[Emc-users] gerber files to g-code?

[Gene Heskett]

Greetings;

I friend has sent me an archive of .gbr files to see what I think of the 
project.  Unforch, gerbview is only showing me a black, blank screen even if 
I surround the filenames, which have winders spaces in them, with either 
single or dbl-quotes.

The format of the files looks legit to me, so what sort of a viewer do I need 
to be able to both see these, and convert them to g-code?

Here is the head from one of them.

[EMAIL PROTECTED] ROM Pak Board]# head -n 30 ROMPAK_Bottom.gbr
%FSTAX23Y23*%
%ICAS*%
%MOIN*%
%ADD10C,00.010*%
%ADD11C,00.012*%
%ADD12C,00.070*%
%ADD13C,00.005*%
%ADD14C,00.062*%
%ADD15C,00.030*%
%ADD16C,00.007*%
%ADD17C,00.050*%
%ADD18R,00.010X00.010*%
%ADD19R,00.062X00.062*%



D10*
%LPD*%D10*
D10*
%LPD*%D10*
D10*
%LPD*%D10*
D10*
%LPD*%D10*
D10*
%LPD*%D10*
X00325Y04100D02*
X00319Y04069D01*X00308Y04038D01*X00288Y04012D01*
X00262Y03992D01*X00231Y03981D01*X00200Y03975D01*X00169Y03981D01*
X00138Y03992D01*X00112Y04012D01*X00092Y04038D01*X00081Y04069D01*

Any idea's folks?

-- 
Cheers, Gene
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
Trying to establish voice contact ... please yell into keyboard.

-
This SF.net email is sponsored by: Microsoft
Defy all challenges. Microsoft(R) Visual Studio 2005.
http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] gerber files to g-code?

[Stephen Wille Padnos]

Gene Heskett wrote:

>Greetings;
>
>I friend has sent me an archive of .gbr files to see what I think of the 
>project.  Unforch, gerbview is only showing me a black, blank screen even if 
>I surround the filenames, which have winders spaces in them, with either 
>single or dbl-quotes.
>
>The format of the files looks legit to me, so what sort of a viewer do I need 
>to be able to both see these, and convert them to g-code?
>
>Here is the head from one of them.
>
>[EMAIL PROTECTED] ROM Pak Board]# head -n 30 ROMPAK_Bottom.gbr
>%FSTAX23Y23*%
>  
>
All the gerber files I've seen have FSLA in them, not FSTA.  The T means 
"Trailing" and the L means "Leading".  I have no idea what they're 
trailing or leading around though :)  (the X23Y23 means X and Y 
coordinates are in 2.3 digit format)

I didn't see aperture information, which could be a problem.  I'm not 
sure I'd recognize it if I did see it though.

If the files aren't huge, you can email me one, and I can see if it 
loads in Altium.

- Steve

-
This SF.net email is sponsored by: Microsoft
Defy all challenges. Microsoft(R) Visual Studio 2005.
http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] gerber files to g-code?

[Javid Butler]

Good point about the aperature data-it should appear as a list very similar 
to a tool list. When I do a PC board the aperature file is a separate file, 
and without it you will not see anything. Did the viewer generate an error 
about a missing aperature file?

Javid

- Original Message - 
From: "Stephen Wille Padnos" <[EMAIL PROTECTED]>
To: "Enhanced Machine Controller (EMC)" 
Sent: Saturday, September 08, 2007 9:02 PM
Subject: Re: [Emc-users] gerber files to g-code?


> Gene Heskett wrote:
>
>>Greetings;
>>
>>I friend has sent me an archive of .gbr files to see what I think of the
>>project.  Unforch, gerbview is only showing me a black, blank screen even 
>>if
>>I surround the filenames, which have winders spaces in them, with either
>>single or dbl-quotes.
>>
>>The format of the files looks legit to me, so what sort of a viewer do I 
>>need
>>to be able to both see these, and convert them to g-code?
>>
>>Here is the head from one of them.
>>
>>[EMAIL PROTECTED] ROM Pak Board]# head -n 30 ROMPAK_Bottom.gbr
>>%FSTAX23Y23*%
>>
>>
> All the gerber files I've seen have FSLA in them, not FSTA.  The T means
> "Trailing" and the L means "Leading".  I have no idea what they're
> trailing or leading around though :)  (the X23Y23 means X and Y
> coordinates are in 2.3 digit format)
>
> I didn't see aperture information, which could be a problem.  I'm not
> sure I'd recognize it if I did see it though.
>
> If the files aren't huge, you can email me one, and I can see if it
> loads in Altium.
>
> - Steve
>
> -
> This SF.net email is sponsored by: Microsoft
> Defy all challenges. Microsoft(R) Visual Studio 2005.
> http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
> 



-
This SF.net email is sponsored by: Microsoft
Defy all challenges. Microsoft(R) Visual Studio 2005.
http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] gerber files to g-code?

