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.
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.
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.
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?
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
ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here.
All logos and trade names are the property of their respective owners.