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.
@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)
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?
I think that this can be set by using the Product Interface Feature in the part.
The dialog has the group " Part Referencing Rules"
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?
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.
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.
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.
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.