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I currently have a design with drawing that i want to copy to begin another design. Is there any way to copy the drawing also so that it recognizes the new design name? Thanks for any help with this.
IIRC, you can only replace the model with another instance from the same family table. Are your two parts members of the same family table? If so, you could save your existing drawing under a new name, and then choose File > Properties > Drawing Models > Replace.
The recommended technique for what I think you're trying to do is via Drawing Templates. The idea behind that is to:
<UL>
<LI>Create a new drawing.</LI>
<LI>Applications > Template</LI>
<LI>Insert Drawing Template Views configured for view type, scale (or sheet area in WF3), dimensions, balloons, appearance, snap lines, etc.</LI>
<LI>Place pre-configured tables such as revision tables and BOMs.</LI>[/list]
Templates really can save a lot of time and effort if you are doing the same kinds of drawings over and over, but require some set up work.
1. I'm using WF2 not related to Intralinkand I open the part then hit save a copy give the new name and it automatically saves the drawing too with the new name.
2. I also use Intralink3.4 with WF2 and from a workspace in Intralink you select both part and drawing , right click , then duplicate objects and in the window that appear you enter the new names for part/drawing and then if you open them PRO-E they will be related.
Set the config.pro option rename_drawings_with_object to BOTH. Now, open the part that the drawing refers to. Select "SAVE AS", and give it the new name. When it saves, it willcopy the related drawing so that it refers to the new part.
If your drawing refers to an assembly, open the assembly and do a "SAVE AS", and give itthe new name. You will now be able to rename any or all of the components. Again, the drawing is copied so that it relates the drawing to the new assembly and components.
First, the drawingmust have the exact same filename as the part or assembly that it refers to. Exmple: "mypart.asm" and "mypart.drw". The number extension that Proe adds to the filename doesn't matter.
Second, set the config.pro option rename_drawings_with_object to BOTH. Now open the part file that the drawingrefers to. Do a "SAVE AS" and give it the new name. When it is saved, a new drawing will be created that refers to the new part.
If the drawing relates to an assembly, open the assembly file and do a "SAVE AS" and give it the new name. You will now be able to rename any or all of the components. When it is saved, a new drawing will be created that refers to the new assembly and its components.
I don't know if I don't understand but we reuse drawings and parts all the time to make other designs. It sound like everybodys answer is to complicated.
All I do is make a copy of my original into another directory. Then I open thedrawing, the assembly, and the part. in that order. I then rename the part and save then I rename the assembly and save and then the drawing.
We are using wildfire(1) but I know this technique will also work in wildfire (2).
If you are using intralink just pick the "duplicate objects" option.
You will be given the option to choose what parts, assys, drw's and instances to duplicate or reuse.
If it is just a part and a drawing the simplest way is to open them both then rename IN SESSION the part and the drawing. Now you have a new part and drawing that are not linked to the one on disk. Make your changes and save the drawing.
The rename_drawings_with_object works only if you name you model the same as your drawing, which we never do.
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