Rename part & drawing with dissimilar names

[ptc-5061493]

A quick search of the web tells me that this question has been asked many times before but none of the solutions I have found work for me and assume that the part and drawing are named the same.

I am running Pro-E Wildfire 5 and have a drawing abc.drw that calls part def.prt. I want to rename my drawing and part so that ghi.drw calls part ghi.prt.

I have tried opening both together then selecting File > Rename for the part with "Rename on disk and in session" set. Although ghi.prt is selected this does not create a ghi.prt file. Instead it keeps the def.prt file and updates the drawing model tree to call ghi<def>.prt.

If I do something similar for the drw file. i.e File > Rename > Rename on disk and in session then I do get a ghi.drw file but it still calls the def<ghi>.prt.

How do I rename my PRT file?

I am a pro-E novice, so would appreciate anyone who can help spell out the steps.

Thanks

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[TomD.inPDX]

You're close. You are probably holding your tongue wrong when you renamed the part file. It could well be that there is a working folder issue in the way.

I do this all the time for drawing revisions where I change both the model and drawing names.

This is -my- process; although you will likely get other tips as well. I just stick to the roots of how Pro|E works.

Open the original drawing

File>save-as>backup ...into a temporary folder. This saves everything!

Close the drawing

Erase not displayed (and nothing is displayed)

Change working folder to the temp backup folder

Open the drawing

Open the part from the drawing

Rename the part file

Save the part file

Close the part file

(Drawing file now active) Rename the drawing file (note it is now calling for the new part file)

Save the drawing file

Close the drawing file

Erase not displayed (again, nothing is being displayed)

In Windows Explorer, move the two new files to your normal working folder or into one of the search path folder.

Set you working folder to where it normally is

Open the drawing - this is now the new drawing name and it calls the new model as well.

This is all really easy once you get use to it. I am so use to it I don't even think about it (don't even realize how many steps are involved!). I don't use any of the new interfaces other than to just accept all the way through.

[TomD.inPDX]

..and welcome to the forum!

[ptc-5061493]

Thanks Antonius for your quick response. I must be holding my tongue the wrong way because I still have troubles. What you described is basically what I was doing, and I have repeated your exact steps just to be sure. The trouble is that when I rename the PRT file it doesn't create a PRT file with the name specified and where you had

(note it is now calling for the new part file)

I get NewName<OldName>.prt

i.e. It saves the part, when I attempt to rename, under the OldName and just gives it a NewName reference. This is what is driving me balmy (and probably the reason why my tongue is hanging out in the first place .

[TomD.inPDX]

Ohhhhh.... are you using family tables?

[Dale_Rosema]

It looks like family tables. If so, are all the instances going to be in the new family?

[ptc-5061493]

Sorry, I don't even know what family tables are - I'm not really a Pro-E user, I just need to make one change to an existing drawing that was created by someone else years ago. The drw and prt files appear to be stand alone.

[TomD.inPDX]

Sustainability of Pro|E files is a very commonly overlooked requirement when people start mucking around with "cool features". That is why I like bare bones, easy to explain, and readily accessible data.

And many will say that they cannot live without family tables, but I've done it for decades.

What are family tables? It is a way to make variations of the same part with one file. In your case, you have a specific variation of the master part, but the thing you are renaming is buried inside that master part file. This certainly makes things a bit more complicated and since I am not an expert at this, I hope someone else can step up to clarify how to deal with this.

[TomD.inPDX]

It always helps to try it myself.

In the model tree of the drawing, when you right click on the model xxx<yyy>, select "Open Generic"

Now you follow all the same steps. The "generic" is the master file. When you rename it, all the family table components will follow.

[ptc-5061493]

Hi Antonius, Thanks for persisting with me on this but I still had no joy. Here is what I get:

I start with two file in folder Test (1076336763.drw.1 & 1150137912.prt.1)

Open the original drawing

I open 1076336763.drw.1

File>save-as>backup ...into a temporary folder. This saves everything!

