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Unlocking Master View Rep

24 REPLIES 24
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Message 1 of 25
sumayo
14332 Views, 24 Replies

Unlocking Master View Rep

I have an assy in which I have created work planes which are huge and annoying, so I make them invisible but when I save the assy I get a message saying the Design Current Design view representation.... blah blah..... or Unlock the Current one.

How do I unlock the Master View Rep.
24 REPLIES 24
Message 2 of 25
stephenrott
in reply to: sumayo

From a previous reply:

Reply From: Peter Maxfield \(Autodesk\)
Date: Jun/27/07 - 08:51 (GMT)

Re: REPRESENTATIONS - VIEW - MASTER
Hello,

This is as-designed. The Master is meant to represent the entire assembly, fully visible
and fully enabled.

We recommend working with a user-created DV, such as "Default" as shipped with the
templates, for allowing customization.

Regards,
Pete
Product Design Lead
Message 3 of 25
sumayo
in reply to: sumayo

Thanks for that.
Message 4 of 25
CAD-One
in reply to: stephenrott

Doe it mean that the master view rep is automatically always locked?

C1
Inventor Professional 2020
Vault Professional 2020
AutoCAD 2020
Message 5 of 25
bobvdd
in reply to: CAD-One

That is correct. hence the lock symbol in front of Master

Bob




Bob Van der Donck


Principal UX designer DMG group
Message 6 of 25
Anonymous
in reply to: bobvdd

I'm super ultra frustrated with this.  I have models with a many planes and sketches in it.  They're all fine, it just crowds the screen when they're all on.  Here's where I pull my hair out:

 

I get the part model looking just how I want.  I mean, instead of using the master view, I make my own called default.  Boy it would be super fantastic if I could just set an option to use the default view when the parts are inserted into an assembly instead of Inventor requiring me to use the master view.  Ok, but for now, I have to insert the part, right click on representation, and choose default view.  So, it’s just a minor inconvenience.  No hair pulled out yet.  Here’s what burns me up.  When I uncheck the visibility box, the part is no longer visible.  So far, so good.  When I check the box to make it visible again, what do you know, it’s switched over to super horrible looking master view.  I never asked Inventor to switch views, but it went ahead and did it anyway.  So, now I have to right click, representation, default view etc.  Still not pulling my hair out, but thinking about it.  Ok ok ok, I have it figured out.  I’ll make the representation associative right?  Then when I turn my model back to visible, it should update the view to wherever I left the default view in my model right?  Fantasic.  But, it doesn’t work.  When I uncheck the visibility box, I get an error message requiring me to remove the associativity.  First of all, why do I get any kind of error message just for unchecking a visibility box, com’on guys…  Second, why can’t the part be unvisible and become visible again with the same representation?  That’s when I pull out hair by the fist full.  Why MUST I have to go through the master view?  It might not be that bad if I could CHANGE THE MASTER VIEW, but I can’t.  Inventor is forcing me to use the master view and won’t let me change it.  Very, very frustrating.

Message 7 of 25
Curtis_Waguespack
in reply to: sumayo

Hi jaxonusa,

 

As a rule of thumb it is best to always right-click on work features and sketches in the part file and turn off the visibility there. This prevents the issues you're having with the visibility of these things turning on and off at the assembly levels.

 

You can then control the visibility of the work features and sketches in the parts at the assembly level as needed.

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com


Message 8 of 25
Anonymous
in reply to: sumayo

Well, that's what I'm doing.  I can get the view in the part file to look the way I want it, but not in the part file master view.  The master view is the one what gets used when the part inserted or checked back into visibility, and that's the one that can't be changed.

Message 9 of 25
bobvdd
in reply to: Anonymous

The only thing that I can think of to toggle the visibility of parts while keeping workfteaures invisible at the end of the ride is to LOCK the viewrep:

 

1) Lock the active viewrep (ie. View1)  in your assembly

2) Turn off the visibility of one or more parts

3) Do whatever you need to do ....

4) Activate the Master view rep of your assembly

5) Activate View1

6) Unlock View1

 

This will bring you back to the initial situation with the parts visible without seeing unwanted workfeatures and withour the need to activate viewreps in any of the parts.

 

Bob




Bob Van der Donck


Principal UX designer DMG group
Message 10 of 25
cadull_rb
in reply to: bobvdd

I have this issue too, also with Enable/Disable. Locking a view representation removes the associative representation links, so it is not without side effects.

 

Also when adding a new component to the assembly I have to remember to link all the representations as desired. I'm thinking of automating the associations as my views usually follow a pattern (Assembly -> Component): Default -> Default, Design -> Reference, Reference -> Default.

 

I wish the visibility of origin features was remembered by the view representations. Also that view representations were applied to iPart members based on the iPart factory, or there was some way of applying visibility/enabled to the derived features.

Message 11 of 25
john
in reply to: Anonymous

Just ran into this same issue today, several years later.  Using inventor 2016.  Still have one or two strands of hair left......

Message 12 of 25
stevenpayne89
in reply to: john

I too have had this issue.  The concept of design views sounds good, but I have yet to see an implementation that doesn't require us to hire people with no hair...

