CAM file types

..gpi is only a ASCII information file. Use an simple text-editor to see its

contents. AFAIR there are examples for the files setup at the end of the

manual.

r

On 03/19/2010 03:59 PM, John Bachman wrote:

I am a bit confused by the file types created by CAM.  I am using

GERBER_RS274X_25 as recommended by my board house.  If I specify the top

copper (2 layer board) and a NAME I get two files NAME and NAME.gpi.

 

The board house says that Eagle should output a file NAME.cmp for this.

All the other layers do similar.

 

Are there not standard file names that Eagle generates for the different

layers?

I've never heard of a standard file naming scheme.  But to make things

clear, I always embed the name of the layer in the file name.

NAME-RevA-TopScreen.gbr

NAME-RevA-TopMask.gbr

NAME-RevA-TopPaste.gbr

NAME-RevA-TopCopper.gbr

NAME-RevA-Inner1.gbr

...

Of course, I'll substitute the NAME with the actual part number of the

board.  In our house, it's usually a 6-digit number.

That way there's no ambiguity at all as to which gerber file describes

which layer.

As for creating the job itself, I usually copy the .cam file from some

other project, and do a global search-and-replace on the old name and

revision.  Then I load it into the CAM processor and run from there.

This seems to be a lot easier than manually editing each section from

the GUI interface.

I have also added a section to each CAM file that various internal shell

scripts external to Eagle understand.  Eagle conveniently ignores these

"extended" sections when loading the .cam file.

Oddly enough, the .cam file has a structure similar to Winbloze's .ini

file.  It'd be nice if they went to an XML or even a properties file

format that could be easily read by Java.  Perhaps that's something I

should post to the suggestion forum.

Enjoy,

    - Chuck

On 3/19/2010 7:41 PM, Chuck Huber wrote:

On 03/19/2010 03:59 PM, John Bachman wrote:

I am a bit confused by the file types created by CAM.  I am using

GERBER_RS274X_25 as recommended by my board house.  If I specify the top

copper (2 layer board) and a NAME I get two files NAME and NAME.gpi.

 

The board house says that Eagle should output a file NAME.cmp for this.

  All the other layers do similar.

 

Are there not standard file names that Eagle generates for the different

layers?

 

I've never heard of a standard file naming scheme.  But to make things

clear, I always embed the name of the layer in the file name.

 

NAME-RevA-TopScreen.gbr

NAME-RevA-TopMask.gbr

NAME-RevA-TopPaste.gbr

NAME-RevA-TopCopper.gbr

NAME-RevA-Inner1.gbr

...

 

Of course, I'll substitute the NAME with the actual part number of the

board.  In our house, it's usually a 6-digit number.

 

That way there's no ambiguity at all as to which gerber file describes

which layer.

 

As for creating the job itself, I usually copy the .cam file from some

other project, and do a global search-and-replace on the old name and

revision.  Then I load it into the CAM processor and run from there.

This seems to be a lot easier than manually editing each section from

the GUI interface.

 

I have also added a section to each CAM file that various internal shell

scripts external to Eagle understand.  Eagle conveniently ignores these

"extended" sections when loading the .cam file.

 

Oddly enough, the .cam file has a structure similar to Winbloze's .ini

file.  It'd be nice if they went to an XML or even a properties file

format that could be easily read by Java.  Perhaps that's something I

should post to the suggestion forum.

 

Enjoy,

     - Chuck

Thanks for the reply.

I dug into the manual a bit more and got even more confused.  Pages 272

and 273 list the file names and extensions that running Gerber274x

supposedly produces:

          %Name.cmp

          %Name.sol

          %Name.plc

          %Name.stc

          %Name.sts

When I run it I get the file name that I entered into that block and a

Name.gpi file and nothing more.

--

John Bachman, W1JGB

AnaTek Corporation

On 03/21/2010 10:35 AM, John Bachman wrote:

On 3/19/2010 7:41 PM, Chuck Huber wrote:

...

