Georg kindly sent me the file and I figured out how to open a dos window and
run it... You have to have a Gerber file that has the extension .gbr and it
reads it a modifies it and creates a new file with the extension .gbx.  The
format to execute it is "protlgbr.exe <filename>. gbr" It then creates a
file called "<filename>.gbx". I tried to load this file into protel and got
an error. It was unsuccessful. 
I examined the 2 files and saw that the new file is reordered in a column
now... It would be interesting to see the source code and try making a few
changes to it... For one it should prompt the user for the file to be
converted... and we still need to understand why protel is choking on the
new file... Some error handling in the program would probably help too...
Are the G04 commands not understood by Protel as being comment lines? 

Here is a sampling of the headers and the first couple of g codes from the 2
files:
------------------------------------------
silk.gbr
------------------------------------------
*G04*G04 PARAMETERS*G04*%FSLAX24Y24*%%MOIN*%%ICAS*%%LNpmss*%G04*G04*G04
APERTURE
DEFINITIONS*G04*%ADD10R,0.02000X0.02000*%%ADD11C,0.01000*%%ADD12C,0.00800*%%
ADD13C,0.00500*%G04------------------------------------------------------*G0
4------------------------------------------------------*
G04*G04 I M A G E   D A T A*G04 PCB NAME: dat19133*G04 LAYER NAME:
pmss*G04*G54D10*X30100Y50900D03*X23000Y47850D03*X6900Y50150D03*X6900Y41100D0
3*X41850Y43850D03*X35350Y43850D03*X52900Y43450D03*X47350Y43900D03*X40850Y314
00D03*X9650Y32600D03*X32600Y21350D03*X40150Y24850D03*X30700Y35250D03*G54D11*
X24200Y5750D02*X60450Y5750D01*


------------------------------------
silk.gbx
------------------------------------
%FSLAX24Y24*%
%MOIN*%
%ICAS*%
%LNpmss*%
G04*
G04*
G04 APERTURE DEFINITIONS*
G04*
%ADD10R,0.02000X0.02000*%
%ADD11C,0.01000*%
%ADD12C,0.00800*%
%ADD13C,0.00500*%
G04------------------------------------------------------*
G04------------------------------------------------------*
G04*
G04 I M A G E   D A T A*
G04 PCB NAME: dat19133*
G04 LAYER NAME: pmss*
G04*
G54D10*
X30100Y50900D03*
X23000Y47850D03*
X6900Y50150D03*
X6900Y41100D03*
X41850Y43850D03*
X35350Y43850D03*
X52900Y43450D03*
X47350Y43900D03*
X40850Y31400D03*
X9650Y32600D03*
X32600Y21350D03*
X40150Y24850D03*
X30700Y35250D03*
G54D11*
X24200Y5750D02*
X60450Y5750D01*

-------------------------------------
Interesting.... Just what is Protel having a problem with? When trying to
import the gerber into a blank pcb file in protel, the error message said
that protel choked on the comment lines with the long set of dashes in
them... go figure...

- Bill Brooks




-----Original Message-----
From: Tommy Åkesson [mailto:[EMAIL PROTECTED]]
Sent: Wednesday, December 05, 2001 8:23 AM
To: Protel EDA Forum
Subject: [PEDA] SV: AW: CAMTASTIC GERBER TO PROTEL TRANSLATOR?


Me to..

[EMAIL PROTECTED]

-----Ursprungligt meddelande-----
Från: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED]]
Skickat: den 5 december 2001 17:02
Till: Protel EDA Forum
Ämne: Re: [PEDA] AW: CAMTASTIC GERBER TO PROTEL TRANSLATOR?


If possible I would love a copy too, Please.

[EMAIL PROTECTED]

-----Original Message-----
From: Georg Beckmann [mailto:[EMAIL PROTECTED]]
Sent: Wednesday, December 05, 2001 12:04 AM
To: 'Protel EDA Forum'
Subject: [PEDA] AW: CAMTASTIC GERBER TO PROTEL TRANSLATOR?


I sent it to Abdulrahman Lomax he wanted to bring it to the file section in
this forum.
But anyway, I send it to your e-mail address.

Georg

-----Urspr ngliche Nachricht-----
Von: Brooks,Bill [mailto:[EMAIL PROTECTED]]
Gesendet: Mittwoch, 5. Dezember 2001 01:47
An: 'Protel EDA Forum'; '[EMAIL PROTECTED]'
Betreff: [PEDA] CAMTASTIC GERBER TO PROTEL TRANSLATOR?


