No. Part and assembly files do not include any information about what assemblies or drawings or any other places they are used.

You may be able to use a text search on the assembly files. The references used to be in plain text near the start of the file.

Ah, I see. Well that makes my job more difficult. Thanks! Do you know on the offchance that if I change a part name and forget to pull a certain assembly into session, that It can locate it on the new name without having to rename the part back to the name the assembly used to reference? If I change a wire from wire1.prt to ground-wire the assembly will say "Can't find wire1.prt; I'd like to be able to point to ground-wire.prt now.

The easiest is to not mess up. If you miss one the software will allow you to replace it with another part, but as far as the software is concerned, it is a different part. Balloons, notes, created dimensions, other components assembled to it will all lose their references.

A more complicated method, but not as difficult to keep straight, is to create a family table in each of the parts, a family table that at the end will be deleted.

The table will have only one instance - that's a line with the new name. Add the instance, Verify, and save the generic. Once in place, you can replace each item in each assembly by family table and every reference will be exactly maintained - drawings, other assemblies, and so on. I think you can select items that are used in multiple places in an assembly for a mass-replace by family table, just in case yo have an assy with 500 misnamed rivets, for example.

When you are certain that all items have been replaced in the assemblies and drawings with the correct names, you can go back and open the each instance, then the related generic; delete the family table entirely and save the generic, then save the former instance - it will be a new, independent part. If this process is messed up, you are in the same position as you would be if the item was overlooked. However, the assemblies and drawings can be dealt with one at a time and can be done by more than one person at a time using the family tables.

The alternative is to open all assemblies and all drawings that use a part into memory at the same time and rename the part and then make sure you save all using assemblies and drawings. Miss one, and you are back to damage control.

An enhancement to the process is to create a parameter call replace_status. I'd go with a string of "old" for the parameter value, In each family table you add that parameter to the table and for the instance set the value to be "New". This parameter can be shown in the model tree for visual feedback of what's getting renamed and if it's been replaced yet.

Use findmymother.exe, it will let you type in a part or assembly name, pick which folders to search and tell you all the drawings and or assemblies that use it.

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• http://files.engineering.com/getfile.aspx?folder=9f0320bb-fb0a-4c4c-947d-70

This is what Google finds on findmymother.exe

http://www.mcadcentral.com/creo-tips-tricks-assemb...

It has a link to the file, but either the file is no longer there or one has to register with MCAD Central first.

I also indicates someone named dr_gallup suggesting a contains-text form of search using Windows Explorer, which I suggested earlier, though dr_gallup added the drag-and-drop enhancement for the Windows Explorer search results.

Current versions of Windoze are totally incompetent at searching files for embedded text strings. I was initially skeptical of findmymother.exe but now I use it without exception before renaming. It is attached in my post above. dr_gallup & I are one & the same.

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OK I see it now. I typically skim over the signature blocks, seen them once ... ; also this forum system doesn't display the whole path so it looked more like a signature picture.

I figured there was more than a passing similarity in the names. I gather that you did not write the program; it's interesting that Google knows so little about it. It doesn't have much press.

Would you like to post this at PTCuser and/or PTC/Community? There are a number of people there who don't use a PDM system who might find this helpful. If not, let me know and I'll link to here and the MCAD post.

Finally - I remember the good old days of fixing assemblies when some user would get the bright idea to change a filename ruining assemblies and drawings farther up the line and when one could read the drawing notes directly from the drawing files in plain text to check for spelling errors and inconsistencies. PTC clamped down on the files before I got a good chance at figuring out how to create or modify features with a text editor.

Post it anywhere you like. I did not write the program. Yes, for most of Pro/E's existence, you could use a text editor with find and replace functionality and simply change the old part name to the new part name in your assembly or drawing file. PTC never endorsed this and eventually took the ability away when they got serious about selling PDM software.

I have no idea why PTC won't let us simply tell Creo that the part it is looking for now goes by a new name except that too might reduce PDM sales.

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I'll look into this Findmymother.exe. Thanks. I'll have to get my Admin's approval on it before I download and install any executable file so hopefully I can find some information on it.

You won't find much info on it. Get your admin to build a virtual machine and install it and verify that it doesn't do anything bad.

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"for most of Pro/E's existence, you could use a text editor with find and replace functionality"

Ahhh, the good old days!

-tg

http://xternal.me

And here's the case when a PDM system would (have) save(d) your life

My guess is that you are not using PRO/INTRALINK?
Because with PRO/INTRALINK, you could simply just request a "Where Used" on your part/assembly and it will tell you exactly where your part/assembly is being referenced.

My advice is to start using PDM.

Thee are lots of us with just a handful of users and no sys admin for whom a PDM system is completely out of the question, not to mention gross overkill.

The best thing is NEVER RENAME PARTS in Pro/E!

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Although this would be time intensive with a lot of data entry: add a parameter to each part for where used before renaming/copying. If you are going this route I would also add it to your start part so you have the spot for new designs.

A part can be used in hundreds of assemblies.

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