Taiko-Nijiiro-Analog-IOBoard/PCB/Taiko IoBoard.kicad_dru
KIT! 7978c214ff Hard fork initial commit
This commit contains the kicad files for the PCB, the updated firmware for this new pcb design.
2024-04-30 17:13:14 +02:00

134 lines
4.4 KiB
Plaintext
Raw Permalink Blame History

This file contains ambiguous Unicode characters

This file contains Unicode characters that might be confused with other characters. If you think that this is intentional, you can safely ignore this warning. Use the Escape button to reveal them.

(version 1)
# Custom Design Rules (DRC) for KiCAD 7.0 (Stored in '<project>.kicad_dru' file).
#
# Matching JLCPCB capabilities: https://jlcpcb.com/capabilities/pcb-capabilities
#
# KiCad documentation: https://docs.kicad.org/master/id/pcbnew/pcbnew_advanced.html#custom_design_rules
#
# Inspiration
# - https://gist.github.com/darkxst/f713268e5469645425eed40115fb8b49 (with comments)
# - https://gist.github.com/denniskupec/e163d13b0a64c2044bd259f64659485e (with comments)
# TODO new rule: NPTH pads.
# Inner diameter of pad should be 0.4-0.5 mm larger than NPTH drill diameter.
# JLCPCB: "We make NPTH via dry sealing film process, if customer would like a NPTH but around with pad/copper, our engineer will dig out around pad/copper about 0.2mm-0.25mm, otherwise the metal potion will be flowed into the hole and it becomes a PTH. (there will be no copper dig out optimization for single board)."
# TODO: new rule for plated slots: min diameter/width 0.5mm
# JLCPCB: "The minimum plated slot width is 0.5mm, which is drawn with a pad."
# TODO new rule: non-plated slots: min diameter/width 1.0mm
# JLCPCB: "The minimum Non-Plated Slot Width is 1.0mm, please draw the slot outline in the mechanical layer(GML or GKO)""
(rule "Track width, outer layer (1oz copper)"
(layer outer)
(condition "A.Type == 'track'")
(constraint track_width (min 0.127mm))
)
(rule "Track spacing, outer layer (1oz copper)"
(layer outer)
(condition "A.Type == 'track' && B.Type == A.Type")
(constraint clearance (min 0.127mm))
)
(rule "Track width, inner layer"
(layer inner)
(condition "A.Type == 'track'")
(constraint track_width (min 0.09mm))
)
(rule "Track spacing, inner layer"
(layer inner)
(condition "A.Type == 'track' && B.Type == A.Type")
(constraint clearance (min 0.09mm))
)
(rule "Silkscreen text"
(layer "?.Silkscreen")
(condition "A.Type == 'Text' || A.Type == 'Text Box'")
(constraint text_thickness (min 0.15mm))
(constraint text_height (min 1mm))
)
(rule "Pad to Silkscreen"
(layer outer)
(condition "A.Type == 'pad' && B.Layer == '?.Silkscreen'")
(constraint silk_clearance (min 0.15mm))
)
(rule "Edge (routed) to track clearance"
(condition "A.Type == 'track'")
(constraint edge_clearance (min 0.3mm))
)
#(rule "Edge (v-cut) to track clearance"
# (condition "A.Type == 'track'")
# (constraint edge_clearance (min 0.4mm))
#)
# JLCPCB restrictions ambiguous:
# Illustration: 0.2 mm, 1&2 layer: 0.3 mm, multilayer: "(0.15mm more costly)"
# This rule handles diameter minimum and maximum for ALL holes.
# Other specialized rules handle restrictions (e.g. Via, PTH, NPTH)
(rule "Hole diameter"
(constraint hole_size (min 0.2mm) (max 6.3mm))
)
(rule "Hole (NPTH) diameter"
(layer outer)
(condition "!A.isPlated()")
(constraint hole_size (min 0.5mm))
)
# TODO: Hole to board edge ≥ 1 mm. Min. board size 10 × 10 mm
(rule "Hole (castellated) diameter"
(layer outer)
(condition "A.Type == 'pad' && A.Fabrication_Property == 'Castellated pad'")
(constraint hole_size (min 0.6mm))
)
# JLCPCB: "Via diameter should be 0.1mm(0.15mm preferred) larger than Via hole size" (illustration shows diameters for both dimensions)
# JLCPCB: PTH: "The annular ring size will be enlarged to 0.15mm in production."
(rule "Annular ring width (via and PTH)"
(layer outer)
(condition "A.isPlated()")
(constraint annular_width (min 0.075mm))
)
(rule "Clearance: hole to hole (perimeter), different nets"
(layer outer)
(condition "A.Net != B.Net")
(constraint hole_to_hole (min 0.5mm))
)
(rule "Clearance: hole to hole (perimeter), same net"
(layer outer)
(condition "A.Net == B.Net")
(constraint hole_to_hole (min 0.254mm))
)
(rule "Clearance: track to NPTH hole (perimeter)"
# (condition "A.Pad_Type == 'NPTH, mechanical' && B.Type == 'track' && A.Net != B.Net")
(condition "!A.isPlated() && B.Type == 'track' && A.Net != B.Net")
(constraint hole_clearance (min 0.254mm))
)
(rule "Clearance: track to PTH hole perimeter"
(condition "A.isPlated() && B.Type == 'track' && A.Net != B.Net")
(constraint hole_clearance (min 0.33mm))
)
# TODO: try combining with rule "Clearance: PTH to track, different nets"
(rule "Clearance: track to pad"
(condition "A.Type == 'pad' && B.Type == 'track' && A.Net != B.Net")
(constraint clearance (min 0.2mm))
)
(rule "Clearance: pad/via to pad/via"
(layer outer)
# (condition "(A.Type == 'Pad' || A.Type == 'Via') && (B.Type == 'Pad' || B.Type == 'Via') && A.Net != B.Net")
(condition "A.isPlated() && B.isPlated() && A.Net != B.Net")
(constraint clearance (min 0.127mm))
)