HELP!? - Inventor vault forcing file updates?

[AlexZW28B]

This forum needs a draft option - page just refreshed on me and lost my mostly completed post... that aside.

I am using Autodesk Vault/Inventor combo - Inventor 2020.3.2(373), and Vault 2020.2(25.2.83.0).

I am having issues with an Inventor assembly which is telling me to update a bunch of parts in the vault - which were previously saved, checked in, and some parts were already existing in the vault as Locked geometry. It is a number of the locked models, bolt/screw/washer components, in our standard components folder in our Vault. I had spent a copious amount of time(more like wasted my time due to Inventor incompetency's) going through the model to make sure all assembly/parts were updated prior to checking in - cause the rebuild doesn't always update fully through the model and save properly - especially the IPNs. After checking in the whole assembly, I deleted all local files related to the assembly I was working on, and then did a "get" on the whole standard parts folder where the Hardware is referenced from. After opening the assembly, I am now getting all kinds of errors saying that I need to rebuild my model...WHAA>>!!?? And most of the components are the bolt components in the locked/standard components folder - which I did a get on...

What in the process of inserting a part into an assembly would conceivably force a model - a locked component file - to require an update? Best part is, that sometimes it will only show a few models that need it to start, and then you rebuild, and then more need it all of the sudden. 

Any help? Inventor is becoming such a colossal waste of my time at work... I should be Inventing models, not ways of work-arounds for the program I am working with!

[johnsonshiue]

Hi Alex,

The behavior does not sound right. To help me understand the issue better, please try the following and let me know what you find.

1) Start Inventor and go to Tools -> Add-Ins -> unload Vault Add-In.

2) Perform the same workflow.

Are the files prompted to be updated and saved? If yes, I need to see the files to understand the behavior better. It is possible the update is indeed required due to change in one of the Inventor files. It is also possible there is a bug. Without seeing the files, it is hard to tell. Please share the files with me directly [email protected].

Many thanks!

[sundars]

Hi @AlexZW28B 

We have some application options to turn off prompting for indirect updates. Sometimes, during the modeling process, some components may get dirty indirectly. Theoretically speaking in your case, the incoming component should not be touched and should not be dirtied but in some cases, some operation may have triggered a smudge. As a result, you might get prompted to save those parts.

Try the following and see if it fixes your issue:

Startup Inventor 2020

Application Options + Save Tab + Prompt to save for re-computable updates 

Uncheck the prompt to save

Unchecking it will no longer prompt you to save those parts which got indirectly dirty.

Try your place operation and see if it fixes your issue. 

Thanks

-shiva

[AlexZW28B]

@sundars , I have already unchecked those - I had done that a while ago after first starting at my current place of employment about 5-6 months ago... the incessant notifications were driving me nuts. So, to clarify, they are already, and still unchecked - I only have the Save Reminder Timer on for notification.

[sundars]

Hi @AlexZW28B 

Thanks for the info. Sorry to hear that didnt quite help. Let's see if we can isolate this issue.

1. Does it happen for ANY vaulted part?

2. Does it happen ONLY for content parts

3. Does it happen ONLY for bolted connection parts.

Can you share a simple dataset which describes and demonstrates the issue. Just a simple assembly + one of these components which show the problem. We can try to isolate and see who is dirtying the part.

You can email the datasets to me or post it here - sundarsATautodeskDOTcom. We will investigate it and create an issue for you once we understand what the dirty problem is.

Thanks

-shiva

[AlexZW28B]

@sundars 

Thanks for the prompt reply, it seems to be only happening with vault/auto generated hardware. Any of the designed components to not seem to exhibit this issue. I have included the images below outlining what the tree looks like, and the message that shows once I open the vault hardware component. I do not usually use "Bolted Connections" - if that is an Inventor feature you are referring to. I mate all the H/W individually using the laborious processes that exist... It does seem to occur on bolts, and some washer/nuts.

I am unsure why it is needed to be updated, as it was originally just pulled from the vault and inserted into assembly. And, if it was auto-generated for my design, it was inserted into vault as an automated new filename, and then I check it in and lock it once it is confirmed for use.

