Bare microphone-flex panel¶
just mic-flex-panel <fresh-output> builds a 74 × 96mm, 8-column × 2-row
array of the common mic flex. There are
16 identical boards per panel, all in the same component-side orientation.
This is for bare fabrication and hand reflow; Standard-PCBA sizing and assembly
BOM/CPL are outside this panel's scope. It includes the requested local fiducials.
The single-board circuit, layout, contacts and stiffeners are preserved.
Fabrication contract — corrected 2026-10-30¶
Authority: JLCPCB's flex panel design guide, updated 2026-10-19, and flex capabilities. Use standard two-layer 0.11mm yellow PI, 12µm copper per side, ENIG, with the existing 0.225mm rear PI tongue and mic supports. Quantity means panels; each delivered panel contains 16 mic flexes. No fabrication order is submitted.
| Feature | Saved panel |
|---|---|
| Overall outline | 74 × 96mm, above the 70 × 70mm minimum |
| Process edges | At least 5mm on all four sides |
| Board spacing | 2.5mm between columns, 4mm between rows |
| Retained carrier | Waste retained between interrupted laser cut lines; no clearance slots |
| Connections | Six solid bridges per unit: two 0.8mm in bare flex and four 1mm beside the mic PI support; 96 total |
| Tab positions | Both sides, 5.5mm behind the tip (0.8mm); 34.5mm and 38.5mm behind the tip (1mm) |
| Depanelisation | Cut the solid tabs; no mouse bites or V-cuts |
| Rail copper | Both sides, 0.3mm from laser edges, 1mm from fiducial copper and 0.5mm from tooling-hole edges |
| Tooling | Four Ø2mm NPTH, one near each corner |
| Global fiducials | Four Ø1mm on each side, Ø2mm coverlay openings, 3.85mm from an adjacent outer edge |
| Local fiducials | One Ø1mm front-side mark beside each board's neck, Ø2mm coverlay opening, no paste; 16 total |
| Orientation | Bottom-left tooling hole shifted 5mm right; fiducials shifted 10mm up along the left rail |
| PI artwork | 32 separate support pieces in pib_0.225.gbr, retaining all 16 acoustic openings |
The user's supplier diagrams distinguish the 0.8mm breakaway bridge width from the 0.8mm clearance slot around metal stiffeners. This panel has PI supports, so it uses interrupted cut lines throughout, with no routed/clearance moat, including around its stiffened ends. The plotted line width is not a slot or a prescribed laser kerf. The waste remains as a carrier until bridges are cut. It is not a rigid hotplate fixture: keep the acoustic ports open during reflow and use an appropriate external support.
Tabs are behind the mating tongue, preserving the tight 5.5mm tongue-width region. Cut them flush without bending or tearing the flex. The original 5.5 ±0.05mm tongue width and 0.30 ±0.03mm finished mating thickness still require supplier confirmation; ordinary outline tolerance is not enough. Request delivery with the waste carrier and tabs retained.
Reproduction and evidence¶
The root recipe stages a fresh single-board validation build, uses the installed
KiKit panel API for copying and net/reference renaming, and native geometry for
the flex-specific cut lines, bridges and copper rails. Konnect has no panelisation
operation. All edits are to build/ copies through supported APIs.
Saved readback checks the 16 copies' pad numbers/nets, tracks, vias, layers and orientations, panel size, local fiducials and acoustic/tooling drills. Unit ERC/DRC/parity and independent panel DRC must pass. Parsed Gerbers compare every unit's copper, coverlay, paste and PI against the standalone export and check acoustic openings. Unit ground-zone outlines are clipped so refilling the panel cannot spread copper into tabs or connect adjacent boards.
KiCad's substrate model cannot represent zero-width open slits as closed holes.
The saved PCB therefore has the outer rectangle on Edge.Cuts and the interrupted
laser paths on User.2 (Laser_slits). Native panel DRC checks that material model;
the CAM check additionally measures copper clearance to every slit. The export
plots User.2 and uses Gerbonara's Gerber merge API to include those paths in the
final mic-flex-panel-EdgeCuts.gm1, alongside the outer profile. A centreline
comparison rejects missing cuts, extra cuts or parallel outlines forming slots.
The panel DRC allowance is restricted to two isolated_copper warnings for the
deliberately unconnected scrap-rail zones, one per side. Electrical errors,
unconnected unit copper and any additional warning fail the build. KiKit does
not rename reference-specific custom-rule conditions; exported copper-to-laser
clearance is therefore also measured independently (at least 0.2mm), in addition
to unit and panel DRC. The standalone rear ground export reaches approximately
0.2005mm from the outline, despite the nominal 0.3mm custom-rule intent. Preserve
that measured geometry here: JLC's clearance guide
specifies 0.2mm for pours/routing. The ear profile's stricter 0.3mm floor is not
evidence that this mic export has 0.3mm everywhere. Panel rail copper is held
at least 0.3mm from the laser cuts as well as the outer outline.
kikit fab jlcpcb supplies the standard Gerbers/drills. A native export adds
pib_0.225.gbr; the Gerber job and fabrication.zip include it. Front/rear,
outline and paste SVGs accompany the generated panel project. The front paste
Gerber is the panel stencil artwork. No assembly BOM/CPL is generated for the
panel; those in unit/ describe the independent single-board validation only.
Source hashes are checked on success and failure; no source is restored over concurrent edits. A completion manifest is written only after validation. Supplier acceptance and physical soldering, connector fit and audio operation remain separate from these software checks.