Derived Assembly select participants

[Bert_Bimmel]

Isn't this the place where I should be able to select which bodies or workfeatures of the source-assembly and its parts show up in my derived part/assy:

Instead, I cannot select or unselect anything in the Dialogue shown above, but it only shows, what Inventor is about to include in my derived part and what not. The only way to control it, seems to be by toggling the visibilities of the things I want and which I don't want to show up in my derived part. Changing the visibilities of the sources afterwards also changes the occurrences (not just their visibilties) in my derived part.

Plus: Multi-Solid-Bodies in some of the source's part's are merged to single solid bodies.

I don't think, that was the idea, was it???

[jtylerbc]

By default, it wants to include/exclude parts based on View Representation associativity.  On one of the other tabs, there will be an option to turn that associativity off.  If you do so, you'll then be able to include/exclude components at will on the main tab.

[johnsonshiue]

Hi! Yes, this is likely a given Design View Rep is selected and the associativity is checked in the Representations tab.

Many thanks!

[Bert_Bimmel]

Ok, nice! IMHO not intuitive!
Now that I have unchecked that Design-View-Associativity, how do I unselect certain solids (aka "surface bodies") , and/or prevent multiple solids from ONE particular part-occurrence beeing merged into a single body?

[johnsonshiue]

Hi! The grey button with a slash is the one to exclude. You may also control it in the source parts. Open each part in the source assembly -> Manage -> Export Objects -> you may exclude the objects that you don't want to be derived by default.

Many thanks!

[Bert_Bimmel]

I know, that the grey slash buttons would be the ones to uncheck. They're not there, when I try to derive the Assembly.
Compare the following screenshot (when trying to derive the part without the detour through the assembly) with the one above:

The two solids within the part are not proposed for unchecking them or not, when deriving the assembly. There I can only choose the entire Part with all its bodies, or nothing (plus the two bodies of the part beeing merged unsolicitedly).

Toggling the export-flag for one of the bodies has no effect - and would be rather counterproductive in my scenario, because I want to export the other body to another derived part.

My convoluted deriving might seem a little bit far fetched, but I came up with that, because I am trying to design a super-complex 3d-Print-Part-Couple, which has become almost unmaintainable when trying to draw it as a single part file with over 300 design features. So I split it up into managable portions, which I then want to merge into two single parts for printing

Anyway, I can though prevent one of the bodies beeing imported by controlling its visibility, and then use the design view associativity-approach. Plus, I CAN derive the now invisible body to another, simple derived part (i.e. without taking a detour through an assembly).  So, I'll go with that, as this way I can achieve what I want, but still I'd say Inventor's behaviour is not very consistent here.

So next question: How do I prevent someone else fumbling with my visibilities, and mess up my derived part? I see, that I can lock the design view... and again I am thinking: WTF??
I lock it, but can still toggle the visibilities of its components (without effecting my derived part 😮 )   ... and am prompted to save the assembly upon closing it (due to the "view-rep (dirty)"*-flag beeing raised) ... just to see, that my changes, which I have made although I was not supposed to be able to make any changes, have been discarded when I reopen the file after granting the save prompt (which it does not, when the file has'nt really been closed, because it's still open in the context of a referencing assembly -> in this case I'll have to switch to and fro between two design views to flush my illegal visibility changes).
Is this supposed to be intended behaviour? Doesn't make sense to me!

*BTW: What's the difference between "view rep (dirty)" and "view rep (smudged)"

[johnsonshiue]

Hi! In Derive workflow, there isn't a way to limit what can be derived. As long as the objects are shown in the tree view, they can be selected. The only way is to create yet another derive limiting the scope of derivable objects.

Regarding "dirty" and "smudged", my understanding is as follows. "Dirty" means the file has been edited and the change has to be saved in order to persist the intended change. Otherwise, the change will be lost. "Smudge" means the file is changed but the trigger to the change is already available in the file. Such change does not need to be saved.

Many thanks!

[torbjorn_heglum2]

You can prevent changed in your derived part by suppressing the derive link in the part. 

RMB the derive feature -> Suppress link

When you want to update, unsuppress and rebuid, the suppress again.

This way you can update on demand.

Torbjørn