[Jon Elson]

Gene Heskett wrote:
> Greetings;
> 
> I friend has sent me an archive of .gbr files to see what I think of the 
> project.  Unforch, gerbview is only showing me a black, blank screen even if 
> I surround the filenames, which have winders spaces in them, with either 
> single or dbl-quotes.
> 
> The format of the files looks legit to me, so what sort of a viewer do I need 
> to be able to both see these, and convert them to g-code?
> 
> Here is the head from one of them.
> 
> [EMAIL PROTECTED] ROM Pak Board]# head -n 30 ROMPAK_Bottom.gbr
> %FSTAX23Y23*%
> %ICAS*%
> %MOIN*%
> %ADD10C,00.010*%
> %ADD11C,00.012*%
> %ADD12C,00.070*%
> %ADD13C,00.005*%
> %ADD14C,00.062*%
> %ADD15C,00.030*%
> %ADD16C,00.007*%
> %ADD17C,00.050*%
> %ADD18R,00.010X00.010*%
> %ADD19R,00.062X00.062*%
> 
> 
> 
> D10*
> %LPD*%D10*
> D10*
> %LPD*%D10*
> D10*
> %LPD*%D10*
> D10*
> %LPD*%D10*
> D10*
> %LPD*%D10*
> X00325Y04100D02*
> X00319Y04069D01*X00308Y04038D01*X00288Y04012D01*
> X00262Y03992D01*X00231Y03981D01*X00200Y03975D01*X00169Y03981D01*
> X00138Y03992D01*X00112Y04012D01*X00092Y04038D01*X00081Y04069D01*
> 
> Any idea's folks?
> 
This IS, in fact, "G-code", although an old dialect of it, for 
photoplotters from Gerber Scientific.  It is the industry 
standard for photoplotters for PCB manufacturing.  Your file is 
in RS274-X format, where the projection apertures are in the 
beginning of the file, in comment form.

The lines such as %ADD10C,00.010 means that aperture D10 (just 
like a tool select in normal G-code) will be circular and .010" 
diameter.

The rest of the file is in a valid dialect of G-code, with 
Trailing zero suppression and suppressed decimal point.  All the 
ancient controls used to run this way, like the Allen-Bradley 
7320.  Anyway, that first line %FSTAX23Y23*% is the format 
specifier, and it says that the coordinates are absolute (same 
as G90 vs. G91) and that the X and Y coords are in a 2.3 format,
so X00325 means X=0.325"  (Actually, I think leading-zero 
suppression is more standard, with the FSLA format specifier.)

The repeated D10* / %LPD*%D10* looks like a program bug, but it
sets the "Layer Polarity", ie dark lines on clear film or clear 
lines on dark film.

Every time a block that contains an X or Y coordinate is 
processed, that means a move, and the D0x tells whether to turn 
the light on or off while moving, or only flash at the end.
D01 is move with light on
D02 is move with light off
D03 is flash at endpoint

All of this is similar to a canned cycle in regular G-code.

But, if you want to cut a PC board from this data, you need an 
isolation program, that converts line width on the PC board to a 
cut-around path for an engraving bit.  It may be the format on 
this file is odd enough to foul up your gerb view program.

Jon

-
This SF.net email is sponsored by: Microsoft
Defy all challenges. Microsoft(R) Visual Studio 2005.
http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] gerber files to g-code?

[Jon Elson]

