How to set the colour for tangent edges in drawing?

[Ben8]

I can't find how to set the colour of tangent edges in the drawing. 

Say I have a a simple extrude with fillets (rounds) on the corners:

The tangent edges (from the Round feature) appear to be green in the drawing:

The tangent edges are dimmed. If i set them to be Solid instead of dimmed, then the tangent edges become black:

When I print the drawing (save as PDF) it gomes through with black lines (not green). But I think i have some config.pro setting to ignore pen tables, but i can't remember exactly what exactly it can be. Anyway, it seems to be only a visual thing at the moment, but it is still doesn't look right.

I looked through Creo settings, drawing settings, pen table and I seem to be unable to find anything that changes this colour. Can somebody guide me into the right direction?

[kdirth]

What version of Creo are you using?

For a PDF, in the options you can choose from Color/Grayscale/Monochrome.

[Ben8]

I am using Creo 9. 

It seems that even with "Color" export to PDF is chosen, the exported file has black tangeng edges (not green).

Im looking for a way how to change the display colour on Creo drawing while it is still in CAD, not after it is exported to PDF.

Let me know if I can provide further information.

[MartinHanak · Accepted solution]

Hi,

in Creo 9.0.2.0

1.] I created new part, set dimmed tangent edges and change their color to green

2.] I created new drawing, set colors from model, set dimmed tangent edges

3.] my config.pro contains following options

use_8_plotter_pens yes
pen_table_file E:\users\creo7_parametric\pentable.pnt
pdf_use_pentable YES

4.] E:\users\creo7_parametric\pentable.pnt contains following pen definition

pen 9 thickness 0.035 cm; dimmed_color

5.] PDF file contains green tangent edges

6.] I uploaded test files.

[Ben8]

Hi Martin,

thank you! It is a secondary highlight setting.

How on earth did it make sense to PTC to call tangent edges a "Secondary highlight" I will never know ...

But thanks for your help, I've set it to black and now they are consistent with the rest of the model view in the drawings.

I've marked your answer as a solution.