External Copy Geom for NX? 2

[jknott]

thread561-343249

Referencing the older closed thread above regarding NX and the External Copy Geometry. The WAVE Geometry Linking is only accessible in the Assembly function. Is there a similar function or workaround to allow you to use it in the Modeling configuration?

When I had Pro, we would often use ECGs of previous versions of the models as a starting point or reference point and modify the new geometry accoding to the existing. Being that NX only allows this funciton in the Assembly configuration doesn't help in this regard.

I used NX for a few years and it was my choice of CAD software however I was forced to use Pro through work for a few years now and have forgotten many of the key functions of NX. I am now returning to it and am having a bit of a hard time remembering things. I am using NX9.

Jarrett

 

[JohnRBaker]

I guess you could use the 'Extract Geometry' function with the 'Associative' option toggled ON. That way you would have another body that would behave exactly as a WAVE linked body would behave except that you would now have TWO solid bodies in the same part file, the original 'parent' and the associative 'child' (you'll probably need to Hide or move to another Layer the 'parent' body).

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
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To an Engineer, the glass is twice as big as it needs to be.

 

[jknott]

John,

Thanks for the quick response. If I use the extract geometry function then how do i import the geometry into my other part file?

Jarrett

 

[jerry1423]

You can copy and paste it from one file to another
but it will be unassociated from the original part, and unparametized.

 

[jknott]

ok got it. That is what I was essentially looking for. Would be nice if they can make them parametrically linked in the future but for now this is a nice workaround.

Jarrett

 

[SDETERS]

Could you add your part as a Component to your part and do the wave link to your part file? Would you even need to do the wave link at this point? Then you can turn this part as an empty reference set. You also could try to make a temporary assembly, do your wave link, then delete the assembly before saving. You only need the assembly to make the link. Once the link is created you do not need the assembly anymore? Not sure if this works or not.

 

[bmarchand]

I'm not following why you are not able to link into your parts, we do this all the time, fully parametric
We create a control assembly that resides inside each or our stages, in that assembly we create or add all construction geometry we need to create each station, set them on reference sets.
In each part file we are working on, make your reference set current to the one you are working on, make part your work part and link in whatever you want to use in your part, make sure associativity is on. Now if you have a change, you change your control part and everything updates.

Brian Marchand-Die Designer

http://www.armotool.com/

NX 10.0.2.6 / PDW 10
Dell Precision T7610 w/Xeon ES-2609
16G Ram - Nvidia Quadro K5000
Win 7 Pro x64

 

[jknott]

Understood. I was trying to find a quicker path which did not require the creation of a regeneration (or control) assembly. Coming from Pro, you can quickly create a fully parametric External Copy Geometry without the use of such as assembly and I was looking for an NX equivalent of this function.

As I get back into working with NX I am sure I will have to create a regen assembly in order to properly model my components so I appreciate the insight and will reference back to this thread.

Jarrett

 

[cowski]

Reading through the thread, I'm not quite sure what you are trying to do. It sounds like one of two things:
[ol 1]
[li]Create a copy of an existing part to use as a starting point for a new part (add/delete features, modify existing features).[/li]
[li]Add a copy of an existing part for reference only as you create/modify an existing part.[/li]
[/ol]

If 1), I'd suggest using "save-as"; this will give you a new copy of your existing part that you can freely modify.

If 2), there are multiple ways to get there; an easy way is just add the existing part as a component in your new part. Keep in mind that NX doesn't have separate model, assembly, and drawing file types. If you are working in modeling, simply make sure that the assemblies application is activated and you can add other parts as components in your current file. Once you have a component you could even wave link or promote the body into your current file if so desired.

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