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F-Ng1-Visitor
1-Visitor
August 22, 2018
Question

3D and 2D drawing update in parallel

  • August 22, 2018
  • 3 replies
  • 2253 views

Due to schedule concern I sent a preliminary 3D drawing to my colleague to generate 2D drawing in advance. Few days later I re-sent updated drawing to my colleague to update his 2D. Suppose the annotation in 2D will update automatically except new features. However all dimensions disappeared when he re-open his 2D with reference to my updated 3D (all outdated version of 3D had been deleted). But I still can read the dimension in preview window. What is the problem and what can I do if I want to update 2D and 3D in parallel?

    3 replies

    M
    MartinHanak24-Ruby III
    24-Ruby III
    August 22, 2018

    Hi,

     

    I suppose that encl_back-left.drw is 3D drawing. What is 2D drawing ?

    D
    dgschaefer21-Topaz II
    21-Topaz II
    August 22, 2018

    By default, Creo saves the dimensions created in the 2D drawing in the 3D model.  This is to allow the embedding of dimensions in other dimensions.  For example, you may want to call out the actual c'bore dept and diameter in the through hold dimension using the &adXX syntax.  To make this work, Creo stores the dimensions in the 3D file.  That's why the dims disappeared when you sent him a new 3D model.

     

    You can set the config option create_drawing_dims_only to yes to force the dimensions to be saved in the 2D drawing, but you will loose the ability to embed drawing dims.  I believe that this only affects dimensions created in the drawing (driven dims), not model dimensions (driving dims).

     

    BTW - In the Creo community the 3D file (part or assy) is commonly referred to as a model, drawing typically means the 2D *.drw file.

    StephenW
    StephenW23-Emerald III
    23-Emerald III
    August 22, 2018

    If the coworker shows the dimensions from the model instead of creating the dimensions, you will have more success in situations like these. Any dimension that was deleted and re-created in the model will not be on the updated drawing. Dimensions that used the "replace" command in sketcher will show as expected in the updated drawing. New features will obviously not have dimensions in the updated drawing.

    Using the create_drawing_dims_only option that Doug mentioned works well too. Beware that if you use Creo GD&T, all of your GD&T that is associated to those dimensions will have to be in the drawing since your created dimensions are only in the drawing. That is the primary reason I don't use that config option.

     

     

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