Help me assemble these two components please NX 7.0

[patriqq]

Attached are two prt files and a TIFF image showing what I'm trying to do. The desired constraints should be apparent from the TIFF; let me know if it is not. I can't get the assembly constraints to cooperate. Please enlighten me. Thanks!

 

[patriqq]

Looks like only 1 attachment took. Here are the rest.

 

[patriqq]

Here is component 2 - guess I should have made a zip. Thanks

 

[dtharrett]

If you add some reference geometry to the swept piece (I added two planes), you can infer center axis to the radius of the black piece. Then a distace from the black piece to the CL of the swept piece... Probably a number of better ways to do this...

 

[patriqq]

I'm new to NX so I apologize if my Q's are dumb:

To add two planes as you mentioned, I would do that on the stand-alone prt file? Then I could use those planes for positioning when I add the component to an assembly? I was under the impression that only solid geometry was imported when components are added. Thanks

 

[JohnRBaker]

There are no 'dumb' questions, although I've encountered some really odd ones ;-)

Generally speaking only Solid bodies are automatically added to the 'Model' Reference Set, however you can use the 'Entire Part' Reference Set, which will include the Datum Planes, when initially creating your assembly. Once constrained, you can then set the Reference Sets back to 'Model' and the relationships will be maintained even if the Datum Planes are no longer visible.

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

http://www.siemens.com/plm

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

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

 

[patriqq]

Great, thanks. Is setting the 'Reference sets back to Model' something I do before I finalize the constraints or after? Thank you.

 

[dtharrett]

Like John said no dumb questions here. OK, what I did was make the handle pc the work part. I added a plane offset from the center plane by a distance and then repeated for the other side. I started a new assembly and brought in both pieces without constraining them. I reight clicked the handle piece and selected replace reference set )entire part). Now you can constrain the planes to the radius of the black piece (2X). Then a disance constraint from the handle to the black piece. Does that help. There are probably 100 different ways so if you find a better one...

 

[mmauldin]

I don't know if 7.5 files are compatible with 7.0 but I created an assembly in 7.5 using "center 2 to 2" and "center 2 to 1" to constrain the sketch curves from clb-08 spacer to the faces of the clamping element using the entire part reference set from the spacer. Attached is the assembly part file.

 

[mmauldin]

Another version using the Datum coordinate system from the spacer.

 

[patriqq]

Thanks for all the help - I'll try out these suggestions and look at the examples tonight.

My original approach seemed like a no-brainer; I was trying to touch the swept piece (spacer) to the sheet metal part (clamping element), and was trying to touch>infer axis the appropriate sections of the spacer to the mating indents on the clamping element with no avail. I also tried to use center and concentric constraints with no luck.

 

[patriqq]

Success! I wasn't able to open the 7.5 files, but thank-you. I moved the datum coordinate system (so thats what that pesky thing is!) to a useful location and used it (via infer center and parallel constraints) to position the part. Thanks!