-
Notifications
You must be signed in to change notification settings - Fork 10
/
ss-front-panel.kicad_dru
133 lines (111 loc) · 4.44 KB
/
ss-front-panel.kicad_dru
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53
54
55
56
57
58
59
60
61
62
63
64
65
66
67
68
69
70
71
72
73
74
75
76
77
78
79
80
81
82
83
84
85
86
87
88
89
90
91
92
93
94
95
96
97
98
99
100
101
102
103
104
105
106
107
108
109
110
111
112
113
114
115
116
117
118
119
120
121
122
123
124
125
126
127
128
129
130
131
132
(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))
)