OK, I have find out, how to add my own profiles to the NX routing library.
As already mentioned, we have to work with Application View file (.apv), the Part Library View file (.plv), the Part Table file (.ptb), and the Part files (.prt). I have uploaded my part file with part families defined, my PTB file and changed PLV file.
Application view file is master file for the whole mechanical routing. It defines disciplines and specifications. What is this in NX? If you open mechanical routing file and then go to preferences/routing, you will see the discipline under the Disciplines tab. This is, where you select Piping, Steelwork, etc. This is controled by APV file. For me, those discipline are defined well enough, so I am not going to change the apv files.
The application view files call the Part Library View files (plv). PLV files have the definition for all the additional options in particular discipline. For example, PLV file will define all the standards for U profiles, I profiles, etc., when you select Steelwork for your Discipline. Here you want to define your own standard. If you open my PLV file, search for this string: MyStock. You will see, that under NODE STEELWORK_STOCK, I have added my own SUBNODE, named MyStock. Then, if you scroll down a bit, you will see the following section:
NODE MyStock
NAME RectTubing
TABLE DS_Rectangular_Tubing.ptb
END_OF_NODE
This is the way to tell NX, which standards you want to add. If you open NX with such PLV file, you will have under steelwork section this new MyStock standard (among others). In the list of all Steelwork standard, this my standard will be represented as RectTubing. And this MyStock is calling DS_Rectangular_Tubing.ptb file.
And now, there is a Part Table file (PTB) and part file itself. You have to define both very carefuly. With some additional utilities, you can update part file with PTB file. This is something, I didn't quite figure it out yet. So, here is how I have add my own part. First, I have created a prt file with part families defined. When defining part families, I have turned off the Importable Part Family Template in main dialogbox. Under chosen columns, I have now only Part_Name. There is no DB_PART_NO and OS_PART_NAME. This is how part families has to be defined. Then, I add my own expressions, that I want to use in routing. And of course, I have qualifiy this part as a routing object.
When this was defined, I have looked for the most similar PTB file. I have edit it so, that it contains my expressions and I have hidden the expressions, that I don't want to use during the selection of this part in routing application. If you check my PTB and prt file, you will find out quite easily, how the ptb file has to be defined. But be careful! PTB file and part family definition must use exactly the same expressions and names. It is also case sensitive. If you use 'X' in part families and 'x' in PTB file, routing will not recognize this member.
Very important variables here in PTB files are:
MEMBER_NAME..this must be the same as Part_Name variable in a part families(excel), defined in your part file
PART_NAME....this must be exactly the same as the name of your part
In my file, width and thickness are important expressionx. They define the shape of the stock. Other variables are there just because they were there in the original ptb file. And I didn't delete them.
And that's it. When you define those files like this, you can use your own parts in routing.
And this is where those parts have to be saved:
DS_Rectangular_Tubing.prt in C:\Program Files\Siemens\NX 8.5\UGROUTE_MECH\metric\parts or inch instead of metric
DS_Rectangular_Tubing.ptb in C:\Program Files\Siemens\NX 8.5\UGROUTE_MECH\metric\tables or inch instead of metric
ugroute_mech_metric.plv in C:\Program Files\Siemens\NX 8.5\UGROUTE_MECH\appview. If you are not working in metric system, then you will edit ugroute_mech_inch.plv file, of couorse.
I hope that this explanation and added files will help in creating your own standards and parts for mechanical routing.
