Update physical properties on save (Parts and Assemblies) setting does not work properly

[ReneRepina]

Hello everyone!

It seems update on physical properties on save (Parts and Assemblies) setting does not work properly. It does not update the mass of the top assembly in case there is a save dialog for multiple documents. It updates the mass of every sub-component (part or assembly), but not the top assembly, unless there is no save dialog for multiple files.

I am using Inventor 2020.4.1.

How to simulate:

1. Check you have setting properly set "Update physical properties on save (Parts and Assemblies)"
2. Create the new empty assembly and save it.
3. Create the new part (use random shape) and save it.
4. Place multiple parts into assembly.
5. Change the part a bit so it gets dirtied (also assembly will get dirtied).
6. Go to the assembly and save it.
7. Because both of the files are dirtied, save dialog will pop up, save them both.
8. Part now has mass updated, but assembly does not.
9. If you save the assembly again (without save dialog for multiple files), it will update the mass with no problem.

Can anybody explain why this happens or it is a bug?

I managed to solve this problem with iLogic:

1. Disable "Update physical properties on save".
2. Use event trigger on before save.
3. Use update2 document iLogic command. Works also with just update() command.
   

   ThisDoc.Document.Update2(True)

4. Use command manager iLogic command to update mass (synchronous - important, otherwise it does not work!)

   ThisApplication.CommandManager.ControlDefinitions.Item("AppUpdateMassPropertiesCmd").Execute2(True)

Taking iLogic solution into the account, I came to few reasons why this happens:

1. Somehow update mass does not run properly on top assembly (it is still enabled after saving, while on other documents is not).
2. It updates the mass before update is executed (asynchronous?).

I hope I explained it understandable. If you have any questions do not hesitate to ask.

Thanks for all incoming help!

[bradeneuropeArthur]

This is a known issue for a long time already in Inventor (at least since 2012 of Inventor).

I have addressed this more than once but still this is not solved.

For a Vault environment this is called a Dirty Maker and is frustrating enough to update everytime.

More is the case that also if the file is not updated and already released, it will write the mass to calculate.

This means a Dirty File in Vault. So solution is to not use the Application Options for this but write an add-in that does the calculation only if the file is checked out and not Read-only.

What I can remember is that the Mass property shown is stored on two different places internally and there sometimes it goes wrong. I need to dig deep again to find the reason again since it was already addressed in 2011 with the release of Inventor 2012.

@johnsonshiue Can you please again take a look at the behavior.

I hope that the development team is aware!

[johnsonshiue]

Hi Arthur,

I could be wrong but I don't think this is a bug. Let me walk through the process of updating mass prop. As we all know, geometry is all stored in individual ipt files and it is where the mass is computed based on the geometry.

At assembly level, the mass is aggregated from the parts (per quantity per Reference). Whenever a part geometry is changed, the mass will need to be recomputed. If the App options is not turned on, the mass of such part will show N/A. Also, any assembly consuming the part will have N/A.

The trouble I can see is that an assembly is released, while some of the parts (shared by multiple assemblies) are still being worked on. Later the parts are updated. The mass need to be recomputed. And, the assemblies will need to be recomputed.

This sounds like a data management issue. When an assembly is released, it means that all components need to be released (not subject to further change).

Many thanks!

[ReneRepina]

@bradeneuropeArthur 

Thanks for pointing out new information, but I think this is a different issue.

@johnsonshiue 

I think you are correct on that one. If we have update everything, all files will have mass, but if we change some low level part, all structure above will have to be computed to get the new mass. I guess this is logical, in this situation we have 2 ways to go, first one is do not change anything, second one is, if we have to change, we would have to change the part and all files which this part is referenced to, which can be a lot of work and inefficient.

But in my problem above, I am stating another problem. I have all files unlocked (ready to be worked on), I shape them as I please, which is OK, then I want to save on TOP assembly, but it does not update the mass of it, eventhough all below assemblies get the mass and also the part. If you save twice, it works.

This problem has nothing do to with above discussion.

[bradeneuropeArthur]

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@johnsonshiue wrote:

Hi Arthur,

I could be wrong but I don't think this is a bug. Let me walk through the process of updating mass prop. As we all know, geometry is all stored in individual ipt files and it is where the mass is computed based on the geometry.

At assembly level, the mass is aggregated from the parts (per quantity per Reference). Whenever a part geometry is changed, the mass will need to be recomputed. If the App options is not turned on, the mass of such part will show N/A. Also, any assembly consuming the part will have N/A.

The trouble I can see is that an assembly is released, while some of the parts (shared by multiple assemblies) are still being worked on. Later the parts are updated. The mass need to be recomputed. And, the assemblies will need to be recomputed.

This sounds like a data management issue. When an assembly is released, it means that all components need to be released (not subject to further change).

