Missing files in assembly should inventor show not responding?

[A.Acheson]

I often end up with missing files in assemblies and inventor looks like it freezes and shows not responding. It could churn away like that for a minute or two then show up missing one part or indeed just freeze like that and maybe an esc keep will jog the reference window into view or ctrl alt delete and kill inventor along with any unsaved work I was working on.

Is this the correct response that everyone else sees? I am using a network and single user project with libraries and content center outside the workspace. The assemblies are small I would think 🤔.  The workspace includes rather a lot of AutoCAD projects spread across 10 something years. Could this be causing it to be super slow in recognizing the component link that is missing? 

[SharkDesign]

As long as your CCentre and libraries are listed in the project file it should be fine. 

If your files are outside the search paths listed in the project it won't be able to find them. 

AutoCAD files should have no bearing on any of this. 

The only time my inventor hangs like that is when my vpn goes down which is my only link to the vault. 

[A.Acheson]

Interesting, yes all paths are defined. It sounds like there is a definite room for improvement here. Is there any testing method to check the file network efficiency when files are crossing a network and or during checking for missing files?

[Curtis_Waguespack · Accepted solution]

Hi @A.Acheson 

I suspect this might be due to the "using unique file names" setting in the project file (*.ipj)

See this link, for more thoughts on this setting:

https://forums.autodesk.com/t5/inventor-forum/using-unique-file-names-option/m-p/6008909#M590217

 I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[A.Acheson]

Thanks  Curtis. This sounds like the symptoms that could cause the delays. I believe this setting is set to yes. I would say I use 80% unique file names and maybe not when it comes to frame generator assemblies, random test assemblies copies etc. 

If I set to no and there was more than one file what would I see?

1. Does it automatically solve it the file near the workspace or from another loacation?
2. Does the file in multiple location dialogue pop up?

3. Or does it say this is not the same file do you want to use.

4.Does it select a file and give no messages?

[Curtis_Waguespack]

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@A.Acheson wrote:

Thanks  Curtis. This sounds like the symptoms that could cause the delays. I believe this setting is set to yes. I would say I use 80% unique file names and maybe not when it comes to frame generator assemblies, random test assemblies copies etc. 

If I set to no and there was more than one file what would I see?

1. Does it automatically solve it the file near the workspace or from another loacation?
2. Does the file in multiple location dialogue pop up?

3. Or does it say this is not the same file do you want to use.

4.Does it select a file and give no messages?

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Hi @A.Acheson 

Going from memory, I think it just tells you that there are multiple files of the same name... unless you've moved or renamed something so that it can't resolve the link, then I think it tells you there are multiple files of the same name, and asks you to choose the correct one.

I might be remembering that incorrectly though... I'd suggest you set it to No as a test and set  some "dummy" files with the same name... to see for sure.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[johnsonshiue]

Hi! I recall if you have "Use Unique File Name" set to false, meaning duplicate file names allowed, Inventor will not automatically resolve files. You will need to manually resolve.

I don't believe it is a good practice to keep duplicate file names. You will run into issues when exporting the model, since STEP can get confused with such duplicated files.

Another thing to look into is the folder path. You may want to remove some unused or less frequently used paths. When excessive number of folder paths is defined in the project, Inventor could try to exhaust all paths on resolve. Also, limit the path depth. You don't want to have very deep path, which can run into 256 characters limit quickly.

Many thanks!

[A.Acheson]

Setting Unique File Names to “no”solved the hanging issue, no longer need to ctrl +alt+ delete and shut down Inventor Application. I can resolve the links manually which I believe you had to do regardless. Thanks @Curtis_Waguespack  

[BDCollett]

Hi @johnsonshiue, I think it's the opposite to what you said.

With it set to "no" it doesn't ask, it just resolves to the first one it finds. Fast.

With it set to "yes" it will stop, find all the duplicates and then give you an option. Hence.. very slow.

@A.Acheson I have been working with data that sounds similar to yours (10 years worth, lots of Autocad DWGs and getting it into Vault. It seems people using Network drives to manage their data end up with some horrible messes. 

[A.Acheson]

In our case the folder for the workspace has sub folders denoted by year so we had to place at the root folder. However we really only have Inventor  files in two sub folder and not 10. So obviously a lot of unnecessary files to churn through. I wonder if there is another way to set up the project workspace to have more than one folder, all without moving files?

[BDCollett]

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@A.Acheson wrote:

In our case the folder for the workspace has sub folders denoted by year so we had to place at the root folder. However we really only have Inventor  files in two sub folder and not 10. So obviously a lot of unnecessary files to churn through. I wonder if there is another way to set up the project workspace to have more than one folder, all without moving files?

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I am not sure exactly what you mean, more than one folder and moving files? It sounds like something that would be easily fixed with Vault. If you are moving or renaming things in windows file explorer you are in for a world of pain.