File > Backup then select folder Destination

Destination folder now has 1076336763.drw.1, 1150137912.prt.1, 1076336763.xpr & Destination.idx

Close the drawing

File > Close Window

Erase not displayed (and nothing is displayed)

File > Erase > Not Displayed offers 1150137912.prt, 1076336763.prt & 1076336763.drw

Change working folder to the temp backup folder

File > Set Working Directory and select Destination folder

Open the drawing

Opened Destination\1076336763.drw

The model tree calls 1076336763<1150137912>.PRT

Open the part from the drawing

I right-click the 1076336763<1150137912>.PRT and select Open Generic

I am prompted to Select Instance (this is a folder sheet metal part). I am offered 1076336763 and 1076336763-BLANK. I select 1076336763 because that is the part that the drawing calls.

Rename the part file

File > Rename Model=1076336763.PRT, New Name is changed from 1076336763 to AAA, Common Name is greyed out but says 1150137912.PRT, Rename on disk and in session is checked.

Save the part file

The Model tree in the part file now shows AAA<1150137912.PRT>

Destination folder now has:

1076336763.drw.1

1076336763.xpr

1150137912.prt.1

Destination.idx

1150137912.prt.2

aaa.xpr

1150137912.prt.3

Close the part file

File > Close Window

(Drawing file now active) Rename the drawing file (note it is now calling for the new part file)

No - The drawing model tree shows AAA<1150137912>.PRT

Save the drawing file

Denstination folder now has 1076336763.drw.2

Close the drawing file

File > Close Window

Erase not displayed (again, nothing is being displayed)

File > Erase > Not Displayed offers 1150137912.PRT, AAA.PRT and 1076336763.DRW

In Windows Explorer, move the two new files to your normal working folder or into one of the search path folder.

I copied 1076336763.drw.2 and 1150137912.prt.3 (AAA.PRT file was never created) to a new folder

Set you working folder to where it normally is

File > Set Working Directory to this new folder

Open the drawing - this is now the new drawing name and it calls the new model as well.

1076336763.drw.2 is opened.

Its model tree calls AAA<1150137912>.PRT

[TomD.inPDX]

We're getting closer. I was not prompted for an instance once I opened the generic. It is in fact 115013912 that you are trying to rename.

When you have the drawing open, try opeing 115013912.prt form the open menu. Then rename that part to AAA and save it. Go back tot he drawing and see if that updated the name as xxx<AAA.prt>

That instance thing is throwing me. Others probably understand it better.

[ptc-5061493]

There are only two files - a drw and a prt. The 1150137912.PRT file is the part file that I have been renaming. Pro-E is mudddling the name of the project with the physical name on disk.

Can I send you the files? We are about to close for a 4 day weekend (Melbourne, Australia stops for a horse race ) so I'd like to continue this next week if that is OK by you.

Thanks for all your asistance so far.

[TomD.inPDX]

I'd be happy to look at them for you, Michael.

You can send me private message after your holiday and we'll get this resolved.

Have a nice vacation!

[Dale_Rosema]

When you are in the drawing in the temporary folder, if you go to the layout tab, right click and select Dwg Models, then click on Del Model (but don't delete anything) does it give you any options as to models to delete, or does the command line say "Cannot delete model with views using it.".

Just trying to see if both the blank and the non blank instance are being used in the same drawing. Sometimes with sheet metal parts, the designer my be showing both the blank and the non blank part on the drawing.

You may then need to open the generic. Rename it. The go into the family tables (Alt-T [Tools], F [Family Tables]) to then rename the instance. Then both will have been rename to the new name. Do this while the drawing is open so that is stays connected to the drawing (in the temporary folder).

(and I hope your vacation was good and that your horse won!)

[dgschaefer]

You have a family table part here. A family table is one part file (the generic) that has many versions (instances). Think of a family of fasteners, same head style and diameter but a variety of lengths. You'd put the length dimension in the family table telling Creo that is what varies. Each line in the table defines the instance name and the dimension value for that instance.

