Skip to content

10 hardening on harder inputs

Before the tool meets real boards, the three places where real boards differ most from what had been tested.

Hierarchical schematic (dogfood/existing/hier/, KiCad's complex_hierarchy demo)

One sub-sheet used twice, so each of its symbols is two parts. - parts at first listed none of them: it read the "Reference" property, which holds one of the two references. References are now read from the symbol's instance list. - set R203 Value=33K says it also changes R303; KiCad's netlist shows both changed. remove R213 refuses, because it would remove R313 too. - set D101 and add C199 (copy of C104, VCC to GND) on the root sheet.

netdiff between KiCad's netlists: C199 added on VCC and GND; D101, R203 and R303 changed. Nothing else.

Router on a 6-layer board (KiCad's cm5_minima demo, read only)

Six two-pad nets that change layer, re-routed over F.Cu, In2.Cu, In3.Cu and B.Cu with each net's own class rules:

Net Result Original
nLED_ACTIVITY 8.5 mm, 1 via 10.2 mm
VBUS_EN 22.5 mm, 1 via 43.1 mm
nLED_SPEED_100_1000 failed after 84 s
ETH_nLED_ACTIVITY 30.5 mm, 2 vias, uses In2 31.3 mm
Net-(D702-K) 4.0 mm, 2 vias, uses In2 5.5 mm
PWM 32.3 mm, 2 vias, uses In2 33.2 mm

Every routed result keeps at least its class clearance (0.13 mm) from other copper by this tool's own geometry. Not checked by KiCad's DRC: the results were not written to a board. A failure now gives up in a bounded search instead of 84 seconds.

Per-net rules

The router read only the Default net class. It now takes each net's class from the project file, by explicit assignment (the Jetson demo) or by pattern (cm5_minima: /*USB_* -> 90ohm, 0.147 mm, 0.2 mm clearance). Rules that live in a .kicad_dru file are not read.

Also

A 9-layer, 22,151-track demo board loads and reports its net classes.

Left open

  • The 6-layer routes were not judged by KiCad.
  • .kicad_dru rules are invisible to the router and the review.
  • add on a sub-sheet; multi-unit parts.