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ShaneV13-Aquamarine
13-Aquamarine
August 23, 2023
Solved

Drawing Draft Edge Display

  • August 23, 2023
  • 3 replies
  • 2872 views

I'm using Creo 3 to create a drawing for an injection molded part. Some edges that have draft on them show as hidden lines when they should be solid. Arris line on the corner is displayed correctly as solid. Area where text and arrows in image below is open without any features.  Anyone ever encounter this issue?

 

Draft_Display.png

 

 

 

Best answer by ShaneV

It is a part model. Edge display was not used to modify the line style. Changing part model accuracy from .0012 to .0005 fixed the issue.

 

Thanks.

 

Draft_Display_3.png

3 replies

tbraxton
22-Sapphire II
tbraxton22-Sapphire II
22-Sapphire II
August 23, 2023

Is this screen shot from part mode or drawing mode? Can you share a shot of a 3D view of that corner of the part? What setting is tangent edge display set to for the view in question? Are these edges in question tangent edges?

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ShaneV13-AquamarineAuthor
13-Aquamarine
August 23, 2023

Image in initial post is from 2D drawing. No, they are not tangent edges. Tried all tangent display options and they have no effect on the display of errant edges. Edges only display as solid when view display is set to wireframe.

 

Thanks for your help.

 

Draft_Display_2.png

 

 

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23-Emerald III
StephenW23-Emerald III
23-Emerald III
August 23, 2023

is that an assembly? Sometimes, in an assembly, interferences between parts will cause unexpected edge display issues.

kdirth
21-Topaz I
kdirth21-Topaz I
21-Topaz I
August 23, 2023

Has Edge Display been used to modify the line style?  Try Appling Default to the lines.

There is always more to learn.
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ShaneV13-AquamarineAuthorAnswer
13-Aquamarine
August 23, 2023

It is a part model. Edge display was not used to modify the line style. Changing part model accuracy from .0012 to .0005 fixed the issue.

 

Thanks.

 

Draft_Display_3.png

    tbraxton
    22-Sapphire II
    tbraxton22-Sapphire II
    22-Sapphire II
    August 23, 2023

    That is unexpected behavior. I have never seen that, but all of my start parts use absolute accuracy.

     

    Based on your comments regarding accuracy it would seem the model is using relative accuracy. I would strongly suggest converting it to absolute accuracy and use a value an order of magnitude smaller than the tightest tolerance (i.e., if tol is .01 length units then set absolute accuracy to .001 L).

     

    Be advised that any model that is a parent or child of this model should match the accuracy setting to avoid Creo issues with shared geometry features. Relative accuracy will also likely cause problems if you use Creo/Mold Design extension.

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