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How to create a "rev B" of a drawing and part from the "rev A"?

Forum|Forum|12 years ago
October 2, 2013
18 replies
13900 views

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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2D Drawing

Best answer by AndyHermanson

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.

J

JamesBurcham

1-Visitor

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.

P

ptc-5160270

Author

1-Visitor

I am only using Parametric, not Windchill. Please explain this family table idea? Thank you.

J

JamesBurcham

1-Visitor

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-tables-in-pro-engineer/

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.

StephenW

23-Emerald III

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.

Steve

J

JamesBurcham

1-Visitor

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.

P

ptc-5160270

Author

1-Visitor

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.

A

AndyHermanson

Answer

14-Alexandrite

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.

Dale_Rosema

23-Emerald IV

For legacy reasons, I might save out the revision A drawing in a pdf, but have an electronic version of the CAD file is going to be tough especially 15-30 years down the road.

Dale_Rosema

23-Emerald IV

I forgot about another option I did several years ago.

I would "back-up" the drawing and model.

Zip the backup and move it to an "Archive directory"

If we had to refer to a previous revision level, you could go back and unzip the files in a separate project folder for use for the specific application and delete when done.

This too is going to eat up a lot of space on the hard drive / server depending upon how many revisions and how big the parts / assmblies are.

Thanks Dale

P.S.

The larger the assemblies, the more files that are going to be created when you do a back up because you'll need all the subassemblies at the rev level they were at when you created the backup (I can see a big nightmare coming down the road in a couple of years with mixed up files).

StephenW

23-Emerald III

Just to be clear, If you have assemblies, you will have to replace the original.prt file model with the new revb.prt model.

In my opinion, you would be better off always keeping the latest revision without a revision letter in the filename and all the older revisions can be renamed to keep history. This method will keep you from having to re-assemble your parts in to your assemblies. All your users would know that if the didn't have a revision number in the filename, it would be the latest and greatest but if you had a file with a revision letter, it would be an outdated model.

Again, this is based on my experiences and may or may not apply to your situation.

Steve

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