topic Design views / view representations in Inventor Forum

Design views / view representations

torbjorn_heglum2 — Tue, 28 Jan 2025 13:01:57 GMT

This is an old story of Autodesk, that I really struggle to understand. I could address many things, but this time I have two that maybe get some help to understand:

Part Design Views:

It is possible to lock part view representations, and it is possible to lock assembly design views. When I lock in in an assembly, any later added parts will be invisible. It is good, and I use it a lot. But it is also possible to lock a part design View, but what is the difference from an unlocked one?

Assembly view representations:

I use design views a lot, and all subassemblies are usually set up with representations associatively locked to the view representation of my assembly. But if I want to turn of visibility of add transparency to that sub, inventor kills the associativity. I try, but I am not able to understand the logic behind this.

The visibility/transparency of the sub is a property of the assembly. I.e I am changing how the whole thing looks seen from the assembly. If I set up a view representation in the sub with transparency I make all its parts transparent, which is a different thing, I believe.

If I turn off visibility and then back on again, the intuitive situation would be to be back where i was. But this is not possible, and I don't understand why it cannot be like this ?

Torbjørn

By the way, sorry for mixing the use of Design Views and View Representations. I am just a little confused, probably like the developers I guess. The name of this feature seems to change depending on environment 😉

Re: Design views / view representations

SBix26 — Tue, 28 Jan 2025 20:45:57 GMT

For your second question, see the discussion in this Ideas topic: Maintain Design View Representation when turning Part Visibility on/off - Autodesk Community

I can't understand, either, why associativity can't be maintained as long as the subassembly is being turned on/off, or enabled/disabled, as a single entity. It's a long-running gripe and a big stumbling block for new users.

If I recall correctly, there is also a regular Inventor Forum topic that goes into some depth on this issue.

Sam B

Inventor Pro 2025.2.1 | Windows 11 Home 24H2

Re: Design views / view representations

johnsonshiue — Tue, 28 Jan 2025 21:29:24 GMT

Hi Torbjørn,

Though Part Design View and Assembly Design View work similarly, they are different. The lock in Part Design View isn't as strong as the Assembly Design View. Even if you lock a Part Design View, any newly created geometry (surface body or solid body) will be shown anyway. We have heard requests that users would like it to behave more the Assembly Design View.

If I recall correctly, there are technical challenges here. The Part browser tree is chronically and dependently ordered. The visibility of a given object can depend on what state the part is at (rollback). But on the other hand, the Assembly browser tree is orderless. At any given moment, the component can be either visible or invisible. There isn't a state the assembly can go back in time, except Undo.

We have not found a good solution to address this deficiency. In the meantime, I suggest you use Part Design View only when the geometry modeling is done, as a means to show what should be available per given Design View. I don't think using Part Design View while the part is still actively being edited is a good approach. You may run into confusing behaviors very easily.

Many thanks!