Part Visibility in Assembly annoyance.

[Anonymous]

Hey all. First post here, and first of all, having a blast with Inventor!

Above all there's one thing that keeps annoying me though.

I work on a lot of different internal parts of a project plus an outer organic shell and everything has to fit perfectly together.

It's so great being able to work in the Assembly and see other parts In "Xray" while adjusting another, however, sometimes I really need to hide certain parts...

Whenever I do so (Alt-v) it works greats in itself, but when I show them again, all otherwise hidden work planes and shared sketches are turned back on which is a huge mess, especially now that my  parts have grown in complexity!

Is there some workflow here or option that I'm missing?

I have experienced the same behavior on 2017 and 2018 and I have to say it feels like a bug, or at the very least an incomplete functionality...

Being a programmer myself I know the easiest to do when toggling "visibility on" would be Not to check whether its sub-parts were specifically set to hidden but instead just turn visibility on on absolutely everything...

Thanks!

Lasse

[Anonymous · Accepted solution]

View representations would be the way to go, if I understand correctly what you are doing. You can set whatever visibility of parts and work features and the settings will be remembered (and recalled) for every representation. Even the viewpoint from where you were looking. Switching from one to the other is only one doubleclick away.

[Fouad-l]

Hi.

You can control work operations visibility inside an assembly from : View --> Object visibility and deselect work operations you want to hide.

I normally hide unconsumed work operations (sketch,planes,axis..) inside each part separately. Then i control assembly work operations from the option above.

There is also an Add-in that looks interesting to simplify the workflow : 

https://apps.autodesk.com/INVNTOR/es/Detail/Index?id=3037553269009106722&appLang=en&os=Win32_64

[Anonymous]

Thanks, but I had seen that menu. Actually my original post should probably have been more detailed. Turning visibility on/off is only one of the cases when this happens.

This approach is fine until I want to edit a sketch in that part, then everything I had already hidden is made visible again...

[Anonymous]

Thanks... After looking around a bit it seems this is a decent workaround!

I will still maintain that the behavior when simply toggling visibility is buggy or at the very least very lazily implemented, but I can get used to this... 😉

[Anonymous]

Editing a part will, "by definition", make work features visible to allow making references to it. This opens another possibility : opening the part that you want to edit separately. This will affect visibility only in the part and switching back to the assembly you will see the part changes without influences on the view. Major negative point about this is that you loose the assembly context to tweak your edits to the surroundings.

Alex

[Anonymous]

Thanks for your reply. I have grown quite fond of representations. There are still some things that annoy me on occasion, but way less now.

Like, for example, when editing a multi-body part I would very much expect a solid I have specifically set to hidden Not to suddenly show up when I edit a sketch...

[Anonymous]

Also struggeling on a regular basis with this same behaviour. I will try the workaround as suggested here but it sure would be nice to have an option to turn off visibility to all reference parts (and I use a lot of them). Would fit nicely in the Object visibility menu I would think.

Having a large top level assembly turn on all references is frustrating to say the least.

[rhenstenburg]

I have found this "feature" to be an irritation also.  Using visibility is OK but requires constant updating to keep current as parts/subs are added below.  I note that the visibility of work features and sketches in PARTS maintain their state when the part is brought into an assembly.  From the assembly level, these visibilities can be modified (editing in place) but if visibilities are set in a part then that part is brought into an assembly, when visibility of that part in the assembly is toggled on or off, the visibilities set in the part are maintained.  This is NOT the case for assemblies. For example, for a sub-assembly , if the visibility of a plane is turned off in the Default View rep (sub-assembly opened in its own window) then the sub is brought into the parent assembly (Default view rep), the plane in the sub assembly will NOT be visible initially.  HOWEVER, if the visibility of the sub is toggled off than back on in the parent assembly, that initially visible plane becomes visible.  The visibility status set in the sub is NOT maintained.  (Repeating this with a part instead of a sub-ass'y, the visibility of the plane set in the part IS maintained).

In reading this thread, I believe that this is the original complaint from @Anonymous. 

I work in a collaborative environment where we make very large assemblies and items are constantly being added.  This limits the value of View Reps.  One can always toggle the visibility of ALL work features and sketches using Object Visibility but many times there are a few key features that I would like to keep visible.  If these could be set to persist through toggling visibility in a parent assembly, this would be desirable.

[johnsonshiue]

Hi Rob,

I believe you are talking about the Design View Rep behavioral difference between part and assembly. It is indeed a bit confusing. Let me explain how it works and hopefully some confusion can be clarified.

A custom Design View Rep (DVR) stores visibility and appearance overrides to Master state. This applies to assembly and part. DVR at lower level can be linked to the higher level. I suggest you change the following option so that component DVR are linked by default.

