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New User Problem- NX 7.5- Concentric Constraints 1

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RichPWade

Mechanical
Joined
Mar 11, 2015
Messages
4
Location
US
I'm a new user to NX having used Solidworks for my entire career. Only been using NX for about a week now.
Currently I'm trying to apply a concentric constraint in an assembly but I cannot select any surfaces on either of the parts. One part is a simple bent tube that I made with a sweep and the other is a flat flange made with an extrusion. I imagine I must be making some simple mistake but I cannot select any surface so long as I have the concentric constraint selected, the whole part turns red when I mouse over it. If I try applying a touch align constraint then I can select any of the surfaces.

Thanks for any help,
Rich
 
Are there circular elements to choose from on your components?

"Know the rules well, so you can break them effectively."
-Dalai Lama XIV
 
Yes, The tube has a straight section with a circular cross section that I want to mate to a circular hole in the center of the flange.
 
Please note that 'Concentric Constraints' can only be applied to the edges and curves of a Component, not to its faces. And generally speaking, the only edge/curves that can be used are arcs or ellipses.

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

To an Engineer, the glass is twice as big as it needs to be.
 
It is possible that you may be able to utilize the sketch curves for constraining by toggling between reference sets
 
I tried re-making the tube part by extruding the section I wanted to mate to the flange and then adding a sweep for the bend. After this I was able to select the edges to get the concentric mate. Not sure why it didn't recognize the edge when the whole tube was swept honestly but I guess it has to have a straight extrusion to reference the arc from.

Thanks for the help!
 
If the tube has a circular cross section, try using the "tube" command with the "multiple segments" output option. This option helps to keep the cross section truly circular. If you use the "single segment" option, you end up with a B-surface approximation; the end face will be a spline that looks circular but isn't a true circle.

www.nxjournaling.com
 
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