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A
AS_109321245-Regular Member
5-Regular Member
May 13, 2024
Solved

PROBLEM EXPORTING DWG FROM CREO 9.0.5 DRAWINGS - SHADED VIEWS

  • May 13, 2024
  • 4 replies
  • 2454 views

Hi everyone,

I was generating the DWG file from a drawing. Some views have the state "Shading With Edges" in the "View Display" properties. This is due to production porpuses and I cannot modifiy their representation.

During the saving operation, Creo displays a warning in the console, I attach the image below.

AS_10932124_0-1715603959087.png

The resulting DWG file is incomplete, the biggest shaded views are missing on the drawing.

I tried changing some export settings, but nothing helped. Even exporting in DXF format resulted in an incomplete drawing, while PDF is ok.

Does anyone know how to solve this problem?

Thanks in advance.

Best answer by MartinHanak

Hi,

create simple test drawing and export it. When you save dwg file, separate png file containing shaded picture should be created.

With your original drawing you can test setting of config.pro option DRAWING_SHADED_VIEW_DPI.

https://creosite.com/index.php/configuration/display-option/?srch=DRAWING_SHADED_VIEW_DPI&ver=creo11&mode=config

 

4 replies

M
MartinHanak24-Ruby III
24-Ruby III
May 13, 2024

Hi,

please ask PTC Support. They must know limits implemented in Creo.

StephenW
StephenW23-Emerald III
23-Emerald III
May 13, 2024

There was a very similar post from 2014 with the same issue with no solution.

https://community.ptc.com/t5/3D-Part-Assembly-Design/Exporting-a-DXF-with-Shaded-Views/m-p/320551

 

Since it says "too large", I would test with an extremely simple test model/drawing just to see if it's capable at all.

Otherwise Martin's suggestion of opening a support ticket is your best option.

KenFarley
KenFarley21-Topaz II
21-Topaz II
May 13, 2024

You might not be allowed to change the view appearances permanently, but why can't you temporarily change to something else, like hidden line removed, export the drawing, then *don't* save it in that state. Presumably you can change the appearance of things in memory as long as you don't overwrite the saved file, yes?

M
MartinHanak24-Ruby IIIAnswer
24-Ruby III
May 13, 2024

Hi,

create simple test drawing and export it. When you save dwg file, separate png file containing shaded picture should be created.

With your original drawing you can test setting of config.pro option DRAWING_SHADED_VIEW_DPI.

https://creosite.com/index.php/configuration/display-option/?srch=DRAWING_SHADED_VIEW_DPI&ver=creo11&mode=config

 

StephenW
StephenW23-Emerald III
23-Emerald III
May 13, 2024

I set  the value to 100 and I was able to export a dwg file and upon opening in autocad, the shaded view was visable.

I didn't test any other values. I didn't test prior to setting the option either.

 

StephenW_0-1715615962040.png

 

A
AS_109321245-Regular MemberAuthor
5-Regular Member
May 14, 2024

Hi everyone,

I tried different values for the parameters DRAWING_SHADED_VIEW_DPI, and it resulted in allowing the DWG file to be created correctly.

I had to use really low DPI resolution (25) but even in this conditions the images where good, being the drawing in format A0.

Thanks to all who participated to this topic.

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