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Combined states - in drawings - question for Creo 3.0 users

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Amethyst

Combined states - in drawings - question for Creo 3.0 users

Does anyone use this "functionality", or do you find it of limited use, and have the config.pro option drw_prompt_for_combined_state set to NO ?

One thing that would be nice is if the layer information from the 3D model would be used to set up the layer state of the drawing view.  Reading the online help for Creo 3.0 it would seem to be the case.

However, I'm on Creo 2.0, and today I defined a combined state of an assembly (in it, a layer state is used in which a bunch of components are on a hidden layer).

I then started a new drawing.  On the first sheet, I used the "No Combined State" to put a drawing view of the assembly with all its components.

On the second sheet, I put a drawing view and when prompted, selected the combined state that I just created in the assembly.

I thought all was hunky-dory - it looked just like what I wanted - a view of the assembly with some of the components not shown.

But to my dismay, I saw that the components also disappeared from the drawing view on the first sheet of my drawing.

Does this work in the same manner in Creo 3.0?

1 ACCEPTED SOLUTION

Accepted Solutions

Re: Combined states - in drawings - question for Creo 3.0 users

I think the problem, at least for your example, lies with the way you are controlling the visibility with the hidden items layer. When you hide the part it gets placed on the hidden items layer but when you un-hide the part it gets removed from the layer, it's in a constant state of change. Place the items you want to hidden on a new layer and try hiding that layer. The other thing that may be happening is when you apply a combined state it is changing the layer status so make sure to save the layer status before saving the drawing.

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5 REPLIES 5

Re: Combined states - in drawings - question for Creo 3.0 users

Hi Paul,

Can you please share a screen capture from the view manager 'ALL' tab? This will show us what combined views you have created and give us a clue how you are working. What are the names of the combined states that you want to use?

look forward to your update

Re: Combined states - in drawings - question for Creo 3.0 users

Since parts are disappearing in views they shouldn't check the Drawing Layer Status, the first option should be checked. For the config option all it seems to do is control whether or not a combined state is asked for when creating a view.

Re: Combined states - in drawings - question for Creo 3.0 users

Ok, I took some screenshots to explain what is happening to me.

1) Essentially, I'm using different layer states as a way to control the visibility of features and components in an assembly:

combined_states_of_the_assembly.png

2) I create a drawing of this assembly; and as I put in the views, I'm prompted for which combined state to use.  So I pick the ones I want:

new_drawing_view1_everything_shown.png

(here, I also show the Layer Status Control setting for the drawing)

So I complete placing all 3 views, and everything looks as though it's working as expected, so I save this drawing:

new_drawing_3views_layerstatus_saved.png

(also note I didn't fail to save the layer status in the drawing)

3) But then, when I close the session and open the drawing, this (unexpected?) result:

new_drawing_after_being_opened.png

This definitely has something to do with hidden components not staying "hidden".  In general, I think this combined states thing in Creo is at worst rather ridden with bugs, or at best poorly described in the help documentation and I just don't have the magic decoder ring.  But for me things are just not working consistently in neither assemblies nor drawings and each new session is a mystery.  I'm talking about the items that are supposed to show up for a given combined state (e.g. "everything_shown") are staying hidden and it takes some kind of a combination of clicking on the combined state tabs in the model to get them to "reappear".

For time being, using layer states seems to work if you wish to hide features, but if you need to hide components, then make a simplified rep in which they're excluded.

I attach the example files for you to examine.

Re: Combined states - in drawings - question for Creo 3.0 users

I think the problem, at least for your example, lies with the way you are controlling the visibility with the hidden items layer. When you hide the part it gets placed on the hidden items layer but when you un-hide the part it gets removed from the layer, it's in a constant state of change. Place the items you want to hidden on a new layer and try hiding that layer. The other thing that may be happening is when you apply a combined state it is changing the layer status so make sure to save the layer status before saving the drawing.

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Re: Combined states - in drawings - question for Creo 3.0 users

Hi Kevin, I think you are right.  Using a dedicated assembly layer makes the whole thing work as expected.

I'll stay away from that "Hidden Items" layer from now on.

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