Gerber files
Gerber files for manufacturing layers (board outline, copper, masks, etc) should not contain any extra data,such as drawing borders, title blocks, comments.
The board outline file should be a closed, non-intersecting polygon which exactly defines the edges of the PCB. The polygon should preferably be represented as a Gerber (G36/G37) region, but may be represented as a series of draws (lines/arcs) where the start coordinate of each segment is exactly the same as the end coordinate of the previous segment. (If defined with draws, the line width is not critical. However, it should be small, preferably. 0.1 mm, to avoid confusion in the display.)
When generating Gerber files, try to use the following settings (where available):
| File format | Extended Gerber (RS-274X), preferably with Gerber X2/X3 extensions |
|---|---|
| Polygons (G36/G37) | Enabled |
| Multi-quadrant arcs | Disabled |
| Stroke width for filled areas (if unable to use polygons) | preferably at least 0.635 mm; avoid less than 0.150 mm |
| Unit | MM |
| Number format | at least 3.5; 4.6 (or 6.6) is best |
| Zero Suppression | Leading |
All Gerber files must have the same origin. If you generate Gerber files with INCH units, you should use at least 2.4 (preferably 2.6) as the number format.
If possible, include the Gerber X2 "File function" attribute in each file.
Drill files
When generating Drill files, try to use the following settings (where available):
| File format | Excellon, or preferably XNC |
|---|---|
| Include tool list | Enabled |
| Unit | MM |
| Number format | 3.3 |
| Decimal points | Included |
| Zero Suppression | Leading (i.e. trailing zeroes included) |
All drill files must have the same origin. Drill files should have the same origin as Gerber files. If you generate Drill files with INCH units, you should use 2.4 as the number format.
File naming
Macaos supports numerous filename conventions. The best to use are Protel/Altium, Eagle or OrCad conventions.
The Protel/Altium convention specifies the layer with the filename extension:
| Board layer | Filename extension |
|---|---|
| Board outline | .GKO (or .GM or .GML) |
| Drill through | .TXT |
| Copper top | .GTL |
| Copper bottom | .GBL |
| Solder mask top | .GTS |
| Solder mask bottom | .GBS |
| Legend (silkscreen) top | .GTO |
| Legend (silkscreen) bottom | .GBO |
| Paste mask top | .GTP (or .GPT) |
| Paste mask bottom | .GBP (or .GPB) |
| Inner layers (x=1-8 or y=2-9 for layers 2-9) | .Gx (or .GyL) |
| Inner ground plane (negative) layers (x=1-8 for layers 2-9) | .GPx |
Other files
If possible, include a Gerber Job file. This file will give additional information about your files, which layers they represent, and more.
