Yellow Text 3

[WDG57]

When I export drawings into the ".dwg" format, and open these drawings with AutoCAD, the text and dimensions are yellow. This causes problems with my vendors. If they print the drawings, the yellow text is too light to read. If they try to change the color, the dimensions change (style and locations). How can I export drawings so that the text and dimensions are black, or some other color? Thanks, WDG

 

[Recneps]

There is a method I have seen in PTC's technical support knowledge base that goes through the steps to export a drawing into a format that can be placed into MS Word.

OR

My personal preference is to create a 300dpi full scale PDF of my drawings (probably because I developed my own method for doing so). I submitted the process and files required to a company called truEinnovations, and they posted it to their knowledge base. You can find the process and required files here:

http://www.trueinnovations.com/support/kbase/selection.asp?id=100061

It creates a 'one-click' solution for creating the PDF files - pretty convenient...small file size, accurate resolution, accessible by anyone (free Acrobat Reader download), and prints out a sheet whose quality rivals a ProE plot.

Recneps

 

[WDG57]

Fantastic! One word of caution to other who might need this; the “.bat” file doesn’t like long folder names. After I moved the folder where the “.pdf” files are stored into the root directory, it worked great. Thanks!

 

[Recneps]

No problem. I had heard that PTC tech support is intrigued by the method and we could possibly see similar functionality in a future release of ProE.

So warm up that keyboard and submit enhancement requests like there is no tomorrow!

Recneps

 

[darlington]

I have had this problem all the time!

I fixed the problem by changing the colours in Autocad.

there is no need to explode, that creates big problems

Using the 'change'
select 'all'
select 'change properties'
select 'change colours'
change the colour to 'w' for white

this will print black lines on a white background

 

[WDG57]

I’m not exactly sure why, but if we change the color in AutoCAD, the dimensions move and change size. This requires too much time to clean up the drawing.

 

[Recneps]

OR...

Before exporting the ProE drawing, use Utilities>Colors>System to bring up the system colors dialog. Click on Scheme at top of window and select Black on White - this loads a color scheme that will export black entities on a white background. Select Scheme>Default to get your colors back afterward.

Recneps

 

[WDG57]

It doesn’t matter what color they are on my screen, Pro/E exports yellow dimensions.

Here is a trick that I discovered in AutoCAD: Using TOOLS>WIZARDS>ADD COLOR-DEPENDENT STYLE TABLE, Select “Start from scratch”, give it a name (“noyellow”), Select both options, then select “Plot Style Table Editor”. In “Plot Styles” box, select the color yellow, in the “Properties” “Color” box, change the “use object color” to “Black”. “Save and Close” and “Finish”. Although the screen still shows yellow dimension, it converts them to black when it prints.

 

[ohio30]

If you are interested in changing the colors of Pro/E lines in a drawing when exporting to .DWG you can build a file named dxf_export.pro.
The file "dxf_export.pro" must be placed in the current working directory when the export to .DWG is performed. More details about line color when exporting to DWG can be found at ptc.com.
1. Create a text file named dxf_export.pro
2. type 'map_color' (space) pro/e color name (space) AutoCad color number.

Example dxf_export.pro file:

map_color BACKGROUND_COLOR 0
map_color DIMMED_COLOR 4
map_color LETTER_COLOR 1
map_color HIGHLIGHT_COLOR 1
map_color EDGE_HIGHLIGHT_COLOR 5
map_color GEOMETRY_COLOR 2
map_color HIDDEN_COLOR 3
map_color SHEETMETAL_COLOR 3
map_color CURVE_COLOR 2
map_color VOLUME_COLOR 2
map_color SECTION_COLOR 4

(For a list of Pro/E color names - modify the linestyle of a sketched entity on a drawing)

FYI: Pro/E entities may not correlate with AutoCad entities with regards to color. Pro/E object lines are one color where (my company) we use several colors in AutoCad.

 

[ohio30]

Check out the dxf_export file supplied with Pro/E.
Pro/E 2001: copy and edit the file '%proe_loadpoint%\text\intf_configs\dxf_export.pro' (replace %pro_loadpoint% with the folder path where you installed Pro/E.)

This file includes everything needed to format a DXF or DWG exported file from Pro/E. I am sure you will find a similar path in previous releases of Pro/E.

Have fun!

 

[Caper1]

Where within Pro/E do you set the print color?
I have yellow display text but it will print black.
Where does this feature live. Display one color print another.

-Caper-

 

[WDG57]

Ohio30, thanks for your replies.

Good morning Casper! I think you'd better have another cup of coffeee and read the thread again.

Don
BCF Technology
Mohawk Industries

 

[WDG57]

It worked! I had given up, but ohio30 found the solution! I was having trouble getting the OEM file correct, so I copied your example and had it in no time. I thank you, my boss thanks you, and my vendors thank you very much! Problem solved.

Don
BCF Technology
Mohawk Industries