Cancel
Showing results for 
Search instead for 
Did you mean: 

Product interface

Valued Contributor
Valued Contributor

In customer default we have selected that any geometry can be wavelinked but it doesnt work. What can it be the reason? I thought maybe is beacause of the template we are using? I think we use a blank template and then we modified with our preferences but nothing about product interface. How can I check it? Thanks in advance.

11 REPLIES

Re: Product interface

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

@Javiduc if you use the search option in the customer default, you can extend the colums until you see scope.

Here you can see if the setting is a session setting or a part setting.

 

A session setting will be applied after a restart of NX.

Part setting is more a back up for the template part (when using the blank template)


Ruud van den Brand
Pre-sales NX CAD
cards PLM Solutions

Re: Product interface

Valued Contributor
Valued Contributor

This is shown as a part setting. So if it is not working I guess it is because our template is customized for product interface not working with no interface objetcs. How can I check/change it?

Re: Product interface

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

I think that this can be set by using the Product Interface Feature in the part.

The dialog has the group " Part Referencing Rules" 


Ruud van den Brand
Pre-sales NX CAD
cards PLM Solutions

Re: Product interface

Valued Contributor
Valued Contributor

Then I think the part is properly set. It must be some other thing what I am doing wrong.

 

I have this menus set to allow any reference. 

When I try to use geometry from partA in partB I open partB then use the command WAVE interface linker, then there select the partA and nothing happens. Should I do it in other way?

Re: Product interface

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

It should work like you descripe.

 

Can you make a movie and upload this here?


Ruud van den Brand
Pre-sales NX CAD
cards PLM Solutions

Re: Product interface

Valued Contributor
Valued Contributor

The texts are in spanish but I think the commands can be identified by icons, menu position...

Re: Product interface

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

If you use the Wave Interface Linker you need to define in a part what is avaible to link

 

So first open te part where you want to link from.

Use Product interface the select the edges, bodies, etc, that you want to be able to link

 

Now go to the Wave Interface Linker and select the part that you want to link.

You will see that the Interface is been filled in with the options that you want to link.

 

https://docs.plm.automation.siemens.com/tdoc/nx/11.0.2/nx_help/#goto:assemblies:xid618280

 

If you use the Wave Geometry linker you can select the geometry from your design space (assembly)

If you use the Wave Interface Linker you always have to define first geometry on the model that you want to link.

 

This is for that the user only link the same geometry and not are able to select something else.


Ruud van den Brand
Pre-sales NX CAD
cards PLM Solutions

Re: Product interface

Valued Contributor
Valued Contributor

Thank you very much Ruud. Then, there is no way of link geometry from partA to partB without assembly and without entering partB and creating product interface? I was used to do that in other CAD softs. Even I have a problem because some "partA" can have finished status so no writting access.

Re: Product interface

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

if you use Wave Geometry Linker it should be possible to link geometry that is inside of a assembly.

 

If you don't have the geometry you can try to open the part and use wave mode (right click component in assembly navigator) and link the geometry to a part.

 

Wave mode is not on all license of NX available.


Ruud van den Brand
Pre-sales NX CAD
cards PLM Solutions