Parts update from solidworks to NX

[macnta]

Hi, I have just started to use NX8 recently. I have lots experience in solidworks and for the moment not too much time to learn how to efficiently create parts geometry and assembly in soldworks.

My current goal is to do flow/heat simulations in NX while continue to create the geometry of the model in soldworks.

When I import the SW model in NX, it works greate and I can do my flow simulations. However, if I update my geometry model in SW it doesn't update in NX.

Is there a way to reload geometry model easely in NX? Is it possible to not redefine the loading and boundery conditions each time I do so?

Thank you,

Tony

 

[JohnRBaker]

The best approach is that after you've imported the SW model as an NX part file, create a new NX part file and ADD the SW-based NX file as a Component. Now CREATE a new Component so that you have a simple Assembly with two Components, one the SW-based NX file and the second one the new empty Component that you just created. Then set the second (empty) Component to be the Work Part while the Assembly remains the Displayed Part. Now go to...

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

...and select the SW model from the first Component and hit OK. This will create an Associatively-linked copy of the SW model in the new Component. Now save all the files.

When you start to work on your Simulation task in NX you only need to use the newest part file, the one with the WAVE-linked copy. Go ahead and do all your analysis work using this part file.

If someone changes the original model in SW, all you have to do is create a NEW NX part file by importing the modified SW model and then open the Assembly where both the OLD SW model and the copied model are displayed. Now just replace the original SW-based component with your latest SW-based NX part file and this will cause the part file with the WAVE-linked copy to update while maintaining all of the simulation-based settings and conditions. Now you may need to make some manual reassignments, particularly of anything where geometry (faces, edges) were selected, but the system will lead you through the steps needed.

This workflow can be repeated anytime there is a need to update the simulation model based on changes in the original SW model.

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

http://www.siemens.com/plm

UG/NX Museum:

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

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

 

[macnta]

HI M. Baker, thank you for your reply.
I will try here to reword the procedure you have written, I have tried many attemps to follow it without success.
So let say I have created 3 files in solidworks, two part file and one assembly file:
A_sw.sldprt
B_sw.sldprt
C_sw.sldasm

I then go to NX: Start -> New -> Model
Give new file name: C_nx.prt
Then, File -> Import -> Part
Click OK
Select A_sw.sldprt and B_sw.sldprt
Then create a new NX part file and ADD the SW-based NX file as a component:
Start -> New -> Model
Give new file name: D_nx.prt
Then: Assemblies -> Components -> Add component…
Select : C_nx.prt
Click OK
Then: Assemblies -> Components -> Create new component…
Model
Give new file name: E_nx.prt
Click OK, OK
Then I go in Assembly Navigator
Right click on E_nx
Click on “Make Work Part”

This is where I get confused: if I am correct I should then go to

Insert -> Associative Copy ->

I should have the menu WAVE Geometry Linker available, but I only get “WAVE PMI Linker”

Could you help me clarify where I was wrong in the procedure?
Thank you, Tony

 

[JohnRBaker]

Are you in the Modeling module when you open the Associative Copy menu?

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

http://www.siemens.com/plm

UG/NX Museum:

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

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

 

[macnta]

I was in Advanced Modeling Module. But I figure out how to wave copy while being in modeling, the button was missing in my assembly toolbar.

That said, I now have problem understanding wave linking. I know it has been a subject in many other threads. I read read read, but just cannot find why if I modify my geometry in SW, then create a new NX file with it and replace the old SW NX based file, changes don't appear in the wave-linked file.

I really look forward to find solution on this, it is beggining to be really time consuming. I have an account on siemens website, is there a place where we can access some sort of tutorial covering wave-link related topics and examples? I have install NX7.5 and NX8.0 documentation, but it did'nt help me pretty much.

Thanks anyway for your suggestions, tony

 

[JohnRBaker]

You may have to 'Reparent' the WAVE Linked body (this can be done my editing it).

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

http://www.siemens.com/plm

UG/NX Museum:

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

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

 

[macnta]

Finally! It worked... I understand better now the importance of "Make work part" and choosing the appropriate context so to edit the broken link...

Thanks, Tony