Splitting a Non-Master Model from the Master Model File

Splitting a Non-Master Model from the Master Model File

This article will just be a quick review of a process that, in essence, splits apart into 2 different files, a model and a drawing of that model that are both created in the same file. This method will also create an associative link so that subsequent changes to the model will update drawing data accurately.

Master Model Approach

The Master Model approach is a common methodology of using the data defined in the model to drive the data of the multiple disciplines downstream of the modeling process. This includes practices ranging from the simplest concept of the assembly to the more complex application of the geometry and specification data in the drafting environment.

Surprisingly, there are a lot of NX customers having legacy data that was created with the drafting information in the actual model part file. This article will show how to take a file containing both the model and drawing and divest the drafting objects and drawing sheets into a separate file while maintaining associativity with the Master Model. This can be accomplished in a managed environment as well, such as Teamcenter.

First, we start with the file containing the model and drawing.

NX Master Model Approach

Notice in the Part Navigator, that “SHT1” is listed under the drawing node while a model with full feature definition is listed under the Model History.

Before beginning the process, we’d recommend that the user fully understand the contents of the file and how it is organized. This would include the use of Layers and/or the Show/Hide status of objects. When we are finished with this exercise, the result will still provide the ability to manage the Reference Set of the Master Model while displaying the drawing since the Master Model will actually be a Component of the 1-piece assembly file. When it comes to controlling the visibility of objects in views placed on a Drawing Sheet, it is much easier to accomplish through the use of Reference Sets as opposed to Layers or Show/Hide.

In this example, we see a couple hundred total objects strewn across several different Layers.

NX Layer Settings

For users who take advantage of Layers, you would notice that Layer 1 contains 106 different objects and in a normal scenario, Layer 1 would only contain the solid body of the model and nothing else. So if we were abiding by some company policies and practices for Layers, we’d probably correct that before splitting the drawing off into another file.

You might also have noticed another little issue in the title block area of the Drawing Sheet – the Title of the drawing appears to be a note with characters that aren’t available in the font style, indicated by the square with diagonal slash. Likewise, the revision letter is an unknown definition.

NX Drawing

These are actually Attributes for Part Description and Revision that evidently don’t exist in this new version (NX12) or has been redefined since the original version that this drawing file is saved in. In fact, there’s a note that references Siemens that we might no longer want on our own company’s drawing sheets.

If you look at the Drafting Tools tab in the Ribbon Bar, you’ll notice that the “Populate Title Block” icon is disabled, indicating that there is no actual NX Title Block on the drawing. This might be typical of legacy drawings in NX where the border and title block were just lines and notes in a “border” or “format” file that was imported onto the Drawing Sheet or are objects embedded into a “Pattern” file that used to be the default methodology of years ago.

Issues like these and many more can be found in legacy drawing files, depending on a particular company’s processes and practices but will not be a major problem in this exercise. It might prove best if some of them were taken care of before the divestiture while others might be best handled later when there are distinct Master Model and Non-master Model drawing files. But we digress. The important part of this is that before moving forward with this process, you would need to edit these kinds of issues and then save the file first. Later, we will just close this part file and this article doesn’t tell you to save so take care of that beforehand. If not, you can always save it on the fly later.

NX file save

The first real step in this divestiture process is to export the drawing out into a separate part file. So you choose File→Export→Part. In the dialog, select Specify Part. In this case, we’d want to name the file consistent with the default NX new drawing process and simply add “_dwg1” as a suffix onto the name of what will become the Master Model file, “sts_cast_pump_rotor”.

NX Export Part

Once you choose OK, the Export Part dialog reappears. Now you choose Drawing Selection. There is only one Drawing Sheet in this file so this is easy.

NX Drawings to Export

If there were multiple Drawing Sheets in the file, you could select any or all.

Once you choose OK there, again you come back to the Export Part dialog. With the rest of the settings as shown above, you select OK.

Immediately, a popup appears prompting you to decide if you want to add the current part (Master Model) into the new file as a component.

NX Export Part

Obviously, you would choose Yes!

At this point, based on your Save Options, you might get other popup alerts prompting you to decide other things like CGM output.

Save CGM

Choose Yes to continue. Then you just close the Displayed Part.

This is the new Window Tab function in NX12 that has many new benefits when working with multiple parts.

After closing the initial part, you are now ready to open your new drawing file. Once opened, you will see the assembly structure in the Assembly Navigator.

Assembly Navigator

Notice that the new Master Model was opened partially according to our Assembly Load Options and that the current Reference Set is Entire Part. Here is where you see the impact of objects on different Layers and where you might want to correct that if you didn’t before.

You will also notice that since this new part file has never been saved in any other application, you are in Gateway. Select the Drafting application. The Drawing Sheet displays.

NX 12 Drafting

Here’s where there might be some anomalies while you are first working out this process, particularly in the area of template files, Drawing Standard, Preferences, etc. And those can be corrected directly here in the new drawing file or with your NX configuration.

So to see the associativity you now have between your Master Model and this new Non-master drawing file, you can make the Master Model your Work Part and do a little design change. We’ll change the size of the center hole to be much smaller so it will be obvious.

In NX12, you can simply press MB3 on the Master Model in the Assembly Navigator and choose Open in Window.

NX Assembly Navigator

It opens the “old” Drawing Sheet which you no longer need anymore. It would be best to delete it just to make sure no one goes to this file to edit the Drawing Sheet but goes to the new drawing file instead. In older days, you used to have to turn off the display of the Drawing Sheet in order to delete it but now you can just press MB3 on it in the Part Navigator and it deletes it. The Graphics Area now shows 3D model space.

NX Drafting

Just change to the Modeling application, make a change to the model, and then change Displayed Part back to the drawing file. In NX12, you can do that simply by double-clicking on the tab for the drawing file!

Remember that, in almost all circumstances, you’ll have to update the drawing to see accurate representation of model objects, silhouettes, and such.

NX Master Model Drawing

Don’t forget that when you save the new Non-master drawing file that the Master Model file will also get saved as well unless you choose Save Work Part Only.

Post by Garrett Koch

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