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Inventor not Responding on Assembly Load - Huge memory consume

Anonymous

Inventor not Responding on Assembly Load - Huge memory consume

Anonymous
Not applicable

Before came here, I have to let know, I spent hours looking for a solution. But all I found was what can be, and not how to find.
I have an assembly with about 15000 parts, usually it consumes something like 7~8Gb when loaded, but in a time window of 2 hours working, Inventor started to show "Not Responding" (Yes I know this is a windows message when something take more time than expected). Then after about no more than 5 minutes Inventor simply close with no apparently reason.
Looking on Event Viewer I found "Resource Exhausted", so to be short, Windows 10 decided to kill Inventor due to Virtual Memory Available (by the way VM was managed by OS).
OK, lets try to set VM and see what happens, then I switched VM from Manages by OS to 50Gb, by the way physical Memory is 16Gb, so I can have about 66Gb, considering OS will take 3Gb, I can have up to 63Gb available for Inventor load my assembly.

Letยดs try again, open assembly, open Task Manger>Memory, wait, wait, then Memory beats about 49Gb, and Not Responding still there, but this time OS does not kill Inventor due to Exhausted Resources. So I can stay for hours and can just see an picture of my assembly on screen.


Good, but just to proof a concept for my user (Engineering Designer), and since I have memory available, lets try to load another Inventor, and surprise, it loads, OK good, now load any other assembly, say one with 500 parts and see.

For user surprise, it load  and works faster as any other assembly or part.

Then I back to my research, that concludes, it can be a bad STEP file, it can be a corrupted IPT, and it can be something related to a Constrain.
My research also points, to some people telling they found culprit file, but they dont say how they find "culprit file".

So, after all history above, my question is, since you have no tools to tell you who is the bad guy, and since there is no way to know who was inserted at certain time window (because assembly does not load), and considering you have 1500 files referenced in assembly.

What can be done to at least get closer to bad file that is wasting my resources and still not loading. I mean, instead of trying move files & directories to a another place to generate a "reference not found", or just remove files created/modified at time window or date.

Am I missing some tool or command?

 

Before someone ask, Inventor 2018, Ram 16Gb, SSD 1Tb

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Xun.Zhang
Alumni
Alumni

Hello,

 

Welcome to Inventor forum!!

 

Thank you for those valuable comments and the investigation and proud of you to come out some solution to solve the problem. In fact, 15000 components is not that many, we are testing more huge number data in door. Regard to your question - 


@Anonymous wrote:


What can be done to at least get closer to bad file that is wasting my resources and still not loading. I mean, instead of trying move files & directories to a another place to generate a "reference not found", or just remove files created/modified at time window or date.

Am I missing some tool or command?


Have you tried the option when open a file in the open dialog?

11.png

 

Hope it helps a little bit.

 


Xun
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Anonymous
Not applicable

Xun.Zhang

Thanks

 

But, we are using this option. Using such option, it load file, switch to Not Responding, show image of assembly, clear Not Responding for a second then back to Not Responding, memory use stabilizes in 49Gb. I can only close windows (but here is OS)

Today we made a try using Nothing Visible & All Parts Suppressed, it loads, I can see parts in browser list click around, no issues. But seems this can not give me a direction of whatยดs going on or who causing the issue.

 

There is no Vault involved, project is on local on SSD

 

 

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johnsonshiue
Community Manager
Community Manager

Hi! You mentioned that if all components were invisible, the performance was fine, right? This leads me to believe the issue is graphics related. Is your graphics driver up-to-date? Do you have an integrated graphics card? Please share your hardware profile (open a simple part and go to Tools -> Application Options -> Hardware -> Diagnosis -> paste it to a text file and send it to me directly johnson.shiue@autodesk.com).

Many thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
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Anonymous
Not applicable

 

 

 

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johnsonshiue
Community Manager
Community Manager

Hi! Many thanks for sharing the hardware profile! I still believe this is graphics card and system memory related. The graphics card on your machine is considered low-end. It only has 2GB RAM. Your system RAM is not much more either. You only have 16GB. If I were you, I would upgrade system RAM to 20GB or 32GB. This will help eliminate the need to use swap space (disk memory). It will help boost performance.

Thanks again!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
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Anonymous
Not applicable

Understand your point but Virtual Memory is set to 50Gb, and I have 63Gb available.
About Graphics Card, until I get a new one, is what I have, anyway Assembly was loading fine even with 2Gb Video card.

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JDMather
Consultant
Consultant

@Anonymous wrote:

...What can be done to at least get closer to bad file.... 


Are you using sub-assemblies in your main assembly?


