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Distinguished Contributor
sumayo
Posts: 175
Registered: ‎09-30-2006
Message 1 of 10 (1,847 Views)

Unlocking Master View Rep

1847 Views, 9 Replies
07-22-2008 10:56 PM
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.
Active Contributor
stephenrott
Posts: 28
Registered: ‎04-11-2006
Message 2 of 10 (1,845 Views)

Re: Unlocking Master View Rep

07-23-2008 04:41 AM 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
Distinguished Contributor
sumayo
Posts: 175
Registered: ‎09-30-2006
Message 3 of 10 (1,845 Views)

Re: Unlocking Master View Rep

07-23-2008 01:03 PM in reply to: sumayo
Thanks for that.
Mentor
CAD-One
Posts: 710
Registered: ‎10-26-2008
Message 4 of 10 (1,699 Views)

Re: Unlocking Master View Rep

07-18-2011 09:59 AM in reply to: stephenrott

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

C1
Inventor Professional 2013
Vault Collaboration 2013
Product Support
bobvdd
Posts: 527
Registered: ‎11-23-2005
Message 5 of 10 (1,677 Views)

Re: Unlocking Master View Rep

07-18-2011 02:53 PM in reply to: CAD-One

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

Bob

New Member
jaxonusa
Posts: 2
Registered: ‎04-12-2012
Message 6 of 10 (1,464 Views)

Re: Unlocking Master View Rep

04-12-2012 01:55 PM 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.

*Expert Elite*
Curtis_Waguespack
Posts: 2,775
Registered: ‎03-08-2006
Message 7 of 10 (1,455 Views)

Re: Unlocking Master View Rep

04-12-2012 02:12 PM 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




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New Member
jaxonusa
Posts: 2
Registered: ‎04-12-2012
Message 8 of 10 (1,449 Views)

Re: Unlocking Master View Rep

04-12-2012 02:24 PM 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.

Product Support
bobvdd
Posts: 527
Registered: ‎11-23-2005
Message 9 of 10 (1,440 Views)

Re: Unlocking Master View Rep

04-12-2012 03:36 PM in reply to: jaxonusa

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

Valued Contributor
cadull_rb
Posts: 79
Registered: ‎11-16-2011
Message 10 of 10 (1,434 Views)

Re: Unlocking Master View Rep

04-12-2012 05:39 PM 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.

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