Running the CAM processor from the command   line

Stewart wrote:

I just lost a few days on a board due to my being in a hurry.  Does

anyone know how to run the "drillcfg.ulp" and then start-up the CAM

processor to do the rest of the steps???  Or, is there a way to

bypass the step to run the drillcfg.ulp??  I have searched the HELP

for running the CAM from the command line, although, every other

conceivable command is in there, where is CAM???

 

The term 'command line' refers to two uses. One is within Eagle and is the

command line you see in each editor window. The other is outside of Eagle.

It refers to launching applications from a command window or terminal

window.

You cannot run the CAM by typing into the editor command line. You need to

click the CAM icon on the toolbar or select from the drop down menus

File/CAM Processor. Using the keyboard you could type Alt-F followed by

Alt-M.

You can launch Eagle with command line parameters which  tell it to run the

CAM processor (command line method) which is useful for scripts and ULPs. I

suspect this is not what you are after.

Warren

--

Viewed / responded via the newsgroup at

news.cadsoft.de

Warren,

Thanks for your reply.  As I thought I had made clear, I want a one command

solution to generating GERBERS and drill information.  I want to automate

the process so that none of the currently required 3 steps get forgotten in

the current manual process.  I want to do a script/ulp that does the whole

thing, that is run the CAM after the drillcfg has been done.  I did add the

settings from "excellon" to my list of job file configurations. Which, now

I am down to 2 steps, just need to get it down to ONE STEP.  (and of course

I want to do this in the layout editor, not as a command line parameter

during the launch of Eagle from the desktop)

Stewart

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

Stewart wrote on Thu, 29 December 2011 19:56

As I thought I had made clear, I want ...

People often ask for the wrong thing or something unreasonable.  Other than

the Cadsoft folks who do chime in here on occasion, the rest of us are free

to answer whatever parts of a question we think is worth it, have time for,

know the answer to, or otherwise just feel like.  Sometimes that means

answering a different question that we think is more relevant.  That's how

peer to peer support works.

Quote:

a one command solution to generating GERBERS and drill information.

You can possibly do this with the information Warren gave you, although

this one command will be difficult since there are various options in the

process.

Quote:

I want to automate the process so that none of the currently required 3

steps get forgotten in the current manual process.

First, it's more than three steps.  Second, this is only once per board, so

you're not going to get much return for taking the time to make this a

automated process.  I have thought about this myself and decided it's not

worth it.

Instead, I use a checklist.  I have a script that gathers all the various

files required by a board house into one zip file.  The checklist is in the

comments of that script:

rem   The steps in creating the right files in Eagle from a completed

rem   board layout are:

rem

rem   1  -  Make sure there are fiducials in two opposite corners.

rem

rem   2  -  Add the layer name to each layer outside the board area.

rem

rem   3  -  Run DRILLCFG.ULP from the board editor.  Specify inches.

rem         Go back and fix hole sizes that aren't in the

~/eagle/holes.txt

rem         list.

rem

rem   4  -  Run the EXCELLON.CAM CAM processor job to create the

rem         drill data (.DRD) file.

rem

rem   5  -  Run the Generic2L (2 layer boards) or Generic4L

rem         (4 layer boards) CAM processor jobs.  This will produce the

rem         gerber files for each photo-plotted layer.

rem

rem         NOTE 1: Delete the solder paste mask output file(s) if package

rem           is for PCB only, not full board manufacturing.

rem

rem   8  -  Run this script to create the ZIP file with all the needed

rem         files.

rem

rem   7  -  Visually verify the Gerber files with a Gerber file viewer.

The whole script is included in my Eagle Tools release at

http://www.embedinc.com/pic/dload.htm

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

Olin,

Thank-you for your rather opinionated response. 

I understand your feelings that Eagle can be controlled and configured

through the use of scripts and ULPs.

I also agree that the generation of GERBERS should only happen once per

board revision, but in the real world, this process may occur several times

during the course of improvements.

Eagle is the only package I have seen that does not have one central

interface to create all of the files required to fabricate a board.

That said, I will concentrate on my main question:

I can not find a console command to launch the CAM interface. 

As Warren suggested, the use of Alt-F, M sounds like a good work around.

Can a script issue such a command line?? (I just tried it with the keyboard

and Alt-F does nothing, but, all of the others; E, D, V, T, O, W, H work as

expected.)

My question remains:  How can I launch the CAM processor from a .scr or

ulp??

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

Concerning the Alt-F comment.....  It is my fault, I assigned Alt-F to

another function.

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

Stewart wrote on Fri, 30 December 2011 13:34

I also agree that the generation of GERBERS should only happen once per

board revision, but in the real world, this process may occur several

times during the course of improvements.

Sure, but the process is still small compared to each chunk of work that

results in you needing new gerber files.  It takes maybe a whole minute

(I'm being pessimistic) to generate the CAM files for a board.  At best

automating this will save that minute once every time you make new files,

each of which probably represents at least a hour or more of work.

There are more productive things to chase aftere to improve. 

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

Op Thu, 29 Dec 2011 21:39:03 +0100 schreef Stewart <koch.energy@gmail.com>:

Does anyone

know how to run the "drillcfg.ulp"

Hello Stewart,

Is there any reason you still want to use "drillcfg.ulp"?. From Eagle 4.12 

on, the excellon drill device (and maybe others) can automatically 

generate the necessary drill definitions and contain them within the drill 

file. After Eagle 4.0 I've never used "drillcfg.ulp" anymore. But, of 

course, there can be special reasons for using it.

Anyway, If you are on Mac or Linux, then maybe this is something for you:

http://www.rocketnumbernine.com/2011/12/14/automating-gerbers-from-eagle

Richard

Richard,

Thank you VERY much, I was not sure what drillcfg really did, all I kept

thinking was, "don't mess with success"

Now I have my single click solution that I wanted.

I just simply added a new tab in each of my configurations to do what the

Excellon config had selected.

Thank you again.

I still wonder why all other commands that you can select with a mouse are

also able to be called by name on the console EXCEPT for CAM

HAPPY NEW YEAR.

Stewart

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.