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Anonymous
Not applicable

Xun.Zhang, johnsonshiue

 

So, considering your comments, and since I was loading assembly in Express Mode.
What comes next is very interesting (at least to me), and now question change.
OK, lets try each of Suppress "options" available in File Options available, but remember, Suppress options are available only if FULL mode is selected.
First try:

"All Content Center Supressed", Skip all unresolved files checked, COOL it loads, some "Relationship inconsistent" fixed, memory use in 6.7Gb

OK looks promising

 

Second Try:

"All Components Supressed", , Skip all unresolved files checked, COOL it loads, some "Relationship inconsistent" fixed, memory use in 4.0Gb

Fine, sounds right direction, lets see if music plays

 

Thrid Try:

Just FULL, no Suppress (Master), do not Skip anything, FANTASTIC it loads, same "Relatinship inconsistent" fixed, memory use 8Gb
5x less that load in Express Mode. Now it is time to rockยดn roll, save (took a long time to be here, canยดt lose)

Now the proof:

Load saved in Express Mode, and donยดt know why or how, but it loads no more not a single Not Responding, memory use about 6.8Gb.
Of course I have to wait until Monday to ask for end user if all is OK.

But a question remains, how this can be explained?
By the way all tests where done in a copy of assembly, so now I have 2 assemblies 1 OK and 1 BAD

 

Appreciate your comments

 

 

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johnsonshiue
Community Manager
Community Manager

Hi! The behavior does sound confusing. Without seeing the actual dataset, I can only guess. I think the particular assembly has high number of repeated occurrences and relatively low number of unique documents. In Express mode, all the component graphics is cached in the top level assembly but only the top level assembly document is loaded. This concentrated graphics segment of many repeated occurrences may not be as efficient as the distributed graphics in Full mode.

In Express mode, only the top-level assembly document is loaded on open. But, you do see how the assembly look like on open. When you start editing parts or adding constraints, the documents will be loaded on demand. The Suppress (LOD) workflows you are talking about are only available in Full mode, not in Express mode. LOD is like loading/unloading documents manually.

To say it for sure, we will need to take a look at the files and see if there is anything wrong.

Many thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
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Anonymous
Not applicable

JDMather,

Yes, main assembly has about 30 sub-assemblies, and each have some more sub-assemblies.

 

johnsonshiue,

Yes, sound confusing, but with your guess, at least to me start to make sense. Considering some data is stored in cached area in file, I think it can be scrambled for some reason, or even because user thinks have a bad computer try to shutdown and donยดt wait all be closed then pull the cable.

You also correct when suggest "high number of repeated occurrences and relatively low number of unique documents", thatยดs my case.
Here some info about Project & Assembly
Project: Process Plant with lots of beams, welded parts, special parts, valves, pipes, bolts, nuts, ball bearings, etc.

Assembly: Total Ocurrences: 15055 | Open Docs in session: 986

Checking BOM Parts List there is about 705 parts and Quantity count total about 13000, a single bolt counts 1200

 

My research about endless "Not Responding", resulted in a list,

a) A corrupted STEP file, or non Inventor file;
b) A corrupted IPT file;
c) A bad Constrain

If you agree,
d) A corrupted Cached Area, try to load in FULL mode.

 

Please your comments

 

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johnsonshiue
Community Manager
Community Manager

Hi! I think my assessment was not too far off. You have an occurrence/unique ratio of 15. I personally do not think Express mode will help you in this case. It is because Express mode concentrates all graphics in the top-level assembly, which makes the top-level assembly quite large. Your hardware is not particular performant to begin with. Based on my experience, I would say Express mode works better when occurrence/unique ration is less than 10 (very rough number). 15 is indeed very high.

I think you will benefit from using Full mode in your case. Start Inventor and go to Tools -> Application Options -> Assembly -> uncheck "Enable Express mode." Then open the assembly. I think you should notice better performance than in Express. But, loading the entire assembly in Full mode may take slightly longer than loading it in Express mode. In Full mode, particularly with high occurrence/unique ratio, the component graphics is managed quite efficiently. It is distributed and it is not concentrated in the top assembly.

Imagine, if you have 15000 components and each one is unique. Essentially, you have occurrence/unique ratio of 1. You will see the assembly works better in Express mode than in Full mode. It is because you will have to load 15000 documents in Full as opposed to 1 in Express. And, due to the extreme low ratio, there is no way to reuse or distribute the graphics, you pretty much have the same size of graphics segment in Full as in Express.

In another extreme case, you have 15000 components and it is the same part patterned 15000 times. You will find Express mode would be much slower than in Full. It is because of the concentrated graphics of 15000 components in the top-level assembly in Express mode. Although you only need to open one document, the file size is probably a few hundred MBs. In Full mode, you will see you only need to open two documents and the two files are quite small.

I hope my explanation makes sense. I am not seeing a corruption yet.

Many thanks!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
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