How to export a suitable imaginary line in Cero 2.0 engineering drawing?
The ratio of the imaginary line in my .drw file is ok(left picture), but the RATIO of the imaginary line changed when I save the .drw file to .pdf file, the ratio is too large as we can see from right picture .
So someone can give me a kind suggest of how to adjust my configuration file to export a suitable ratio?
This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.
Thanks for your support.
I am sorry that I CAN NOT find line_style_length in drawing options, without this option in cero2.0.
What I should do next? Thanks.
Thanks for your patient support!
The matter in my side has solved by using your advises.
I set following two options in my .dtl file, then the line style arrived my expected when I save as .pdf file.
TWO options:
line_style_length CTRLFONT_S_L 10
line_style_length CTRLFONT_L_L 10
This could becaused by a number of things, depending on if you are using a pen table, user-defined line fonts, etc. Creo automatically scales the line fonts based on the size paper you are plottting on, and if you want the "scale" of the line font to be smaller you probably need to create a new line font. In the drawing Format section of the ribbon, select Line style->edit fonts->new->Copy from->CTRLFONT. Edit the default value of unit length as desired. Now go set your centerline to the new style under line style->modify lines. This is the only solution that worked for me. Setting the line_style_length CTRLFONT drawing option only works for sketched entities, it does not affect a datum axis created in the model. Creo does not scale user-defined line fonts by default, so you may need to set the use_software_linefonts config option.
use_software_linefonts
- no*—Plots lines using the line font that most closely resembles the font used in Creo Parametric. (default)
- yes—Plots the exact line style used in Creo Parametric, dot by dot, dash by dash, and space by space.
Also, if this works and you need to use the new line font in multiple drawings, you can set the aux_line_font drawing option.
see http://www.proesite.com/cgi-bin/find_option.cgi?srch=aux_line_font&ver=wildfire2&mode=drwsetup
Here is a sketched line and a datum axis both with line style set to CTRLFONT, and line_style_length CTRLFONT set to .1
http://www.proesite.com/cgi-bin/find_option.cgi?srch=aux_line_font&ver=wildfire2&mode=drwsetup