[sundars]

Hi @AlexZW28B 

Thanks for the info. When you said bolts I assumed that you were working with bolted connections - ignore that. no worries.

Couple of more questions:

1. Your images show an iPart with a table - does this problem manifest with regular parts (non iparts)

2. When you say vault generated data - does that mean, that vault is generating and saving the members? And a        subsequent consumption of the ipart causes issues?

The prompt itself looks like a vault prompt. If indeed that this is a non-edit operation, then vault should also honor the prompt for recomputable updates. Secondly, you should be able to suppress the prompt by saying "no to all"? I am not sure if the ">>" on the prompt button gives you more control on how frequent you want to be prompted.

Thanks for the info.

-shiva

[swalton · Accepted solution]

Are you editing the iPart table?  

I have found that I need an "update assembly' when I work with Vaulted iParts and iAssemblies.

This update assembly is used to force Inventor and Vault to check out and update all the generated member files at once.  I use it every time I migrate the iPart/iAssembly between Inventor versions, whenever I make a change to the iPart/iAssembly table, or if Inventor decides to dirty any of the factory or member files.

How it works:

Create the iFactory file to control the design.

Generate all the members.

Create a new assembly file.  I usually name it  FactoryName Update Assembly.

Add all the member files to it.  I don't bother constraining anything.

Check the Update Assembly into Vault.

Later, when I need to make a change to the iFactory file, I do Get/Checkout all on the Update Assembly.  This checks out all the member files and the factory file.  I then make my edits to the factory file.  Once the edits are complete and saved, I open the Update Assembly and do a rebuild all, then save.  This forces Inventor to update all the member files at once.  I then check in the Update Assembly and all its children.

Any time I add a row to the factory file, I generate that member and add it to the Update Assembly.

[AlexZW28B · Accepted solution]

Well, after some back and forth with an Autodesk person... and finally having time to respond, thank you @johnsonshiue... I was able to figure out that yes it was indeed by .ipt Factory file... aggravatingly so. Thank-you @swalton for the advice on that update - very helpful. I have included some of the summary correspondence below - with my side notes added in this post

[JS]: Essentially iPart is like a derived part. It has a factory ipt file and member ipt files (deriving from the factory). It is best used as library parts, stored in library folders and managed by the admin.

I will say though, that this seems like a really convoluted mess, or opportunity for mess, for the parts to have 1 file which will then cause all the others to then experience data/version/update issues…

[JS]: Yes, it can be. This is why I keep telling our users that iPart/iAssembly was meant for creating library components. Do not attempt to use it as a replacement for SWX Config or Creo Flexible Part.  -----   Side note:(***Ohh how I miss SWx at previous employer***)

So, as an example, with that factory, if a new part is “generated” from said factory – or a new variation is input into the table of that source “component”, then it will cause all the subsequent individual parts tied to that first part to initiate a need for an update? Even if it was only 1 component/variation adjusted in that source “factory file”?

[JS]: Yes, the change in factory will propagate to all members if the change applies to all members. Then the members will be updated (checked-out/saved/checked-in).    -----   Side note:(***Ughh... this kinda sucks***)

I am also assuming – referring to the image I posted on the forum thread – that the “Bolt.ipt” is the factory component, and all the other components are related from that factory… So, if I happened to create a new variation or modify one existing variation of that “Bolt.ipt” then it will flag all subsequent parts for an update?

[JS]: Correct!   -----   Side note:(***Ughh... this really kinda sucks*** I now have to update a whole whack of parts if I add something)

I am unsure where the bolts would be stored alternatively on our vault – I don’t see a “Workspace” location in the vault. We are occasionally adding new hardware to the vault, or variations of the same component. By moving our standard/hardware components to a library, which I am not too sure where/how to do that yet, it sounds like we will still have the same issues?

[JS]: The bolts need to be saved in library folders. Based on the file structure I am seeing, I suspect these iParts are copied over from else where. Essentially, there may be duplicate iParts in different folders within the project. This is not a good practice to begin with.

[AlexZW28B]

I will also add, that I had to ensure I was checking out the base "Factory File" when doing this. The Bolt.ipt, nut.ipt, etc. for the corresponding component/factory had to be checked out do also capture the relationship updates...