More companies are beginning to recognize the value in leveraging a model-based definition (MBD) strategy and use of Product & Manufacturing Information (PMI) as part of their product development process. One of the biggest barriers to implementing such a strategy, though, comes in the form of legacy data. What do you do with all of those legacy 2D drawings?
Fortunately, NX 11 solves the problem with the new Convert to PMI command. Convert to PMI works with both master and non-master model drawings. The tutorial today focuses on the latter, so if you would like to see a workflow to convert master model drawings to 3D PMI objects, be sure to check out our previous NX Quick Tips video.
The conversion process is actually quite similar, regardless of the model type with which you begin. The only difference is that first you must create a master version from your non-master model. If you are left wondering “What is this master model business about, anyway?” a master model contains the geometry model and drawing in separate files. The master model concept is based on the idea that one model drives the entire product development process—design, simulation, drafting, assembly, manufacturing, and inspection. Any changes you make update automatically anywhere, because everything is based on this one master model file.
Before we can execute Convert to PMI, we must first change our model to a master model. Open the file to view the drawing in the NX Modeling application. Under Model History in the Part Navigator, you can see all of the features included in this particular design. Now open the Drafting Application and look under the Part Navigator. The drawing is out of date, as the clock to the left of each view indicates. Click to update all views, and wait a few seconds for it to finish.
Now that our drawing views are up to date, let’s go ahead and save the file with a new name. The existing file name casting_dwg is incorrect; we saw in the first steps that this file contains the design and all of the drafting information. Rename the file to casting and save.
The next step is to create a new drawing. The goal here is to create a particular sheet that is related to this casting, so in the Drawing Template underneath the Relationship filter, select Reference Existing Part and then select OK.
In the Assembly Navigator, right-click the casting and select Make Displayed Part. Go into the Part Navigator, highlight all of the drawing views, right-click and select Copy. We are going to paste these views into the drawing. So go ahead and open the casting_dwg file again.
Now paste the copied views into the Part Navigator in Drafting. A notification pops up to warn that the operation may create objects on an invisible layer. Hit OK to proceed. In the Layer Settings dialog, there is a checkbox and you’re able to turn those layers back on.
There is an angular dimension on the drawing that is off. You may have more than one. To fix this, open the Angular Dimension dialog and change the object selection. Once the First and Second selections are correct, apply the changes and zoom back out to the whole drawing. Drag some of the views around to fit within the drawing borders.
Now let’s go back to view the note on that original casting. Open it up, and copy the text. We are also going to paste the note into the new drawing file. Once the note is pasted, click and drag to place it on the drawing within the boundary of the borders as well. Now go back and change the drawing border colors, make those a little lighter to help distinguish the details of each view better.
Now go back into the original casting and remove the drawing sheet. Save the casting. The casting file should now only contain the 3D geometry and all features. Congratulations, you’ve successfully moved a non-master model into a master model format! From here, you follow the same steps to convert a master model to 3D PMI objects.
Watch Sam Kuan demonstrate this workflow in the NX Quick Tips video below.