Stephen Wille Padnos wrote:
> Gene Heskett wrote:
> 
> 
>>Greetings;
>>
>>I friend has sent me an archive of .gbr files to see what I think of the 
>>project.  Unforch, gerbview is only showing me a black, blank screen even if 
>>I surround the filenames, which have winders spaces in them, with either 
>>single or dbl-quotes.
>>
>>The format of the files looks legit to me, so what sort of a viewer do I need 
>>to be able to both see these, and convert them to g-code?
>>
>>Here is the head from one of them.
>>
>>[EMAIL PROTECTED] ROM Pak Board]# head -n 30 ROMPAK_Bottom.gbr
>>%FSTAX23Y23*%
>> 
>>
> 
> All the gerber files I've seen have FSLA in them, not FSTA.  The T means 
> "Trailing" and the L means "Leading".  I have no idea what they're 
> trailing or leading around though :)  (the X23Y23 means X and Y 
> coordinates are in 2.3 digit format)
> 
The X and Y coords have the decimal point suppressed, as you say 
the industry standard is "L" for leading zero supp.  That means 
(for 2.3 format) the coords are just plain mils, ie. 12345 + 
12.345 inches.  This format is Trailing zero suppression, so 
12345 would be the same, but 12 would be 12.000"
> I didn't see aperture information, which could be a problem.  I'm not 
> sure I'd recognize it if I did see it though.
> 
The aperture info is the %ADD100.010* which defines aperture D10 
as .010"
> If the files aren't huge, you can email me one, and I can see if it 
> loads in Altium.
I suspect the T is going to prevent Altium from processing it 
properly, or at all.  They used to send CAM350 or some gerber 
viewer with their Protel software, which is a lot more general 
Gerber file reader.

Jon

-
This SF.net email is sponsored by: Microsoft
Defy all challenges. Microsoft(R) Visual Studio 2005.
http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] gerber files to g-code?

[Stephen Wille Padnos]

Jon Elson wrote:

>Stephen Wille Padnos wrote:
>  
>
>>Gene Heskett wrote:
>>
>>
>>>Greetings;
>>>
>>>I friend has sent me an archive of .gbr files to see what I think of the 
>>>project.  Unforch, gerbview is only showing me a black, blank screen even if 
>>>I surround the filenames, which have winders spaces in them, with either 
>>>single or dbl-quotes.
>>>
>>>The format of the files looks legit to me, so what sort of a viewer do I 
>>>need 
>>>to be able to both see these, and convert them to g-code?
>>>
>>>Here is the head from one of them.
>>>
>>>[EMAIL PROTECTED] ROM Pak Board]# head -n 30 ROMPAK_Bottom.gbr
>>>%FSTAX23Y23*%
>>>  
>>>
>>All the gerber files I've seen have FSLA in them, not FSTA.  The T means 
>>"Trailing" and the L means "Leading".  I have no idea what they're 
>>trailing or leading around though :)  (the X23Y23 means X and Y 
>>coordinates are in 2.3 digit format)
>>
>>
>The X and Y coords have the decimal point suppressed, as you say 
>the industry standard is "L" for leading zero supp.  That means 
>(for 2.3 format) the coords are just plain mils, ie. 12345 + 
>12.345 inches.  This format is Trailing zero suppression, so 
>12345 would be the same, but 12 would be 12.000"
>  
>
Heh.  I remembered our discussion about G-code formats on a short car 
ride (maybe headed to Peoria?), and I figured you'd know what all of it 
meant.

>>I didn't see aperture information, which could be a problem.  I'm not 
>>sure I'd recognize it if I did see it though.
>>
>>
>The aperture info is the %ADD100.010* which defines aperture D10 
>as .010"
>  
>
I didn't recognize the aperture list, but it makes sense as you 
explained it.

>>If the files aren't huge, you can email me one, and I can see if it 
>>loads in Altium.
>>
>>
>I suspect the T is going to prevent Altium from processing it 
>properly, or at all.  They used to send CAM350 or some gerber 
>viewer with their Protel software, which is a lot more general 
>Gerber file reader.
>  
>
Altium comes with something called "Camtastic", so it may work.
- Steve


-
This SF.net email is sponsored by: Microsoft
Defy all challenges. Microsoft(R) Visual Studio 2005.
http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] gerber files to g-code?

[Gene Heskett]

On Saturday 08 September 2007, Stephen Wille Padnos wrote:
>Gene Heskett wrote:
>>Greetings;
>>
>>I friend has sent me an archive of .gbr files to see what I think of the
>>project.  Unforch, gerbview is only showing me a black, blank screen even
>> if I surround the filenames, which have winders spaces in them, with
>> either single or dbl-quotes.
>>
>>The format of the files looks legit to me, so what sort of a viewer do I
>> need to be able to both see these, and convert them to g-code?
>>
>>Here is the head from one of them.
>>
>>[EMAIL PROTECTED] ROM Pak Board]# head -n 30 ROMPAK_Bottom.gbr
>>%FSTAX23Y23*%
>
>All the gerber files I've seen have FSLA in them, not FSTA.  The T means
>"Trailing" and the L means "Leading".  I have no idea what they're
>trailing or leading around though :)  (the X23Y23 means X and Y
>coordinates are in 2.3 digit format)
>
>I didn't see aperture information, which could be a problem.  I'm not
>sure I'd recognize it if I did see it though.
>
>If the files aren't huge, you can email me one, and I can see if it
>loads in Altium.
>
The src zip:

>- Steve
>
Thanks Steve.

