Eagle freezes if run from ulp to generate gerber files

Not sure why, but Eagle is waiting for input from the stdin.  Even if

stdin is not a tty, it sits there and waits.

I managed to fix this by echoing an "n" to stdin.  It's been working

consistently ever since.  Even if it never eats the character, there's

one ready to be read.  Here's a few lines I use to generate a complete

set of gerber files:

echo n | eagle -X -N- -f+ -O+ -c- -x0 -y0 -dGERBER_RS274X -o

516800-RevA-TopCopper.gbr 516800.brd 1 17 18 || exit 1

echo n | eagle -X -N- -f+ -O+ -c- -x0 -y0 -dGERBER_RS274X -o

516800-RevA-BotCopper.gbr 516800.brd 16 17 18 || exit 1

echo n | eagle -X -N- -f+ -O+ -c- -x0 -y0 -dGERBER_RS274X -o

516800-RevA-NonPTHoles.gbr 516800.brd 20 || exit 1

echo n | eagle -X -N- -f+ -O+ -c- -x0 -y0 -dGERBER_RS274X -o

516800-RevA-TopSilkScreen.gbr 516800.brd 21 25 || exit 1

echo n | eagle -X -N- -f+ -O+ -c- -x0 -y0 -dGERBER_RS274X -o

516800-RevA-BotSilkScreen.gbr 516800.brd 22 26 || exit 1

echo n | eagle -X -N- -f+ -O+ -c- -x0 -y0 -dGERBER_RS274X -o

516800-RevA-TopMask.gbr 516800.brd 29 || exit 1

echo n | eagle -X -N- -f+ -O+ -c- -x0 -y0 -dGERBER_RS274X -o

516800-RevA-BotMask.gbr 516800.brd 30 || exit 1

echo n | eagle -X -N- -f+ -O+ -c- -x0 -y0 -dGERBER_RS274X -o

516800-RevA-TopPaste.gbr 516800.brd 31 || exit 1

echo n | eagle -X -N- -f+ -O+ -c- -x0 -y0 -dGERBER_RS274X -o

516800-RevA-BotPaste.gbr 516800.brd 32 || exit 1

echo n | eagle -X -f+ -N- -O+ -c- -x0 -y0 -E+0.1 -R 516800-RevA.drl

-dEXCELLON -o 516800-RevA-ExcellonDrill.exc 516800.brd 44 45 || exit 1

HTH,

    - Chuck

On 02/17/2014 06:02 AM, Magnus H-C wrote:

I have a ULP to automate generation of gerberfiles.

In the ULP I use the following command:

 

system("\"" + EagleExe + "\" -X -x0.0 -y0.0 -O+ -c- -dGERBER_RS274X

-o\"" + GerberFileName + "\" \"" + B.name + "\" tPlace tNames");

 

This usually works fine but in some cases it just freezes and nothing

happens.

If I run the CAM processor manually i get the following warning:

 

The ULP probably freezes because of this warning, but the warning is not

shown.

Eagle is probably waiting for me to answer the non visible dialog.

Is there some "silent mode" without warnings or some other way to sole

this problem?

 

--

To view any images and attachments in this post, visit:

http://www.element14.com/community/message/104018

Thank you!

This works great, but since I use a ULP and (I think) you use a bat-file i had to add "CMD.EXE /c echo y | " in the system call.

system("CMD.EXE /c echo y | \"" + EagleExe + "\" -X -x0.0 -y0.0 -O+ -c- -dGERBER_RS274X -o\"" + GerberFileName + "\" \"" + B.name + "\" Top Pads Vias");

Simple explanation of variables used:

"EagleExe" is a string set to the full path of Eagle.exe

"GerberFileName" is a string set to output path and filename

B.name is the filename of the board

On 02/18/2014 11:29 AM, Magnus H-C wrote:

Thank you!

This works great, but since I use a ULP and (I think) you use a bat-file

i had to add "CMD.EXE /c echo y | " in the system call.

Excellent.  Glad it worked out for you.

The excerpt I posted earlier is part of a shell script that is created

from a ULP, then just prior to exiting, the ULP calls

system("./camprep.sh &"); where the ampersand causes the script to be

executed in the background, thus causing the system() call to return

immediately, which, in turn, allows Eagle to continue executing while

the CAM jobs are being created.  I don't know if Windows has some

equivalent, but you may consider having the argument to system() execute

in the background - just to prevent freezes.

The ULP determines from the board design which gerber/Excellon files

need to be created, and which layers to include with each.  The script

includes the recursive removal of a directory and recreation of it.

Then all the output files and the associated .gpi files are moved to

this new directory, and a zip file of the gerbers is created ready for

uploading to the board fabricator.

So, all in all, it's a clean way to generate a zipped collection of

gerbers for a particular design - just "run camprep" in the Eagle

command line.

HTH,

    - Chuck

Hi @Chuck Huber,

Your camprep ULP and associated sh script sound very useful indeed! I don't suppose you'd consider sharing them with the community here http://www.cadsoftusa.com/downloads/ , would you?

Thanks and best regards,

On 02/18/2014 04:37 PM, Daniel Wainwright wrote:

Hi @Chuck Huber,

Your camprep ULP and associated sh script sound very useful indeed! I

don't suppose you'd consider sharing them with the community here

http://www.cadsoftusa.com/downloads/ , would you?

I'd be happy to.  There's four files involved, and I need to sanitize

one of them before uploading.  I'll zip them up and throw in a quick

read-me within the next few days.

    - Chuck

 

Thanks and best regards,

 

--

To view any images and attachments in this post, visit:

http://www.element14.com/community/message/104169

Thanks, I'm sure plenty of folks will appreciate it

Thanks, I'm sure plenty of folks will appreciate it