what is the advantage of using Master model for detailed drawings?
what is the disadvantage?
We are trying to reuse our models and drawings and it seems that it would be easier if they are both in the same file?
American Tool and Mold
Benefits I have heard:
1) Drafters can be working on drawing while (at same time, sort-of) modelers can be tweaking model. Obviously if the modeler completely changes the model, the drawing may have to have extensive edits. Or at least the model can be "released" while the drawing can still be edited...Note using PMI on the model eliminates this "parallel processing" capability
2) Other users of the model (assemblies in CAD, or CAM/CAE/etc.) don't have to deal with the "baggage" of the drawing (the extra bytes of the file size & processing time to wade thru the extra data)
3) If you go "all in" in Teamcenter (also native, I guess) the drawing can have a different revision history than the model (e.g. changes in notes/callouts/tolerance don't require a model rev change) (note depending on your desires, having the drawing a separate item may not be supported well in "as installed" TC, e.g. if you want the drawing & model to ALWAYS have the same revision)
4) (depending on your policies of who has write access to what) you can set things up so drafters only have write access to drawing files, and can not edit the model files.
A) particularly with part families, it becomes hard to have a specific drawing of each family member as a separate file/dataset
B) (not sure about this) If you aren't religious about updating the drawing when the model changes (opening w/ latest components & saving) you can get an out-of-date drawing displayed (you may have to do "dumb" stuff like load "structure only" or "load as saved" or whatever to load the out-of-date model).
Summing it all up, I would tend to use master model, except perhaps for part families (depending on how the drawing(s) for the PF members need to be done)
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled
In addition to what Ken said, the master model approach allows you to use a reference set in your drawing file; this allows you to easily filter out unwanted geometry (datums, sketches, etc). You'll have to use "layer visible in view" when you keep the drawing in the same file as the model. The "layer visible in view" command works best when you have a well-defined and observed layering standard (I've yet to see such a beast in the wild). NX will manage the "MODEL" ref set for you, avoiding many of the layer convention headaches.
I've seen some rare occasions where some surrounding components were brought into the drawing to give context (the surrounding components were rendered in a dashed or dotted linestyle). With the master model method this was all managed by the drawing file; without master model, your part file becomes a part/assembly file and carries the extra baggage that goes with it.
However, using the master model method in native NX can lead to a number of file maintenance headaches.
I think it depends how your company is set up. If the same person does the model and the drafting then in my opinion it should be the same file. It makes for easier file managment and less wavelinks between the file.
If your company has separate modeling and drafting departments then you probably would want to keep them separate.
We have had a couple parts that did not have the master model approach. These parts when put into an assembly were very difficult to move. Very time consuming with the extra overhead of the drawing. From the Old I-Deas days this is just the way it was done. Us old I-Deas users were very used to this concept.
Are you using teamcenter?