Think about stray capacitance and inductance everywhere. Components and PCB layout.
Primary stray for chip resistors is shunt capacitance. RF chip resistors are thin film on low dielectric substrate with single sided solder pads. Normal thick film ceramic (high-k substrate) chip resistors with full end cap terminations are good for a couple tenths of pF shunt capacitance. PCB solder pads for chip resistor are worth a couple of more tenth of pF. Ground plane to component solder pad are worth a couple more tenths of pF.
PCB strays can hurt. Avoid ground plane behind chip solder pads.
Metal film leaded resistor are disaster for series inductance. They are often trimmed to value with a barber pole spiral laser cut which makes a lossy inductor.
@RCinFLA
OK, I get that leaded resistors are history for VH frequencies and that metal film resistors may the the worst of the pick.
"PCB strays can hurt. Avoid ground plane behind chip solder pads" I think this means I cannot have a continuous ground plane under a solder pad. Seems to rule out using double sided PCB for VHF attenuators?
enut11
To bring some subtlety to this -- the spiral cut isn't a problem, in and of itself. Consider the spiral itself: it can be analyzed as a helical waveguide. I don't pretend to know the inner workings of this myself, but the consequences are, it's a structure with impedance, velocity, all that -- just like any other transmission line. It's not an ordinary, well-behaved transmission line -- the impedance and velocity aren't constant with respect to frequency, it's dispersive. But we can still use a transmission line model over a modest range, or for that matter, reduce it to a low-frequency equivalent all the same!
Of note, helical waveguides and resonators typically have quite high impedances. While typical TL geometries are 50-150 ohms, helices can be 100s, even a few kohms.
So what does it mean for the transmission line to have resistance and impedance? If they're equal, it'll be very much a resistive element.
Therefore: spiral-cut resistors, of values close to their transmission line impedance, have the widest bandwidth (largest resistive range, from DC to cutoff). Lower values are inductance-dominant, and higher values are capacitance-dominant. And the drop in bandwidth is approximately the same ratio as the ratio of resistance to Zo.
Typical spiral-cut resistors have a sweet spot around maybe 50-300 ohms. That's partly driven by the size of the body over the ground plane, as well (assuming the PCB has one). Don't forget that the resistor's leads are usually welded to larger metal end caps, so an equivalent circuit (lowpass CLC) may be useful. (Fitting values to the equivalent is an exercise for the student..)
So, relating back to attenuators -- you'll find the best results come using resistors in this range. If you need to use other values, you may find it's worthwhile staging it instead.
As for SMT pads, be
very cautious about cutting grounds. Consider: pads are just more metal on the signal path. It's a transmission line segment, likely very much shorter than the wavelength of interest, so manifests as a stray capacitance or inductance as the case may be. The chip's body does the same, too. If your Zo trace width is thinner than the component/pad width, that component will have a lower impedance, or manifest as capacitance; else, inductance. The further off they are, the less flat bandwidth you will have, etc.
And the component forms a transmission line segment of known length. Is that enough to matter to your application? A few mm won't be sensible until GHz, don't worry about it. Or if you are up there, well,
do worry about it -- and consider using 0402s or smaller, or perhaps an integrated module that can offer better characteristics than board-level components can.
Removing ground under a trace or pad, increases the ground impedance, obviously; it acts as a series inductor. Be
very careful about putting anything near that opening, whether trace or component: it's a radiating source, a slot antenna (even if an electrically short one).
Or if you're on multilayer board, you can pour ground on bottom and cut it out in the middle, to give a higher substrate thickness. Do use a via fence along this, to keep the planes from forming patch or slot antennas.
Tim