Help: Export assembly PRT to STP or Parasolid, import with new names. 2

[JNieman]

Here's what I am trying to accomplish:

I'm using NX8.0.3.4

Customer sends us a NX model. It's an assembly of components. What I need to do is create a copy of that model with completely new names in order to modify the model and create drawings as needed. The new names must comply with our company naming convention. Let's say the original model is "123.prt" and the components are "123-1.prt through 123-n.prt"

My current process is to export the authority/original assembly file to a STP model. I will them import that STP model into my template PRT model I created. The new model has the right name. I want them to be "ABC-123.prt" with the components being "ABC-123-1.prt" through "ABC-123-n.prt" for example. However, when importing the STP model, it automatically creates PRT models of all the components, and keeps the original names "123-1.prt" through "123-n.prt" without the desired ABC- prefix in the example.

Without renaming & replacing every single component one by one, or requiring some kind of journal to do it for me - is there a way to set up the default naming procedure NX uses to create assembly components from an imported STP model so that it accomplishes my needs?

 

[JNieman]

If there is a better way to accomplish the goal, that doesn't involve STP model translation, I'm open to that as well. It's just a heavy-handed approach that works, which a coworker showed me. Up until now I've gotten by with this, but I'm finally tired of the extra work.

 

[Toost]

I assume that you haven't heard of the Clone Assembly tool in NX ?
( I would stay away from Step as long as possible, "Data translation has never added value and never will". )

The Clone assembly will create a copy for you , and it can copy all components into proper names also.
The issue is the drawings, you have to make sure these are loaded into the cloning session, ( else they will not be cloned)

Have a try and respond back if you need assistance.

Regards,
Tomas

 

[JNieman]

Well there's a nice bit of "duh" for me. I was unaware of that. It appears to be exactly what I need. I'm fiddling with the naming rules now but it appears like it will work 100% as-is.

Thank you very much.

 

[JNieman]

Well, it does work as advertised. However, I forgot that one of the primary reasons for importing into a blank template file was so that all my preferences and standards were set according to our company templates. Now I just have to figure up a routine/journal to change everything with the push of a button, I suppose. Unless there's a magic button for THAT already, too..

 

[cowski]

Are you talking about drawing templates?
If so, this would be a great time to use the master model method (drawing file references the model as a component). The master model method has the advantage of separating the model preferences from the drawing preferences. You could, if desired, use the model files as-is from the customer and your drawings would all be set up with your preferences.

www.nxjournaling.com

 

[JNieman]

I do believe I'm overdue to switch to a master-model method for drawings. Right now, I insert sheets into existing models. We do modify our customer models, sometimes slightly, sometimes greatly, so I'd still need to clone the assembly.

It's possible that the best practice solution, given the way NX is geared, is to switch to a MMM. I'll look into that for the next job I set up.

 

[cowski]

In the drafting annotation preferences, there is an option "load all defaults". I believe that this will load up your preferences from your customer defaults; but I'm not sure. I rarely used that function and the interface/wording has changed in NX 9. Perhaps someone can confirm what this command does, exactly...

www.nxjournaling.com

 

[JNieman]

@cowski, that appears to be exactly what happened when I tried it. I have to change my customer defaults to match the company standards (the few of us using NX have standalone installs) but that's exactly what it seems to have done. Another menu item I did not know was even there...

I really wish the boss man would approve my training requisition soon...

 

[Toost]

the option is probably what you are looking for. It does import the customer defaults, provided that it is the customer defaults settings you select in the dialog.

Regarding the training on this matter,... there is no "NX system management" training sadly.

What you should do , on your and your fellows computers is to set , in the windows control panel, the variable "UGII_SITE_DIR" where the value of the variable should be a directory on a common server. ( example: H\NX_settings\ or: \\servername\nx_settings\ )
depending on you and your colleagues, only you should have write access to this directory, or you and your colleagues.

When this variable is there , NX will in the customer defaults dialog present an option to set "site" settings. These will be saved in that new directory and will apply to everybody who has the windows variable set.

There is a customer default ( for drafting settings only ) which controls if it is the settings in the existing part file which should "rule" or if it is the customer defaults which should "rule". - this options is "slightly" unreliable in that all settings doesn't work as designed but overall it does the trick.


Regards,
Tomas

 

[Rob_N]

The NXCustom scripts work very well , you can find them on the Siemens community site
I only have a couple of licenses, but I have NX on multiple PC's and with NXcustom I can keep all settings and GUIs consistent.