I've never heard of a standard file naming scheme.  But to make things

clear, I always embed the name of the layer in the file name.

 

NAME-RevA-TopScreen.gbr

NAME-RevA-TopMask.gbr

NAME-RevA-TopPaste.gbr

NAME-RevA-TopCopper.gbr

NAME-RevA-Inner1.gbr

...

 

Thanks for the reply.

 

I dug into the manual a bit more and got even more confused.  Pages 272

and 273 list the file names and extensions that running Gerber274x

supposedly produces:

 

        %Name.cmp

        %Name.sol

        %Name.plc

        %Name.stc

        %Name.sts

 

When I run it I get the file name that I entered into that block and a

Name.gpi file and nothing more.

I took a look at gerb274x.cam that was distributed with 5.7.0.  It

should be producing more than just the .gpi's.  The file name extensions

of ".cmp", ".sol", and such are left over from the pre-surface-mount

days when all the components were put on one side of the board and

soldered on the other.  With the advent of surface mount technology,

components can be placed on both sides of the board rendering the

nomenclature "component side" and "solder side" obsolete.  These are

generally replaced with "top" and "bottom".

Getting back to the original problem, the "%N" will expand to the name

of the file that is currently opened.  So if the file you have opened is

called "test.brd", you should expect files named:

    test.cmp

    test.sol

    test.plc

and so on.

Each section of a cam job will produce its own .gpi file.  So Section 1

titled "Component Side" will produce  "test.cmp" and "test.gpi".

Section 2, which is titled "Solder side" will produce "test.sol" and

"test.gpi".  Notice that the .gpi file produced in the first section

gets overwritten with the gpi produced in the second section.

Therein lies the reason for doing more with the file name as described

in a previous post.

May I suggest trying this: copy gerb274x.cam to a new file "test.cam".

Edit "test.cam" in your favorite plain text editor (notepad, vim, emacs,

etc) and change the output names of each section to something like:

    %N-TopCopper.gbr

    %N-BotCopper.gbr

    %N-TopScreen.gbr

    %N-TopMask.gbr

    %N-BotMask.gbr

Save it, load it in the cam processor, and run it.  What output do you get?

Hope this helps.

Enjoy,

    - Chuck

On 03/19/2010 03:59 PM, John Bachman wrote:

I am a bit confused by the file types created by CAM.  I am using

GERBER_RS274X_25 as recommended by my board house.  If I specify the

top copper (2 layer board) and a NAME I get two files NAME and NAME.gpi.

 

The board house says that Eagle should output a file NAME.cmp for

this.  All the other layers do similar.

 

Are there not standard file names that Eagle generates for the

different layers?

After re-reading your original post, I think I see what's happening.

Are you clicking on "Process Section" or on "Process Job".  The former

will run only the section that's selected; the latter will run all sections.

I have attached a CAM file for a 4-layer board.  Perhaps it will serve

as an adequate example.

Enjoy,

    - Chuck

On 3/21/2010 11:35 AM, Chuck Huber wrote:

On 03/19/2010 03:59 PM, John Bachman wrote:

I am a bit confused by the file types created by CAM.  I am using

GERBER_RS274X_25 as recommended by my board house.  If I specify the

top copper (2 layer board) and a NAME I get two files NAME and NAME.gpi.

 

The board house says that Eagle should output a file NAME.cmp for

this.  All the other layers do similar.

 

Are there not standard file names that Eagle generates for the

different layers?

 

After re-reading your original post, I think I see what's happening.

Are you clicking on "Process Section" or on "Process Job".  The former

will run only the section that's selected; the latter will run all sections.

 

I have attached a CAM file for a 4-layer board.  Perhaps it will serve

as an adequate example.

 

Enjoy,

     - Chuck

OK, that helped a lot.  I think that I have it now.  Thanks very much.

Now on to making a drill file.

--

John Bachman, W1JGB

AnaTek Corporation