Many thanks!

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The only thing I expect is that if files are saved and checked into Vault, with the application options on:

That the mass is calculated and filled in correctly.

Also and more critical that if the file is to be released in Vault that the mass is filled in correctly, this is often not the case.

One more thing is that the mass is also written even if the file is read-only, and that is not correct if you use a release process.

Hope you understand the issue here and maybe it is more or less only needed when using Vault and released files.

All other situations are more or less not that critical.

Regards,

[johnsonshiue]

Hi Arthur and Rene,

It seems that we have two different issues here. If possible, I would like to see examples. If the Update Physical Properties on Save options is turned on, the affected files should be prompted to save. However, there is another option which may obscure the request. Go to Tools -> App Options -> Save -> "Mass Prop Update", "Implicit Update", or "Recomputable Update" -> set it to Yes.

If the option is set to No, the files will not be prompted to saved. It is because the feature recipes and the parameters are already captured (saved), the mass prop can be evaluated when the geometry becomes up-to-date. There isn't anything lost. For PDM workflow purpose, I suggest the files to be prompted to save, so that the Vault always has the latest and greatest version of the files.

However, this behavior may not be desirable for some users, who complain excessive prompting to save. Unfortunately, we cannot have both. Either you save or you don't.

Many thanks!

[bradeneuropeArthur]

Hi @johnsonshiue 

I see a real big progress in the newest version of Inventor of course, regarding the application options.

I also like the replies you give "In General" and try to understand what is different sometimes between the theory and the practice.

I think you are one of the persons that are familiar with the world of Autodesk users outside Autodesk, isn't it, or am I wrong!?

Furthermore since you have highlighted it:

For (at least a Vault Environment) some application options should have been fixed and only to be changeable by an administrator. 

In Vault we have that possibility.

For here internal we have written an add in that will the normal user not allow to change some application options and we have given only the Admin the rights for this.

By doing this we have reduced a lot of our Vault/Inventor related issues. This is one of the thing between the theory and the practice.

I know that we as person/generation are asking every time more, but on the other hand the software resellers promise us also more every time!

Regards,

[ReneRepina]

@bradeneuropeArthur 

This option works, but only if you save it few times (at least 2), BUT if any sub-model is changed after top assembly is released, it will always need to update for the new mass, except if you "quick change" whole structure from changed part and above, which can be really tiem consuming and not effective.

This options should at least save proper mass, if you save it once and release it, but it does not, if it is not saved correctly as you described and as in above pictures.

If some settings could be changed only by admin, that would be great in Inventor!

@johnsonshiue 

We have "Recomputable update" set to yes. It was also set the same in example above. They are prompted to save, you can even see in above pictures, but TOP assembly does not compute the mass first time, it does on second save (when save dialog is not shown).

No problem about prompting to save, it is OK with us. The mass issue occurs if we changed some sub-part in assembly (assembly being released), then it always wants to compute, which is logical since we would need to save (quick change) whole structure from that part above.

[bradeneuropeArthur]

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@ReneRepina wrote:

@bradeneuropeArthur 

This option works, but only if you save it few times (at least 2), BUT if any sub-model is changed after top assembly is released, it will always need to update for the new mass, except if you "quick change" whole structure from changed part and above, which can be really time consuming and not effective.

This options should at least save proper mass, if you save it once and release it, but it does not, if it is not saved correctly as you described and as in above pictures.

Because this mechanism is written in more than only one "Object" before it is displayed as "Mass" this is not always saved correctly within the assembly. I need to search again for it but I am sure the mass is first written internally to the assembly and the part before it is written to the Physical Property, and there it goes wrong.

I fully agree that this is one of the bigger problems regarding"Dirty files" files that need a save. Also if the file is already released this mass is alwasys written tot the part or assembly without checking if the file is editable in Vault terms. 

There are many other application options that have similar consequences!

See one of my ideas in the Idea station:

https://forums.autodesk.com/inventor-ideas/application-options-changeability-blocking 

If some settings could be changed only by admin, that would be great in Inventor!

@johnsonshiue 

We have "Recomputable update" set to yes. It was also set the same in example above. They are prompted to save, you can even see in above pictures, but TOP assembly does not compute the mass first time, it does on second save (when save dialog is not shown).

No problem about prompting to save, it is OK with us. The mass issue occurs if we changed some sub-part in assembly (assembly being released), then it always wants to compute, which is logical since we would need to save (quick change) whole structure from that part above.

To my opinion it should either work in Inventor and In an environment with Vault to.

In principle every feature; Option and tool that is available in Inventor should work with no problem in a Vault Environment too.

See one of my ideas in the Idea station:

https://forums.autodesk.com/inventor-ideas/application-options-changeability-blocking 

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