Go to Tools -> App Options -> File -> File Open Options -> set DVR to last active for both assembly and part.

When DVRs are linked, it means the given component will be displayed in the hosting assembly the same way it looks like in its own document window with the DVR active. When you edit the part in place and hide the workplane, the "override" is actually stored at the top-level assembly DVR, not at the part-level DVR. As a result, the workplane remains visible within the part. You will need to open the part in its own window and turn off the visibility.

There is a subtle difference between assembly DVR and part DVR. At assembly level, Master DVR means there is no override and everything is visible. At part level, Master DVR also means there is no override but workplanes and sketches can be made invisible (as the base state).

In a hindsight, DVR was made too powerful. By hooking up visibility control and the appearance control, it inter-mingles modeling and touching-up processes. DVR is best for post-modeling workflows, meaning the geometry has already been clearly defined and the focus is on tweaking the appearance. There should be a global, non DVR-driven process to control sketch and work geometry visibility, particularly when editing and modeling happen extensively.

Many thanks!

[rhenstenburg]

Thanks for your reply @johnsonshiue.  I reread my post and realized I was confusing (in the 2nd sentence I said "Using visibility is OK ..." but meant "Using Design Reps is OK ..." - you got my meaning anyway).

My App Options settings are as you suggest.  I appreciate your description of the difference between DVR in a part and in an ass'y. 

In my work environment, we make "one offs".  When the design is complete we have no time to clean it up because we are moving on to the next design (we design an build human centrifuges for pilot training among other things).

Specifically for work features, it would be nice if these worked the same for parts and assemblies.

Consider the following workflow.

1) Create a plane in an ass'y ("A") then turn off it's visibility in the "Default" DVR.

2) Insert the above ass'y into a parent ass'y ("B").  "A" will be displayed in "B" with the plane visibility off. Good.

3) In "B", turn off the visibility of "A".  (You may get warned of associativity being removed, no matter).

4) In "B", turn the visibility of "A" back on.  The plane is now visible.  In addition, the DVR (under Representation) of "A" in "B" is now Master.  I can set the DVR back to Generic but this is a two step process.

Thus the crux of the situation is that the DVR set for a sub is lost at the moment you turn visibility off (you can check the DVR under Representation of the invisible "A" sub).  It would be nice if the DVR setting of a sub in a parent ass'y is retained, even when visibility is toggled off.  The goal is that when visibility is toggled back on again, the same DVR for the sub is set in the parent.

[SBix26]

Yes!  This is the subject of at least one idea in the Inventor Ideas forum, but I'm too lazy to search for it right now.

---

Sam B
Inventor Pro 2021.2.1 | Windows 10 Home 2004
LinkedIn

[rhenstenburg]

The link to the idea that @SBix26 refers to is here . I found it and voted for it.  If anyone else is annoyed by this behavior, follow the link and VOTE.

[johnsonshiue]

Hi Rob.

Yes, I agree there is room for improvement. But, at the moment, we just don't have a good solution. In terms of prompting for "disassociate DVR" or "modify DVR." Actually, you may want to select "modify DVR" instead. It will make sure the visibility change is saved back to the subassembly or part DVR itself.

Many thanks!

[rhenstenburg]

Thanks @johnsonshiue  but what is desirable to me is more simple.  When toggling visibility of a sub-ass'y in a parent, I want the selected DVR for that sub (set in the parent) to remain the same and NOT be switched to the Master DVR (in the parent) when the visibility is turned off.  This is independent of the active DVR in the sub itself.  This is similar to a host of other overrides that can be set in the parent and do not get pushed to the sub.  (Changes to the sub should be made in the sub itself, changes made to a sub in the parent are in the parent only ... that seems to be the general rule and is easy to follow).

[Anonymous]

Thanks, this was the answer and worked for me

[armansesar]

setting specific view representations generally helps a lot when repeatedly switching between specific cross sections, colors (such as solid vs. transparent appearances)...etc, but hiding and unhiding still resets representations within each view rep. Hiding visibility or changing the appearance of any component resets the representation of that component from associative (model view) or any other view representations and adjustments made in each view to the primary view representation, which is locked. The only work around I see is developing unique view representations, locking said representation, the when changing part visibility and inevitably resetting the view rep to 'primary', clicking on another view and returning back to the intended view. This still creates a lot of work as you are now required to re-adjust everything back to the intended configuration (if any other changes were made) just to avoid having to go back and resetting the parts view representation each time. Over all, a simple fix would be to store the current view representation on RAM and resetting the view REP to the previously assigned view for each part.

This may seem like a slight inconvenience, but it is a huge burden when dealing with complex, interactive assemblies, where parts need to be hidden or isolated repeatedly, and making custom view representations to accommodate for all possible configurations would require countless view representations, clearly this is an issue that should be resolved with inventor, unless I'm missing something.