-- 
Cheers, Gene
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
Q: What do Bill Gates and Bill Clinton have in common?
A: Their ratings climb whenever they do something unethical.

-
This SF.net email is sponsored by: Microsoft
Defy all challenges. Microsoft(R) Visual Studio 2005.
http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] gerber files to g-code?

[Gene Heskett]

On Saturday 08 September 2007, Javid Butler wrote:
>Good point about the aperature data-it should appear as a list very similar
>to a tool list. When I do a PC board the aperature file is a separate file,
>and without it you will not see anything. Did the viewer generate an error
>about a missing aperature file?
>
No, its looking (gerbview) for .pho files, doesn't allow any other choice.
gerbv-1.0.2 can see the files in the directory I unpacked them to, but "failed 
to load" any of them.
gerbv reports this for a session:
[EMAIL PROTECTED] opt]# gerbv
Error: eval: unbound variable: %fstax23y23*%
Error: eval: unbound variable: %
Error: eval: unbound variable: %fstax23y23*%

Apparently one line per attempt to load a file.

>Javid
>
>- Original Message -
>From: "Stephen Wille Padnos" <[EMAIL PROTECTED]>
>To: "Enhanced Machine Controller (EMC)" 
>Sent: Saturday, September 08, 2007 9:02 PM
>Subject: Re: [Emc-users] gerber files to g-code?
>
>> Gene Heskett wrote:
>>>Greetings;
>>>
>>>I friend has sent me an archive of .gbr files to see what I think of the
>>>project.  Unforch, gerbview is only showing me a black, blank screen even
>>>if
>>>I surround the filenames, which have winders spaces in them, with either
>>>single or dbl-quotes.
>>>
>>>The format of the files looks legit to me, so what sort of a viewer do I
>>>need
>>>to be able to both see these, and convert them to g-code?
>>>
>>>Here is the head from one of them.
>>>
>>>[EMAIL PROTECTED] ROM Pak Board]# head -n 30 ROMPAK_Bottom.gbr
>>>%FSTAX23Y23*%
>>
>> All the gerber files I've seen have FSLA in them, not FSTA.  The T means
>> "Trailing" and the L means "Leading".  I have no idea what they're
>> trailing or leading around though :)  (the X23Y23 means X and Y
>> coordinates are in 2.3 digit format)
>>
>> I didn't see aperture information, which could be a problem.  I'm not
>> sure I'd recognize it if I did see it though.
>>
>> If the files aren't huge, you can email me one, and I can see if it
>> loads in Altium.
>>
>> - Steve
>>
>> -
>> This SF.net email is sponsored by: Microsoft
>> Defy all challenges. Microsoft(R) Visual Studio 2005.
>> http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
>> ___
>> Emc-users mailing list
>> Emc-users@lists.sourceforge.net
>> https://lists.sourceforge.net/lists/listinfo/emc-users
>
>-
>This SF.net email is sponsored by: Microsoft
>Defy all challenges. Microsoft(R) Visual Studio 2005.
>http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
>___
>Emc-users mailing list
>Emc-users@lists.sourceforge.net
>https://lists.sourceforge.net/lists/listinfo/emc-users



-- 
Cheers, Gene
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
Fortune finishes the great quotations, #9

A word to the wise is often enough to start an argument.

-
This SF.net email is sponsored by: Microsoft
Defy all challenges. Microsoft(R) Visual Studio 2005.
http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] gerber files to g-code?

[Gene Heskett]

