Layouts

Places the schematic's footprints on the board and routes them.

name = "lna"
board = "lna"
schematic = "lna"

[[footprints]]
ref = "U1"
at = [13.0, 8.05]
rotation = 90                  # degrees, counter-clockwise
# side = "bottom"              # mirrors the footprint and swaps F./B. layers
label = { at = [9.9, 7.4], rotation = 90 }   # move the silk reference; size = 0.8, hide = true
# mlcc = false                 # this part is not a ceramic capacitor, over the footprint's `mlcc`
# locked = true                # `agentee place` never moves it

[[tracks]]
net = "RF_OUT"
layer = "F.Cu"
points = [[18.68, 10], [25.5, 10]]
# width = 0.36                 # default: the net class width

[[vias]]
net = "GND"
at = [7.2, 8.9]
# via = "std"                  # a [[vias]] name from the board, default the first class via
# count = 6                    # a row, like pads
# pitch = [1.2, 0]

[[fanouts]]                    # a via in every connected pad of a BGA
ref = "U3"                     # * and ? globs: ref = "*" with nets = [...] fans out every plane pad
# via = "bga"                  # or a list, the first reaching the pad layer; default the class vias
# skip_rings = 2               # leave the two outer rings for escape on the outer layer
# always = ["GND", "LVDS_*"]   # nets that get a via even in those rings, globs allowed
# skip = ["A1", "B7"]          # pads to leave alone
# skip_at = [[4.5, 3.0]]       # no via at these spots (the viewer adds one when you edit a via)
# nets = ["GND", "3V3"]        # only pads on these nets, globs allowed
# exclude = ["C2?", "J1"]      # refs to leave out when ref is a glob; a glob never
                               # matches test points, a probe pad keeps no via

[[stitching]]                  # ground vias wherever they clear every other net and silk text
net = "GND"
# via = "std"                  # default the net's first class via
# pitch = "2.5mm"              # grid pitch, or the spacing along a fence (default 1mm)
# outline = [[x, y], ...]      # default the board outline
# margin = "0.6mm"             # extra distance from the board edge
# fence = ["RF_*"]             # instead of a grid: a row either side of these nets' tracks
# offset = "0.5mm"             # fence row distance from the track centre, default just past
                               # the class coplanar gap
# skip_at = [[4.5, 3.0]]       # no via at these spots (the viewer adds one when you edit a via)

[[zones]]
net = "GND"
layers = ["F.Cu", "In1.Cu", "In2.Cu", "B.Cu"]
# outline = [[x, y], ...]      # default: the board outline
# clearance = 0.25             # default: the net class clearance
# priority = 1                # higher fills first; other nets' zones on the layer pour around it
# min_island_area = 2.0       # mm2; a piece touching one item of the net is kept only this big
# pad_connection = "relief"    # solid (default) | relief: pads of the net join the pour by four
                               # spokes across a gap, so they heat like a track-fed pad;
                               # none: the pour keeps its clearance from the pads. A pad's
                               # own zone_connect wins, and BGA balls (16 or more round SMD
                               # pads) stay solid, since spokes starve a ball of solder heat
# relief_tht_only = true       # relief on through-hole pads only, SMD pads solid (KiCad's
                               # thru_hole_only)
# relief_gap = "0.3mm"         # default: the zone clearance
# spoke_width = "0.3mm"        # default: the net class track width, at least min_width

[[cutouts]]                    # keep zones off an area, e.g. under an SMA centre pin;
                               # a hole through the board is [[outline.cutouts]] in the board file
layers = ["In1.Cu"]
points = [[0, 9], [5.4, 9], [5.4, 11], [0, 11]]

[[graphics]]                   # board text and lines, same keys as footprint graphics
kind = "text"
layer = "F.SilkS"              # F.SilkS, B.SilkS, F.Fab or B.Fab
at = [7.4, 7.6]
# locked = true                # `agentee place` never moves it
text = "RF IN"
size = 1.0                     # mm, the fab minimum is in the board rules

[[artwork]]                    # a filled logo or icon
layer = "F.SilkS"
icon = "arrow"                 # built in: arrow, warning, ground, antenna, lightning, pin1, ce
# file = "logo.svg"            # or any SVG, relative to this file
at = [7.4, 6.3]                # centre of the artwork
height = 0.8                   # mm, the width follows the aspect ratio
# rotation = 90