Message 13 of 25

Hi Steven,

 

This is a very old thread. Some of the comments may not apply to more recent releases. Design View Representation can be applied to an assembly or a part. It depends on what you want to achieve, there are workflows to help you accomplish your goal. I don't want to get into detail yet because it can overwhelm you. Could you tell me what exactly you want to do? I should be able to tell you the best workflow to do that.

Many thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 14 of 25
50h9j
in reply to: Anonymous

I think it is worth pointing out that the padlock symbol means different things depending on whether you are in a part or an assembly.

I may be simplifying a bit here but...

In the part file it locks out only section view (use other view reps sparingly for sections if you don't want view rep lock errors on save)

In the assembly file it locks out section, visibility, appearance overrides

 

Therefore in a part file you should turn off work features in master view. Place the part into an assembly so that the default and other views display the part master view - no change of view rep necessary.

 

It is a conceptual mess but works 98% of the time.

---------------
Autodesk Inventor 2017 Certified Professional
Inventor Professional 2019, Nastran In-CAD 2019, 3ds Max 2019
Windows 10, 64 bit
HP Z800 X5680 16x 3.33GHz NVidia Quadro 5000
Message 15 of 25
johnsonshiue
in reply to: 50h9j

Hi! Just put a little bit historical perspective here. Indeed, the Master Design View in Assembly has a different behavior in Part. DV:Master in Assembly was implemented more than 15 years ago. It allows users to configure component appearance in a given assembly along with work geometry visibility. There was no Part Design View until 2012. Part Design View generally works fairly similar to Assembly Design View. But, there are major differences.

First, DV:Master in Part is basically as is. Overrides can be saved in Part DV:Master, which is not allowed in Assembly DV:Master. The reason why it is designed this way is to support the legacy files already contain part level and body level color overrides. If Part DV:Master strips off the existing overrides, the files will have to be migrated and a new DV will have to be created on open. As a result, the behaviors are different.

Second, Part DV has to interact with feature history. For example, you can move EOP or edit a body generating feature, the body will not exist and the body color will be put on-hold. Work geometry and sketch would have similar behavior. Assembly DV pn the other hand only needs to care about individual component occurrence. There is no history tree in assembly except assembly features. However, Assembly DV does not control assembly feature appearance anyway.

Anyway, this is a design choice made by the Inventor team. There are certainly pros and cons. So do other proposals.

Many thanks!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 16 of 25

Hi, I have a skeleton model that I use for our design process.  It uses work features to place and size components in our assemblies and parts.  However, because of the large number of parts that we need it is difficult to manage.

 

I was trying to use the design views to change the "mode" of our skeleton.  Modes could be Part Design, Component Placement, etc.  Each mode shows different work geometry and features that the end user will leverage while creating parts.  Unfortunately, I wasn't able to wrap my head around the design view concepts.

 

Thanks to @50h9j for explaining that assembly and part design views are intended to operate differently.  At the end of the day, I am trying to setup design views, but when i have to change/ add components, where should I be working?  In the Master Design View?  If so, I then have to go through each other design view and hide all the new features.  Just seems like a lot of extra time.

 

If anyone wants to pm me for more info, I can provide some models.

Message 17 of 25

I know this is a slightly older thread, but I have been having a similar issue. The view representations are all well and good, but what I don't like is Inventor changing the view representation of my assemblies back to locked Master every time I go to save. I have NO idea what is causing it to switch back and it's really annoying. Looking for any insight because I've looked in Options if there is a setting that tells it to switch to Master, but haven't found anything.

Message 18 of 25
mcgyvr
in reply to: karipates6709


@karipates6709 wrote:

I know this is a slightly older thread, but I have been having a similar issue. The view representations are all well and good, but what I don't like is Inventor changing the view representation of my assemblies back to locked Master every time I go to save. I have NO idea what is causing it to switch back and it's really annoying. Looking for any insight because I've looked in Options if there is a setting that tells it to switch to Master, but haven't found anything.


@karipates6709  Often that is due to suppressing parts or similar..

Are you trying to suppress parts in view reps?



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Inventor 2023 - Dell Precision 5570

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Message 19 of 25
karipates6709
in reply to: mcgyvr

No. I may turn things off or on visibly, but avoid suppressing so I'm not changing the level of detail. I've only noticed this start happening in the last couple weeks. Visibility of parts shouldn't change the view representation. When I see the error about saving with it in a locked view representation then I switch it to the unlocked Default, but it doesn't stick for some reason.

Message 20 of 25
mcgyvr
in reply to: karipates6709


@karipates6709 wrote:

No. I may turn things off or on visibly, but avoid suppressing so I'm not changing the level of detail. I've only noticed this start happening in the last couple weeks. Visibility of parts shouldn't change the view representation. When I see the error about saving with it in a locked view representation then I switch it to the unlocked Default, but it doesn't stick for some reason.


@karipates6709  Do you have an assembly in which this issue is repeatable/reproducible to share with Autodesk?

 



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Inventor 2023 - Dell Precision 5570

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