On Sunday 09 September 2007, Jon Elson wrote:
>Gene Heskett wrote:
>> Greetings;
>>
>> I friend has sent me an archive of .gbr files to see what I think of the
>> project.  Unforch, gerbview is only showing me a black, blank screen even
>> if I surround the filenames, which have winders spaces in them, with
>> either single or dbl-quotes.
>>
>> The format of the files looks legit to me, so what sort of a viewer do I
>> need to be able to both see these, and convert them to g-code?
>>
>> Here is the head from one of them.
>>
>> [EMAIL PROTECTED] ROM Pak Board]# head -n 30 ROMPAK_Bottom.gbr
>> %FSTAX23Y23*%
>> %ICAS*%
>> %MOIN*%
>> %ADD10C,00.010*%
>> %ADD11C,00.012*%
>> %ADD12C,00.070*%
>> %ADD13C,00.005*%
>> %ADD14C,00.062*%
>> %ADD15C,00.030*%
>> %ADD16C,00.007*%
>> %ADD17C,00.050*%
>> %ADD18R,00.010X00.010*%
>> %ADD19R,00.062X00.062*%
>>
>>
>>
>> D10*
>> %LPD*%D10*
>> D10*
>> %LPD*%D10*
>> D10*
>> %LPD*%D10*
>> D10*
>> %LPD*%D10*
>> D10*
>> %LPD*%D10*
>> X00325Y04100D02*
>> X00319Y04069D01*X00308Y04038D01*X00288Y04012D01*
>> X00262Y03992D01*X00231Y03981D01*X00200Y03975D01*X00169Y03981D01*
>> X00138Y03992D01*X00112Y04012D01*X00092Y04038D01*X00081Y04069D01*
>>
>> Any idea's folks?
>
>This IS, in fact, "G-code", although an old dialect of it, for
>photoplotters from Gerber Scientific.  It is the industry
>standard for photoplotters for PCB manufacturing.  Your file is
>in RS274-X format, where the projection apertures are in the
>beginning of the file, in comment form.
>
>The lines such as %ADD10C,00.010 means that aperture D10 (just
>like a tool select in normal G-code) will be circular and .010"
>diameter.
>
>The rest of the file is in a valid dialect of G-code, with
>Trailing zero suppression and suppressed decimal point.  All the
>ancient controls used to run this way, like the Allen-Bradley
>7320.  Anyway, that first line %FSTAX23Y23*% is the format
>specifier, and it says that the coordinates are absolute (same
>as G90 vs. G91) and that the X and Y coords are in a 2.3 format,
>so X00325 means X=0.325"  (Actually, I think leading-zero
>suppression is more standard, with the FSLA format specifier.)
>
>The repeated D10* / %LPD*%D10* looks like a program bug, but it
>sets the "Layer Polarity", ie dark lines on clear film or clear
>lines on dark film.
>
>Every time a block that contains an X or Y coordinate is
>processed, that means a move, and the D0x tells whether to turn
>the light on or off while moving, or only flash at the end.
>D01 is move with light on
>D02 is move with light off
>D03 is flash at endpoint
>
>All of this is similar to a canned cycle in regular G-code.
>
>But, if you want to cut a PC board from this data, you need an
>isolation program, that converts line width on the PC board to a
>cut-around path for an engraving bit.  It may be the format on
>this file is odd enough to foul up your gerb view program.
>
>Jon
>
Thanks Jon.  This was just recently generated on a Mac, a simple pcb board for 
mounting a 27xxx eprom chip and plugging it into a color computer.

Is there a convertor in the geda suite (or any linux & free) that can convert 
this to our dialect of g-code, RS-274D?

-- 
Cheers, Gene
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
I fill MY industrial waste containers with old copies of the "WATCHTOWER"
and then add HAWAIIAN PUNCH to the top ...  They look NICE in the yard ...

-
This SF.net email is sponsored by: Microsoft
Defy all challenges. Microsoft(R) Visual Studio 2005.
http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] gerber files to g-code?

[Dale]

have you tried Eagle PCB from cadsoftusa.com there is a free for 
non-comercial use. There may be a User Language Program or a built in 
Greber converter. If you can get it into eagle then milling a PCB is easy.