[test]                         # in-circuit and flying probe test access, all optional
# nets = ["3V3", "*RST*"]      # nets that need a probe, globs, any case; default below
# exclude = ["LED_*"]          # nets to leave out
# side = "B"                   # probe side, F or B
# through_holes = true         # exposed plated through-hole pads count as access
# vias = false                 # vias count as access; opens the probe side mask over every via
# min_test_pad = "1.0mm"       # smallest test pad
# min_test_pad_pitch = "1.27mm"   # centre to centre between test pads
# min_test_pad_to_body = "1.0mm"  # to another part's body on the probe side
# min_test_pad_to_edge = "3.0mm"  # to the board edge and tooling holes

[place]                        # optional, for `agentee place`
# edges = { J1 = "left", J2 = "right" }   # pin a connector to an edge: left, right, top
                               # (smallest y) or bottom
# keepouts = [[[0, 0], [8, 0], [8, 6], [0, 6]]]   # polygons no courtyard may enter

[watermark]                    # optional: where the agentee version watermark goes
# at = [30, 21]                # centre of the text, default a clear spot found by check
# layer = "B.SilkS"            # default B.SilkS, else F.SilkS
# rotation = 90                # default 0, or 90 where only a tall gap is clear

Every layout carries silk text agentee vX.Y.Z-HASH: the version of the agentee that built the package and the short git hash of its source, with -dirty when the tree had uncommitted changes, or unknown outside git. It is always plotted and cannot be turned off. It is min_silk_text_height tall, centred, and by default goes on B.SilkS (F.SilkS when the bottom has no room or the board has no bottom silk) at the clear spot nearest the board's bottom left corner, rotated 90 degrees if only a tall gap fits. A clear spot keeps off pads, vias, other silk text and lines, artwork and part bodies, and stays min_copper_to_edge inside the outline. The viewer, render and assembly drawings show it, and fab-notes.txt names it. When no spot is clear, check reports a watermark error with the size to clear and the least crowded spot, and fab refuses; clear room there or set [watermark] at (plus layer, rotation) yourself. A [watermark] spot that is not clear is a watermark error naming what it hits, and a stackup with no kind = "silk" layer is a watermark error asking for one.

Test access: by default the nets that need a probe are power nets (a class with current, or a name like 3V3, 1V8, +5V, VCC*, VDD*, VBUS*, VBAT*, VIN*, VSYS*), ground (GND, *GND, GND*) and nets named like *RST*, *RESET*, *EN*, *PG*, *CLK*, *TX*, *RX*, *SCL*, *SDA*, *SWD*, *TCK*, *TMS*, *TDI*, *TDO*. The defaults leave out switch nodes and regulator feedback, soft-start and noise-reduction nets (SW*, *_SW, LX*, FB*, SS*, NR*, matched on the whole name or its last / segment), even when their class is power: a probe's capacitance and the stub to the pad couple switching noise into a feedback divider or slow a soft-start or noise filter, and a stub on a switch node radiates. nets replaces that list (name such a net there to probe it anyway) and exclude takes nets out of it. A test point is a part with a reference TP and a number, or a footprint named TestPoint*; like every part it must be in the schematic. The built in TestPoint_Pad_D1.0mm footprint (a 1.0 mm round SMD pad, mask open, no paste) and TestPoint symbol are written into footprints/ and symbols/ by agentee testpoints.

agentee testpoints NAME --nets "3V3,*RST*" [--side B] [--pitch 2.54] (MCP testpoints) adds a test pad to each matching net that has no probe access yet (nets are the [test] defaults when --nets is left out, impedance and pair nets are skipped): it looks on the probe side for a free spot on a --pitch grid near the net's copper, keeping min_test_pad_to_edge from the edge and tooling holes, min_test_pad_to_body from part bodies, --pitch from other test pads, and the net clearance from other copper and from the pads, stubs and vias it placed for other nets. It adds a TP part joined to the net to the schematic sheet that names the net, a [[footprints]] entry on the probe side to the layout with a short stub track to a via beside the pad, then routes each new pad to the net's copper with the autorouter and appends those tracks and vias. A pad the router cannot join is taken out of the schematic and layout again and listed with the nets that found no spot. Labels of the new pads are moved to a clear spot or hidden, and when the layout stores zone fills they are refreshed as agentee fill would. --dry-run reports the spots without writing.

