File Corruption Prevention??

[jnewon]

Hey all.

I writing this as I sit and wait for my assembly to update and hopefully it will come back. 

I design factory conveyor systems. I use Factory Design Utilities. I put in hundreds of hours on layout design, presentation, and changes. I use Model States a lot. I add and delete to show different layouts to customers.

Inevitably this assembly file ends up corrupted. I have done enough layouts and this is how most end up. I don't know why.  Generally I will delete all Model states. This will help a little but the file is just muddy. It's slow, it hangs and no matter how clean I try and keep it, it just seems internally sick. 

I have learned (bitten) enough to use grounded origins with my sub assemblies so I can rebuild fairly easily but why should I need to rebuild. Time wasted but again here I am waiting for an assembly update/model state change. Have to weigh the pro's and con's of doing so.

Oh it's back. 18min to update assembly since I pressed the update button. 😞 Brand new BOXX apexx s3 6G machine. Clean install of Inventor 2023. I have to agree with many users that I fuss with Inventor more than I use it. It is sad but true much of the time.

My question is; How can I prevent file corruptions? Is there a utility to fix/clean said files? I'm I just destine to rebuild my assemblies?

Thanks

jnewon

[NigelHay]

I'm not aware of any utility to fix or prevent corruption, they just creep in every now & then. We don't suffer as much as you describe but perhaps our assemblies are less complicated.

For a critical assembly that gets referenced often such as your conveyor, I keep a 2nd back-up clean assembly saved on my C drive (parts & assemblies are stored on a server). That way, I know I have a fall back assembly that I can use to overwrite the 'working' one if it gets corrupted.

[Gabriel_Watson]

Invest in Autodesk Vault Pro, keep a separate layout for presentations from the one for manufacturing, and use Navisworks NWD format exports for visualization whenever possible.

[CCarreiras]

Hi!

All the files are locally in the machine, or stored outside on a server?

It's normal for big assemblies to take some time, it's not normal to corrupt.

[jnewon]

Thanks for reply
We do use Vault Pro. Maybe I should keep a second assembly. I don't see how this will help. I don't want to keep and maintain two separate files.

The main assembly will go thru many iterations of just factory asset adds and deletes, and propertied changes. Months of what if scenarios and planning before a final. Isn't this why Model states exist? But I feel model states is the main culprit for a lot of my slowness because if I delete all the model states the file get better. And using Factory assembly as a base doesn't help.

I don't have any trouble exporting for Autodesk Drive or pdf's. I have vault create those files.

It just ends up being a slow creep of slowdown. where it takes a very long time to change model states, add components, and update.

Thanks
jnewon

[jnewon]

Thanks for reply

We run a Vault Pro server but when the files are checked out the file work is local in the workspace.

Maybe corruption isn't the right word. It's just very slow. Constipated with internal remnants of old work??

It got to a point that I couldn't open the original assembly so I recreated a fresh FDU assembly with all the same sub assemblies as the original and it doesn't have any trouble. The only difference is that the new assembly didn't have to go thru all the design iterations. Maybe I will need to add this to my workflow, --> create clean final assembly.



jnewon

[LT.Rusty]

It sounds to me like there's probably something very specific at the root of your problem: one of the files or assemblies that you are reusing across projects- I had an assembly that kept getting corrupted and the root was one of the subassemblies. As soon as I replaced that, the problems vanished.

[Gabriel_Watson]

These are the key here: you mentioned how you leave remnants of old work, you didn't mention how many Model States (dozens??) are included, you did not mention the size of a pack and go for the whole assembly (how many GB when you perform a "Get" from Vault without any prior content already in your local workspace), and you now said there is no actual corruption, just slowness.
You can add more RAM if you have any less than 32 GB (I know that with models over 2 GB you could use it). But aside from that, I would say Model States is not like the old LOD suppression, as everything in MS gets loaded because Inventor became more efficient in rendering/loading geometry. Doesn't mean all users and their models will do better now without LODs.

EDIT: as rusty points out above, that is very very true... you must revise your libraries and perhaps migrate them or simplify sub-elements. I forgot to say above that the whole point of using Inventor Factory is to use generic and simplified blocks/assemblies for assets in your factory line, but if you are loading every nut and bolt used in production as a de-factor digital twin, you are not using this properly (in my opinion).

[jnewon]

Thanks for the reply.
I thought that as well. All sub assemblies have been gone thru, cleaned, no errors, and the model states work correctly. This did help but still the top assembly is slow.

[LT.Rusty]

---

@jnewon wrote:
Thanks for the reply.
I thought that as well. All sub assemblies have been gone thru, cleaned, no errors, and the model states work correctly. This did help but still the top assembly is slow.

