pdf export pen pattern Creo 8.0.5.0

[SP_saro]

The drawing must be exported as a PDF. We have phanthom and hidden lines in the drawing.

If I set the Pen 3 pattern . it will only accept one Line style.

(pen 3 thickness 0.010 cm; pattern 0.1 0.05 0.025 0.05 cm)

How could different line styles be used? Hidden line and Phanthom line both use Pen 3.

Please assist me in solving this problem.

[MartinHanak]

Hi,

what happens when you remove pattern 0.1 0.05 0.025 0.05 cm from pen definition.

[SP_saro]

PDF Output

Drawing

If I can use the pen 3 thickness 0.010 cm; pattern 0.1 0.05 0.025 0.05 cm

Its shows hidden line also in phanthom line style.

[MartinHanak]

Hi,

once again ... remove pattern 0.1 0.05 0.025 0.05 cm from pen definition.

[SP_saro]

if the pattern line is removed, hidden line and the Phanthom line looks good.. but I need a different pattern for the hidden line and the phantom.

[MartinHanak · Accepted solution]

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@SP_saro wrote:

if the pattern line is removed, hidden line and the Phanthom line looks good.. but I need a different pattern for the hidden line and the phantom.

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Hi,

so it looks like you do not like default patterns assigned by Creo to hidden and phantom lines.

One possible solution = changing phantom component display. Please play attached video and use uploaded data.

[SP_saro]

Wow, Nice Idea, I can use this option .

If we can change the Pen 1 pattern its not effect geomentry line and etc (below mentioned as Pen 1 line styles?

• Visible geometry
• Cross-section cutting plane lines: plot as phantom lines
• Cross-section cutting plane arrows and text
• Drawing format and boundary
• Tag text
• Centerline line font with white color
• Brown portion of datum planes

Thanks a lot for your workout

[MartinHanak]

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@SP_saro wrote:

Wow, Nice Idea, I can use this option .

If we can change the Pen 1 pattern its not effect geomentry line and etc (below mentioned as Pen 1 line styles?

• Visible geometry
• Cross-section cutting plane lines: plot as phantom lines
• Cross-section cutting plane arrows and text
• Drawing format and boundary
• Tag text
• Centerline line font with white color
• Brown portion of datum planes

Thanks a lot for your workout

---

Hi,

look into pentable_02.pnt

pen 1 thickness 0.010 cm; color 0.5 0.5 0.5; pattern 0.1 0.05 0.025 0.05 cm
pen 3 thickness 0.010 cm; pattern 0.1 0.05 cm
pen 10 thickness 0.050 cm; drawing_color

pen 10 thickness 0.050 cm; drawing_color

... drawing_color keyword causes that Creo will draw visible geometry by pen 10 instead of default pen 1

You can use other keywords to resolve your needs.

Notes:

1.] All user colors are drawn by pen 1.

2.] All system colors have assigned their keyword which enables you to assign them specific pen.

https://support.ptc.com/help/creo/creo_pma/r10.0/usascii/index.html#page/data_exchange/interface/Default_Pro_ENGINEER_System_Colors.html

[SP_saro]

Thank you very much for the clear explaination and your time .

[SP_saro]

Hello Martin

Your choice to manually adjust the view color in Phantom_hidden_PDF.mp4 results in output PDF phanthom and Hidden line utilising the Pen table.

Can we choose a different colour for the phantom line and hidden line details in system color ?

Note: In system colour, I only saw only Hidden line color only

[MartinHanak]

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@SP_saro wrote:

Hello Martin

Your choice to manually adjust the view color in Phantom_hidden_PDF.mp4 results in output PDF phanthom and Hidden line utilising the Pen table.

Can we choose a different colour for the phantom line and hidden line details in system color ?

Note: In system colour, I only saw only Hidden line color only

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Hi,

I guess you are asking how to change colors in Creo window.

Hidden Line color:

Custom color assigned to phantom components in Drawing mode:

See phantom_hidden_PDF.mp4 video again.

You can select any User-defined color -OR- create new one. AFAIK you cannot set user-defined color as default one for phantom components.