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renaming parts

43 REPLIES 43
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Message 1 of 44
safiredesignengineers
9853 Views, 43 Replies

renaming parts

hey group

 

is it possible to simply rename a part?

I quite often make up quick parts to try stuff out and call them random things but if I want to change the name it is not just a simple case of renaming the part as a few things need updating.

 

is there a simple quick way to rename a part in one hit without going through other stuff?

 

regards Adrian

43 REPLIES 43
Message 2 of 44

Quickest way is just to rename in windows explorer.

You will lose the references to the part in assemblies,drawings and derived parts.

On opening any of these files just point to the newly renamed part.

For multiple parts you need an excellent memory or meticulous notes.

 

Remember if they are used elsewhere all where used references need to be updated.

 

If you have a lot to do, use design assistant, but beware that you cannot rename parts to existing names in one step, unless you do a copy to another folder rather than rename.

 

Alternatively save copy as new name then replace which is about the same effort as the explorer rename.

A few different ways but no simple rename - finished, as references must be maintained and the filename is the reference.

I may be wrong but I think Vault will rename and update references, Vault users should be able to confirm yea or nay.

 

Message 3 of 44

Hi Harco

 

thanks for your reply, this is somthing that should be made easier. for an instance if you make an error when naming a part e.g a spelling mistake then it should be just a case of editing the name and done, but it seems such a work up to do such a simple task?

 

regards Adrian

Message 4 of 44

> but it seems such a work up to do such a simple task?

 

It's a simple task to name in words, but so is "cold fusion".  What is Inventor supposed to assume when you rename a part?  Start searching the current project for references?  Start searching the entire drive?  All drives to which your computer has access?  How on earth could Inventor possibly know the scope of the change you are making?  Even if you're using Vault, making searching unneccessary, you could have references in lots of places; should Inventor simply assume that you want to change them all?  If I'm understanding your request correctly, you'd like Inventor to read your mind.  You might check the Labs site to see if that add-on is posted yet....

Message 5 of 44

Wow Sam, do you work for Autodesk?  I would guess so if you are comparing the renaming of a part to "cold Fusion" or even "mind reading"  8-)

 

Rgrds  Adrian

Message 6 of 44

I'm curious how you would expect this to work?  Right click on a component in an assembly and pick "Rename"?  Then what?  It offers you a Rename Part dialog box?  You type the name you want, hit OK, then what happens?  The part/assembly file is renamed, and the current assembly's reference to that part/assembly file is updated.  Now what?  What about other files that reference that component?  Drawings, other assemblies, derived parts?  How does Inventor know what to do without reading your mind?

 

No, I don't work for Autodesk.  But I have a certain amount of sympathy for programmers who get told by users that the new functionality they want is simple.

Message 7 of 44

Sam, i guess your having a bad hair day!  8P

 

I use, edit and build a database and if i change a field name it updates the field, the table, the relationships (comlicated), it updates the forms and any calulation (really complicated) that it appears in. it works simply and effortlessley. it is a program on a computer.

 

now in this scenario you are assuming that the name to be changed is a part that has gone through many processes and is used in many files and drawings etc..

But I am talking about at the creation of the design stage when a lot of data is unknown or if it is a typo and it needs editing. this means there is no other files involved. I guess once a part has got pass the initial design stages it can be locked down as a final version this would not be changed as a general rule of thumb and would need a process to make sure all parts are up dated as required.

 

 

 

 

Message 8 of 44

Nope, never have bad hair days...

 

>> But I am talking about at the creation of the design stage when a lot of data is unknown or if it is a typo and it needs editing. this means there is no other files involved.

 

I understand that at this point in a project it's simple.  But how on earth can you expect Inventor to know that you're at this point in a project?  If the programmers give you a button to change part names early in the project, other users are going to expect it to work for them any time they want, which will potentially wreak havoc in their designs.  Then they'll be screaming at the programmers for all kinds of unintended consequences they didn't foresee.

 

Nothing wrong with asking for additional functions in the application.  But asking for something that is in a completely different kind of application and then suggesting that since it exists there it should be easy to do in Inventor is rather insulting to the people responsible for Inventor.

 

I imagine that what you want to do might be relatively easy to accomplish in Vault (a database), but since I don't use Vault, I can't be sure.

Message 9 of 44

Hi Sam

 

I think your over engineering the problem / solution. I think that most designers will know if they are using or editing a "stock" part or a new part. if really required a warning window could pop up to warn of potential issues and this can have a simple ok or cancle button. I don't use vault and I am sure this will handle your issues much better, but on a project level this should not  be a problem to solve 8-)

 

rgds Adrian

 

Message 10 of 44

In general I agree with Sam but not quite so vociferously.

I also agree with you Adrian as far as database is concerned but basic Inventor is not a database, Vault is the database.

Inventor is a stand alone program and can only save, save copy as or save as the same as Word,Excel, Photoshop etc which cannot rename files either.

Can you give an example of a program which can rename files while they are open, this would be contrary to Windows file management would it not.

The only program I can think of which could do what you require would be Mechanical Desktop but only when all references were contained in the parent file, don't even go there!!!

Because of the references to other files you need an intermediate program to maintain links if you alter file names.

If you are on a small project with limited references Design assistant will rename and update references as you require.

 

Message 11 of 44
MiSt2047
in reply to: harco

> Can you give an example of a program which can rename files while they are open

 

Pro/Engineer. Since every version I seen from 1997 and forward.

