Derived part, why does my base component require an update?

[Silvia.van.Emmerik]

Hi , I want to make a derived part from an .ipt.

I get the message that the base component requires a change. WHY is this?

the Inventor version is ok (2016), I tried unchecking computable updates with no effect.

I don't want to change the base file, because it is in the Vault and Released.  

[ShayaGhanbar]

Make sure that you have the file on your C drive. Go to the properties of the file and make sure that it's not read only. Since the file is in Vault, you have to make sure that you go to the file properties and uncheck mark read only.

Now, you can do the derive and if it needs to save on the original file you can save on the original file because it is not read only.

Once everything is done, delete the files from C drive so you still have the latest in your Vault.

[SBix26 · Accepted solution]

I don't understand what happens under the hood, but this generally means that the items that you are deriving in the base component have not been marked for Export.  This is a change to the base component file and is required for the link to work.  I have gradually gotten in the habit of marking solids, surfaces, sketches, etc. for export as I'm creating them so I don't run into this issue.

I'd be glad to hear an explanation for why this is necessary-- @johnsonshiue, can you explain, please?

Sam B

Inventor Professional 2018.2.3
Windows 7 SP1

[johnsonshiue]

Hi! Without seeing the actual file, I guess this is related to the fact that the derive source objects were not marked as Exported. Back in the very old days, Inventor used to make all derivable objects (solids, surfaces, sketches, parameters, and work geometry) from the source available for the user to choose. However, the performance of such operation is not good particularly the source part or assembly is big. In order to speed up the process, the scope of derivable objects are reduced. Only the objects marked as "Exported" are listed in Derive dialog by default. Also, by default, none of the objects are made "Exported."

When you derive an object, either it is already set to "Exported" or it is made "Exported" within Derive dialog. In your case, I assume the solid was not made "Exported" but Derive dialog made it for you when you selected. As a result, the source document is dirtied and it has to be saved. To check the status, go to the source document and go to Manage -> Export Objects. You will see if a given object has been set to "Exported."

Many thanks!

[SBix26]

Thanks for the explanation, @johnsonshiue.  I wish it were possible to get to an in-between functionality where some entities (solid bodies, for instance) would be automatically marked, and others, such as sketches and work features, would not.

Actually, in 2018, it seems to me that I've been pleasantly surprised a number of times to find that solid bodies were already marked for Export, even though I had not done so manually, nor to that point used them as derived bodies.  I wonder if my wish has been granted?

Sam B

Inventor Professional 2018.2.3
Windows 7 SP1

[Silvia.van.Emmerik]

Thanks for your explanations, it was indeed the Export. I checked the Export option for solids in the base file, saved it and now I don't get the message anymore.

Now I just have to change all released files in the Vault 😉 (we didn't pay attention to this in the past). So, like Sam I do hope that in 2018 at least the solid will be set to export by default.

[johnsonshiue]

Hi! I don't believe there is behavioral change here. The first solid is always exported by default. But, other objects and any other solids are not set to Exported by default though.

Many thanks!