What is the meaning of the “Keep legacy body status” command?

Some of you might have noticed a new context menu in the drawing environment of Inventor 2013.

When you open a pre-2013 Inventor drawing in release 2013, you will see following "Keep Legacy Body Status" menu when using the right mouse button on any drawing view.

Once you turn off this option on a view, you will never see the menu on that particular view again.

Turning off this option has to happen on a view-per-view basis. You cannot turn it off for all views in a single operation.
Why would you uncheck the command and what is this mysterious command exactly doing?

Fig 1: Keep Legacy Body Status command

The command is new for 2013 and it controls how legacy drawing views react to design views.

We introduced design views in parts in 2012. But in 2012, design views did not have the capability to change the visibility or the color of bodies in a part.

In 2012 when you created drawing views of multi-body parts, you could only influence the visibility of the bodies in the drawing by using the "Visibility" context menu.

 

 Fig 2: Controlling body visibility in Inventor 2012 drawing

Since 2013, the visibility and color of bodies is stored in design views and by consequence in a drawing view you can now also manage body visibility by applying a design view representation.

So when you see the "Keep legacy body status" context menu checked, you are using the 2012 way of controlling visibility of bodies.

Once you uncheck the "Keep legacy body status" checkmark, you will be using the 2013 way of controlling visibility.

And there is no way in going back. Once you uncheck the checkmark, that context menu will disappear on that particular view forever.

   

Let me illustrate this with a small example.

When you create a drawing view of a part with 2 visible solid bodies in 2012, you will see something similar to this.

 

Fig 3: 2012 drawing view of part with two bodies

Now save the drawing in 2012 and open the drawing in 2013.

You will see the "Keep legacy body status" context menu checked on the view.

 

 Fig4: New context menu in 2013

Open the part and add a design view representation that turns off the visibility of one of the bodies.

Call this view representation View1.

Fig5: Visibility of Solid2 turned off

Return to the drawing and try to apply the view representation View1 to your drawing view.

Fig6: Applying a view representation to the drawing view

You will see that applying the view representation has no effect and body Solid2 continues to be visible in the drawing because the 2012 method is still in effect (and we had not turned off explicitly the visibility of that body in 2012).

Now turn off the "Keep legacy body status" on the view. You will get below warning message which is OK because that is exactly what we want to do.

Fig 7: Switching from the old way to the new way of controlling bodies

The message indicates that the body visibility in the view is now allowed to change when the view gets associated with a Design View Representation.

Here is the result: the visibility of the second body is controlled by the view representation.

Fig 8: Visibility of one of the bodies turned off via the representation associated to the view

This command remains undocumented in the Inventor Help wiki, so consider yourself lucky that you have read my little article J

 Bob

Comments

[sky]

is it possible to turn it off for all views in a single operation via VBA?

thanks

[Bob]

Unfortunately there is no automatic way of turning this option off in all views because we don't have an API call to do this in 2013.
Bob