Copy/import attributes 1

[DaveJFT]

Hi Folks,

I have a part that has been started without using our native Start Part so it is missing all our standard part attributes (used in the drawing frame and PDM). How can I copy the attributes from our Start Part into this new part?

Import part doesn't seem to do the job.

Thanks.

Dave

 

[JohnRBaker]

Well the simplest thing to do (if you're running NX 8.0 or newer version of NX) is to open up a copy of your standard 'Start Part', go to...

File -> Properties -> Atributes

...select all of the Attributes of interest and select the 'Copy' icon from below the list of Attributes. Now open your part file of interest, go to....

File -> Properties -> Atributes

...and you will see that a 'Paste' icon has been activated on the Attribute dialog. Just select it and the Attributes will be added to your existing part file.

Now if this is something that may likely happen again, there is a more elegant solution available.

Start a new part file and go to...

File -> Utilities -> Attributes Templates...

...and select the 'Catalog' option at the top and then create all of the 'standard' Attributes that you would like ALL of your parts to have in them. You can include default values or leave them empty. And go ahead and create ALL possible attributes which you might ever want to use in this 'Catalog' and when you're done, simply hit OK. What has just happened is that an .XML file named 'NXAttributeCatalog.xml' has been created/updated wherever you indicated where you wanted it to be at...

Customer Defaults -> Gateway -> User Attributes

Now what happens is that whenever you open ANY Part file, new or existing, when you go to...

File -> Properties -> Atributes

...you will find these 'standard' Attributes in the the 'Unset' group of Attributes. All you have to do to activate them is to select the Attribute, and hit the Green checkmark Icon. And if you share that Customer Default location with everyone in your organization they can all access the same set of standard attributes even if they've never added them to any of their existing files. Note that ONLY the attributes which you explicitly activate in the manner described above will be ADDED to the part file. The remaining 'Unset' attributes defined in the 'Catalog' will NOT to be saved when the part file is save but they will be available once more when that part if opened again in the future. The 'Catalog' acts as just what it sounds like, a predefined 'catalog' of attributes which has been 'published' so that anyone can access them whenever the need to. And the nice thing is that you can add to or remove items from the 'Catalog' and the next time that someone opens a Part file, that revised list of available attributes will now appear in the 'Unset' group of Attributes when in the Properties dialog.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[DaveJFT]

Brilliant!

Thank you John, that was a massive post - did you have it saved somewhere ready for just this question or did you type it from scratch?!



Dave

 

[JohnRBaker]

I just now typed it in, but I might archive this thread since I suspect that something like this will come-up again.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.