I am after some advice about updating drawing views when the source part file name has been changed.
Our file names include the issue status, eg Part_Issue_A.par, Part_Issue_A.dft.
When a change is required I would like to make copies of the original files with the new name Part_Issue_B. Then apply the changes to the issue B part file and use this to update the drawing views in the issue B drawing file.
The problem I have is the views in the issue B drawing file obviously still reference the issue A part, can this be change to the issue B part? I don't want to regenerate views, dimensions, etc. every time a change note comes along.
I am using ST8 and have just moved over from 2D (Autocad LT). The system in place archives existing drawings to be replaced with new versions with revised file names. This how I have always worked in 2D, but I didn't have the problem of inter-file dependecies then!
Thanks for any help with this.
Solved! Go to Solution.
SE button (top-left)
In this window, click on te file to change
If you use Revision Manager to do your save-as (a move or copy action) you can optionally search for linked drafts and move or copy them too. These copies will be automatically updated to refer to your new part or asm file.
You should do this at asm level (even if the asm is not being revised) so the assembly will be updated to point to your new Rev B, and you can also revise multiple parts in one go.
I would further reinforce what @Alex_H said. If you use Revision Manager, you don't have to do any manual work. Use the "Increment" command in Revision Manager to automatically copy Revision A to Revision B -- it will automatically update the Revision property in the files also to B (as of ST7).
Final trick -- if you pick the assembly DRAWING as the top level to revise, it will find the assembly and all parts under that without needing to do a where used for the Drawing. If you think about it, the drawing is kind of like an assembly of the 3D stuff. It is definitely that way architecturally (Drawing is parent and asm/part is child). That is why this trick works.
ALso another thing to consider is to have create a location on your server for latest release drawings and a place for obsolete drawings.
After you totally finish a drawing and it is approved--"Save As" a PDF of it to the "Approved" folder. Anytime a change is issued, move the one in the Approved to the Obsolete folder and affix a -"latest revision letter" to the end.
Then save the newest change into the Approved PDF folder.
This way you have PDFs of your drawings that CANNOT change. The thing with .DFT files, especially coming from AutoCad is that they are parametric. So ANY change you make to a part or assembly will affect that drawing. If you are only going by DFT files and not creating PDFs of approved drawings, you are setting your self up for disaster!!
Please see below screenshots of what I am talkiing about:
Approved PDF Folder:
^^^Everything in the folder is the latest & greatest approved by engineers drawings.
^^^Everything is this folder is previous revisions.
So as you can see, I have a copy of all of the previous approved drawings in the obsolete drive. This way if ANYTHING ever happens to the CAD system files, you have a copy of the drawing that cannot change parametrically.
Just a hint for you. Please dont control it all via the DFT files; create PDFs of your drawings as well.
Thanks for the advice, it looks like we need to make improvements in these areas in line with your suggestions. And Revision Manager seems like a very handy tool to get to know.