Rules

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

Syntax

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

Description

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

Rule Statement	Description
`min-copper-width`	Minimum size of a copper feature on a `geom`.
`min-copper-copper-space`	Minimum distance between copper features on the same layer.
`min-copper-hole-space`	Minimum distance from a hole or cutout feature to a copper feature on any layer.
`min-copper-edge-space`	Minimum distance from the edge of the board to a copper feature on any layer.
`min-annular-ring`	Minimum size of the annular ring around a hole or via.
`min-drill-diameter`	Minimum diameter of a hole, either in a pad or via.
`min-silkscreen-width`	Minimum size of a silkscreen feature.
`min-pitch-leaded`	Minimum distance between pad centers of a leaded component.
`min-pitch-bga`	Minimum distance between pad centers of a BGA component.
`max-board-width`	Maximum size of a board in the `x` direction.
`max-board-height`	Maximum size of a board in the `y` direction.
`min-silk-solder-mask-space`	Minimum distance between silkscreen and solder mask features.
`min-silkscreen-text-height`	Minimum height of text on silkscreen layers.
`min-pth-pin-solder-clearance`	Minimum distance between a through hole pad and solder mask.
`solder-mask-registration`	Minimum distance from the edge of a copper pad and solder mask feature.
`min-soldermask-opening`	Minimum size of a solder mask shape.
`min-soldermask-bridge`	Minimum distance between solder mask features.
`min-hole-to-hole`	Minimum distance between two holes in pads or vias.
`min-th-pad-expand-outer`	Minimum distance from the outer edge of a PTH pad's annular ring to any copper feature.

Statements

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

Statement	Description
`description`	Description
`name`	Name