Pv panel

PV panel Rev D — KiCad

Open pv_panel.kicad_pro with KiCad 10. The project contains the recovered schematic, routed PCB, project-local footprint libraries, and solar-module STEP model. Diode and connector models are embedded in the board and footprints.

The recovered schematic follows the routed PCB's six nets and eleven named components. The original free pads and mounting holes remain board-only items. Footprints are linked to the recovered symbols; their placed geometry is retained in individual project-local library variants.

Onshape exports

• exports/pv_panel_rev_D_presentation.step includes colored components, solar-cell detail, copper, pads, soldermask, and silkscreen.
• exports/pv_panel_rev_D_mechanical.step provides simpler board/component geometry.

Both files use millimeters and a board-centered XY origin. They reopen as valid OpenCascade shapes; an actual Onshape import has not been tested.

Geometry and assumptions

• Board outline: nominally 82.5 × 98 mm, with the original rounded corners.
• Mounting holes: four 3 mm drills at the original positions, spaced 76.2 × 91.6 mm.
• Board thickness: 0.41116 mm from the original layer stack. Confirm against physical hardware for precise fitting.
• Solar modules: nominal 70 × 23 × 1.2 mm bodies based on the ANYSOLAR product table, with an assumed 0.15 mm stand-off. Surface detail is illustrative; dimensions represent nominal geometry rather than a tolerance envelope.
• Original diode and connector bodies are retained as package representations; their geometry has not been certified against the fitted manufacturers' drawings.
• Screws, mating cables, and solder fillets are not modeled.
• D1, the through-hole diode, is mounted on the outside solar-cell face (F.Cu). The connector and surface-mount diodes remain on the inside face (B.Cu). Its legacy 3D body is raised by a 1 mm model Z offset to clear the nearest solar module. This is an assembly-height assumption to confirm against hardware; both diode holes and their net assignments are unchanged.

Recovery changes

Removed zero-length outline segments, repaired PV2 pad 1's net assignment, restored the original 10 mil zone clearance, refilled the ground zones, removed isolated copper and a tiny dangling track stub, and corrected through-hole paste settings and silkscreen collisions. Corner copper rings were reduced from 6.4 mm to 5 mm to satisfy the existing 0.5 mm edge-clearance rule; drill diameters, mounting centers, and the outline are unchanged.

The native schematic import had scale and connectivity defects, so the working schematic was reconstructed with standard KiCad symbols and checked against the PCB pin connectivity. The archived sources disagree on diode population: the older drawing omits D1 and labels CR1–CR5 as RBR1MM60ATR, while the PCB includes D1=SB140 and labels CR1–CR5 as STPS1L30MF. This project follows the PCB. Confirm the intended/fitted diode part numbers before fabrication.

Validation

The saved project passes KiCad DRC, ERC, and schematic parity with zero findings. All six nets match pin-for-pin across the eleven named components. Both STEP exports contain valid CAD shapes (58 solids for mechanical, 129 for presentation), and top/bottom renders were visually inspected. These checks cover the recovered design and mockup export; hardware qualification remains a separate activity.