So, in your case 1150137912.prt is the generic part, 1076336763 is the instance. That's why it appears as1076336763<1150137912>.prt. The generic part file contains all the information needed to make all the instances (there may be many), there is not file on disk needed for the instance. Once you open an instance and save it, however, Creo creates a *.xpr accelerator file to speed up opening the instance. Without it, Creo opens the generic, reads the table and then builds the instance. The *.xpr file is necessary, it just makes things faster.

All that siad, you can rename the instance just as any other part and Creo will change its entry in the family table.

When you renamed 1076336763 to AAA and it shoed AAA<1150137912>.prt instead of 1076336763<1150137912>.prt, that's exactly what should have happened.

The question is, do you want to rename 1076336763 or make a new part with a new name? Because 1076336763 is an instance of 1150137912, renaming changes the generic 1150137912 and once backed up into your master file database will eliminate 1076336763.

There are a couple ways to proceed depending on if you want a new part, truly replace the old part with the new and if the new part should be tied to the old generic or not. Rather than go through all the scenarios, tell us what you are tyoign to accomplisha dn I'll guide you through it.

[TomD.inPDX]

Doug, Michael is on vacation for a few days, but he is trying to rename the master (generic) part 1150137912. For some reason, it is not allowing him to open the generic and is prompted for an instance to open.

I went through this, but I was not prompted to open an instance when I opened the generic. Is it possible to lock the generic so you cannot open it from the drawing?

I will have a look at his files when he gets back. But I am interested in learning more about family table "issues".

[dgschaefer]

I had to go back and reread it because I, admittedly, did not read everything carefully. He said above:

Open the part from the drawing

I right-click the 1076336763<1150137912>.PRT and select Open Generic

I am prompted to Select Instance (this is a folder sheet metal part). I am offered 1076336763 and 1076336763-BLANK. I select 1076336763 because that is the part that the drawing calls.

It sounds like it is prompting him for the instance and it is the instance he is trying to rename.

Later, however, he says:

There are only two files - a drw and a prt. The 1150137912.PRT file is the part file that I have been renaming.

I'm not 100% sure what he's trying to do, but I think he wants to rename the instance. What I'm not sure of is if he's trying to replace this part (the instance) or create a new one. The path forward depends on the answer to that question.

I guess we'll have to wait until he returns next week.

[ptc-5061493]

Wow, You guys have been busy while I have had a relaxing 4 day weekend. Thanks for all of your comments.

Dale - I tried your steps (it was slightly different as I am using Wildfire 5 and not the latest Creo). When I click Del Model the command line shows "Cannot delete model with views using it".

When I enter the generic model of either the folded metal part or the blank part and call up the Family Table they each say "This model currently has no family table design variations." So I don't think that there is an instance here that I can rename.

Doug - Thanks for your explanation of family tables. What I am trying to do is create a new part based on an existing part. I am an old school AutoCAD guy with no Pro-E experience. I hadn't even considered making a variantion of the part within the original part file. I was trying to rename the drawing and part to something else and then edit them as competely separate entities from the original part. I am sure that this is considered bad practice, as the old and new parts will both be current at the same time and come from the same tooling, but given my zero knowledge of Pro-E, this was the simplest way for me to go.

Following on from my reply to Dale, would you still say that this drawing uses family tables? The change that I need to make is to create a variant of the part with one side missing. I literally need to open the file, delete a flange and save it. A family table sounds like an excellent way to achieve this. The hard part is editing the titleblock info and maintaining the files in our doc library.

Antonious - I'll send you a PM after posting this and see if I can get the file to you. It is probably me just being a dumb novice and the solution will be obvious to someone who knows Pro-E.

[TomD.inPDX]

email sent.

[TomD.inPDX]

For everyone's benefit: Indeed the part model has a family table that was likely created when you make a flat pattern instance in sheetmetal parts.

Something I did learn, however, that is very useful; you can go to the Drawing Models dialog and -replace- the instance with the generic and all the views and dimensions... etc. remain intact.

[TomD.inPDX]

...Oh, and all the Format Table data was hidden in part's Parameters rather than Relations.

