A pcb-rules definition represents the set of design rules associated with a specific circuit board manufacturer.


pcb-rules bay-area-circuits-std-rules :
  min-copper-width = 0.127
  min-copper-copper-space = 0.127 
  min-copper-hole-space = 0.2032
  min-copper-edge-space = 0.381
  min-annular-ring = 0.1524
  min-drill-diameter = 0.254
  min-silkscreen-width = 0.0762
  min-pitch-leaded = 0.35
  min-pitch-bga = 0.35
  max-board-width = 457.2
  max-board-height = 609.6
  min-silk-solder-mask-space = 0.127
  min-silkscreen-text-height = 0.75
  solder-mask-registration = 0.106
  min-th-pad-expand-outer = 0.2032
  min-soldermask-opening = 0.152
  min-soldermask-bridge = 0.102
  min-hole-to-hole = 0.254
  min-pth-pin-solder-clearance = 3.0


All design rules are required to have a value. The supported design rules are :

Rule StatementDescription
min-copper-widthMinimum size of a copper feature on a geom.
min-copper-copper-spaceMinimum distance between copper features on the same layer.
min-copper-hole-spaceMinimum distance from a hole or cutout feature to a copper feature on any layer.
min-copper-edge-spaceMinimum distance from the edge of the board to a copper feature on any layer.
min-annular-ringMinimum size of the annular ring around a hole or via.
min-drill-diameterMinimum diameter of a hole, either in a pad or via.
min-silkscreen-widthMinimum size of a silkscreen feature.
min-pitch-leadedMinimum distance between pad centers of a leaded component.
min-pitch-bgaMinimum distance between pad centerss of a BGA component.
max-board-widthMaximum size of a board in the x direction.
max-board-heightMaximum size of a board in the y direction.
min-silk-solder-mask-spaceMinimum distance between silkscreen and solder mask features.
min-silkscreen-text-heightMinimum height of text on silkscreen layers.
min-pth-pin-solder-clearanceMinimum distance between a through hole pad and solder mask.
solder-mask-registrationMinimum distance from the edge of a copper pad and solder mask feature.
min-soldermask-openingMinimum size of a solder mask shape.
min-soldermask-bridgeMinimum distance between solder mask features.
min-hole-to-holeMinimum distance between two holes in pads or vias.
min-th-pad-expand-outerMinimum distance from the outer edge of a PTH pad's annular ring to any copper feature.


In addition to the set of supported design rules, pcb-rules may have some additional, optional statements.