# What to think about when designing HF PCB's?

I am currently designing a small PCB in Eagle Cad that has a GPS 1PPS signal (one short pulse per second) as input. The pulsetime for the 1pss is something like 1us.

Ok, I know thats not super HF but still.

What are good design practises when designing PCB's for HF?

• Are curved corners of routes better then perpendicular?
• Is thicker routes better than thin or opposite?
• Groundplane = good?
• etc..
• Dave Jones' PCB design tutorial has lots of useful information. Commented Oct 15, 2010 at 10:06
• @Theodor, what is the rise time of the signal? This determines the spectral content more then then length of the signal. Commented Aug 21, 2011 at 1:25

Howard Johnson has a massive collection of high-speed digital design newsletters.

http://www.sigcon.com/pubsAlpha.htm

One of my favorites visibly demonstrates the return currents that darron mentioned. DC will flow in a straight line (the path of least resistance; a straight line on the ground plane), while AC will flow underneath the signal conductor (the path of least inductance; a mirror image of the signal path on the ground plane) So avoid having that return path cross a split plane, avoid having it cross too many other high-speed return paths, etc. Also, power planes can act like ground planes for a return path, and the return path can jump planes through a capacitor (remember, cap is a short to high frequencies); the return path always chooses the plane closest to the signal. http://www.sigcon.com/Pubs/news/8_08.htm

I believe there are other newsletters. For instance, 90 degree angles aren't really that bad; they merely add excess capacitance to the trace. At "regular" high speed frequencies, this is no big deal. But when you hit microwave, the parasitic capacitance can do you in. http://www.sigcon.com/Pubs/edn/bigbadbend.htm

Regarding trace size, this largely depends on your stackup. If you use a solid reference plane (ground or power!), then your trace impedance is a function of trace width and distance from the plane. If you don't care about the impedance, then trace size largely doesn't matter, as long as it's not too small. Unless you're trying to carry obscene amounts of current (amps?), in which case you need traces big enough that they won't melt!

Try to keep signal planes adjacent to reference planes. i.e. for an 6 layer board, signal layers 1 and 3 reference ground plane 2, and signal layers 4 and 6 reference power plane 4. If signal planes are adjacent, be careful that there are no long parallel runs that could induce cross-talk. This is less of a concern if there's a reference plane (although the return currents can still cross-talk, it's not as bad)

Keep clock traces and other strong sources of noise as far away from other traces as you can (I think the rule of thumb is 5x the trace width away for clocks and 3x for other switching signals).

Yeah, that's not really HF. Still...

Ground plane, definitely.

The one big thing about noise if you remember anything is to think in terms of current loops. All signals must have return current going back to complete a loop. All else being equal... the larger the area formed by the path of the signal and it's return current, the more noise you'll emit and receive. So, if you've got a signal with a ground wire half a foot away, you're going to be spitting out a lot of noise and coupling a lot of external noise onto your signal.

One major reason for ground planes is that they provide a very very close return path for the signal. Strangely, the HF components of return current tend to follow underneath the path of the signal trace and not just the straight path across a ground plane to the battery/input voltage.

If you think of minimizing noise in terms of minimizing return loops... then most other noise-reducing steps become self-explanatory if not self-evident. Like, you don't want to have a signal trace going across a big slot on ground plane if you can help it... since the return current will have to divert around the slot and create a larger return loop area. Putting traces on your ground plane can also cause problems for the same reason. You can do these things, you just need to try your best to route other signals in ways that don't cross them.

Vias are tricky. If you have a typical signal-ground-power-signal 4 layer board, then when you transition to the bottom layer through a via, then the HF components of the return current may have to detour to the closest decoupling capacitor in order to follow underneath the bottom layer signal trace on the power plane. So, put decoupling caps relatively near to any vias.

On cabling, twist the signal wires together with a ground wire. If you've got ribbon cable, alternate ground and signal. (Or ground-signal-signal-ground-signal-signal-ground-... so that a signal is always next to a ground)

Probably best to keep the high frequency signals as direct as possible. Place the IC/components you are going to feed the signal into right next to the input where possible.