Autodesk Vault 2020 Updates

[Heather Mitchell]

Iam 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.

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 johnso...@autodesk.com.

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.

@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.

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.

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.

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.

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.

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.

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.

[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.

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...

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