Gerber files

[pawihte]

I've been designing and making PCBs for my own use for almost 40
years now. The few times I needed more than a couple of units, I
had the pattern printed by local silk-screen printers. It's only
recently that it has become practicable to outsource them from
where I live in a remote location in India (I still have to send
them off to distant cities).

I used to design on graph paper, then with Amiga painting
programs, and now with CircuitMaker 2000 for the past 8 years. As
I always made my own PCBs, I never bothered with gerber files
before. When I generate the Gerber files, I get 5 files with
..Apt, .GBL, .GTL, .GTO, and .MAT extensions; and 3 more for the
drill files with .DRL, .TOL and .TXT extensions. All except the
..DRL are text files.

My question is: Do I send all eight files along with the main
pattern file to the PCB people? I know I should discuss it with
them (including whether they can use CircuitMaker 2000 designs),
but I wanted to have some background information first.

Thanks in advance.

 

[Herman]

"pawihte" <pawihte@invalid.com> wrote in message
news:hdr2c0$8sm$1@news.eternal-september.org...

I've been designing and making PCBs for my own use for almost 40 years
now. The few times I needed more than a couple of units, I had the pattern
printed by local silk-screen printers. It's only recently that it has
become practicable to outsource them from where I live in a remote
location in India (I still have to send them off to distant cities).

I used to design on graph paper, then with Amiga painting programs, and
now with CircuitMaker 2000 for the past 8 years. As I always made my own
PCBs, I never bothered with gerber files before. When I generate the
Gerber files, I get 5 files with .Apt, .GBL, .GTL, .GTO, and .MAT
extensions; and 3 more for the drill files with .DRL, .TOL and .TXT
extensions. All except the .DRL are text files.

My question is: Do I send all eight files along with the main pattern file
to the PCB people? I know I should discuss it with them (including whether
they can use CircuitMaker 2000 designs), but I wanted to have some
background information first.

Thanks in advance.
I also have been making my own boards for 40 years now and have been using
CircuitMaker 2000. For production quantity I use http://www.pcbcart.com
I send them all of the files and they use what they need. They are not
expensive and ship world wide in 10 days.

 

[John Larkin]

On Mon, 16 Nov 2009 13:56:33 +0530, "pawihte" <pawihte@invalid.com>
wrote:

I've been designing and making PCBs for my own use for almost 40
years now. The few times I needed more than a couple of units, I
had the pattern printed by local silk-screen printers. It's only
recently that it has become practicable to outsource them from
where I live in a remote location in India (I still have to send
them off to distant cities).

I used to design on graph paper, then with Amiga painting
programs, and now with CircuitMaker 2000 for the past 8 years. As
I always made my own PCBs, I never bothered with gerber files
before. When I generate the Gerber files, I get 5 files with
.Apt, .GBL, .GTL, .GTO, and .MAT extensions; and 3 more for the
drill files with .DRL, .TOL and .TXT extensions. All except the
.DRL are text files.

My question is: Do I send all eight files along with the main
pattern file to the PCB people? I know I should discuss it with
them (including whether they can use CircuitMaker 2000 designs),
but I wanted to have some background information first.

Thanks in advance.

We produce a pcb fab drawing, showing the pcb outline dimensions,
stackup, materials notes, solder mask and silk colors, all that sort
of stuff, and make a PDF of that. We email that, zipped along with all
the Gerber files, to the pcb house, and they seem to be able to figure
it out.

Our Gerbers have file names like

art001.pho layer 1 nc stuff
art001.rep layer 1 aperatures
drl001.drl drill locations
drl001.rep drill size/speed/feed data

and so on for silks, solder masks, etc.

John

 

[George Herold]

On Nov 16, 3:26 am, "pawihte" <pawi...@invalid.com> wrote:

I've been designing and making PCBs for my own use for almost 40
years now. The few times I needed more than a couple of units, I
had the pattern printed by local silk-screen printers. It's only
recently that it has become practicable to outsource them from
where I live in a remote location in India (I still have to send
them off to distant cities).

I used to design on graph paper, then with Amiga painting
programs, and now with CircuitMaker 2000 for the past 8 years. As
I always made my own PCBs, I never bothered with gerber files
before. When I generate the Gerber files, I get 5 files with
.Apt, .GBL, .GTL, .GTO, and .MAT extensions; and 3 more for the
drill files with .DRL, .TOL and .TXT extensions. All except the
.DRL are text files.

My question is: Do I send all eight files along with the main
pattern file to the PCB people? I know I should discuss it with
them (including whether they can use CircuitMaker 2000 designs),
but I wanted to have some background information first.

Thanks in advance.

Your best bet is going to be to contact the board house that will be
making the PCB's. See if they know the software you are using. Some
software mirrors the boards before making the Gerbers and this has
caused me mistakes in the past. (At some point I resorted to writing
"dummy" text in copper to make sure everything was as it should be.)
Also ask the board house which files they want and how to designate
them.

George H.

 

[pawihte]

pawihte wrote:

I've been designing and making PCBs for my own use for almost
40
years now. The few times I needed more than a couple of units,
I
had the pattern printed by local silk-screen printers. It's
only
recently that it has become practicable to outsource them from
where I live in a remote location in India (I still have to
send
them off to distant cities).