Georg Beckmann mentioned having a little utility to convert the GERBER
output from CAMTASIC to PROTEL compatible Gerber.... for import to Protel.
Does anyone have this file they can make available to me? I would like to
test it on some boards I am plying with. Could be very useful.... thanks
Bill Brooks
[EMAIL PROTECTED]


-----Original Message-----
From: Brooks,Bill [mailto:[EMAIL PROTECTED]]
Sent: Monday, December 03, 2001 9:59 AM
To: 'Protel EDA Forum'; '[EMAIL PROTECTED]'
Subject: Re: [PEDA] AW: imported Gerber info missing


Hi Georg, Could I get a copy of the Gerber translator program you mentioned
in this post?
- Bill Brooks

Bill Brooks
PCB Design Engineer , C.I.D.
DATRON WORLD COMMUNICATIONS, INC
3030 Enterprise Court
Vista, CA 92083
Tel: (760)597-1500 Ext 3772 Fax: (760)597-1510
mailto:[EMAIL PROTECTED]
IPC Designers Council, San Diego Chapter
http://www.ipc.org/SanDiego/
http://home.fda.net/bbrooks/pca/pca.htm


-----Original Message-----
From: Georg Beckmann [mailto:[EMAIL PROTECTED]]
Sent: Saturday, October 20, 2001 2:17 AM
To: 'Protel EDA Forum'
Subject: [PEDA] AW: imported Gerber info missing


Thanks for the advice, someone made me a simple program to convert the
gerber files generated by camtastic that protel can inport it.
The program adds the Dnn and cuts the first 3 lines of the gerber
that protel don't understand.

It is a simple DOS program you can start in a dos-box with the name of the
source gerber to convert. The result is a file with the same name but a
gbx instead of a gbr extention. So you have to rename it and preserve your
source somewhere.

With this I was able to import the gerber.

The drills I first imported in camtastic and had to make a tool file.
( In my sources the drill tools and the apertures are only in a text-Doc )

Then I exported the drills as a gerber and imported to protel on a mech
layer. With global change it was possible to add a hole of the same size
then the pad on this layer.

Now I can make the post processes and even make minor changes on this pcb.


--> If anybody wants the program, please let me know, it's free.


Georg

> -----Urspr ngliche Nachricht-----
> Von: Abd ul-Rahman Lomax [mailto:[EMAIL PROTECTED]]
> Gesendet: Freitag, 19. Oktober 2001 07:57
> An: Protel EDA Forum
> Betreff: Re: [PEDA] imported Gerber info missing
>
>
> At 03:40 PM 10/18/01 -0600, Colby Siemer wrote:
> >Ted,
> >
> >The reason Protel will not import the gerber properly is
> because of the way
> >the DCodes are done in the CAMTastic version being used.
> >
> >Protel needs to have the DCode listed each time, it does not
> assume the last
> >used DCode if it is missing.  CamTastic only lists it one
> time until the
> >code changes then it lists it again.
>
> Note that this refers to the D-Code for flash or for draw,
> which is D01 or
> D02, I forget which is which. The line format, at least the
> usual one, is
>
> X[x1]Y[y1]Dnn*
>
> where x1 and y1 are integers formatted according to the
> settings. When you
> want to examine a file, it can be useful to set zero
> suppression to none,
> so every coordinate will be the same length. That makes it
> easy to set up
> field in a database.
>
> Anyway, the RS-274 standard is that a parameter remains the
> same unless it
> is changed. So if you have, for example, two points with the same X
> coordinate, you could draw a line between the two without
> having to specify
> the X coordinate twice. Protel reads this correctly.
>
> The same thing is true for the D-codes which specify the
> aperture. One does
> not have to specify the aperture over and over again, it
> simply remains
> what it was when it was last set.
>
> It had never occurred to me that the D-command at the end of
> the line would
> be the same way. But it is. A line like
> X[xvalue]*
> will either draw or flash depending on the last used D-code.
> The asterisk
> is sufficient in that case. (CR/Line Feed is irrelevant to
> Gerber code as I
> recall, but it is usually used, makes it much easier to read!
> And Protel
> might require it, I think.)
>
> I could not see any option in CAMtastic which would control
> this feature in
> the output. CAMtastic apparently assumes that it is
> universally known;
> indeed, it should be. It was an error for the Protel
> programmers to assume
> that imported gerber was Protel-generated. Yes, they might
> not have wanted
> to implement the full standard, but this item was trivial. It would
> probably take me about twenty minutes to write a program to
> restore the
> D-codes, and that is long because I haven't done any
> programming recently,
> and I tend to make lots of dumb mistakes.
>
> If someone has the time and inclination to write it, we could
> put up a
> utility to restore the missing D-codes. The algorithm is
> 1. read line, drop asterisk
> 2. parse D-code, save as X$
> 3. if no D-code, write previous X$ at end
> 4. add asterisk
> 5. write line
> back to 1 until file end.
>
>
>
> [EMAIL PROTECTED]
> Abdulrahman Lomax
> Easthampton, Massachusetts USA
>

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to