Turn off work planes and sketches in assemblies

[Anonymous]

Hi 

I have created an assembly with multiple parts and sub assemblies. Some of these sub assemblies have user work planes in them.

My question is this, how does one go about turning off these work planes and sketches in the main assembly? I know that a person is able to create a view representation and turn off the planes and sketches through the Object Visibility which works well. The issue comes in when I now want to create a part within the main assembly and I start creating user planes, this action now turns on all of the user planes from the sub assemblies as well as some sketches. This makes is extremely difficult to see which plane I have created in the part that I am editing as I have so many other planes visible. 

The only work around I have seen is to go to each and every part and sub assembly and select the planes in the model browser and select the visibility to be off, this however is tedious work. Does anyone have a work around to this issue? 

[Curtis_Waguespack]

Hi markben,

It's best practice to turn them off at the level that they were created.

You can use this method to do so, if it wasn't done to begin with:

http://inventortrenches.blogspot.com/2013/03/turn-onoff-all-workfeatures-with-ilogic.html

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

[Anonymous]

Edit: Nevermind, just realized you already stated this in OP, but can't figure out how to delete my post.

The other option is "Object Visibility" under the View tab. However, I believe that this is only for your user session and will not impact the "Visbility" settings of the assembly file.

[SteveMDennis]

@Anonymous @Anonymous

The object visibility setting IS stored in the design view.

But we have a long standing decision that if you start creating a class of object (sketch, WP, etc) and the object vis. is turning that class off we remove the OV setting, the assumption being you want to SEE what you are creating! If we didn't do this you would create a WP and it would immediately disappear.

As mentioned the only solution is to turn them off at the source before you leave the part or turn them off individually in the assembly.

[cbenner]

---

@SteveMDennis wrote:

@Anonymous @Anonymous

The object visibility setting IS stored in the design view.

But we have a long standing decision that if you start creating a class of object (sketch, WP, etc) and the object vis. is turning that class off we remove the OV setting, the assumption being you want to SEE what you are creating! If we didn't do this you would create a WP and it would immediately disappear.

As mentioned the only solution is to turn them off at the source before you leave the part or turn them off individually in the assembly.

---

That IS generally true, @SteveMDennis, but not always.  When one has an assembly that might have thousands of user work planes AND all of the origin planes, and wants to create one more work plane.... it may not be necessary to have all of the existing work planes suddenly become visible just to create the one.  From experience (I know you're tired of me talking about tube & pipe... lol), turning work planes off at the source can be a very lengthy process.  I sometimes have a single pipe run that has a dozen routes... and each route can contain as many as a dozen work planes (from include geometry).  That is a lot of individual work planes to have to manage one at a time.  Having the choice to set view reps at the sub-assembly level, and then activate them at the top level (if I'm saying this right) such that the work planes of just ONE sub-assembly are currently visible.... that would be a wow factor.  That would be worthy of a standing ovation at your "Meet the Developers" class this fall.

[Curtis_Waguespack]

---

@SteveMDennis wrote:

...If we didn't do this you would create a WP and it would immediately disappear. 

---

I started to reply to this earlier, then decided I'd pass, then saw cbenner's reply, and decided to yell "Dogpile!" and run in and pile on:

So, you might be aware already, but from the average user's point of view, none of this is clear, discoverable, or (in many cases) usable.

I have tried in the past to find a clear and concise reference to how and why this works in the help files, to pass along to users when this question arises, and have failed. I once attempted to write a tutorial to demonstrate how it works/ doesn't work, and I ended up "punting" on that, because it all became so removed from the reality of real world use that it was simply academic and of little value to the user.

Ideally, the current Object Visibility state would just get updated/modified when a new sketch or work feature is created, leaving what was off to remain off, and the new object to be on. Obviously if the current state were a "standard" state such as All Work Planes Off, etc. that would need to be modified, to a "custom" state, with all but the new plane(s) off. 

Do you have some idea if that is possible or not?

Also, I think most (many?) users would just like to have a one button solution like that iLogic example, that reaches into each component and turns everything off at that level. That is the perception of what the Object Visibility tools do is, and why users become confounded when everything turns back on after they think they've turned them back off.

I wonder if an option to reach down and truly turn them off could reside in the Object Visibility menu as well?

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

[SteveMDennis]

All right you two... @Curtis_Waguespack @cbenner let's look under the hood for a minute.

When you turn an occurrence of a WP or sketch off for example we hang an attribute on the scene saying "this path to this object" is off, so all the other occurrences of that object (referenced through other paths) are left on.

The Object Visibility is implemented as a master valve outside your house... when we turn off OV for a class of objects, whenever the object is encountered during the scene traversal it is simply not drawn and all the other attributes (if any) are ignored.  The master valve is the easiest to implement and to me makes complete sense but than again I'm the one who implemented it!

What you are describing is when OV is turned off, we would need to find and hang attributes for each occurrence (1000s perhaps) of that class of object. Then when you cleared that OV for that object we would have to clear them (and not clear any path specific visibility you may have added).

