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How do a dimension the true (diagonal) distance between two points on a drawing?

dave_franchinodave_franchino Member Posts: 5
Hey folks,

I am truly stumped on how to get Onshape to dimension the true diagonal distance between two holes on a drawing. No matter what I've tried the dimension keeps snapping between the orthogonal horizontal and vertical. How can I get Onshape to show me the diagonal true distance between these holes?

Thanks!!!



Comments

  • StephenGStephenG Member Posts: 340 ✭✭✭
    I know 2 workarounds...

    1. Use "Maximum or minimum dimension (m)" and select the circle centers.


    2. Create sketch that contains a construction line between the 2 points of interest, then use "Show/Hide sketches" to make the sketch visible in the view. Then you can use the normal "Dimension (D)" function, select the line to create a diagonal dimension along its length.

       

  • glen_dewsburyglen_dewsbury Member Posts: 29 ✭✭
    2 point linear dimension will behave as you were expecting or pick the holes with basic dim tool not the center point.
    Odd behaver to give only vert & horizontal when using basic dimension tool between points.
  • Hans_Leirvik_1Hans_Leirvik_1 Member Posts: 17 PRO
    edited June 4
    Create a plane that goes through the two points.
    Select the plane and press keyboard N to view it from top.
    Then create a Named View.
    In a drawing create a View showing the part/assembly and select the Named view.
    Now you can dimension the two diagonal holes in the drawing.
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