I'm trying to set the standard in PMI to either keep it in the ASME Y14.5-2009. I can go to All Preferences -> PMI -> Tolerance Standard and change the standard each time. Since I'm mostly going to be using the ASME standard, how can I set it so I don't have to change it each time I create a new part in NX?
Thanks in advanced!
Thanks for the response. What do you mean by "Template Part"? Is it an external file? Is it something I have to edit in the Utilities or Preferences?
I don't think users would want to set a macro to set a GD&T standard everytime they create a new part or assembly file.
Please let me know any more detailt.
The PMI tolerancing standard in NX9 can be set for new parts by modifying the existing Drafting ASME standard in the customer defaults.
File->Utilities->Customer Defaults, and under the Drafting node, select the General node, then click the Standard tab. You will have to customize an existing ASME drafting standard. From the GD&T General node, click the Standard tab and in there you will see the Standard options.
ASME Y14.5-2009 was added on the Text with Symbols dialog, the Annotation Editor and the
PMI Standards menu (Preferences->PMI->Tolerancing Standard). The reason it was
not added to the Standard and Gage default is because this setting is only
applicable to the legacy GDT solution.
To create an NX part template that uses the ASME Y14.5-2009 Tolerancing Standard, you need to create the NX part (Save As from an existing model template part is recommended), set the PMI tolerancing preference, then save and place it in the ugii\templates directory. You must also modify the existing ugs_model_templates.pax file by adding this new part entry. The template part will then be available to use while creating a new part in NX.