Gene Heskett wrote:
> On Sunday 09 September 2007, Jon Elson wrote:
> 
>>Gene Heskett wrote:
>>
>>>Greetings;
>>>
>>>I friend has sent me an archive of .gbr files to see what I think of the
>>>project.  Unforch, gerbview is only showing me a black, blank screen even
>>>if I surround the filenames, which have winders spaces in them, with
>>>either single or dbl-quotes.
>>>
>>>The format of the files looks legit to me, so what sort of a viewer do I
>>>need to be able to both see these, and convert them to g-code?
>>>
>>>Here is the head from one of them.
>>>
>>>[EMAIL PROTECTED] ROM Pak Board]# head -n 30 ROMPAK_Bottom.gbr
>>>%FSTAX23Y23*%
>>>%ICAS*%
>>>%MOIN*%
>>>%ADD10C,00.010*%
>>>%ADD11C,00.012*%
>>>%ADD12C,00.070*%
>>>%ADD13C,00.005*%
>>>%ADD14C,00.062*%
>>>%ADD15C,00.030*%
>>>%ADD16C,00.007*%
>>>%ADD17C,00.050*%
>>>%ADD18R,00.010X00.010*%
>>>%ADD19R,00.062X00.062*%
>>>
>>>
>>>
>>>D10*
>>>%LPD*%D10*
>>>D10*
>>>%LPD*%D10*
>>>D10*
>>>%LPD*%D10*
>>>D10*
>>>%LPD*%D10*
>>>D10*
>>>%LPD*%D10*
>>>X00325Y04100D02*
>>>X00319Y04069D01*X00308Y04038D01*X00288Y04012D01*
>>>X00262Y03992D01*X00231Y03981D01*X00200Y03975D01*X00169Y03981D01*
>>>X00138Y03992D01*X00112Y04012D01*X00092Y04038D01*X00081Y04069D01*
>>>
>>>Any idea's folks?
>>
>>This IS, in fact, "G-code", although an old dialect of it, for
>>photoplotters from Gerber Scientific.  It is the industry
>>standard for photoplotters for PCB manufacturing.  Your file is
>>in RS274-X format, where the projection apertures are in the
>>beginning of the file, in comment form.
>>
>>The lines such as %ADD10C,00.010 means that aperture D10 (just
>>like a tool select in normal G-code) will be circular and .010"
>>diameter.
>>
>>The rest of the file is in a valid dialect of G-code, with
>>Trailing zero suppression and suppressed decimal point.  All the
>>ancient controls used to run this way, like the Allen-Bradley
>>7320.  Anyway, that first line %FSTAX23Y23*% is the format
>>specifier, and it says that the coordinates are absolute (same
>>as G90 vs. G91) and that the X and Y coords are in a 2.3 format,
>>so X00325 means X=0.325"  (Actually, I think leading-zero
>>suppression is more standard, with the FSLA format specifier.)
>>
>>The repeated D10* / %LPD*%D10* looks like a program bug, but it
>>sets the "Layer Polarity", ie dark lines on clear film or clear
>>lines on dark film.
>>
>>Every time a block that contains an X or Y coordinate is
>>processed, that means a move, and the D0x tells whether to turn
>>the light on or off while moving, or only flash at the end.
>>D01 is move with light on
>>D02 is move with light off
>>D03 is flash at endpoint
>>
>>All of this is similar to a canned cycle in regular G-code.
>>
>>But, if you want to cut a PC board from this data, you need an
>>isolation program, that converts line width on the PC board to a
>>cut-around path for an engraving bit.  It may be the format on
>>this file is odd enough to foul up your gerb view program.
>>
>>Jon
>>
> 
> Thanks Jon.  This was just recently generated on a Mac, a simple pcb board 
> for 
> mounting a 27xxx eprom chip and plugging it into a color computer.
> 
> Is there a convertor in the geda suite (or any linux & free) that can convert 
> this to our dialect of g-code, RS-274D?
> 


-
This SF.net email is sponsored by: Microsoft
Defy all challenges. Microsoft(R) Visual Studio 2005.
http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] gerber files to g-code?

[Jon Elson]

Stephen Wille Padnos wrote:
> 
> Heh.  I remembered our discussion about G-code formats on a short car 
> ride (maybe headed to Peoria?), and I figured you'd know what all of it 
> meant.
> 
Well, after having written my own Gerber to raster converter 
program, I know the format fairly well.  I haven't put RS274-X 
format features into my program yet, but it supports all the 
stuff I generally have in my PCB artwork.  Unfortunately this 
code is written in Turbo Pascal, and not too portable.  Sometime 
I might have to try running it through p2c to see how bad a mess 
it makes.

It actually would not be hard at all to write a little program 
that would convert this Gerber format to standard G-code, and it 
would draw out the traces with the EMC preview programs. 
Converting from Gerber to a trace isolating cutter path would be 
a good deal harder.
> Altium comes with something called "Camtastic", so it may work.
That's right.  I knew they sent some gerber viewer with the 
software.  I don't think I got camtastic, but I may have 
something older.

Jon

-
This SF.net email is sponsored by: Microsoft
Defy all challenges. Microsoft(R) Visual Studio 2005.
http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] gerber files to g-code?

