component

HR911130A

Public Made by Adom

HANRUN(Zhongshan HanRun Elec) Modular/Ethernet Connector (RJ45) Jacks With Magnetics, Through Hole. KiCad symbol, footprint and 3D as used on Adom boards; pin functions from the manufacturer datasheet.

Verified HR911130A

by Claude, at Caleb Taylor's request · last 27 Oct 2026 · 1 record · files match

SymbolFootprint3D modelPins

Verification log 3 records

27 Oct 2026Claude, at Caleb Taylor's requestValidated against HanRun's HR911130A datasheet (Rev. B)files match

SymbolFootprint3D modelPinsfor all variants

✓Datasheet: replaced the JLCPCB copy with HanRun's own PDF, linked from the HR911130A product page on hanrun.com (https://www.hanrun.com/rj45_1000/203.html) and served from HanRun's file store; 4 pages, Rev. B (no date printed; PDF created 2020-02-28), retrieved 2026-10-27
•Datasheet text layer: HanRun's PDF draws the schematic and drawing labels as vector outlines, so the attached copy is the same 4 pages with an OCR text layer added (ocrmypdf 15.2 / tesseract 5.3) for the pin-name text check; the unmodified HanRun file has sha256 d3a5d7212145ea71b6f643d90478eac1cdb08ef26a191cac525d4ab7fb344ac1
✓All 14 numbered pins match the schematic (p.1) by number and name: P1, MDI 0+ P2, MDI 0- P3, MDI 1+ P4, MDI 2+ P5, MDI 2- P6, MDI 1- P7, MDI 3+ P8, MDI 3- P9, P10, LED pins 11-14; the page keeps MDI0+ etc. without the space the drawing prints between MDI and the pair number, with ASCII hyphens for the drawing's minus signs. No pin renamed
✓LED polarity from the schematic (p.1): green 11 anode -> 12 cathode, yellow 14 anode -> 13 cathode; green is the left LED and yellow the right LED seen from the front (p.2); 568/585 nm, VF 1.8/2.8 V, 20 mA (p.2)
✓All 16 descriptions rewritten from the datasheet. The old ones had wrong cable-side routing for pins 5, 6 and 7 (the schematic routes MDI 2+ to J4 C+, MDI 2- to J5 C-, MDI 1- to J6 B-) and described P1 as the termination return (P1 is the chip-side centre-tap common; P10 is the 4 x 75 ohm / 1000 pF 2 kV termination return)
•Shield pins S1/S2 are unnamed in the drawing (two 1.63 mm holes on the layout, p.3); the page keeps the name SHIELD
✓Footprint vs the recommended PCB layout (p.3, component side view): signal pins 1-10 on 0.89 mm drills at 1.27 mm stagger (2.54 mm within a row), rows 6.35 and 8.89 mm behind the post line, pin 1 at the right end of the rear row; footprint pads at x = +/-5.72, 4.44, 3.18, 1.90, 0.64 vs the drawing's 0.635-mm grid (5.715, 4.445, ...), within 0.005 mm; LED pins on 1.02 mm drills at 13.25 mm outer / 2.54 mm pairs, 4.90 mm in front of the post line; 3.25 mm NPTH posts 11.43 mm apart; 1.63 mm shield holes 15.49 mm apart, 3.05 mm behind the post line. Pin 1 position and LED order (14, 13 ... 12, 11 left to right) match
✓3D body vs the mechanical drawing (p.2, tolerance +/-0.25): 16.04 x 21.30 x 13.50 mm against B 16.00, A 21.20, C 13.30; front face 10.92 mm and rear 10.38 mm from the post line against 10.80 / 10.40 (p.3); Z-up, seated on z = 0, the model's 18 pins sit on the footprint's 18 holes
•3D pin tails reach 3.05 mm below the seating plane against D 3.50 +/-0.30 mm (p.2): 0.15 mm shorter than the minimum; body and footprint unaffected
•DigiKey and Mouser do not carry HR911130A (searched 2026-10-27); LCSC C54408 kept
✓Symbol and footprint Datasheet properties point at the manufacturer datasheet URL
✓Symbol Datasheet / MPN / Manufacturer / DigiKey / Mouser / LCSC properties agree with page.json; footprint Datasheet property points at the manufacturer datasheet URL
✓component-page-verify: all checks pass

Evidencedatasheet (HanRun, Rev. B)product page (hanrun.com)

Verified files✓ hr911130a.kicad_sym✓ hr911130a.kicad_mod✓ hr911130a.step

9 Oct 2026Claude (AI build)Datasheet text layer: the manufacturer drawing is a scanned image; the attached PDF is the...superseded

reviewfor all variants

•Datasheet text layer: the manufacturer drawing is a scanned image; the attached PDF is the same pages with an OCR text layer added (ocrmypdf/tesseract) so pin names can be checked against it.

9 Oct 2026Claude (AI build)Automated build checks (awaiting human validation)superseded

SymbolFootprint3D modelPinsfor all variants

✓Footprint extracted pad-for-pad from the source board and normalized to the footprint frame (back-side parts un-mirrored)
✓3D model seated z=0 at footprint origin (placement inverse; method centroid-matched to KiCad library models on 59 cases)
✓adom-lbr generate + lint passed
✓16 of 16 pins described from the datasheet (adom-ds2sf, page-cited)
•Not yet checked by a person: land pattern vs datasheet, pin-1/orientation, 3D body vs drawing

Evidencedatasheet

Verified files! hr911130a.kicad_sym! hr911130a.kicad_mod✓ hr911130a.step

Spot something wrong? Report it as an issue · Propose a fix Records are signed by members of adom.

Overview Files Discover Packages Releases Dependencies Issues Breadcrumbs Pull Requests Activity

← Commit history

Set visibility: public

Caleb ·73703248a3 ·1d ago ·parent 5b338d2

1 file changed +1−1

page.json+1−1

@@ -232,4 +232,4 @@   "visibility": {     "public": true   }-}+}\ No newline at end of file