Best way to rename content center file

[MatthijsAstratec]

[Inventor Professional 2024 + Vault Basic]

I have a part, which is imported as a content center file. I put the dimensions in the part file name, so our machinists and mechanics know which material to use straight from reading in file explorer.

For design purposes, I want to change the size of the content center part. (However I cannot change the size within the part environment, I must do so in the assembly environment. Please, have us change the size in both environments. This is a hint for great success.)

So when I change the file name in windows file explorer, the drawing's file name is not changed, while I think this should be Inventor's job (this is also a hint for great success).

Thus I also manually change the drawing's file name to the likes of the part file name.

But when I reopen the part and open the drawing, the reference is still the old part. The old part that shouldn't exist because I renamed it. And boom there it is, the old part has reappeared in the project folder.

So I'm kind of baffled by this backwards behaviour. It seems the only good method to rename a part and keep it's references in a correct manner is to start over. New part, new drawing, new references, new part name, new everything.

While you were reading this, you were obviously thinking "dude use design assistant" the whole time. But the rename action in design assistant is greyed out. It also doesn't say WHY I can't use rename. What good is a software if half the functions aren't working? (Hint: ditch Design Assistant and integrate it's functions to the main program INVENTOR).

Yes we use Vault, but should this matter?

I'm wondering if there are any bright minds on these forums that are willing to share their splendid method of renaming files with little or preferably no frustrations.

Thank you for reading.

[CGBenner]

@MatthijsAstratec 

Hi, what kind of Content Center component is this, and how is it being added to your assembly?  As Standard, or As Custom?

[MatthijsAstratec]

Hi Chris, thank you for your reply.

I think Inventor is wrong in how it handles standard components. For renaming, it shouldn't matter if this is a standard or custom. A standard is a standard and can't be changed on the whim. In real life, you cannot use a standard as a custom. You cannot buy a bolt and a nut, and then say "look I made these, these are now custom parts". They are two different things and can't be both. Inventor should not have the option to import as a custom, because you're importing a standard part. This is a very very simple concept. If you want to make a standard part custom, you make a derive, because that is what it is. You start with a standard part and you edit to a custom part, just like in the shop. The result is a custom made part with a standard part as base/template (which I understand as a derived part).

And then the reverse: for example, if you import a content center file: hot rolled euronorm profile HEA200. That is not a standard part, only the profile geometry is standard. There is no standard length, a HEA beam is never a standard part, the length dimension is not defined. It has to be sawn, it needs a machining process, and when a standard part needs a machining process, the result is no longer a standard part. If you import a part that needs a parameter completed or edited, it should always be imported as a custom part, but in Inventor, where fantasy and magic are allowed, you're given the surreal choice.

But that is not the discussion, that's solely the background/context of my situation.

What I really want, is a method to RENAME files without losing references and functionality. That's what Autodesk should do.  I don't know why a renaming method for content center files should be different from renaming custom parts.

[CGBenner]

@MatthijsAstratec 

Thank you for elaborating.  Currently a CC Component placed "As Standard" is a library part and may not be edited, but it can either be placed "As Custom", or the part may be opened, and a copy saved and then renamed (you would have to replace the standard part with this one), so there are more stpes involved in what you want to do.

For the future, if you would like to request this functionality, feel free to post your suggestion in the Inventor Ideas Forum, and explain what problem this would solve so that the development team understands your need.  Good luck, sir!

[jtylerbc]

Could you just make a custom Content Center family that already has the naming format you want?  It seems like that would make the issue irrelevant, since there would be no need to rename it, and it would be less work in the long term.  It seems to me like even if you had the renaming functionality you want, it would be even more efficient to not need to rename the files at all because they are already correct on initial placement.

[MatthijsAstratec]

Hello jtylerbc and thank you for your suggestion.

Indeed, I wouldn't have a problem if I'd just set up all content center families to my liking. But then again, your suggestion is a valuable as switching to another CAD package which has the functionality I'm looking for, since it would make all my Inventor issues irrelevant, because I wouldn't use Inventor anymore.

So apparently there aren't enough people who have seen my post or people don't want to share their method. And since I've already received 3 noreply mails from Autodesk begging me to accept an answer as a solution, I'm just going to leave this message here and mark it as solved.

