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cscouller1-Visitor
1-Visitor
November 8, 2018
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Creo 4.0 M060 - Can annotations in combination states from a model be shown on a drawing?

  • November 8, 2018
  • 5 replies
  • 5872 views

We have recently upgraded from Creo 3.0 M120 to Creo 4.0 M060.

I have been modelling a part and started to generate a drawing for this, is it possible to use combination states in the models and then use these in the drawing sheets? The simple answer is Yes you can and I have established this however if on my combination state 1 I have certain annotations visible and I want to display these on the drawing how would I do this?

If I select show annotations in the drawing on that specific view that is using the combination state it still displays all annotations for the part (This would result in duplicated effort) is there a method of showing only the annotations selected in the models combination state? Is there a config setting or have I missed something very basic?

    Best answer by dmccandless

    Annotations from combination states can be shown in drawings using Config option:

     

    option auto_show_3d_detail_items yes

     

    Yes is the default so this will also work as long as it is not explicitly set to NO

     

    Annotations will only appear from combined view aligning with the basic orientations front, right, left, top, and bottom, and each annotation will only appear once, if a dimension is already placed on the drawing it will be omitted from the drawing view for that combined view.

     

    Once the view is placed it will not add or remove annotations based on changes to the models combined view, likewise changes to the drawing view will not effect the models combined view.

     

    Annotation position can be restored through the "restore 3D dependencies" option.

    5 replies

    Mahesh_Sharma
    Mahesh_Sharma22-Sapphire I
    22-Sapphire I
    February 20, 2019

    @cscouller 

    I tested this in Creo 4.0 M080 and seems working for me. Added couple of annotation in front orientation in default or new combined state and that displayed in drawing without any duplicate efforts.  

     

    Additionally refer 

    https://www.ptc.com/en/support/article?n=CS254422

    https://www.ptc.com/en/support/article?n=CS273062

    C
    cscouller1-VisitorAuthor
    1-Visitor
    February 20, 2019

    Thank you!

    We are awaiting deployment of Creo 4.0 M080 from M060 - when we have this I will test.

     

     

    Mahesh_Sharma
    Mahesh_Sharma22-Sapphire I
    22-Sapphire I
    February 20, 2019

    @cscouller 

    Just to clarify about my test. In my test I created a part with some combined states and added and created some annotations. When creating views in drawing, it displayed the annotations from combined state. 

    D
    dmccandless10-MarbleAnswer
    10-Marble
    February 28, 2019

    Annotations from combination states can be shown in drawings using Config option:

     

    option auto_show_3d_detail_items yes

     

    Yes is the default so this will also work as long as it is not explicitly set to NO

     

    Annotations will only appear from combined view aligning with the basic orientations front, right, left, top, and bottom, and each annotation will only appear once, if a dimension is already placed on the drawing it will be omitted from the drawing view for that combined view.

     

    Once the view is placed it will not add or remove annotations based on changes to the models combined view, likewise changes to the drawing view will not effect the models combined view.

     

    Annotation position can be restored through the "restore 3D dependencies" option.

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