I am working with Creo Parametric 2.0 to create drawings of revised sheet metal parts. These are large parts and assemblies with multiple sheet drawings. What is the quickest/easiest way to create a new revision of a part and its drawing? For example, I added some basic holes to one to create a rev B part, but now I am faced with how to easily make the drawing for the rev B with out having to redo all the dimensions, views, etc.
I used to use Inventor, and there you could change the referenced part in the model tree. I tried to do the same thing here by highlighting the part, clicking the drawing models button, then clicking "add model" to insert my revB part. This changes the name in the model tree, but doesn't show the changes to the part. I tried to delete the old revA part by clicking "del model", but no luck. Also, if I save this drawing then reopen it, the part in the model tree reverts back to the revA.
I also tried seeing if I could do some magic with save as, where I saved the revA drawing as a backup to a different directory. Then changed the part that came with it to the rev B, but if I do a save as, it just duplicates the part. Then there are both a revA and a revB, and the drawing is still referencing the revA. If the revA is deleted, the drawing, when opened, freaks out that its original part is gone.
There has got to be an easy way of doing this... Please help!
Thanks in advance.
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Have you tried opening both the part rev A and drawing rev A, and tried to do a rename on both? So while both are open, rename part rev A to part Rev B, this should also rename it in the drawing rev A if it is open or in memory, then rename drawing rev A to rev B.
Do you use Windchill? If so you can do a "save as" in Windchill for both the part and the drawing. If you are not using Windchill then having your parts family tabled would work. If the parts are part of a family table you can simply save a copy of the drawing then replace the model in the drawing with a memeber of the family table.
If you want more details on either of these options let me know I can explain how to accomplish either.
I am only using Parametric, not Windchill. Please explain this family table idea? Thank you.
Since I don't know how familiar you are with family tables, here is a helpful link about creating and editing family tables. http://www.brighthubengineering.com/cad-autocad-reviews-tips/24487-how-to-create-and-use-family-tabl...
If you are not familiar with family tables this may not be the best option for you in this particular case, simply because learning family tables can take some time. If you do have the time I highly recommend learning about family tables as they can be very useful.
In your case it seams you already have one part completely modeled, so I would use that part as the Generic for your family table and create the second part as an istance. To do that you make all the modifications in the generic part and use parameters and programing to turn features on and off based on which part you want.
With these parts as family table members you can simply open the orginial drawing, select file>save a copy and save that drawing. Then open the newly created drawing, right click and select drawing models, then select "replace". Since these parts are part of a family table a box will open with the family table members. Select the member of the table you want the drawing to be of. The drawing should regenerate automatically, if it doesn't select regenerate. The new part should now be in the drawing and all dimensions and notes should update.
Remember if any surfaces where removed those dimensions will fail as they have lost their reference.
Do you have to save an electronic version of the revision A part?
If not, I just have a parameter - Revision in my model. When the part is bumped a revision, I update the model parameter to the new level and it automatically updates the parameter in the drawing by the same name. I just that have to add a line to the revision block stating what the changes are.
Revision parameter in the model:
Revision parameter in the title block:
Adding a row to the table of the revision block:
I would if for no other reason then to have a copy of it for reference or to track part history.
With Creo, using different filenames for each revision is not standard practice. If that part is in an assembly, you will have to replace the "rev a" part with the "rev b" part. Easy for one assembly, but if it is used in 20 assemblies, you'll have to replace the part 20 times.
Obviously I am making some assumptions here, I don't know your situation or even the reason you are doing what you are doing. Years ago, we used to do this with CADkey (just like autocad). But that was before parametrics and reuse of data and single model definition. It was our way of keeping history.
If you are using CREO without file management, each time you save it will create a different "version" of the file .1, .2, .3, etc. Using this along with file dates, you can copy out the old revision and save it in a history folder. Or simply copy it out before you make changes so you can keep it. That way you can always keep your latest revision file name the same and all your history can be saved separately.
Just some thoughts. If I am completely incorrect in my assumptions, please ignore me as I am old and mostly crazy.
Halle, are you actually creating a part revision? I just took Rev A and Rev B as generic names, thinking you didnt want to give actually part names. If you are creating a part revision and not 2 seperate parts, I believe I have lead you in the wrong direction.
These are part revisions I am talking about. I am taking the revision A part, making a few small changes, then saving it as the revision B.
I do want to keep the revisions separated. That way I can keep track of everything for engineering history. So each part revision needs its own part and drawing.