This has a few problems

• OV would take a LONG time to execute, today it's only as costly as a repaint of the screen really.
• The more attributes we process the slower general repainting is, we have to "compile" and process all these attributes
• We would probably end up sucking more data into memory to turn OV on/off. Today we don't suck anything extraneous.

[Curtis_Waguespack]

---

@SteveMDennis wrote:

Today we don't suck anything extraneous.

---

I could assemble a bus load of Solidworks guys that would argue otherwise. Sorry, I couldn't pass that one up.

So my first thought of not turning on everything when a new plane is created, sounds like its out.

A one button solution to truly turn everything off from the current file (be it part or assembly) would still be well received. The Object Visibility tools simply do not do what most users (at least initially) think they do. 

Using your example of turning the water off at the main:

When users use the Object Visibility tools they think they are standing at the kitchen sink turning off the faucet. But instead they've simply turned off the main. And then a bit later when they flush the toilet, somehow the bath room faucet comes on, the shower starts running, the kitchen faucet turns on, the toilet flushes downstairs, and that faucet and shower comes on, the ice maker starts shooting ice across the room, and the lawn sprinklers start spraying the mail carrier... and we tell them, best practice is to... And it doesn't really even register, because the whole experience makes no sense to them.

This is why the question comes up over and over.

Thanks for explaining the under the hood part of this, it has helped me better understand it! 

[swalton]

Its the inconsistency that I don't like.

If I edit a component from an assembly and change the visibility of an existing work feature, and then return to the top level, that work feature is only visibile in the one instance of the component.  All 1000 other instances are unchanged. Ok so far and easy to compute.

When I edit a component from an assembly, and then create a workplane (at the component level), the work plane is visible for all instances of that component in the top level.  That seems harder to compute.

Once I'm done with my edit, I turn off visibility of that workplane and return to the top level assembly. Now the workplane is off in one instance but on in all the others.  I tried to turn it off but failed. 

In order to actually turn off the visibility of the newly created workplane in all instances in an assembly, I have to open the component in a new tab and turn off the visibility there. 

Inventor has what I think is the same workflow (RMB on a workfeature and turn off visibility) that gives me a different result depending when the workfeature is created or on where in the model tree that I invoke the visibility command.

When I edit a feature, all instances of a component change if I edit it either in the stand alone component or in the context of an assembly. Why don't workfeature visibility setting changes behave the same as geometry changes? 

[Curtis_Waguespack]

---

@swalton wrote:

...

When I edit a component from an assembly, and then create a workplane (at the component level), the work plane is visible for all instances of that component in the top level.  That seems harder to compute. Can we assume these instances are set to use a view rep other than Master in the assembly?

...

When I edit a feature, all instances of a component change if I edit it either in the stand alone component or in the context of an assembly. Why don't workfeature visibility setting changes behave the same as geometry changes?  Are you using the Object Visibility tools at all, or just right clicking on it at the assembly / sub assembly level, and never touching the Object Visibility tools?

---

Hi swalton,

I have no answers, but a couple of questions that might (or might not ) help clarify?

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

[swalton]

Curtis,

My ipt files start with just the "Master" view rep.  My iam files start with both "Master" and "Default" view reps.  Others are added as needed.  I have checked all all options in the Object Visibility dropdown. I use the RMB menu to set the visibility checkmark on items in the model browser as needed.  My templates have all origin workfeatures hidden.

I'll try to make a quick screencast this weekend to show the issue. 

[cbenner]

@swalton @Curtis_Waguespack @SteveMDennis  Boy, we opened the proverbial can of worms with this one, didn't we.

Steve, thanks for the technical explanation of why these work the way they do.  That actually helps, sometimes it's just a matter of needing to know why things behave the way they do (or don't).  We all still want that magic button.... but for me at least, understanding it from your perspective does help.

[Anonymous]

Hi Curtis.

Thanks for the iLogic rule this did help me somewhat, for some reason the rule does not switch off all of the planes but it does help to clear the majority of the WP's.

I did come across an app in the Autodesk Inventor App store called RefGeo Toggle that turns on and off all sketches and WP at all levels. I have used it briefly and it seems to work very well. 

[Curtis_Waguespack]

@ markben,

Hey, thanks for mentioning that app. That is good to know about, maybe it'll help swalton as well.

@ swalton,

Yeah, that's the kind of situation I've seen in the past that I've not been able to resolve for people. There is some mix of the Object Visibility and View Reps that causes behavior that is not logical to me. I actually never use the Object Visibility tool, just to avoid those issues. Maybe the RefGeo app will help:

https://apps.autodesk.com/INVNTOR/en/Detail/Index?id=7928398839252798271&appLang=en&os=Win32_64

@ cbenne,

It's a can of worms that probably should be discussed more often I think, I've been guilty of throwing my hands up in the air and walking away from Object Visibility conversations in the past, but it's certainly an area that offers a challenging experience to users, new, intermediate, and experienced alike. I feel like it works "on paper", or on simple data sets, but too often it falls down when users put to work in the real world.

