Projecting Features from one assembly piece onto another

[bjohnson86]

Hello,

I am a new user to NX 6.0 and I was wonder how I can project the features (i.e. in my case holes) from one piece, onto another piece.

Thank your very much for your help,

Brandon

 

[jerry1423]

There are probably at least a few differnt ways to do what you need, but here is what I do:

I go in the assembly then make the part that I want to add the hole to as the work part (click on part > rmc > make work part)
I then find the hole that I want to project and extract the edge curve of that hole (insert > curve from body > extract > edge curve > pick edge of hole)
Now make the part that the curve was added to the displayed part and you will see the edge curve of the hole in there.

The next time you go into that assembly make sure the assembly is the work part.

rmc > right mouse click

 

[JohnRBaker]

OK, with your Assembly open, set the Component which you wish the new holes to be in as the Work Part while the assembly remains the Displayed part. Now go to...

Insert -> Associative Copy -> WAVE Geometry Linker...

...and at this point you have a couple of choices, you can either create circles extracted from the edges, using Composite Curves, of the holes in the current part(s) which could extrude and subtract forming holes in the Work part or you could just create Points at the centers of the existing holes which could be used as origins for creating normal holes in the Work part. In either case, the new holes in the Work part will be associatively linked to the original holes in the other part(s).

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

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[bjohnson86]

Thank you for your reply but I having difficulties following your directions.

1) The two different parts where made by different people, and are in different units. I am unable to "make part work part" due to difference in units. How do you change the units of a part?

2)What version of NX are you using. At my company, we are using NX 6.0.

In my version of NX I do not have the option to insert > curve from body > extract > edge curve > pick edge of hole

I have insert/intersect, section. I do not have the extract curve option.

Thank you very much for your time, your help is greatly appreciated.

-Brandon

 

[JohnRBaker]

We just covered the procedure for converting part units in the thread:

http://www.eng-tips.com/viewthread.cfm?qid=261407&

As for the recommendations, I based mine on NX 6.0 and should work if you follow my proposed workflow.

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

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[jerry1423]

That's too bad about the parts being differnt units.

What you can do is go into the model that you want to add the holes to and bring in the other part (that you want to project from) into that model as a component using "assemblies"
If that does not work out for you then you can import one part into the other using parasolids. Let me know if you want to do that.

 

[bjohnson86]

I have tried running the "ug_convert_part.exe" program. When I run it, nothing happens. It starts to execute (in does format) and closes in less than one second. It runs to fast for me to be able to read the command line as to what happened. Is this because I do not have administrative access?

Thank you very much for your time and have a great day!!

-Brandon

 

[bjohnson86]

Thank you all, I was able to project the curve using the insert>curves from curves


My problems was that I had my filter to work part only, it should have been entire assembly.

Have a great day everybody, and thanks again for the help.

-Brandon

 

[hudson888]

I don't know if it will work for you any better across parts of different units, but for hole centres I often find that linking points based on the hole centres is more stable than linking the edge curves. I don't know why, and I don't tend to use this method very frequently, but it may also help.

Best Regards

Hudson

www.jamb.com.au

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