Is it possible to have different layer state for a part/assembly and its associated drawing.
For instance, I have a manufacturing file with many milling windows. I have created a layer driven by a rule to isolate these. I would like to hide milling windows in my manufacturing document for the workshop, and keep these milling windows displayed in the manufacturing assembly.
Solved! Go to Solution.
In fact, I'm still having a problem.
In my model I made a layer with a rule to select all milling windows
In the drawing I configured as Stephen shown. In the drawing I hide the layer then save the layer status. I go back to the manufacturing file, the windows are still shown, that's cool. But if I go back to the drawing the milling windows are shown again even if the icon in the layer status shows it's hidden !! (Milling windows are shown in purple on the drawing). What am I doing wrong ?
I can only think of one reason, you have that view controlled independently from the drawing layers.
You can see this if you select the arrow icon in the layer tree. Notice on the image below, all the view boundaries are shown in blue (this may be a different color on your setup, I have custom colors assigned). If any of your view are green (or different colors) you have independently controlled the layers for this view.
If you don't want the view to be controlled by the overall drawing layers (recommended), select that view boundary. Then in the layer menu, select DRAWING DEPENDENT.
Thanks Stephen for this answer.
I did what you explain. It's ok until I switch to the manufacturing file, back to the drawing the milling windows are shown again !!
I have to find what I am doing wrong. I f I can't find it by myself I'll open a support case.
In my reply above, I mis-typed. The last sentence should have read:
If you want the view to be controlled by the overall drawing layers (recommended), select that view boundary. Then in the layer menu, select DRAWING DEPENDENT.
Instead of "If you don't want"
Thanks for you detailed answer. In fact it works fine with standard parts and drawings, but with manufacturing files it sometimes works sometimes not !! I'm currently working on an old manufacturing file. I'll have a look on a new one.
Unfortunately, I don't know anything about the manufacturing side of Creo. I assumed it follows the same rules but possibly not.
There might be a bug or something. I tried on an all new manufacturing file and unfortunately I notice the same behavior. I open a support case.
Just giving some fresh news about this. I opened a case and the conclusion is that when you use a shaded view in a drawing, it always follows the layer state of the model. To use a different layer state, the view must be defined to something different than shaded view ! So it works to product specification, and I now have to create an idea.
This is really interesting. It starts doing some odd things when I play with the layers in the model and drawing once I add the shaded view to the drawing. They are definitely not independently control (drawing/model) once a shaded view is added.
Yep, from my point of view this looks like an unexpected behaviour, but PTC pretends this works to product specification. I really would like to talk to the person who specified that.
Imagine the thing : "Just for the shaded views I decide the layer state will always follows the model layer state" !!
What a strange idea !
It's the standard explanation when they don't have an explanation. If you really wanted to pursue it, you can demand to see the specification where that is stated. It is likely not worth the effort on your part to take the time and likely the *best* result you could probably expect is either an admission that they didn't have a specification or that they solved some sort issue by making it behave this way.
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