need to create a single part from an assembly

[greggor]

I have a customer who requires me to submit my assembly (multiple parts) to them as a single part and maintain all the paremetric features of each individual part of the assembly in the delivered part. How do I achieve this?

 

[jerry1423]

What version of NX are you on ?
You can build all the parts in one file, then when you are ready you can export them as individual components using:
Assemblies -> Components -> Create New Component
It may take a little bit of practice to get it right the first time so come back on here if you are having problems.
I guess the thing to do is make sure your menus are expanded all the way (so you see what's available to you), and read the command prompts as you go along.

 

[greggor]

Sorry should have stated I am on version 7.5. The asssembly has already been created as multiple parts now I must combine all these parts into a single part to include all the intellegence (features) each separate part.

 

[jerry1423]

What type of product is this ?
What other CAD systems do you have experience with ?

 

[greggor]

I have used IDEAS and CATIA about 5 years ago. This is an sweeping multi surface intake duct produced from many surface cuts trimsand joins. 4 main parts with a few additional brackets

 

[jerry1423]

WOW . . . I think you need to ask the customer exactly what he means. The way I read it he wants all parts of the assembly as one part, not multiple parts ~ and not added as components.
It's really hard to tell from here.

 

[nithink]

Looks like your customer wants this for Analysis purpose. I dont think there is an easy way to do this.

one option export - Part will remove all the parameters.

Nx 7.5.5.4

Teamcenter 8

 

[obe0009]

Hello,

This probably works only when the parts are positioned correctly within the absolute origin of the assembly.
Then you can copy the history of the partnavigator into the mainassembly. But this does not work when assembly constraints are used.

Regards,

Olaf

 

[greggor]

Yes all parts are modeled in position. Customer is Chrysler and as I understand they ask this of all suppliers so it is not an obscure request. It is just to populate their TDM not sure of the thinking behind why they want it done this way. I suppose since it is a supplier part with a single P/N they require it to be a single part. I had hoped there was a way to copy and paste the features from one file to another but it isn't that easy.

 

[obe0009]

Hello Greggor,

What do you mean by not easy. when they are modelled that way. You save the assembly under a new name. Copy the history tree of the parts that make up the assembly. Paste them in the top level of the assembly (you must be in modlleing app). Delete the copied component in the assembly.
Continue.



By the way. Automotive is using this way of assembly, so when something gets a bit larger, you get a collision and your engine is not moving through the hood.



Regards,



Olaf

 

[cowski]

I had hoped there was a way to copy and paste the features from one file to another but it isn't that easy.

Actually, it is pretty easy using "import part" (or "export part"); just you will end up with a large file that is difficult to navigate and use down the road. Start a new part and use File -> Import -> Part... to import each of your individual parts. As mentioned above, you will need each one to be modeled in position and I hope you do not have multiple occurrences in different assembly positions...

I would suggest after importing each part, use Format -> Group -> Feature Group to group all the features of each individual part. This will at least indicate to the next user what features belong to each part.

Not a recommended way to work, but if that's what the customer wants...

www.nxjournaling.com

 

[cowski]

Automotive is using this way of assembly, so when something gets a bit larger, you get a collision and your engine is not moving through the hood.

I don't understand this. Using a proper assembly (with individual component files) it would still report a collision.

www.nxjournaling.com

 

[obe0009]

Hello Cowski,


Yes it will report a collision, but with constraints, something get pushed when one part becomes larger.
With constraints you see the end results. And how Chrysler is working you see the collison of the part which creates
the problem. So you don't have to look for what is causing the problem.



Regards,



Olaf

 

[DSikes]

If you export a parasolid of your assembly (File > Export > Parasolid > then select all of the assembly components) and then re-import it into a new part file you will basically get 1 part file that includes all of your individual components as solid bodies (which you can rename to match your part file names) rather than actual parts. You wouldn't be able to modify any of the geometry but this gets you your one part file while also keeping all of your parts "separate."

 

[cowski]

Yes it will report a collision, but with constraints, something get pushed when one part becomes larger.
With constraints you see the end results. And how Chrysler is working you see the collison of the part which creates
the problem. So you don't have to look for what is causing the problem.

That makes sense, thanks for the clarification.

Sounds like using an assembly without constraints would be the easiest solution...

www.nxjournaling.com