[dave.cutting · Accepted solution]

I think your frustration is coming from you renaming all of you files in explorer. If, as you say you use Vault, then you should be doing all of you renaming inside Vault. This will automatically update every assembly that the part occurs in.

If you had your own custom content centre as mentioned previously, you could set it up so that the dimensions that you require for production are concatenated into the filename. You could rename any old files that you have to your new naming convention (inside Vault), or leave them as is and replace them in any assemblies that you have with you new CC files.

With regard to the drawing, you need to replace the model that the drawing is referencing, Inventor will not do this automatically. If you have renamed both of your files, when you open the drawing you should get an error message (if you aren't seeing this, I'd check that your options) , and you can tell Inventor not to download the file from Vault. You can then browse and point it to the new file.

[jtylerbc]

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@MatthijsAstratec wrote:

Indeed, I wouldn't have a problem if I'd just set up all content center families to my liking. But then again, your suggestion is a valuable as switching to another CAD package which has the functionality I'm looking for, since it would make all my Inventor issues irrelevant, because I wouldn't use Inventor anymore.

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Using the software correctly and efficiently is equivalent to not using the software?  Even if the renaming functionality you want existed, using it instead of setting your CC files up properly to make the renaming unnecessary would be less efficient.  

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@MatthijsAstratec wrote:

So apparently there aren't enough people who have seen my post or people don't want to share their method. And since I've already received 3 noreply mails from Autodesk begging me to accept an answer as a solution, I'm just going to leave this message here and mark it as solved.

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I shared my method.  I set up my Content Center libraries such that I haven't needed to rename any CC hardware in years.  Eliminating the problem before it ever existed is my method.

[MatthijsAstratec]

I feel that I was not being clear enough in the original post, so try to reason with me please.

I'm asking for a method to rename. And your solution is: don't rename, just make sure everything you make already has the correct file name from the start.

That's not what the discussion is about. The discussion is about renaming, not about an alternative to get my file names correctly.

Another alternative to get my file names in a correct manner, is to switch CAD package that I know has the functionality I'm looking for. This is a hyperbole to trying to convey to you that I'm not looking for alternatives that don't touch existing files. Of course, it's really absurd to consider changing CAD software solely for this renaming purpose, I just expected it would be taken as a deadpan joke. (Just for a second I forgot that humour is culturally specific and can be interpreted in an unintended way.)

I try to be consistent in my libraries and nomenclature, but it's my predecessor who was playing games with it. I want to tackle and solve the results of the inefficiency of another person. Now I'm trying to get it right, and some individual components are not correct.

I cannot eliminate a problem that already exists. I'm not making new parts, it's about parts that are named incorrectly. If I set up CC parts to my liking, the incorrect parts will not have their file name changed by the finger snap.

Setting up my own content center libraries is otherwise an excellent suggestion.

I believe I can work something out with all the info you people provided. Thanks for your efforts.

[jtylerbc]

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@MatthijsAstratec wrote:

I cannot eliminate a problem that already exists. I'm not making new parts, it's about parts that are named incorrectly. If I set up CC parts to my liking, the incorrect parts will not have their file name changed by the finger snap.

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You are correct that my suggestion does not help with the existing issues.  However, it prevents new instances of it, thus containing the scope of the problem to the current instances, instead of it being an ongoing problem. 

Unless there is an immediate pressing reason to change the file names first, I would prioritize the CC library before the file name fixes.  Otherwise the number of instances you'll need to fix may continue to grow.  Stop the bleeding first, then treat the infection.

Additionally, it may help streamline the "renaming" process by changing it from a "rename" to a "replace" operation.  Once the custom CC family exists, you can relink the drawing to a part that already has the correct name.

From your original post, you questioned why the Rename function was grayed out in Design Assistant for CC parts.  Because those parts are placed as Standard, they are a library part, which is by definition not supposed to be changed in any way (geometry, iProperties, or even file name).  DA is just following those rules.  

One thing to consider is that the only thing that makes a Content Center part "read only" is the folder it is saved in.  There is nothing special about the files themselves.  If you move those files to a location that is not defined as your CC library by your Project File, they then act just like any other part file as far as Inventor and Design Assistant are concerned.  You can even keep the entire folder structure below that - just move it out of the Content Center folder, do your renaming, then move it back if necessary.  Alternatively, you could leave the files where they are, but make a Project File that doesn't use that location as the Content Center folder, and do all the renaming with this temporary Project File active.