combined states

[nrollins]

Hi all,

Whenever I create a new drawing in Creo2, I get a message asking me if I
want to include a combined state... I don't know what I am being asked, why
and most importantly, how to stop the prompt. I always check "don't ask me
again" but that seems to only stick for that drawing.

Any clues?

Thanks.

-Nate


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[StephenW]

Funny, This just came over one the PTC Community.

Config.pro option:

Drw_prompt_for_combined_state NO

I added but haven't tested it.

[bokm9606]

combined states is a state in your model that can combine:

Explode states
View orientation
Simplified rep
and xsections
Style states? not sure on this one.

I believe this started in WF5.0.

You create these with the - in 3d space- with the VIEW MANAGER - it is the
tab labeled "ALL" (at least in WF5.0)

I actually do use this on assembly drawings a lot. I have a predefined
views, exploded state, and simplified rep that i save to "combined states"
to walk through the assembly step by step. When i create the drawing
views, i can simply selected the combined states that i have defined and
the views come in the way intended without have to do all sorts of clicking
and selecting.

Not sure how to shut off this query for good if you want to do that?
Config.pro? or the DTL file of your template drawing(s) might have
switches to turn this off


On Wed, Aug 20, 2014 at 8:08 AM, Nathan Rollins <->
wrote:

> Hi all,
>
> Whenever I create a new drawing in Creo2, I get a message asking me if I
> want to include a combined state... I don't know what I am being asked,
> why and most importantly, how to stop the prompt. I always check "don't
> ask me again" but that seems to only stick for that drawing.
>
> Any clues?
>
> Thanks.
>
> -Nate
>

[nrollins]

Thanks Pete – I also use it a lot – but for whatever reason (aging gray matter?) I never thought of using “combined states” on a drawing. And I never made the connection between that term and the “all” tab on view mgr. I was thinking “combined states” was a simp rep thing…



I guess my next question is – why is it asking me if there are n combined states defined in my model? Does it ask you for every new drawing regardless?



Apparently, (thanks to Steve) somewhere between builds m070 and m120, there is a config setting to shut this off.:

drw_prompt_for_combined_state NO



And thanks to everyone else that chimed in. The exploder is still a winner over the community forum in my opinion. Except, we don’t get points here… so we’ll never know who wins ;^)



-Nate

[dmartin]

Combined States are sort of the output of Model Based Definition / 3D Annotations. Once you have a Combined State set up, it's easy to use it as the basis for a drawing view. (Unfortunately, using it to define a drawing view does not display the 3D Annotations associated with that state in modeling mode.)

Combined States currently do not support Style States in drawing mode. And I can't remember if they support Layer States as well.

David R. Martin II

Senior CAD Application Specialist

Amazon

[llie]

Dave,

Could you please clarify your email. In Creo 2 I am able to shown the MBD
model annotations in my drawing views as long as my combination state model
orientation is one of the basic views; front, right, left, top, and bottom.
I am also able to show annotations in a projected bottom view, which is
also one of my combination states.

The issue that I found is that Combination State Model Orientation is not
saved as a Named View.

Lance Lie
Sr. Info Sys Technologist II
Global Business Services - Information Technology
Raytheon Company



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714-402-7858 (cell)
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www.raytheon.com

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[dmartin]

Hi Lance,

The configuration option auto_show_3d_detail_items is set to yes by default, and when I've created a drawing view using a combined state, the 3D Annotations are not being shown by default. I need to test this some more to figure out the nuances; perhaps the combined view is not using one of the saved views as you have pointed out. But ideally, I'd like to select a combined state for a view and also see all its 3D annotations (except of course for any shown dimensions displayed in another view).

David R. Martin II

Senior CAD Application Specialist

Amazon