---

How thoroughly were they gone through?

The thing that was causing my issues didn't show up as an error anywhere, and in the end I had to go through every sketch from 300+ parts to find that the issue was from some projected geometry in a frame generator skeleton that had originally been adaptive to a part that had been deleted several iterations ago. That was causing ridiculously slow performance in drawings and my top-level assembly was getting corrupted on every other save. 

[swalton]

I've noticed that Vault and Inventor can decide to spend 5-30 minutes doing something in large assemblies.   Some days it happens, others it does not.  It may be an issue with our setup.

Does your performance improve if you open the assembly when not logged into Vault?

[The_Angry_Elf · Accepted solution]

Ok, I know full well what you are going thru. I have spent the better part of the last 5 odd years dealing with files just like yours. 

We used factory design to build conveyors as well, it's a great setup as long as it's done correctly.

We're talking on avg about 5 miles worth of conveyors under roof, 10s of thousands of parts per assembly.

To give you an idea, when I started, it was taking 2-3 hours to activate a typical file (Assembly or drawing).

After doing a lot of digging, proper model building, and purchasing some much-needed hardware, I got the activation times down to under 1 minute for the very same file! Researching I found numerous issues with the processes used and very poor habits of the users.

1. check the errors, on activation, do you get a notification of blown constraints or is the Red Cross, Design Doctor icon lit up? If so, address those first. Upon activation/regeneration, Inventor is feverishly attempting to fix those errors in the background, slowing things way down. It goes thru each error until it has no more automatic fixes to apply then moves on to the next. Granted it all happens far faster, but consider you have 50 errors and it takes Inventor 1 minute to attempt to fix each, that 50 minutes you're waiting.

2. Double-Clicking to open files. That was a habit that was very hard to get users to break.

3. Close ALL open applications and then open a Windows File Explorer window and type in the address bar: %temp% and hit a return. Select all the files, right click and select "Delete". For any pop-ups, select the "do this for all future..." and select "Skip" (you may need to do this 2 or 3 pop-ups).

4. On the Programs listing, navigate to Autodesk Inventor 202x and expand the listing, at the end you'll see "Task Scheduler". Open that. The Link below will walk you thru the steps, this, THIS is the application I trust most to fix issues like this. It typically works wonders.

Inventor 101 – Knock Knock Knock, “Housekeeping!” — Celtic Design Services (cdscad.com)

If you have access to the old Autodesk University classes, search for my CADZilla series. They specifically focus on working in very large assemblies and tips & tricks you can use in such. If you don't have such access, PM me, I can offer up some help.

[jnewon]

I just wanted to say thanks for your post. I'm out of the office but I want to take a couple of days to digest your post. I have been doing large assemblies for the last 12 yrs and have learned a lot over that time but still feel I'm missing something. Generally have resolved to the fact that inventor is just not good at it.

Thanks again for you post and support.
jnewon

[Frederick_Law]

ModelState remember every changes.

Dimension, properties, constrain, suppress, everything.

Open the table and take a look.

Probably got a few you didn't want to change.

Use Factory Scope to reduce the table size.

I had a few corrupted ModelState.  Need to delete it and rebuild.

Support is looking at one of the assembly now.  Hope they find something to prevent it.

[The_Angry_Elf]

I understand your frustration, but considering your comment of "Generally have resolved to the fact that inventor is just not good at it." is a bit off.

In fact, Inventor is very good at dealing with large assemblies. But, one needs to build solid datasets as well.

doo doo in, doo doo out, right?

There are no doubt some steps/processes one must take into account and perform with files of this size and get them to work as they should.

Things to also consider when using Factory Design assets, keep them as simple as possible, keep in mind the Connection Dots, these retain a lot of intelligence and can use a lot of memory/CPU usage on regeneration as it validates those settings.

But honestly, Inventor is pretty darn good dealing with large assemblies.

[jnewon]

Thanks Again
I agree with the doo doo in = doo doo out. We work hard to keep our files very clean and error free.
The factory assets are very simple with a couple of connectors for chains.

I did read thru your knock knock article and I think this is my missing link to clean the files. Going thru the steps now and I hope to have my mind changed on the inventor large assemblies.

jnewon

[jnewon]

@The_Angry_Elf 

The migration routine from your article is a game changer. It has greatly improved the responsiveness of my large layout assembly. Not just loading but everything to adding components, model state changes, to saving, and updating.

I hope this post helps many.

Many many thanks

jnewon

[Frederick_Law]

I used to migrate all CC, library and template before moving to new version.

No Vault.

Of course keeping backup of old.

Projects are migrate when needed.

3 steps migration.

ipt, iam and ipn then idw