I guess that's just a matter of preference but it always throws me.

[dgschaefer · Accepted solution]

You definitely have a family table. When you see a part name like this:

instance<generic>.prt

That indicates a family table driven part. The generic name is in the brackets, the instance name is before.

So, am I correct in assuming that you have generic master part 1150137912 with a version 1076336763 and it's flat 1076336763_flat. You want to create a new version of 1150137912 but keep 1076336763 and the flat. Correct?

If so, it's a bit complicated, but not too bad. Try this:

1. Open the drawing and save it as a new name. We'll come back to it later.
2. Open the generic 1150137912.
3. Open the family table inside the generic by going to tools > family table. It looks a bit like excel, but it's not as friendly. Each row represents an instance, each column a variable item. It could be a feature turned on and off or a dimension to vary. Your table likely has two instances (or maybe more) and at least one column, the flat pattern or unbend feature to make the flat.
4. Click in the part name cell for the last row (instance) and hit enter. That creates a new row and a new instance. Type in the name you want.
5. Hit enter again and type in the name of the flat for the new part.
6. Now, duplicate the entries in each column from the old part to the new. For example, the old will have "N" in the unbend, your new should have "N" in the unbend. The old flat will have "Y" in the unbend, your new flat should have "Y" in the unbend. This will give you duplicates of the original instance and flat.
7. Select the column to the left of the unbend. Click the "insert column" icon on the toolbar. It should be next to the binoculars. This brings up a dialog box.
8. In the dialog, at the bottom select "feature". now select the flange you want to remove from the new instance.
9. Select OK.
10. All the cells in the new column will have * in them. This means that it is just like the generic. If suppressed in the generic, it will be in the instance. You want it to say "Y" for all the old instances and "N" for the new. Keep in mind, removing this from the instance will also remove all its children from the instance.
11. Click OK in the Family Table dialog. You've just made two new instances.
12. Save
13. Go back to the new copy of your drawing. You now need to replace the models with the new instances you created. Right click in an empty part of the drawing and select 'Drawing Models'. In the pop up menu, select replace. Pick the model you want to replace and then the corresponding new family table instance you just created. I'm assuming your drawing has both a formed and flat state, so you'll have to do this for each.
14. Save and then clean up your drawing as needed.

You now have the new instances in your existing generic with the old. I typed this up with WF5 open, so it ought to be accurate, but I did do it rather quickly. Let me know if you have more questions.

[ptc-5061493]

Thank you Tom, Doug and Dale for persisting with me - you were all spot on. I used Toms emailed instructions yesterday to get the job done and just came in this morning to write up this thank you and the steps that I took to find out that Doug had beaten me to it and spelled out exactly the method I ended up using.

The first problem that I had was that I was not opening the Generic version of the part. Even though I right-clicked the part in the drawing model tree and select "Open generic" it would then offer me a selection (of what I now know are the flat and folded family table instances) under what I thought was a heading "The generic". I took this to mean "The generic" folded part or "The generic" flat part. What I wasn't realising was that "The Generic" was not a heading but a selection itself. So even though I had selected "Open Generic" already I then had to select "The Generic" again. Once I did this, all of your previous instructions made sense as I was able to open the family table.

I was able to make a new part instance as Doug has just described. I made a copy of my original drawing and had it call the new part instance. As all of the titleblock entries were in parameters of "The generic" I was able to apply the same method to add the relevant parameters to the new parts in the family table so that each drawing now called parameters specific to it e.g. Product A or Product B.

Apart from my computer crashing several times along the way I had no real issues. Thanks all for your time and patience in answering my question.

[dgschaefer]

Glad it worked for you. Family tables can get complex, but once you understnad the concept they become easier.

[Dale_Rosema]

About opening the generic and then having to select again the generic, here is a product suggestion that you may wish to vote on:

http://communities.ptc.com/ideas/1687

Thanks, Dale

As Doug mentioned, family table can be confusing at first, but also can be vary powerful for similar parts.