[Jon Elson]

Gene Heskett wrote:
> Thanks Jon.  This was just recently generated on a Mac, a simple pcb board 
> for 
> mounting a 27xxx eprom chip and plugging it into a color computer.
> 
> Is there a convertor in the geda suite (or any linux & free) that can convert 
> this to our dialect of g-code, RS-274D?
> 

Well, no.  The Gerber file is designed to draw the pattern on 
film with light, with the apertures setting the shape of the 
light beam.  It can flash round, square, oval and thermal relief 
pattern in one blink, with one like of G code.  You can't do 
that with a mill.  If you want to actually cut a working PC 
board with a router bit, you need to "convert" the file quite 
radically with a trace isolation program.  It figures out which 
traces and pads are connected, then draws a series of moves 
around the entire extent of the net.  Eagle is one of the 
programs that can do this, but the somewhat odd format of this 
file may be an obstacle.  Could the person who made the file on 
the Mac specify for trailing zero suppression on these files and 
re-generate it?  I believe I could then read it on my Protel 
software, for instance, or make it plot on my photoplotter.

The industry standard is for Gerber photoplot files to have 
Leading zeros suppressed, and for Excellon drill files to have 
Trailing zeros suppressed!  All part of the history of the 
electronics industry, dating back to punched paper tape.

Jon

-
This SF.net email is sponsored by: Microsoft
Defy all challenges. Microsoft(R) Visual Studio 2005.
http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] gerber files to g-code?

[Sven Mueller]

Dale schrieb:
> have you tried Eagle PCB from cadsoftusa.com there is a free for 
> non-comercial use. There may be a User Language Program or a built in 
> Greber converter. If you can get it into eagle then milling a PCB is easy.

At least there is pcb-gcode which outputs nice gcode from layouts. There
really also seems to be a ULP or external program for gerber import, but
I don't know anything about it, just heard it exists.

cu,
Sven


-
This SF.net email is sponsored by: Microsoft
Defy all challenges. Microsoft(R) Visual Studio 2005.
http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] gerber files to g-code?

[Gene Heskett]

On Sunday 09 September 2007, Dale wrote:
>have you tried Eagle PCB from cadsoftusa.com there is a free for
>non-comercial use. There may be a User Language Program or a built in
>Greber converter. If you can get it into eagle then milling a PCB is easy.
>
Unforch, the copy of eagle I have here won't touch that code.  It is maybe 8 
months old.

-- 
Cheers, Gene
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
I guess I've been wrong all my life, but so have billions of other people...
Certainty is just an emotion.
-- Hal Clement

-
This SF.net email is sponsored by: Microsoft
Defy all challenges. Microsoft(R) Visual Studio 2005.
http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] gerber files to g-code?

[Gene Heskett]

On Sunday 09 September 2007, Jon Elson wrote:
>Gene Heskett wrote:
>> Thanks Jon.  This was just recently generated on a Mac, a simple pcb board
>> for mounting a 27xxx eprom chip and plugging it into a color computer.
>>
>> Is there a convertor in the geda suite (or any linux & free) that can
>> convert this to our dialect of g-code, RS-274D?
>
>Well, no.  The Gerber file is designed to draw the pattern on
>film with light, with the apertures setting the shape of the
>light beam.  It can flash round, square, oval and thermal relief
>pattern in one blink, with one like of G code.  You can't do
>that with a mill.  If you want to actually cut a working PC
>board with a router bit, you need to "convert" the file quite
>radically with a trace isolation program.  It figures out which
>traces and pads are connected, then draws a series of moves
>around the entire extent of the net.  Eagle is one of the
>programs that can do this, but the somewhat odd format of this
>file may be an obstacle.  Could the person who made the file on
>the Mac specify for trailing zero suppression on these files and
>re-generate it?  I believe I could then read it on my Protel
>software, for instance, or make it plot on my photoplotter.
>
>The industry standard is for Gerber photoplot files to have
>Leading zeros suppressed, and for Excellon drill files to have
>Trailing zeros suppressed!  All part of the history of the
>electronics industry, dating back to punched paper tape.
>
>Jon

I'll check with the author, it could be he isn't that fam with the usual ways 
of doing things.  Thanks Jon.

-- 
Cheers, Gene
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
"Mach was the greatest intellectual fraud in the last ten years."
"What about X?"
"I said `intellectual'."
;login, 9/1990

-
This SF.net email is sponsored by: Microsoft
Defy all challenges. Microsoft(R) Visual Studio 2005.
http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] gerber files to g-code?

[Sven Mueller]

Jon Elson wrote on 09/09/2007 19:24:
> Stephen Wille Padnos wrote:
>> Heh.  I remembered our discussion about G-code formats on a short car 
>> ride (maybe headed to Peoria?), and I figured you'd know what all of it 
>> meant.
>>
> Well, after having written my own Gerber to raster converter 
> program, I know the format fairly well.  I haven't put RS274-X 
> format features into my program yet, but it supports all the 
> stuff I generally have in my PCB artwork.  Unfortunately this 
> code is written in Turbo Pascal, and not too portable.  Sometime 
> I might have to try running it through p2c to see how bad a mess 
> it makes.

