a bit clumsy, but it will work. Perhaps you could give the offset features a meaningful name or add a comment that shows up in the part navigator to flag that these are intentional and necessary.

www.nxjournaling.com

 

[carlharr]

You could put a sheet in where the two "non-joined" faces are, which would then show up it's edges in your drawing, and be parametric should the profile change.

Still think I'd go with a very small gap though (see attached) which is more realistic.

http://www.jcb.com

NX 8.5 with TC 8.3

 

[MortenTN]

I tried with offset - unite - offset, but it unites the faces pr. default.

Carlharr, I think you are correct, in that it is not possible, in the physics of CAD, to have the same body with different faces in the exact same space.

 

[carlharr]

Hi Morten, it's not possible in physical bodies either, which is what made me think about CAD.

Thanks, have a good weekend.

http://www.jcb.com

NX 8.5 with TC 8.3

 

[JohnRBaker]

Yes, this is one of the situations which results in a non-manifold body. By definition, non-manifold bodies cannot exist in nature, therefore we've decided to limit NX to producing only manifold solid models. The only exceptions are some special cases which are allowed when creating finite element models but this is done as part of the model preparation and meshing tasks and does not actually alter the topology of the parent models.

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