i've started to use nx11 after a lot of years using nx7.5.
i need to make a drawing for my assembly with master model.
with nx7.5, with master work part and switching to model environment, i can place a wcs wherever i want and with the command
i "freeze" the wcs (a new csys in generated and shown in green color).
after this, moving to drafting, in each view i can show this new csys.
with nx11 it seems to be impossible: i've saved the wcs as usally but i cannot find the way to show it in views.
where is my mistake?
Solved! Go to Solution.
i've try all the solution in my mind (layer 1, assembly in entire part or solid but i've added to this ref set the new csys).
the only solution that i've found is to save the wcs in assembly (in make a dispalyed part), it seems to work (but not often and i don't understand why) but to do this i have to open and save the assembly and it's not everytime possible to do it
My guess is that it has to do with the source of your base (drafting) view. When adding a base drafting view, you have the choice of adding the view from the drawing file or directly from the model file. Older versions of NX defaulted to adding the view from the drawing file, newer versions default to views from the model file. What this means is if you create extra geometry in the model views of the drawing file, it won't show up in the drafting view (by default). After saving your csys, try adding a new base view to your drawing. Click on the "Select part" step, expand the loaded parts list and select your drawing file. Choose the rest of the options as you like and place the view.
To see where the existing views are coming from go to information -> object and select the drafting view. In the information shown, you will find the "part name"; this indicates the source part of the view. Note that if you use (or plan to use) PMI annotations, you will probably need to create the view from the model.
Good luck with this.
I remember contacting GTAC back in July 2015, regarding an IR document I found in Solution Center, that mentioned the environment variable, to make sure it was supported by them.
The main answer I got from GTAC was
"I checked with Development and that Environment Variable was never meant to be published. It was created for a very specific issue and is not supported other than that."
Then, a little bit later, the IR document was removed from Solution Center.
Later, I was asked for justification to have access to this variable.
I think I didn't followup that request, and my IR was closed as "No Customer Response"
LEGACY PARTS, LEGACY PARTS, LEGACY PARTS: Siemen's always ignores this little gem.
We clone 95%-99% of our parts AND DRAWINGS.
This little change on their part caused major headaches on our end.
Thus we were given the Environment Variable to fix their oversight.