Howard Johnson (of
High-Speed Digital Design fame) has an article on the ESL of 0402 and 0603 bypass capacitors. He used an interesting method to determine the parasitics - He assumed that it's caused by mostly layout and geometry, not components. This allowed him to avoid doing a delicate microwave VNA measurement or any computer simulation, instead, he made a huge metal block and measured that as a 100x scaled model
- a time-honored technique in engineering. As far as I know, his results are comparable with the numbers from E&M solvers. It's around 0.2-0.4 nH with optimal layout. For resistors the number should be similar.
http://www.sigcon.com/Pubs/news/6_09.htmBut practically, 100 MHz is really forgiving. For RF, you can easily get 20 dB return loss without doing any layout optimization. At a higher frequency like 1 GHz, if you don't have access to an E&M solver, the standard RF/microwave design procedure is basically trial-and-error: do a return loss or TDR measurement, tune the layout at the discontinuity, try again until satisfactory results are obtained.
The actual performance is greatly affected by the PCB stackup (mainly the distance between a trace and its ground plane), or the size of the mounting pad. In a 4-layer digital board, the pads are huge compared to a 50-ohm trace, thus there exists two strong capacitive discontinuities around the resistor, this is often performance bottleneck, not the ESL of the resistor. A ground plane cut-out under the pads is often used as compensation. In a classic two-layer PCB for microwave, the traces are much thicker, and the situation is a bit different. Also, sometimes there can be a measurable inductance reduction if the resistor is mounted up-side down because the resistive ink is closer to the ground plane.