Identify assembly in OS 1

[skas31]

In catia V5 and other softwares it's possible to identify a part, assembly or a drwaing files by file extension in OS. How do I find if a *.prt is an assembly or a component without opening in NX.
Thanks.

Shankar K

 

[uwam2ie]

NO,
for your information this can be mixed geometry,assembly and drawings - you must know what the designer did...
hope it helps

 

[JohnRBaker]

NX does NOT classify .prt files based on their 'usage' by NX since there is NOTHING special about any particular file (there's one user-controlled but limited exception, which I'll cover later). NX looks at what the file contains, but only after the file is opened, before it decides how NX will leverage the files data or the way it will behave. This is the result of a very long evolution of Unigraphics/NX files. In fact, the current version of NX (whatever it is) can DIRECTLY OPEN any .prt file from ANY version of Unigraphics/NX back to UG V9.1 without EVER needing to do anything special, that's approaching approximately 17 years of legacy data. That's the UPSIDE of the approach we have taken to our .prt file structure decisions. The downside of course is that until that part file is open, there is no practical way to query that sort of information.

Now with the advent of PDM products, such as TeamCenter, that responsibility can now be turned over to data manager. Now the file's content has not changed, just that we now have a mechanism where we can automatically segregate and tag the file records so that this information can now be determined by simply looking at the data record master.

Now if you're NOT running in some sort of managed mode, i.e. you're running in 'native mode', you'll have to create your own scheme if you wish to be able to divine the information from 'outside' the part file. Now in anticipation of that (it's been there from way before the days of PDM systems) there are what we can 'file header records', some of which can be edited and accessed interactively and some which can only be done using NX Open (including GRIP).

For the interactive options, after you open a Part file, go to...

File -> Utilities -> Edit Work Part Header...

...and when the dialog opens, you'll find several options, including a Status, which is just an integer value, and a 'Description' which can be any string of text and which is then used as if it were a system Attribute with the name '$DESCRIPTION'.

Now using NX Open (and this includes GRIP), there is another data record called the User Area which can also contain a 'description' which can only be defined, modified and read with a user written application. Some customers have written applications which they run before releasing their files which will write a record into the User Area recording whether the file is a piece part, assembly, drawing, etc. Later, with the use of a user-written application, you can find and report what files are used for what by reading the User Area records.

I mentioned earlier that there's nothing special about an NX part file and that they could potentially be used for anything. Well there is one thing that you as a user can do to limit what a file can be used for. If you were to go to...

File -> Utilities -> Enforce Piece Part...

... which will 'flag' the current part file as being used as a 'piece part' only, meaning that you can NOT add any Components to the file. In other words, it can NOT be used as an Assembly.


John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[hudson888]

The obvious solution would be to adopt a naming standard that includes something like "_asm" in the file name. At least for you own files you would then be able to tell.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[looslib]

You can also use the utility UG_INSPECT to see if the file has components in it.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli