Revert part to last saved / Close and discard changes

[s_benjamin]

Is there a way to revert an open, edited part back to its most current save? Or to close an edited part without its changes persisting in assemblies that reference it?

I often work on parts with their associated assemblies open; Inventor won't let me discard changes until all related assemblies are closed. Searching brought me to a thread describing the same issue from 2006. I'm using Inventor 2010.

Help?

[cbenner]

Look in your file folder, there should be a folder called Old Versions.  You may be able to go back that way.  Also, if you have a part open and are editing it, but HAVE NOT saved, you can simply close without saving your changes... this is pretty dangerous though and not really a best practice, more of an emergency "oops!" thing.

If you use Vault you can open old versions of Vaulted parts or assemblies and save them over the current version, effectively backing your part up in time.

[s_benjamin]

I may not have explained myself clearly. I desprately want to "close without saving changes," but as long as the part exists in an open assembly somewhere it never really gets closed. The part, and the changes I'm trying to forget, stay in memory until everything that contains the part gets closed, too.

I'm not trying to get back to an earlier save, I'm trying to get back to when I opened the part in the first place. Ideally without having to close everything down to get there.

[mcgyvr]

I'm not aware of a way to do what you want.. Would be a good feature to have though.. Just a "revert changes" button in the file menu.

Actually now that I'm thinking about it I'm really surprised thats not how it works when you close a file and don't save the changes.. I'd expect Inventor to sync up the parts right after you close the file.. Guess not.. 

[cwhetten]

There is a Refresh command that seems like it should do exactly this, but it doesn't work.

So, I guess the only way to deal with this scenario is to close all files referencing the file in question.

Cameron Whetten
Inventor 2014

[cbenner]

What does UNDO do in that case... can you get back far enough?

[mcgyvr]

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@cbenner wrote:

What does UNDO do in that case... can you get back far enough?

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Undo showed a repeatable bug.. At least for me anyways..

I opened a subassembly..added another part to it.. then closed the file without saving it.

I kept hitting undo (in the top level assembly) till the step exactly before when I added another part.. Then I opened the sub I made a change to and there was NOTHING in the graphics window at all for that sub.. Everything graphically was gone.. 

[s_benjamin]

I tried forcing the issue by using Replace All to replace the part with itself in the affected assemblies. Without luck.

If I point Replace All to a renamed copy of the offending part ( copyOfA.ipt instead of A.ipt, for example ), the assemblies will successfully update to it and no references to the original part should remain. But if I then Replace All back to the original part file, it loads all the phantom changes again. It doesn't seem to matter if I save the assemblies or refresh them, the edits always come back unless the assemblies are explicitly closed.

I'm out of ideas.

Edit:

I had an idea.

Suppressing the part ( and any sub-assembly that contains the part ) will purge the part from memory. When they are then unsuppressed, they revert to their proper, last saved state. Still a hastle, but a hastle that can likely be scripted away...if wonton suppression doesn't cause too many problems.

[cwhetten]

Ah, brilliant!  I should have thought of suppression.  Kudos to you, sir.

Suppressing a part will create a custom LOD (if your assembly isn't already set to one), so you will have to set it back to master and delete the custom LOD if you don't want to deal with LOD messages popping up everywhere.

But aside from this, it's a good solution.

Cameron Whetten
Inventor 2014

[stephengibson76]

i like this... as hardware improves I tend to have more assembly tabs open and it is a pita to close them all an reopen them just to try something out on a part

[mcgyvr]

I've never had this problem though..

Because I always just undo the temporary changes by just deleting the added features or changing them back to what there were and then save the part..not close it without saving..

Just a difference in modeling techniques.. 

[Teunsegers]

So it's 2021 now and I don't think this is possible yet? The only solution seems to be is to turn of autosave (which I don't want to do for obvious reasons). I'd love to see a "Discard changes" option is the file menu to revert to the last save state.

Often I will open a sketch just to look at the design and when I finish the sketch (without even touching it) it will cause random errors downstream. This mostly happens in very models, but I've seen it occur in smaller ones too. Point is, there is nothing to undo but now I have a corrupt version and all I can do is take a previous version and promote it to the latest version. That can lead to a lot of useless versions. I also cannot delete versions.

[johnsonshiue]

Hi! The last saved Inventor file copies are stored in \OldVersions\ folder at the same folder path. You can find them there and rename the file extension to restore the files.

Many thanks!

[alain.miltenburgU6LCJ]

(Wrong account.)

[alain_miltenburg]

Hi Johnson,

That is an answer to different question. ‌🤓

I too was looking for a way to revert in memory edits of sub components in an assembly back to the state saved on disk (and/or Vault). In my search for a solution I stumbled upon this forum post, which confirmed my fears; there is currently simply no command for that! I always close the assembly in question, not saving the subcomponents and reopening the assembly again. Which is of course crazy if you think about it! Especially for large factory layouts. The workaround suggested by s_benjamin relieves the pain a bit, but in my humble opinion there should be a command implemented for this. Don't you think?
Could you consider to report this in the Autodesk issue tracking system?

Kind regards,

Alain

[johnsonshiue]

Hi Alain,

I believe you are asking an Auto-Save option. It has been discussed for many years. Unfortunately, we don't have a good solution. There is an app on Inventor App store doing Auto-Save. You may want to take a look. However, I have been told there were corrupted files related to the app.

You may want to look into Fusion 360, which has an Auto-Save option.

Many thanks!

[swalton]

@johnsonshiue, no not autosave.

What is needed is a way to reload a file from disk or Vault in order to discard any changes that the user has made to the copy in RAM.  This function has existed in Creo/Wildfire/ProE for decades.

The workflow is this: 

1. Open a 10k instance assembly with 6 levels of subassemblies.
2. Drill down to a file at the bottom of the assembly tree by opening each successive subassembly.
   1. This give the user 5-20 tabs open, each showing a different part of the top-level assembly.
3. Modify the file.
4. Make several changes to other files.
5. Switch to the top-level assembly and regen to see the changes propagate through the structure.
6. Realise that the change in Step 3 does not work, but the ones from Step 4 are worth keeping.

How does a user discard the changes in Step 3 but keep the others?

Closing and reopening all the open tabs that reference the file in Step 3 is a significant time sink. 

Undo is not helpful because there is not a different buffer for each open tab.

[Teunsegers]

In the latest versions of Fusion360 this has now been solved. You can close
an open model with changes and it will no longer auto-save those changes,
you will instead get a prompt. This prompt now allows you to discard the
changes and just close the model. You can then open the model again in the
last saved state. For me, this works well enough.