Loading parts from your last session when opening NX

It's possible to have NX load all your parts/assemblies that were open the last time you worked with NX.

First, you need to switch on the customer default "File → Utilities → Customer Defaults → Gateway → General → Part → Write Bookmark File on Exit". This will make sure that a bookmark file is written as "yourusername_last_context.plmxml" under TEMP directory.

When you want NX to load this bookmark, you can launch NX with the following command :

ugraf.exe -retrieve:%TEMP%\%username%_last_context.plmxml

Or, you could use File-Open to load the .plmxml file.

Using revisions in native NX

For those who don't have Teamcenter, there's a way to have NX recognize your part numbering/revisioning scheme. Here is one scenario :

assembly1__01.prt
|_mypart1234__01.prt
|_otherpart1235__01.prt

The numbering scheme here is, "partnumber__revisionID.prt"

Suppose you open mypart1234_01.prt without the assembly, and save it as mypart1234__02.prt. Normally, you would need to open the assembly, and replace the 01 revision with 02.

With the revision logic setup, if your load options say "load latest" and "allow substitution", mypart1234__02 will load automatically without doing the part replacement..


How do we set it up?

First open your customer defaults. Go to Assemblies - Site Standards - Part Name Versions.
Fill this window :

Full Part File Name Format :
([a-hj-np-z0-9A-Z]+)(__([0-9][0-9]))

Version independent section of part file name
\1

Part File Name Match
\1(__([0-9][0-9]))

Version section of the part file name match
\2


Version type
Alphanumeric

What we say here, is that the full part name (mypart1234__01) consists of any number of small/capital letters/numbers followed by a double underscore, and a 2 digit numeric revision ID. The way we say it is, "Regular Expressions", a very detailed method of specifying patterns like these.

Now that you've set your customer defaults, next step is making sure that your load options say "load latest" and "allow substitution". Also, you should not be using "As Saved". Instead, you can load from a folder or search directories.

How it works is, when you are loading the component mypart1234__02, NX knows that the part name portion is mypart1234, and the revision is 02. Listing all the parts that matches the pattern mypart1234__[revid] , it loads the latest one. So it is very imporant that you should name your parts according to this pattern. For example, the number of underscores should be exactly 2, or there should not be a letter in your revision ID etc.

It seems this functionality has been available for a long time, only to be found in the depths of your UGDOCS installation..

Hole Table functionality without the Mold Wizard license

Here's one reason to consider upgrading to NX6.0.3.

You can now insert a hole table just like the mold-wizard-people do by setting the following environment variable :

UGII_DRAFTING_HOLE_TABLE = 1

Free NX CAST training access for students

I'm not sure for how long this has been available : if you are a student, you can freely access the CAST training system for NX. CAST is basically a very helpful set of tutorial based training that covers modeling, assemblies, drafting, machining, simulation, etc. (the abbreviation CAST stands for Computer Aided Self Teach)

You'll need an email address that ends with ".edu", ".ed", ".ac.uk" to register:

http://castedu.ugs.com/review/freeAccess.shtml

If you're not a student, but want to get some information how to obtain CAST, here's where you can.

Existing CAST owners : here's a tool that will help you to create your own set of trainings: http://cast.ugs.com/ccb/index.shtml