Hey Ridgh!
Gerbers and NC's can be a little confusing the first time you
generate them, especially since Protel likes to spit out a lot of
ultimately superfluous files at the same time. In regards to what your
board house actually needs, here is an example of a 4 layer board's
output as provided to our board house, with text annotations as to what
the files are.
'NC Drill Output'
'OST3MR1B.TXT' generated -- ASCII format drill file
'OST3MR1B.DRL' generated -- binary format drill file
'OST3MR1B.DRR' generated -- drill report, detailing the tool
assignments, hold sizes, hole count, and tool travel
'Gerber Board Data'
'OST3MR1B.APR' generated -- D-codes / Tool list
'OST3MR1B.GTL' generated -- Top Signal Layer Copper
'OST3MR1B.GP1' generated -- Power Plane 1 (GND) Copper
'OST3MR1B.GP2' generated -- Power Plane 2 (+3.3V) Copper
'OST3MR1B.GBL' generated -- Bottom Signal Layer Copper
'OST3MR1B.GTO' generated -- Top Overlay Silkscreen
'OST3MR1B.GBO' generated -- Bottom Overlay Silkscreen
'OST3MR1B.GTS' generated -- Top Solder Mask
'OST3MR1B.GBS' generated -- Bottom Solder Mask
'OST3MR1B.GM1' generated -- Mechanical Layer 1 (contains the board
outline and dimensioning)
My board house (Advanced Circuits - 4pcb.com - check them out if you
are in North America!) asks for a README.TXT file inside the ZIP of
board file submissions for reference, so I generally keep a template
version around and then rename things as necessary for each new job
going out. Obviously some of these files may or may not be required
depending on your board specifications (such as 2 vs 4 layers, bottom
silkscreen, etc) but this list helps keep thing consistent and works as
a checklist for me to make sure everything is there.
Keep in mind that your board house will require a layer (GM1 -
General Mechanical Layer, in this case) which calls out the board
outline, dimensions, and any other important details that may be custom
to your job. Because the Gerber data format does not inherently include
information regarding the actual boundaries of the PCB you need to
generate this call-out manually. In addition, because of some nuances as
to how the gerber format works internally, there can be some confusion
as to the unit of dimensions the board is designed with, so doing length
callouts on the board layer (5500 x 2000 mils, for example) will allow
the board house to both identify the base units the file has been
outputted with, as well as use this data as a kind of "sanity checksum"
to ensure that the boards you are ordering indeed match the boards you
are submitting, by allowing their CAM department to quickly verify the
physical size of the PCB.
I hope this helps you out! The first time it can be a bit confusing,
but give it a few goes and it will seem like old hat! :D
Regards,
-- Matt
Ridgh wrote:
> Dear friends,
> I really wish to thank you all for the efforts, time spending and the
> extraordinary good will of all of you.
> I think I've succeeded, at last partially. I can see now all the layers I
> need (the Top and Solder mask) - and I wrote "partially" because there is a
> layer that I cannot see (maybe I'm not supposed to see) - the hole places. I
> got 8 files: .apr, .GD1, .GG1, .GM1, .GTL, .GTS, .REP and .RUL
> The only one which I cannot see I Camtastic (I'm getting a black screen) is
> the .apr file.
> I really appreciate all you've done for me :)
> As my local time is now 2:30AM, and I'm near my PC about 12 hours... I think
> I'll have to "retire" for several hours.
> If you may have any ideas about the .apr file - I'll be very thankful of
> course.
> Sincerely yours,
> Ridgh
>
> -----Original Message-----
> From: Brad Velander [mailto:[EMAIL PROTECTED]
> Sent: Thursday, June 28, 2007 12:24 AM
> To: Protel EDA Discussion List
> Subject: Re: [PEDA] Need help to convert .pcbdoc to Gerber files
>
> Ridgh,
> Having read all the previous comments, I can't help think that you
> are just confusing the Camtastic CAM file display. Yes the Camtastic cam
> file is a composite of all your Gerbers. It displays each Gerber file as one
> layer and each layer should align directly over it's counterparts. In that
> way it is a composite view but it is not a composite Gerber file. Each layer
> is a different Gerber file all read into the Camtastic viewing window to
> show an overlaying view of all layers.
>
> For each layer (Gerber file) you can set different colors. That way
> you can see the different layers just as you would in the actual PCB design
> tool.
>
> While the files are Camtastic you could regenerate the Gerber again
> from what is viewed on screen and export them to another directory. That
> would be kind redundant unless you changed/edited them in Camtastic, because
> the originals that were read into Camtastic are already in your directories
> somewhere as others had indicated already.
>
> Hope this is what was confusing you, seemed like a possibility from
> what I had been reading.
>
> Sincerely,
> Brad Velander
> Senior PCB Designer
> Northern Airborne Technology
>
>
> -----Original Message-----
> From: Ridgh [mailto:[EMAIL PROTECTED]
> Sent: Wednesday, June 27, 2007 4:27 PM
> To: 'Protel EDA Discussion List'
> Subject: Re: [PEDA] Need help to convert .pcbdoc to Gerber files
>
>
> Thank you Dave,
> I did exactly what you said, and all I got is the composite .cam file in
> Camtastic. No drilling, just a nice but useless picture.
> I'm sure I'm missing something - but have no idea what....
> Regards,
> Ridgh
>
>
>
> ____________________________________________________________
> You are subscribed to the PEDA discussion forum
>
> To Post messages:
> mailto:[email protected]
>
> Unsubscribe and Other Options:
> http://techservinc.com/mailman/listinfo/peda_techservinc.com
>
> Browse or Search Old Archives (2001-2004):
> http://www.mail-archive.com/[EMAIL PROTECTED]
>
> Browse or Search Current Archives (2004-Current):
> http://www.mail-archive.com/[email protected]
>
>
>
>
>
> ____________________________________________________________
> You are subscribed to the PEDA discussion forum
>
> To Post messages:
> mailto:[email protected]
>
> Unsubscribe and Other Options:
> http://techservinc.com/mailman/listinfo/peda_techservinc.com
>
> Browse or Search Old Archives (2001-2004):
> http://www.mail-archive.com/[EMAIL PROTECTED]
>
> Browse or Search Current Archives (2004-Current):
> http://www.mail-archive.com/[email protected]
>
>
>
____________________________________________________________
You are subscribed to the PEDA discussion forum
To Post messages:
mailto:[email protected]
Unsubscribe and Other Options:
http://techservinc.com/mailman/listinfo/peda_techservinc.com
Browse or Search Old Archives (2001-2004):
http://www.mail-archive.com/[EMAIL PROTECTED]
Browse or Search Current Archives (2004-Current):
http://www.mail-archive.com/[email protected]