Does any sort of publicly available documentation exist for the gerber
file format?

> It actually would not be hard at all to write a little program 
> that would convert this Gerber format to standard G-code, and it 
> would draw out the traces with the EMC preview programs. 
> Converting from Gerber to a trace isolating cutter path would be 
> a good deal harder.

Not _too_ hard though, I think and certainly a task I would like to
tackle. This would result in a commandline tool* (or QT based, I don't
like GTK that much), which takes a text based configuration and a gerber
file. Also I think that at least Eagle is able to output an inverted
gerber file (i.e. "printing" not the traces but the non-trace/isolation
areas), which would make this whole thing a lot easier.

regards,
Sven

*: Probably a prototype in Perl with final implementation in C/C++

-
This SF.net email is sponsored by: Microsoft
Defy all challenges. Microsoft(R) Visual Studio 2005.
http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] gerber files to g-code?

[Dale]

If Eagle can import the gerber file and convert it to an Eagle board the 
n the trace isolation gcode from an Eagle board program is already done. 
I'' look later tonight to see if Eagle will import the gerber files or 
if a User Language Program is needed and/or available. I've never needed 
to try it but I'm very familiar with Eagle for initial drawing and 
converting/milling boards.

Dale

Sven Mueller wrote:
> Jon Elson wrote on 09/09/2007 19:24:
> 
>>Stephen Wille Padnos wrote:
>>
>>>Heh.  I remembered our discussion about G-code formats on a short car 
>>>ride (maybe headed to Peoria?), and I figured you'd know what all of it 
>>>meant.
>>>
>>
>>Well, after having written my own Gerber to raster converter 
>>program, I know the format fairly well.  I haven't put RS274-X 
>>format features into my program yet, but it supports all the 
>>stuff I generally have in my PCB artwork.  Unfortunately this 
>>code is written in Turbo Pascal, and not too portable.  Sometime 
>>I might have to try running it through p2c to see how bad a mess 
>>it makes.
> 
> 
> Does any sort of publicly available documentation exist for the gerber
> file format?
> 
> 
>>It actually would not be hard at all to write a little program 
>>that would convert this Gerber format to standard G-code, and it 
>>would draw out the traces with the EMC preview programs. 
>>Converting from Gerber to a trace isolating cutter path would be 
>>a good deal harder.
> 
> 
> Not _too_ hard though, I think and certainly a task I would like to
> tackle. This would result in a commandline tool* (or QT based, I don't
> like GTK that much), which takes a text based configuration and a gerber
> file. Also I think that at least Eagle is able to output an inverted
> gerber file (i.e. "printing" not the traces but the non-trace/isolation
> areas), which would make this whole thing a lot easier.
> 
> regards,
> Sven
> 
> *: Probably a prototype in Perl with final implementation in C/C++
> 
> -
> This SF.net email is sponsored by: Microsoft
> Defy all challenges. Microsoft(R) Visual Studio 2005.
> http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
> 


-
This SF.net email is sponsored by: Microsoft
Defy all challenges. Microsoft(R) Visual Studio 2005.
http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] gerber files to g-code?

[Jon Elson]

Sven Mueller wrote:
> Jon Elson wrote on 09/09/2007 19:24:
> 
>>Stephen Wille Padnos wrote:
>>
>>>Heh.  I remembered our discussion about G-code formats on a short car 
>>>ride (maybe headed to Peoria?), and I figured you'd know what all of it 
>>>meant.
>>>
>>
>>Well, after having written my own Gerber to raster converter 
>>program, I know the format fairly well.  I haven't put RS274-X 
>>format features into my program yet, but it supports all the 
>>stuff I generally have in my PCB artwork.  Unfortunately this 
>>code is written in Turbo Pascal, and not too portable.  Sometime 
>>I might have to try running it through p2c to see how bad a mess 
>>it makes.
> 
> 
> Does any sort of publicly available documentation exist for the gerber
> file format?
> 
Umm, probably.  I got a copy of the Gerber file spec from 
circling a "bingo card" in a magazine many years ago.  I have no 
idea if they still give this out in hardcopy, but this appears 
to be the same manual :
http://members.optusnet.com.au/~eseychell/rs274xrevd_e.pdf
I have no idea if this is authorized, so you might want to 
download it rather than bookmark it.

Jon

-
This SF.net email is sponsored by: Microsoft
Defy all challenges. Microsoft(R) Visual Studio 2005.
http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users