Assembly drawings 1

[bbylls]

NX5.0.6.3
I have a sub-assembly for a mold with 1 plate and some other components in it.
Each plate in the mold is a sub-assembly with components in it.
I open the sub-assembly, go to drafting, create a sheet and add a TFR-TRI view and a DIMETRIC.VIEW.D4 view of the sub-assembly.
Then I add a sheet and creat a drawing of the plate.
I save and close it.
I open the main assembly file.
The sub-assembly is there, except it now has 2 plates in it.
The main assembly interprets the drawing of the plate in the sub-assembly file as an extra plate in the main assembly. It also shows as a quantity of two in the parts list. It only shows a quantity of 1 in the parts list of the sub-assembly file.
If I delete (or suppress) the extra plate in the sub-assembly of the main assembly file, it deletes the plate drawing views in the sub-assembly file. The TFR-TRI and the DIMETRIC views are OK.
Am I doing something wrong?
I have also tried it in v7.5 and get the same thing.

 

[GeoffD00]

It sounds to me like you have created the view of the plate using "part view" rather than "base view". This adds another occurance of the part into the assembly structure.

Your options are:
1. create an arrangement in the subassembly that supresses the other components, leaving only the plate visible. On your 2nd sheet create a base view of that new arrangement. Only the plate will appear. Note the new arrangement should not be the default one or your views on the first sheet will be affected.

2. Instead of creating the drawing inside your sub-assembly, use the master model approach to drawing and create a new part file for your drawing. Make the sub-assembly a component of this new file. Keeps the structure clean as is the preferred method of drawing creation. can use base or part views in this file without affecting the main die assembly.

 

[bbylls]

Thank you.
I never would have thought that the way you do drawings would have that kind of affect on models.
Great tip.