Silk text must keep 0.4 mm from other silk text and 0.2 mm from silk outlines, stay off pads, vias and other parts' bodies, and stay on the board. Each of these is an error, except text under another part's body, which is a warning. When a reference label fails, check names a spot that passes every rule, as a label = { at = [...] } line to paste. agentee silk NAME (MCP silk) pastes them all for you and repeats until the labels settle; --hide hides the references that have no clear spot, typically small passives under a BGA.

A fill piece is kept only if it touches two items of its net, or one and is at least min_island_area; the rest reach nothing new and are removed. Check verifies every fill against other nets: a fill that overlaps another net's zone, track, via or pad, or comes closer than the clearance, is an error, and copper tips sharper than 30 degrees are flagged.

Zones on the same layer fill in order of priority, then smallest first, and each keeps its clearance from the fills already placed, so a small switch-node or supply pour inside a board-wide ground pour is poured around rather than shorted to it.

Pours keep min_via_hole_to_copper from other nets' via holes and min_npth_to_copper from non-plated holes as well as the clearance, with arcs drawn outside the true circle so the gap is never short. Stitching vias go only where the via clears every other net's copper on each layer it spans, keeps its hole min_via_hole_to_copper from that copper and min_hole_to_smd_pad from SMD pads of any net, keeps min_hole_to_hole from every drill and the edge rule from the outline, and lands inside a zone of its net; check reports how many it placed. They are drilled and plotted like any via.

Zone fills are exact polygons: the zone outline less every other net's copper grown by its clearance, with round corners, so pours render and plot without stair steps. Necks and slivers narrower than the zone's min_width (default 0.25 mm) are removed, the way a fab would etch them. Where two clearance areas (antipads, track and pad clearances) come closer than min_width, the pour is cut back to the straight lines joining them, within about 1.5 min_width of the gap, so no stub or hairline waist is left pointing into it. The same holds between a clearance area and the board edge's clearance, a cutout, or the clearance around another zone's fill.

Zone fills are cached: each fill is keyed by a hash of everything it depends on and kept in ~/.cache/agentee/fills, so a load only fills the zones whose copper, clearances or neighbours changed (set AGENTEE_NO_FILL_CACHE to skip the cache). agentee fill NAME (MCP fill) also stores the fills at the end of the layout file, one [[fills]] table per zone and layer, so a fresh checkout loads without filling; a stored fill whose hash no longer matches is ignored, and check notes it with --info. Importing a board stores its fills. Leave the [[fills]] tables to the tool.

A track that only grazes a pad (its centre line misses the pad) is flagged; run it into the pad. Two segments of one net that lie on top of each other on a layer (parallel, overlapping by more than a track width) are an error, since the copper is doubled; a bend sharper than 90 degrees is flagged as an acid trap. A track may neck down below its class width, to no less than the fab minimum, for up to 0.5 mm (the class neckdown) where it meets a small pad; the router draws such necks itself (see Autorouting). Drilled holes, vias and plated pads alike, must keep the board's min_hole_to_hole apart; check counts the pairs that do not and names the first. Two vias of one net at the same spot are an error too: the fab would drill the hole twice. Mask openings are the pad outlines, with no expansion, and vias are tented. Two openings of different nets (or no net) that overlap or leave a mask web under min_mask_web are an error, counted per part pair with the first place named. Pads of one fine pitch part are checked too: fix it in the footprint with narrower pads, or set a smaller min_mask_web when the fab allows it. A footprint with mask_web = false has its mask opened as one window over its pads (a gang opening), so pairs of its own pads are skipped; its pads are still checked against other parts.

Artwork on a bottom layer is mirrored so it reads correctly from below. SVG fills and strokes are flattened to polygons; text in an SVG is ignored, so convert it to paths first. Silk text and artwork get the same checks as reference labels: overlap, pads, silk outlines, board edge.