layout_default_rules module#
A board’s default layout rules, and tagged nets whose rules override them.
Rules sit at three levels, and each level has its own home:
Fab floors live on the substrate.
SampleSubstrate.constraintsholds the fabricator’s minimums (min_copper_width,min_copper_copper_spaceand the rest). They are limits, not choices: the rules below must not go under them, andcheck_against_fabrefuses a rule that would.Board defaults live on the
Design.layout_default_rules_designsets a 0.2 mm trace width for every trace (IsTrace), a 0.2 mm clearance between any two copper objects (IsCopper,IsCopper) and a thermal relief for every pad (IsPad).Rules on tags assigned to nets override the defaults at a higher priority.
PowerTagis assigned to the power net andGroundTagto the ground net, and a priority-2 rule gives the nets carrying either tag a 0.5 mm trace. Nets taggedPowerTagalso get a 0.3 mm clearance to any object.
The default relief is part of the defaults, not an extra. On jitx 4.6 a pad
that no thermal_relief rule matches is joined to its pour with no relief
at all: the pour meets the pad on every side. IsPad gives every pad a
relief, here four 0.25 mm spokes across a 0.25 mm gap. A relief rule at a
higher priority than the IsPad rule overrides it where it matches. Keyed
on a net tag, it relieves every pad on the net. Keyed on a tag on a pad, a
landpattern or a component, it picks out some of a net’s pads;
layout_thermal_classes shows such tags, one relief class per pad size.
Here GroundTag carries a width rule only, so the GND pads take the
IsPad relief.
The circuit has one power route, one signal route and two GND pads inside a
GND pour. GND is not routed, so the GroundTag width rule has nothing to
act on in this design. Measured on jitx 4.6:
the SIG route is 0.2 mm wide and the pour stops 0.21 mm from it, the default clearance plus 0.01 mm;
the VCC route is 0.5 mm wide and the pour stops 0.31 mm from it, the
PowerTagclearance plus 0.01 mm;each GND pad meets the pour through four spokes 0.25 mm wide across a 0.25 mm gap.
Here the tag rules’ values are also the larger ones, so these numbers alone do not show whether priority or the larger value decided. A separate run with the tag rules’ values set below the defaults (0.15 mm width and clearance) gave a 0.15 mm VCC route with the pour 0.16 mm from it: the higher-priority tag rule applied.
- DEFAULT_WIDTH = 0.2#
Trace width for any trace no tag rule covers, mm.
- DEFAULT_CLEARANCE = 0.2#
Clearance between any two copper objects, mm.
- RELIEF_GAP = 0.25#
Gap between a pad and its pour, mm.
- RELIEF_SPOKE = 0.25#
Width of each thermal spoke, mm.
- RELIEF_SPOKES = 4#
Spokes per pad.
- POWER_WIDTH = 0.5#
Trace width for power and ground nets, mm.
- POWER_CLEARANCE = 0.3#
Clearance from power copper to any other object, mm.
- check_against_fab(rules, fab)[source]#
Return
rulesunchanged, or raise if one goes under a fab floor.Widths are checked against
min_copper_width; clearances and relief gaps and spokes againstmin_copper_copper_spaceandmin_copper_width.- Return type:
- Parameters:
rules (list[DesignConstraint])
fab (FabricationConstraints)
- class TwoPad[source]#
Bases:
ComponentA fictional part: two 1 mm square pads 3 mm apart.
- reference_designator_prefix: str | None = 'U'#
Reference designator prefix for this component. This will be used to generate a unique reference designator for each component of the same type.
Note
This field is a required data point for matching components between builds. If this value changes (including changing from unset to set), it will be treated as a new component, even if nothing else changes.
- class DefaultRulesCircuit[source]#
Bases:
CircuitA VCC route and a SIG route through a GND pour, and two GND pads in it.
- class layout_default_rules_design[source]#
Bases:
SampleDesignThe circuit on the sample board, with the board defaults and the power and ground tag rules on the design.