AnsweredAssumed Answered

LAYOUT Gerber Export Settings

Question asked by ROB_LEFEBVRE on May 27, 2003
Since Gerber export is so popular, we are constantly improving the quality of the output.  With GENESYS 2003, you should have little or no problems with Gerber output provided that you are using the "274X" file format.

The Gerber algorithm is very complex, so sometimes the settings must be adjusted to see what works best. We usually recommend that:

1) 274X is turned on.
2) Resolve to polygons is turned off.
3) >RASTER SCAN< is checked.
4) Generate Custom Apertures is checked.

Curves are drawn as a series of line segments. The tolerance specifies the maximum deviation from the actual curve for these segments. Smaller numbers give better approximations but can cause mathematical underflows (and possibly erroneous Gerber objects) if it is set too small. The minimum polygon fill diameter is the minimum diameter or width a polygon must have before it is filled.

Another thing to watch out for is the Gerber viewer that you are using. Also, be aware that some Gerber viewers may be displaying gaps, spaces, errors, etc. that are not really there. If your viewer is suspect, we suggest that you try another one. We use GCPrevue here and it is freeware that is available on the web at

The simple fix, and a rule for us to remember, is to put the Polygon Fill Min. Aperture Diameter to 2. This allows the pen to fit, and you will get no gaps. You should also make sure that this number can be represented evenly in the gerber number format selected (3 trailing zeros gives 0.001 inch/1mil resolution, so don't set it to 0.25). Otherwise, round-off errors will result, and you may get small (0.1mil) gaps.

These recommendations should work on every file, as long as the tolerance is considerably smaller than the Min. Aperture Diameter and that the Aperture Diameter and number formatting are sufficient for the smallest feature on your board.

Another technique that will get rid of gaps, even if they are accidentally in your original layout, is to specify an etch factor of 1 mil. If your board is being etched, this will compensate for over-etching, and will remove any gaps of 2 mils or smaller.