[DRoam]

---

@Curtis_Waguespack wrote:

Also, I think most (many?) users would just like to have a one button solution like that iLogic example, that reaches into each component and turns everything off at that level. That is the perception of what the Object Visibility tools do is, and why users become confounded when everything turns back on after they think they've turned them back off.

I wonder if an option to reach down and truly turn them off could reside in the Object Visibility menu as well?

---

 I think Curtis hit the nail on the head here.

I think most users would benefit greatly from a magic button that does what the Object Visibility toggle does, except when it turns all of the work features, it actually TURNS OFF their visibility in the assembly's View Reps, so that if the user adds more work features later, those new ones can be displayed without turning all the old ones back on again

Both the existing "toggle" and this new button could be in the Object Visibility menu like Curtis suggested. Maybe it could look something like this:

If the user clicked the "Turn off visibility" button, Inventor would turn off the visibility of all objects of the selected type in the Top Assembly's view rep, and then present the user with an option to either modify any associative View Reps, or remove their associativity (same as we get when turning on/off the visibility under a component with an associative view rep active).

[Side note: This dialog box is confusing to most users, so it might help to give it a little explanation, like "Some of the sub-components you're trying to modify have an Associative View Rep active. How would you like to handle these? (   ) Modify associative View Reps    (   ) Turn off View Rep associativity    (   ) Do not affect components with associative View Reps" ]

I think implementing this would help users be much less confused and befuddled by this issue.

[DRoam]

Also..... maybe a button to do the same thing but to a specific sub-component would be useful and appreciated. This one is very near an dear to my heart.... take a look at one of my very first posts to this forum (number 8 to be exact) .....  (which no one replied to... )*

Turn off work feature visibility in particular sub-parts/-assemblies

*don't feel too guilty, the therapy has helped.

[Halleffect24]

I believe I have found a way to achieve what people are asking for without any iLogic. If you select the 'find' function (In Inventor 2018 it's to the right of the search magnifying glass icon, under the drop down menu) you can use this to select all the workplanes. To do this select 'Features & Sketches' in Look For and add Property of 'Type to equal Value 'Workplane'. Hit Find Now and all the Planes are now highlighted in the Model window. Then you can simply right click and turn the visibility off on all the Planes. It's a bit convoluted and it would be nice to be to just select all workplanes with the normal selection tool but it does the job. I hope this helps others as it was driving me mad not being able to do this one simple thing.

[Manuelcamposcosta]

But does that change at top level or at bottom level? Do you do that in which view representation Master or any other?

[doug.johnston]

Here is an ilogic rule that I use to turn off workplanes, sketches, etc. that I found on this forum site.

It generally works to turnoff work features in assemblies, sub-assemblies and parts.  However, I have started using master ipts in my assemblies that contain all information to build assemblies ("Master Skeleton" I believe is the correct term I've seen used).  Sometimes, the rule will not turn off the main origin planes of that master ipt, but turns off the majority of what I was trying to accomplish inside an assembly model.

''*** ilogic rule to turn off work planes, work axis, work points, sketch visibility in Assembly Models
''*** created -- 16.aug.2019 -- DJ  -- from Inventor forum 



''*** Catch and skip errors
On Error Resume Next

''*** Defines Inventor Models (assemblies and parts)
Dim oAssyDoc As Inventor.Document
oAssyDoc = ThisApplication.ActiveDocument



''*** Checka all referenced docs 
Dim oDoc As Inventor.Document
For Each oDoc In oAssyDoc.AllReferencedDocuments

    ''*** Set work plane visibility
    For Each oWorkPlane In oDoc.ComponentDefinition.WorkPlanes
	    oWorkPlane.Visible = wfBoolean
    Next
	
    ''*** Set work axis visibility
    For Each oWorkAxis In oDoc.ComponentDefinition.WorkAxes
    oWorkAxis.Visible = wfBoolean
    Next
	
    ''*** Set work point visibility
    For Each oWorkPoint In oDoc.ComponentDefinition.WorkPoints
    oWorkPoint.Visible = wfBoolean
    Next 
	
    ''*** Set sketch visibility
    For Each oSketch In oDoc.ComponentDefinition.Sketches
    oSketch.Visible = wfBoolean
    Next
	
Next




    ''*** Set work plane visibility
    For Each oWorkPlane In oAssyDoc.ComponentDefinition.WorkPlanes
	    oWorkPlane.Visible = wfBoolean
    Next
	
	    ''*** Set sketch visibility
    For Each oSketch In oAssyDoc.ComponentDefinition.Sketches
    oSketch.Visible = wfBoolean
    Next

''*** Updates the files
iLogicVb.UpdateWhenDone = True

[Kay_Rethmeier]

Hi,

unsing the Object Visibility is the beginning of the most worse behavior and after you started with it, you implemented a virus inside your models!

As Curtis wrote, switch it REALLY of, where it is created via toggling the visibility (or the use of a script...)!!! Via the Object Visibility it is only off within your current Inventor session only for now. And if you "release" a part with this setup, all work geometry (planes, axis, points) is still visible inside the assemblies. And then you have to use this f****** function again and again and again and again and again and again and again......

Do it right from the beginning ! Write down CAD-guidelines! Use methods!

Cheers, Kay