CRE2512-FZ-R001E-3 - Bourns
Public Made by Adomby adom
Metal strip current sense resistor 1 mOhm +/-1 %, 3 W, +/-50 ppm/C, AEC-Q200, 2512
| Name | Last updated |
|---|---|
| land-check.json | 1d ago |
| land-pattern-icon.png | 1d ago |
| land-pattern.png | 1d ago |
| README.md | 1d ago |
Land pattern check: CRE2512-FZ-R001E-3
The footprint on this page, R_2512_6432Metric_Bourns_CRE2512_CRE2512-FZ-R001E-3, is Bourns' recommended solder pad layout for CRE2512-R001 ~ R004:
two rectangular pads 3.1 mm long and 4.0 mm wide with a 1.3 mm gap, 7.5 mm overall
(datasheet p.1). KiCad's standard Resistor_SMD:R_2512_6332Metric was compared with it and not used, because it is drawn for a
thick film 2512 with narrow end terminals and differs from Bourns' land by much more than a placement tolerance.
Grey is the part body at its datasheet nominal size, teal is KiCad's IPC-7351 nominal 2512 copper and the dashed amber outline is Bourns' recommended land, the copper this page's footprint uses.
Numbers
| Dimension | KiCad R_2512_6332Metric | Bourns recommendation (used) | Difference |
|---|---|---|---|
| gap between lands | 4.700 mm | 1.30 mm | +3.40 mm |
| land length | 1.225 mm | 3.10 mm | -1.88 mm |
| land width | 3.350 mm | 4.00 mm | -0.65 mm |
| overall length | 7.150 mm | 7.50 mm | -0.35 mm |
Bourns' letters: L = gap between pads, B = pad length, A = pad width (Bourns letters).
Source: Bourns CRE2512 datasheet REV. 06/25, p.1 Recommended Solder Pad Layout, CRE2512-R001 ~ R004 (PDF).
Result
KiCad's pads are 1.225 x 3.35 mm with a 4.70 mm gap; Bourns asks for 3.1 x 4.0 mm with a 1.3 mm gap. The CRE2512-R001 terminals are 2.00 mm long (C, p.2), so their inner edges sit 1.2 mm from the centre: KiCad's pads start 2.35 mm from the centre and would leave more than 1 mm of each terminal off the copper, while Bourns' pads start at 0.65 mm and cover the whole terminal. The difference is material for a 3 W, 1 mOhm part (current path, heat spreading and the resistance seen between the sense points), so this page ships Bourns' land.
Bourns' drawing also shows where to take the measurement: the high-current copper trace on the outer end of each pad and a separate sensing trace leaving each pad from its inner edge. The footprint has two pads; route the two sense traces from the inner edges of pads 1 and 2 as drawn (a four-terminal Kelvin footprint variant is not provided here).
The footprint is written by provenance/tools/build.py; the drawing and land-check.json come from
provenance/tools/landcheck.py. KiCad's file is kept unchanged in ../provenance/kicad-reference/R_2512_6332Metric.kicad_mod.