How to hide a Part in a drawing from Browser_2010

[SolidCreative]

Before 2010 I could simply right click the part or assembly in the browser and uncheck visible? The visible command is still there but grayed out.

How can I hide a part I dont want to show in the drawing?
I dont like levels of detail, and I would like the part to remain visable in the assembly.


Thanks
Matthew

 

[rollupswx]

You can create Design Views in assembly to be used in idw.

 

[EngAddict]

If you want to manually override it you must make sure the view is not associative to the model. Double click the view and then uncheck the associative box.

Generally this isn't good practice, your view should be associative. Hence you should do as rollupswx suggested and set up VewReps.

However there will always be some occasions where it is required.

 

[SolidCreative]

I'll try it out, Thanks!
But I still belive its more complicated then way it was in 2008.

 

[mcgyvr]

If you like how it was in 2008 simply uncheck the associative check box in the edit view dialog. That "unchecked" state is maintained even when restarting Inventor.. Then you have 2008 functionality until you check that box again.

However like said above it is a better workflow to simply create design view reps in the model to control the visibility of an idw view.

 

[SolidCreative]

What exactly does associative check box do? I tried unchecking it and made a change to the model. The drawing still updated automaticly when opened. I use Inventor.dwg not idw; does that impact this situation?

Thanks
Matthew

 

[mcgyvr]

If checked a parts visibiliy can only be controlled in the assembly (via a design view rep). Basically you cannot toggle visibility in the idw (the visible option is grayed out in the drawing browser).

If unchecked a parts visibility can be toggled in the IDW or in the assembly. (the visible option can be toggled on/off) Changing the visibility in the drawing will not change the visibility in the model.

It is a better workflow to have it checked but there are situations when it is easier to have it unchecked.

For example suppose you have an assembly that you want to have a cover shown in the front view but not shown in the top view. In this case I would uncheck the associated box.