I have a NX7.5 CAD file which is having MATERIAL attribute defined and now I am opening same file in NX10 CAD tool.
But MATERIAL attribute is not getting displayed on Object properties page.
Kindly help me to understand how to map MATERIAL attribute in NX10. Other Attribtes from NX7.5 are getting populating properly in NX10.
Since you mention mapping, are you using Teamcenter? If you are, what does your mapping syntax look like for the material property? MATERIAL is now reserved as a System Attribute, so I suspect that whatever you have used in the past is now getting read as an alias.
Do you change the names of the attributes within the materials section of the Customer Defaults?
The 'Material' attribute name changed in NX10. There is a short statement about it somewhere in the NX 10 documentation (maybe the What's New or Release notes).
You need to start using the new attribute name (NX_Material I think) in NX10.
Thanks for your reply.
But I am not using Teamcenter. Its only CAD upgrade. Previously we have NX 7.5 and now we are using NX10.
We have around more than 10 attribute mentioned in the properties file of NX 7.5 and except MATERIAL all attributes are properly getting displayed when i open same NX7.5 file in NX10.
Could you please suggest me in this regards.
Thanks Larry for yor help.
I will go through the NX10 documentation and also try workaround suggesed by you.
I saw the note in the NX10 "whats new", but I didn't see a best practice on how to migrate from the older attributes to the new. I tried changing one, making the old the alias, and got an error saying "the alias and the title of the attribute are identical", when I opened an existing part.
This has been enhanced in NX11. If the MATERIAL attribute is found when opening a part (and your customer defaults are OOTB) you will get an information window appear reporting: "The Material Attribute was reset because it did not match the material assignment. This action was taken based on your Customer Default setting" and it will list the material value. In NX10 the attribute is not listed in the properties dialog and no message is raised when the part is opened.
If you manually created a MATERIAL attribute in NX7.5, OOTB that attribute is converted to NX_Material when opened in NX10 and the value is reset. If you edit the alias in the Customer Defaults for Part Material from "Material" to "NX_Material" you will get the error message that the alias and the title of the attribute are identical and the part will not load.
There's a "Create Attribute" checkbox in the same section of the customer defaults for Part Material. If unchecked your NX7.5 files will load, and the "MATERIAL" attribute will display, but shown as "NX_Material". However, if you assign new materials to parts using the Materials Library, a material attribute will not be created, nor will your existing NX_Material attribute be overwritten. You will have to continue to manually create the NX_Material (MATERIAL) attribute. Note that you cannot enter "MATERIAL" as the title for your attribute, it will be converted to "NX_Material" (fixed in NX12).
One option is to leave the checkbox checked, to allow NX to create a material attribute when a material is assigned from the library, and enter a different Attribute Title Alias for Part Material, such as "Material_Lib", or something that reflects NX assigning a material and creating the attribute. Note that with older parts, this may now present you with two material attributes - the NX7.5 "MATERIAL" attribute (which is no longer renamed to NX_Material), and your new attribute "Material_Lib". Note that selecting the "Material_Lib" attribute in the properties dialog and clicking "Information" will tell you that "Material_Lib is an alias for the title NX_Material. The part material".
Hope that helps.