Land pattern check: RC0603FR-073K65L

The footprint on this page is KiCad's standard library footprint Resistor_SMD:R_0603_1608Metric, renamed to R_0603_1608Metric_RC0603FR-073K65L so it can sit beside other parts in one library folder. The copper is unchanged. This page compares those pads with the land pattern YAGEO recommends for reflow soldering.

Grey is the part body at its datasheet nominal size, teal is the KiCad copper and the dashed amber outline is YAGEO's recommended land at its printed nominal size.

Numbers

YAGEO's letters: A = overall length, B = gap between lands, C = land length, D = land width (YAGEO letters). YAGEO's placement accuracy for this size: +/-0.25 mm.

Source: YAGEO Chip Resistors Mounting V.10, p.4 Table 1 (reflow), size 0603 (PDF).

Result

The KiCad pads differ from YAGEO's nominal land by up to 0.15 mm: KiCad's pads are 0.80 mm long and 0.95 mm wide (YAGEO 0.90 x 0.80 mm), so KiCad's copper is shorter and wider, and the overall length is 2.45 mm against YAGEO's 2.60 mm. The gap between pads differs by +0.05 mm. KiCad generates this footprint to IPC-7351 nominal density (its own description says so), not to YAGEO's table. Both lands cover the underside terminal (I2 0.25 +/-0.15 mm) with margin and both are usual reflow patterns. A design that wants YAGEO's exact land should make each pad 0.90 mm long and 0.80 mm wide with pad centres 1.70 mm apart.

KiCad pad centres are at +/-0.825 mm, pad size 0.80 x 0.95 mm, rounded rectangle (corner ratio 0.25). The numbers are in land-check.json; the drawing is made by provenance/tools/landcheck.py from the footprint file and YAGEO's table.