 

It has always been a paragon of virtue in this regard. The parts and subassemblies in an assembly are the same memoryspace that the parts are, so if you have an assembly open in the background and open and manipulate one of its parts, the changes are transferred to the assembly instantaneously.

 

This includes renaming parts and subassemblies. Rename a part, and when you switch window to the assembly it is in you see that the name in the tree is changed as well.

 

Caveat: all assemblies that includes the part must be opened and in memory, and saved to retain the new part name information. Thus it is not much better than Inventor for renaming articles that are used in many different (and possibly unknown) assemblies.

 

Message 12 of 44

I do this quite often too, play around with a part, and if I end up using it and it requires a part number to be assigned and cataloged, this is my workflow:

 

-use the save as option to make a exact duplication of the part and give proper name

-if that part was used in an assembly, I find the "old/bad named part" right click and use component->replace all

-this ensures that all the parts with the bad name is replaced with my newly named part and all work done including

 constraints are kept.

- i typically don't have drawings done at this point, because the part was basically a test part, not sure what the

  workflow would be for ensuring newly renamed items would keep associativity to drawing views.

 

Good Luck!

 

edit: maybe you should make an ideastation thread, get some upvotes for it, I think it would be possible to have a renaming process addin for inventor, to kinda do what I do above. real handy tool to have for sure...

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
Message 13 of 44
misterkoenig
in reply to: harco

Harco,

I'm coming from a Solidworks background. I've used ProE (last time Creo 2.0) as well though we used Windchill for file management which had it's own quirks.

>Can you give an example of a program which can rename files while they are open, this would be contrary to Windows file management would it not.

The functionality in Solidworks is this.
-If you want to "rename" a part that is relatively new you open up the files that reference it (assemblies and drawings) and then open the file you want to change. You do a save as and it updates the references in the open files. Then you simply delete the old file. You can also select "save as copy" which doesn't update the references.

Like inventor you can also change it in windows explorer and then "find" it for the assembly/drawing when you open the upper level drawing.

-Mark
Message 14 of 44


@safiredesignengineers wrote:

hey group

 

is it possible to simply rename a part?

I quite often make up quick parts to try stuff out and call them random things but if I want to change the name it is not just a simple case of renaming the part as a few things need updating.

 

is there a simple quick way to rename a part in one hit without going through other stuff?

 

regards Adrian


Treed, as they say in car forums

Guess I should have finished reading the thread, The SW stick has already been used.

 

This is one of the things Solidworks does so much better and I was shocked that Inventor made it so difficult. In SW going to an assembly, opening a part and doing a "save as" put the new part in the assembly. "Save as copy" made a new part but did not put the new part in the assy. To my surprise and fustration in Inventor "Save as" and "save as copy" do exactly the same thing.

 

So what I do now is open the part in question, save as making the changes I need to make and then use component replace to insert the new part into my assembly. This way all the constraints etc stay in place. 

 

Vault has a rename function but parts have to be checked out, checked in, relaoded, way too much effort

 

 

Message 15 of 44
pball
in reply to: Mario428

I don't know if this feature was around when this thread was created, but at least 2013 and newer have a command called"Save and Replace Component". This command will save a copy of a part and replace it at the same time. This is probably the closest you'll get to renaming a file while inside of an assembly for the time being. The only caveat is if there are multiple instances of part1 lets say, that command will only replace the part you have selected and every other part1 remains unchanged.

I actually created a "Save and Replace All Components" macro if anyone is interested. It does exactly the same thing as the built in command except it replaces all instances of the component.

Of course either of the methods above still have the issue of not affecting anything except the assembly you are working in, since it's not really possible to rename something and have it magically update in everything it was used in (unless you have vault perhaps).
Message 16 of 44
DevinCurrie
in reply to: pball

Do you mind sharing the macro? Thanks!

Message 17 of 44
pball
in reply to: DevinCurrie

It crossed my mind to add it to my last post, but then I forgot lol. I attached it in a text file so you just need to copy it to your vba project. Simply run the macro and select the part/assembly you wish to save and replace and a save as dialog will appear. Then every instance of said part/assembly will be replaced automatically. Only difference I know of between my script and the built in function is you can not have a part highlighted and run the command, you have to select something after the script is ran. I could fix that but haven't felt the need.

Message 18 of 44
DevinCurrie
in reply to: pball

I have tried the macro and it is working great except for one small thing.. after renaming part/assembly within Inventor, the macro will create a copy of the original file with a new filename. The macro didn't delete the original file.. can you please tweak the code that will remove the original file after successful rename? Thanks again!

Message 19 of 44
DevinCurrie
in reply to: DevinCurrie

FYI

 

Additional test revealed that renaming part from Content Centre (CC) will work too as long the IPT file is saved to the project folder via "As Custom".

 

Things began to go awry after replacing the renamed CC part with another CC part (e.g. longer screw).

Message 20 of 44
Mario428
in reply to: DevinCurrie


@DevinCurrie wrote:

I have tried the macro and it is working great except for one small thing.. after renaming part/assembly within Inventor, the macro will create a copy of the original file with a new filename. The macro didn't delete the original file.. can you please tweak the code that will remove the original file after successful rename? Thanks again!


Personally I do not want the original file deleted unless I replaced it for a typing error.

 

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