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file references

file references

file references

(OP)
I have just noticed this behavior in SW2005 SP2 and am wondering if this is a bug or not.

I have an assembly fully developed and am now starting on component drawings.  Some of the components are similar, such that I'd like to get one part detailed and copy the drawing (and then re-reference the correct part).

For example:

AssemblyA
  Part1
    Drawing1
  Part2
  Part3

Parts 1, 2, and 3 are very similar, so Drawing1 gives me a great starting point for Drawing2 and Drawing3

I have Assembly A open, all parts resolved, and finish Drawing1.  I save Drawing1.  I then Save As (checking save as copy) Drawing2 and close the drawing.  AssemblyA is still open.

I then open Drawing2, changing the reference from Part1 to Part2.  I get the dialog box saying that the Internal ID of Part2 which is already open doesn't match that of the referencing document and click Yes to accept anyway.

So now I have AssemblyA open as well as Drawing2, which references Part2.  I then go back to the assembly to find that Part1 has been replaced with Part2!

Is this what I should expect to happen, or is this a new "feature" of 2005?  I am pretty sure that I've done this before and not had my assemblies get messed up.  I thought that I was changing the reference in the drawing only, not the assembly, but apparently that's not the case.


Thanks,
Dave Gowans

RE: file references

This is what you should expect to happen. To do this so that you do not get this result you should copy "Drawing 1" twice and rename it for "Drawing 2 and 3".

Now close all parts/assemblies/drawings.

Select Open, then browse to "Drawing 2" but do not open it yet. Just select it. You should see a "References.." button beneath the "Open & Cancel" button.

Click that button to open the "Edit Reference File Locations" window. under where it says "New pathname" there should be a box to check to the left of the pathname. Once that box is checked browse to find "Part2" and select "OK" after you are done. Now when you open "Drawing 2" it will be referencing "Part2"

Repeat for Drawing 3 and so on.

Doing the above method I have not had any problems.  However there may be a better and faster way. but this works for me.

Best Regards,
Jon

Challenges are what makes life interesting; overcoming them is what makes life meaningful.

Solidworks 2005 SP2.0

RE: file references

(OP)
That is what I was doing with the exception of closing the assembly before changing the part referenced by the drawing.  I now realize that having the assembly open is causing my headache.

Why does changing the drawing reference change the assembly reference?  Seems counter-intuitive to me.

Thanks,
Dave Gowans

RE: file references

The easiest way for me is to create part1, then part1 dwg. Open the dwg1 and part1, in part1 "save as" part2, then dwg1 "save as" dwg2. Same for part3/dwg3. THEN create assembly last. I always finish parts/dwgs first, especially if they are similar, before creating the assemblies. Saves a lot of time.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP1.1 / PDMWorks 05
ctopher's home site

RE: file references

dgowans,

Another way to try, go to File, Open, in the open window highlight Drawing 1, rmb, copy, then rmb where you need the file and paste.  You will now have a file called "Copy of Drawing 1", rename to what you want, with the new name highlighted click the References button in the Open window and browse to the part that you want (essentially replacing part1 with part2).  After closing the Reference window open Drawing 2 and you should have what you want.  You want to have all of the files closed to perform this or you run into the problem that you had.

mncad

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