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JonathanHodgson13-Aquamarine
13-Aquamarine
November 12, 2018
Solved

Drawing scale, dimensions, and sketched entities

  • November 12, 2018
  • 3 replies
  • 6243 views

For reasons of expediency I'm showing some features on a drawing by importing a DXF and apply created dimensions.

My drawing sheet is at 1:2 and the DXF is scaled correctly to suit that on the sheet.  However, when I create dimensions they show the actual size on the drawing, i.e. half the value they should be.

How do I make created dimensions of what are effectively sketched entities respect the drawing scale?  Creo 3.

Thanks!

Best answer by StephenW

For this reason, I pretty much never sketch in the drawing. I usually import my DXF in to a .prt file and then add that part file to a drawing. Its the same "speed" with but I absolutely hate the drawing sketch functionality, it's just way to flaky.

3 replies

KenFarley
KenFarley21-Topaz II
21-Topaz II
November 12, 2018

I'm going to take a guess, based upon behavior when I'm using sketched geometry to get dimensions. You might need to, if it lets you, select all the geometry that was imported, and "Relate to View". This works for sketched entities, maybe it's useful for your situation.

J
JonathanHodgson13-AquamarineAuthor
13-Aquamarine
November 12, 2018

Thanks Ken.

 

At present I don't have a view; the geometry is effectively sketched in an empty drawing frame.  I'm surprised it doesn't use the drawing scale though.

S
23-Emerald III
StephenW23-Emerald III
23-Emerald III
November 12, 2018

There is no drawing scale until a model is added to the drawing. 

scale.jpg

S
23-Emerald III
StephenW23-Emerald IIIAnswer
23-Emerald III
November 12, 2018

For this reason, I pretty much never sketch in the drawing. I usually import my DXF in to a .prt file and then add that part file to a drawing. Its the same "speed" with but I absolutely hate the drawing sketch functionality, it's just way to flaky.

    J
    JonathanHodgson13-AquamarineAuthor
    13-Aquamarine
    November 12, 2018

    You're right... I should have done it that way.

    R
    rreifsnyder15-Moonstone
    15-Moonstone
    November 12, 2018

    Take a look in the File > Prepare > Drawing Properties and then change the detail options. In the section of the options controlling dimensions is one called draft_scale. Try changing that option.

      J
      JonathanHodgson13-AquamarineAuthor
      13-Aquamarine
      November 19, 2018

      Thanks... if I hadn't already re-created by pulling the DXF into the part as above, that could have worked.  Looks like it's just an independent value though; it doesn't appear to have the ability to link it to the actual drawing scale.

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