Not able to constrain parts in assembly, NX8

[Lunder]

Hello,

I have a swept route made in mechanical routing, which have several holes through it. I am trying to do a concentric constraint with one of these holes and another part, but the Assembly Constraints navigator won't let me choose the hole at all. I was able to make this constraint earlier, but have made some changes and now it's like this. The swept route is also transparent. Running NX 8.0.0.25.

Suggestions?

Thanks,

Lunder

 

[JohnRBaker]

Concentric constraints can only be used with circles or ellipses. Try performing an 'Info' on the edges of the holes to see if they are actually circles/ellipses or not.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[Lunder]

The hole is definitely a circle, it's just a substract extrusion of a simple circle sketch. Do you know why the swept route is transparent?

 

[JohnRBaker]

Just because the 'hole' was created as the result of subtracting an extrusion of a circle doesn't guarantee that the edges of the 'hole' are circular (or elliptical in the case where the extrusion direction was not normal to the face of the body in which the 'hole' was created). So I ask you again, have you interrogated the model to determine whether the edges of the holes are actually circles (or ellipses)?

Also, it might help if you provided at least an image of what these parts look like.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[Lunder]

The extrusion is normal to the face which the hole is going through. When i select the edge of the hole, only information about the routing stock comes up. Part file is attached.

 

[Lunder]

Picture of the hole attached.

 

[JohnRBaker]

I'm sorry, but the edges of the 'hole' are NOT circles but rather were created as 'intersection curves', which is not a valid curve type for use with the Concentric constraint.

That being said, WHY did you use a 'Routing' object to create what is clearly the frame of a purely mechanical model? If you had used the traditional 'Sweep Along a Guide' or even using a free-from Swept feature with the proper options set, you would have ended up with much better behaving geometry (planar faces which would have resulted in circular edges on the holes).

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[Lunder]

Hmm, okey. I was able to extrude the routing and make concentric constraints earlier, but then it just didn't work anymore. The faces seemed to planar too, as I could make sketches on them.

I thought mechanical routing was an equally good method to making structures as any of the swept functions, but now I know better. Thank your for your time!

 

[crecore]

I assume you did routing because if you changed the routing, the holes in the mechanical parts would update. You could also wave link the swept feature body into each part then do a boolean subtract. This would do the same thing; albeit a little more cumbersome if the swept feature intersects many parts.

NX 8.0.1.5