I used to design on graph paper, then with Amiga painting
programs, and now with CircuitMaker 2000 for the past 8 years.
As
I always made my own PCBs, I never bothered with gerber files
before. When I generate the Gerber files, I get 5 files with
.Apt, .GBL, .GTL, .GTO, and .MAT extensions; and 3 more for the
drill files with .DRL, .TOL and .TXT extensions. All except the
.DRL are text files.

My question is: Do I send all eight files along with the main
pattern file to the PCB people? I know I should discuss it with
them (including whether they can use CircuitMaker 2000
designs),
but I wanted to have some background information first.

Thanks in advance.

Thanks for the replies. I couldn't reply earlier because I could
not log on to the eternal-september server.

One thing I gathered from your replies is that there doesn't seem
to be a universal standard for sending instructions and that it
pretty much depends on communication between PCB house and
customer. Is that correct?

 

[Peter Bennett]

On Tue, 17 Nov 2009 16:36:14 +0530, "pawihte" <pawihte@invalid.com>
wrote:

pawihte wrote:
I've been designing and making PCBs for my own use for almost
40
years now. The few times I needed more than a couple of units,
I
had the pattern printed by local silk-screen printers. It's
only
recently that it has become practicable to outsource them from
where I live in a remote location in India (I still have to
send
them off to distant cities).

I used to design on graph paper, then with Amiga painting
programs, and now with CircuitMaker 2000 for the past 8 years.
As
I always made my own PCBs, I never bothered with gerber files
before. When I generate the Gerber files, I get 5 files with
.Apt, .GBL, .GTL, .GTO, and .MAT extensions; and 3 more for the
drill files with .DRL, .TOL and .TXT extensions. All except the
.DRL are text files.

My question is: Do I send all eight files along with the main
pattern file to the PCB people? I know I should discuss it with
them (including whether they can use CircuitMaker 2000
designs),
but I wanted to have some background information first.

Thanks in advance.

Thanks for the replies. I couldn't reply earlier because I could
not log on to the eternal-september server.

One thing I gathered from your replies is that there doesn't seem
to be a universal standard for sending instructions and that it
pretty much depends on communication between PCB house and
customer. Is that correct?

To some extent.

There seems to be no standard for naming the gerber files, so I have a
standard "readme" file that I include with the Gerbers. It looks
something like:

=======================
[my contact info and PO # removed]

The following files are required for this job:
S0930_pcb.GTO Component side silkscreen photoplot file
S0930_pcb.GTS Component side solder mask photoplot file
S0930_pcb.GTL Component side copper photoplot file
S0930_pcb.GBL Solder side copper photoplot file
S0930_pcb.GBS Component side solder mask photoplot file
S0930_pcb.GBO Component side silkscreen photoplot file
S0930_pcb.TXT Drill file
readme.txt This file


Note: the Gerber files include embedded aperture data.

Drill Information

Tool Hole Size Hole Type Hole Count Tool
Travel
---------------------------------------------------------------------------
T1 25mil (0.635mm) Round 2 7.80 Inch
(198.15 mm)
T2 35mil (0.889mm) Round 51 28.56 Inch
(725.39 mm)
T3 40mil (1.016mm) Round 30 20.97 Inch
(532.61 mm)
T4 50mil (1.27mm) Round 3 6.56 Inch
(166.72 mm)
T5 55mil (1.397mm) Round 30 21.34 Inch
(541.92 mm)
T6 67mil (1.7018mm) Round 8 6.38 Inch
(162.15 mm)
T7 105mil (2.667mm) Round 2 7.20 Inch
(182.96 mm)
T8 180mil (4.572mm) Round 4 16.27 Inch
(413.20 mm)
---------------------------------------------------------------------------
Totals 130 115.08 Inch
(2923.11 mm)

Board Specifications:


This board is 6.00" x 4.00", +/-.010", 4 layers

..0625" nominal thickness, FR-4 material
1 oz or greater copper
Standard through-hole plating, standard white tin (or gold) plating on
exposed copper.
Standard gold plating on edge connector

Solder mask both sides (different masks)
Component Ident silkscreen on component side

Trim boards to outline on component side artwork

Please make at least 20 boards.

===========================

I expect that most board shops now expect RS274X (I think that's the
designation) Gerber files, which include aperture data.

The Drill Tool table is produced by my CAD program (Protel/Altium) -
not sure it is really required, as the tool information is in the
drill file.

Protel puts the layer name in the file extension - a system I used to
use called the files "layer1.ger, layer2.ger...").

Protel makes both an "EIA" drill file (which nobody understands) and a
plain text file - make sure you send the text file.

The Gerber files do not contain any information on the board outline
unless you put it there. I use a thin track (.005) to define the
outline. In Protel, I can put that on a mechanical layer, then ask
Protel to include that layer in all Gerbers.

--
Peter Bennett, VE7CEI
peterbb4 (at) interchange.ubc.ca
GPS and NMEA info: http://vancouver-webpages.com/peter
Vancouver Power Squadron: http://vancouver.powersquadron.ca