Part View Rep Behavior

[DewayneH]

We recently made the jump from 2010 to 2014 and I am seeing unexpceted behavior with part representations.

These were not available in 2010, so I may be misunderstanding the concept of view reps in parts.

My expectations were that they would function just like an assembly view rep.

In an assembly I am able to achieve the desired visibility state and lock the view.

No matter what visibility changes occur in the assembly, the locked view can be activated and it is always, as it was, when it was locked.

The behavior I am seeing with parts is, after locking the view, it doesn't stay locked.

If new work features or sketches are added, after the view is locked, they will be visible when the locked view is activated.

Please verify if this is the normal behavior.

[wimann]

First off, Sp-2 is out if you haven't downloaded it yet. But I doubt that has anything to do with what you're observing.

2014 is the first version to include view reps for part files. As I understand them, they're not there to determine the visibility of features. View reps will handle colors as well as the visibility of solids if you have a multi-body part. If you want to not show certain features based on a part view rep, I'd recommend making those features into seperate solids which would allow you do to so.

My knowledge of part view reps is limited due to a lack of utilization. I think they could be useful, I just don't have a use for them at the moment. So there may be more to them than I have indicated, but that is my understanding so far.

Hope this helps.

[DewayneH]

I do have SP2 installed, so that is definitly not the problem.

I realize feature visibility is not controlled. That is not really a visibility thing.

What I'm referring to is only work features, planes, axis, and points. I would think these, and sketches, could be controlled by the view rep in the same manner as the assembly view rep. Once the view is locked nothing new will be saved to the view rep unless you explictily unlock it.

What make it more confusing is that initially it works, but as you add new work features or sketches to the part they are included in the locked view.

I would expect to lock a view and not be concerned about other things displaying if additions are made.

I was really hoping this was not how it was designed to function.

[wimann]

Good deal. The only reason I mention SP2 is because your signature says SP1.

Oh yeah I could see work features being controlled that way for sure. This may just be a portion of the software that's newly added and not fully developed. Maybe in Inventor 2015 you can control work feature visibility with part file view representations.

I've pretty much given you all I have to offer on the topic. Looks like you may end up having to stick to assembly view reps to control those features for the time being. That and, as I'm sure you're aware but I feel obligated to mention, ctrl+. ctrl+/ ctrl+] alt+. alt+/ alt+]

In the off chance that you're unaware of those commands, they control the visibility of work features.

Oh yeah, and F10 for 2D sketches. 🙂

[bob_holland]

DewayneH,

Locking the view prevents any future changes to camera angle or color from affecting this view.

This does not control the visibility of work geometry work planes and sketches.

[DewayneH]

To make sure I understand:

Locked View representations in parts will preserve the view state of work features and sketches, as long as you don’t add anything else. If new work features or sketches are added, the view has to be unlocked, visibility adjusted, and relocked if you want the features and sketches visibility off.

Being they are called view reps and they have a lock, I just expected them to function the same as assembly view reps.

I was hoping this feature would be helpful, but due to the inconsistency in function, so far, it has not.

For now we probably still need to make sure the visibility is turn off for work features and sketches in the master view of the part. This will at least give us the same results as we are accustomed.

If we need to save color states or camera angles, we will have to check the visibility of any features that may have been added and fix if needed.

[johnsonshiue]

Hi! Though generally Part Design View works similiarly to Assembly Design View. there are differences. First, Master ADV is locked and it means all color overrides or visibility setting or camera angle cannot be saved in Master ADV. Master PDV can be saved Second, feature color or face color in a part cannot be saved in PDV. Only body color and part color can be saved in PDV. On assembly level, there is no concept of feature color, face color, or body color. Only component (part and subaasembly as a whole) color can be overridden.

There is another complication in Part environment affecting PDV. Part is history based. A sketch or a workplane visibility can be changed in rolled back since they may not exist when the parent feature is edited. I have seen cases of confusing behavior. I personally think PDV is best used after major modeling operation is done to configure the appearance of almost finished model.

Thanks!

[DewayneH]

Totally agree that in the part the design view should be applied to the finished model.

For what it is worth...I also noticed this behavior is now present in assemblies with sketches.

We have sub-assemlbies that must be cut at the assembly level. When a sketch is added to the sub-assembly to layout the cut, the view rep must be reset, just like in the part environment.