unlocking view representation

[wolf1o]

Hi,

I've looked and saw quite a few messeges on the same topic but couldn't find some good resolve : I'm in an assembly, trying to hide/supress some component, and it keeps saying that the view is locked (I do see "lock" logos on all the views) and I should unlock it or create a new one, which I don't want - I want the changes to be on the main "master" view)

How do I "unlock" or resolve it?

Right clicking on the view doesn't give me any option to unlock it..

Many thanks ahead!

[SteveMDennis]

Can you supply a small dataset that shows this or give me some more detailed explanation?  Are the view reps at the top level or the sub assembly level?  Arey ou doing visibility of components or suppressing them (they do different things).

When you say you can't unlock, is the unlock command in the menu but grayed out?

[wolf1o]

No - I don't have any "unlock" option at all! Do I suppose to see it when doing right button click?

The views are at the top of the assembly I'm using. It just keeps adding views when ever I'm supressing some component or sub assembly, and I wish to save all changes in the "master" view. How can I do it?

[SteveMDennis]

View reps are for visibility (and color, etc.)  If you are using suppression that should be modifying Levels of Detail only...

So I'm still a bit confused as to what exactly is happening...

Can you give me pictures of what you are seeing?

[wolf1o]

It might be that I was wrong.yes - it had me adding additional level of detail, even though I wanted to save it on the master.

But when trying to hide (visibility) the sub assembly inside, it kept saying that it won't save it under the master "view" unless I'll unlock it or add a new one.

So How can I resolve two issues? (I.E If I decide just to hide it, what do I do with the view, and if suppresing, how can avoid making a new level of detail?

[SteveMDennis]

OK, we are starting to get on the same page I think! 🙂

Can you describe the exact steps because I can't reproduce any "locked" message myself here...

Here is what I am doing.

1. Create a locked view rep
2. Suppress a component, creating a LOD in the process
3. Save/Activate that new LOD
4. turn off visibilty of some sub components

No warning dialog

Is this what you are doing?

[wolf1o]

Hi,

I'm using an exisiting assembly - and BTW, I checked and even if I'm creating a new assembly, I see that the "Master" view is already locked! How can I change that so new assemlies views aren't lock - is this the way it supposed to be???

In any case, I'm attaching the message I'm getting.

I don't understand how come I'm suppresing something and this thing makes me to create a new "View" (configuration right?) and a new level of detail.

Please help:-)

[SteveMDennis]

I'm trying! 🙂

I actually saw that same message myself testing some workflows in 2013 this week...

Just to make sure I'm on the same page as you, you are suppressing something and you immediately get this message?

And you are in LOD Master when thsi happens?

[wolf1o]

Hi,

I get this messge when I'm trying to save the assembly, and because I'm not adding (I don't want to because I want it to be the main view) a new view, when I'm using it in another assembly, or when I open the file again, it brings back the other pieces I suppresed...i brought me to a point which I just deleted the componets I wanted to suppress...not the correct/best way to resolve it!

Again, Is there any way - button, option etc., to go and "unlock" the locked (as you see in the picture) views - I'm sure there's way, How come when I'm creating a new assembly the "master" view is already locked?

[SteveMDennis]

Now we're gettign somewhere!!  I am seeing the same behavior when saving...

I will touch base with some other developers and get you some answers now that I understand the workflow.

Master is not really under your control, it is our "copy of record" so to speak... but I will ask some questions and get some info for you in the next day or so.

I don't think the padlock means the same thing for Master but that's not real clear and I have to investigate some of the concept changes we've made to view reps over the last couple of years while I have been doing other non-Assembly work.

Thanks for digging through this with me.

[wolf1o]

I suspect that only the master is "un lockable"!, which doesn't make sense...if someone wants to changes it and use it as the default....

[Anonymous]

I am unsure if this a related issue, but, as I am having a similar issue, I though I should try here first.

I am running Inventor 2011. I have downloaded parts from McMaster (IGES) and used them in a sub-assembly. When I create a view in a .idw file, none of the imported components are visible. Even if I use the sub-assembly as the base view, there is nothing. The parts are visible in the model.

I have the same lock issue as the other users; are these two issues related?

If this should be a separate topic, I'll repost.

Thank you.

Marc Zuckerman

[wolf1o]

Another related question: I just created a new (And it's not locked) view, and suppressed the items I don't need in it.

What happened is that it did make me create a new LOD - why is that? Why can't I make the changes on the "Master" LOD? Why does it make me create a new one?

[SteveMDennis]

Marc,

  Are the imported components surfaces perhaps? We don't display surfaces by default in IDW views. They must be included by checking the option at view create time (I think) or manually after the fact.

I don't think your issue is related to the locked view rep.

Can you look for surfaces? If they are solids then repost and I'll t ry to help you in that thread.

[SteveMDennis]

MASTER LOD is special.  it is the "world", we need this for things like mass properties, BOM, etc.

We need to know what the entire unadulterated model is, and you modify that, by creating new LODs, etc.

This is how LODs have worked since day 1. Master is the master (sorry), and other LODs are derived from it.

When you create a new LOD we only track what is suppressed from Master.  It does make the bookkeeping easier internally.

[Anonymous]

Steven,

Thank you very much. They were in fact surfaces, and your instructions were right on.

Marc Zuckerman

[SBix26]

wolf1o: I think that you are not understanding the distinction between supress and visible.  Making a part invisible (unchecking Visible) changes the view of an assembly.  View representations show different views of an assembly, with differences in visibility, color, etc.  Suppressing a part changes the Level of Detail representation, and, if you are working in the Master LOD rep, forces creation of a new LOD, which wants to be saved when the file is closed.  LODs are for saving on memory in really large assemblies (or on really poor computers).

If you are wanting only to turn off visibility of components, then use the visibility attribute and save yourself the trouble of managing LODs.

Hope this helps.

[wolf1o]

Ok. Two question regarding that:

1. I noticed that when choosing the master view in the assembly, it will also show all the other parts and sub assemblies in their "master" view mode - this is how it's supposed to be?

2. If I really want a part to be not just "invisible" - not shown, but also not included in the BOM, is there a way (like solidworks) to just hide it (or show it) but exclude it from the BOM? (it's not by "enable" right? What does "enable" do when I unchoose it?)

Thanks!

[Steve_Bahr]

Right-click the .igs part/assembly in your drawing browser and select "include all surfaces".  Your .igs part/assembly should now be visible in your drawing views.

I don't think the two issues are related.

[SBix26]

1. Master View, or Master Level of Detail?

2. The easiest way to keep a component from showing in a Parts List is to make it a Reference component.  It will still appear in the BOM, though; visibility is controlled separately.

2.5 Deselecting Enabled makes the component transparent and not selectable in the graphics area-- very useful for working inside an assembly.