Toggle part visibility, view representation changes back to Master?

[PAULBIELA6426]

Just a small issue that keeps bugging me when working in my assemblies.  I have child part in an assembly set to view representation "body" which only contains the solid body (no working geometry). If I turn the child part visibility off, then turn it back on, the child part view rep changes back to "master" and I see all of my unwanted working geometry in my assembly. Is there a way to keep the same representation when toggling visibility on and off?

I've tried playing with locking and unlocking my assembly view rep, changing reps to associative, and still can't figure this one out.

[innovatenate]

Which version of Inventor are you using? Do you have the latest Service Packs and Updates installed? You can check in the About Autodesk Inventor dialog.

Service Packs and Updates can be downloaded from the below link.

http://knowledge.autodesk.com/support/inventor-products/downloads#?sort=score

The below AU class on is a great (and free) training resource on nested view representations and nested levels of details.

http://au.autodesk.com/au-online/classes-on-demand/class-catalog/2012/autodesk-inventor-products/now...

For diagnostic purposes:

When the part file is opened by itself (not from within the assembly), what is the active view representation? Have you tried changing the active view representation and seeing if this impacts the behavior?

Hope this helps.. Thanks,

[PAULBIELA6426]

I updated inventor to 2014 SP1 update 3, Build 222.

The problem still exists, the active view rep in the open child part does not affect its view rep in the assembly. Here is an example:

-Opened Assembly

-Opened child part

-Set view rep of child part to "Default" within the assembly (1st picture)

-Turned visibility of child part off (2nd Pic)

-Turned visibility of child part back on (3rd Pic)

-View rep of child part is now set to "MASTER" showing all working geometry

-Manually change view rep of child part back to "default"

[PAULBIELA6426]

Any ideas??

[-niels-]

Nathan, the behavior described by the OP is what i am used to and, i believe to be, standard behavior.
From your post you are suggesting this should not be happening...?
Can you please doublecheck.

As for the Representations resetting to master, the only way i know of that doesn't do that is using "isolate" and "undo isolate".
That would require you to select everything, except for the parts you want to be invisible....

[mrattray]

As Niels mentioned, this is the typical behavior.
However, you could try using the enable/disable function instead. It's not quite the same, but may work for you.
Also, it's not related, but there is a service pack 2 out for Inventor. I recommend always having the latest service packs and updates installed.

[PAULBIELA6426]

Thanks guys, I'm just used to other CAD software where changing the visibility/hiding a part doesn't change it's selected reference set/config/etc.

Am I the only one that thinks it should maintain the same representation? It's not a huge deal, but when you're designing all day the little things start to bother you.

I'll try the enable/disable function for now and see if it helps. Thanks for the input!

[innovatenate]

Paul,

I just tried to reproduce this on a smaller scale, but I'm not able to reproduce the behavoir. One thought I have is to create a new Design View representations and to delete the "Default" View Rep in the assembly. You should repeat this action with the part or subiassembly document, then re-test. It may be an issue related to a specific Design View Representation, in the assembly or the part.

Would it be possible for you to share the data set in question with me? I would like to investigate this behavior further. You may use the Pack and Go command to collate all of the referenced files into a single location.

Feel free to e-mail it to me directly if you would prefer, nathan (DOT) chandler (AT) autodesk (DOT) com. 

Thanks,

[PAULBIELA6426]

A new Inventor IdeaStation tciket has been made for this. 

http://forums.autodesk.com/t5/Inventor-IdeaStation/Maintain-Design-View-Representation-when-turning-...

[STRIKER-360]

Hi,

Just want to add myself (and all of my colleagues) to the list of people that find this behaviour not only very very annoying but SERIOUSLY time consuming and inefficient.

I work with large assemblies and taking visibility on & off of subassemblies is a task I do hundreds of times, and each time I have to go and select the default view representation again as I use a lot of construction geometry. Also, I do use several view representations to work, review, etc. It’s also worth mentioning this issue being a big problem when using Frame Generator and having skeleton 3D sketches and other construction geometry that should remain invisible after use.

I don’t think this should be the standard behaviour as the logical approach would be to the software to remember the desired user setting (including when switching visibility on and off!).

I really hope Autodesk takes this into consideration.

Thanks

Jonathan M.

[STRIKER-360]

---

@mrattray wrote:
As Niels mentioned, this is the typical behavior.
However, you could try using the enable/disable function instead. It's not quite the same, but may work for you.
Also, it's not related, but there is a service pack 2 out for Inventor. I recommend always having the latest service packs and updates installed.

---

A thought on this idea:

If you go to the Application Options>Display Tab>Inactive Component Appearance and reduce the "% Opaque" value, you can get the "disabled" part completely invisible.

I’ll use this tool from now on instead of Visibility and see how it goes..

Thanks for this, very much appreciated!

Jonathan M.

[SBix26]

Bumping this thread back to the top of the list, hoping for some additional votes for the IdeaStation thread that @PAULBIELA6426 posted a year ago...

Sam B

Inventor Professional 2016 R3 SP1 Update 1
Vault Basic 2016 SP1
Windows 7 Enterprise 64-bit, SP1

[erikjanR42TZ]

Very desireable!

I supported you idea on Ideastation.

[checkcheck_master]

What about this phenomenon really?

A Part with different Views, when used in an assembly and set visibility off and on will force the part to go to the Master view representation.

What is useful or logical about this?
How can you use this correctly?

Am I missing something and I see an Autodesk employee assuming years ago that it would not be desirable behavior.

Please shed some light on this situation, I run into the same thing, try to use it to have certain Solid visible or not, but unfortunately.

[tomasz.sztejka]

This is a known problem since 2010 version. This is a primary reason to not use View Representations inheritance at all. The problem is that Level Of Detail, which creates alike effects is also burdened with own problems.

I have no blind idea how to fix it, even going through API did not help. Internally it appears as if "visible=off" would have been implemented as "nothing is visible" view representation.

[johnsonshiue]

Hi Folks,

This behavior has been discussed repeatedly in this thread and others. You can easily reproduce it by doing the followings.

1) Create an assembly, ASMB1-> Sub1 -> Part1.

2) Open Sub1 and make Part1 invisible. Save all. Now, Part1 is invisible in Sub1 since Default DVR is active. Part1 is also invisible in ASMB1 because the DVR is linked (Default -> Default).

3) Right-click on Sub1 -> turn off the visibility. You are prompted for two choices: "Modify DVR" or "Remove associativity." The first one is grayed out because there isn't anything to modify. Part1 is already invisible. "Remove associativity" option simply reset the Sub1 DVR to Primary (Master).

This is the only way the sub component visibility can be overridden in the context of the top-level assembly ASMB1.

Many thanks!

[checkcheck_master]

Thank you Johnsonshiue for this clear explanation, I have experienced that it works that way, but the logic behind it escapes me for a while.
When I have clearly indicated that I want to show the part in a certain design view, what is the reason to convert it to the master as soon as the visibility is turned on?
I would like to take you along to my thinking/working method with regard to the following with the request to advise us in this regard:
I have a part that can be folded in and out and I get 2 STEP files from the supplier, one in the collapsed state and the other in the expanded state. I unpack both STEP files and place the ipt's in an assembly where I then make a simplyfied part, I go for the solids option. In the simplyfied part I create a design view 'In' and 'Out' and suppress the solids alternately.
The aim is to be able to show both states during the design process and after. That works fine by switching from design view.
That works fine until you turn the visibility off and on again and you are condemned to the master view.
We buy the part as one thing, a simplyfied part of it is nicely compact.

Can we do this differently?
Which method do you recommend to follow in order to achieve the same?

Thanks in advance.