Can you give me a basic (approximate) formula for the inductance of a PCB trace as a function of trace geometry [in two conditions]?:
- Bare trace
- Trace over an adjacent plane
Thanks for any help.
Thanks for your interest in high-speed digital design.
I can't do the case of a "bare trace".
You have to stipulate the shape of the returning current path to calculate total inductance, because stray fields from the returning current interact with the outgoing trace to affect the overall result.
Assuming you have a trace running parallel to one or more solid plane layers, and further assuming that the trace has a uniform cross-section the inductance L (pH per inch) may be found from the trace impedance (Z0 ohms) and delay (DLY in units of ps per inch):
For a stripline trace embedded in a dielectric material, the delay equals 85*sqrt(Er) ps/inch, where Er is the relative permittivity of the dielectric (about 4.3 for FR-4 material).
This gives us a delay of 176 ps/inch for a typical FR-4 stripline.
For a microstrip trace exposed to air on one side, the delay in FR-4 is a little bit less (about 140 ps/inch).
A 70-ohm trace, with a delay of 140 ps/inch, yields about 10,000 pH/inch (10 nH/inch).
Approximations for the impedance, delay, inductance, and capacitance of microstrips and striplines, as a function of trace geometry, are reproduced in my book, High-Speed Digital Design ISBN:0-13-395724-1. Even more elaborate approximations are included in Brian Wadell's book, 'Transmission Line Design Handbook' ISBN: 0-89006-436-9.
Dr. Howard Johnson