Gerber files
in [Basics]
|
Prev: $5,000 Retro Fit Hybrid Kit
Next: "6000 count" display?
From: Peter Bennett on 17 Nov 2009 20:10 On Tue, 17 Nov 2009 16:36:14 +0530, "pawihte" <pawihte(a)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 |