PCB trace impedance (equations) don't seem to take into account frequency, I have (previously) been considering this to be a characteristic impedance i.e the distributed impedance of the line 'viewed' from a certain point on the line for a given frequency (but not sure if this is valid)
So is the PCB trace impedance an impedance or a resistance?
(Edits awkward wording)
So is the PCB trace impedance an impedance or a resistance?
It's both (short story)...
The difference between a cable and a printed circuit board track is length. Cables can be miles long but a PCB trace is likely to be no longer than a foot. At a foot length (300 mm), a signal frequency having this wavelength is about 1 GHz. However, we say in EE that anything approaching one tenth of a wavelength is starting to be significant hence, for a foot (300 mm) anything around 100 MHz or above is relevant to start thinking about characteristic impedance and, importantly anything seriously higher than 1 MHz is going to have a purely resistive impedance.
The general formula for a t-line is this: -
$$Z_0 = \sqrt{\dfrac{R + j\omega L}{G + j\omega C}}$$
As frequency rises beyond several hundred kHz, the \$j\omega\$ terms dominate and we get this: -
$$Z_0 = \sqrt{\dfrac{j\omega L}{j\omega C}} = \sqrt{\dfrac{L}{C}}$$
That formula is not related to frequency and it is also resistive.
Finishing off; any PCB t-line calculation won't bother thinking of anything other than resistive terms because it just won't be physically long enough to be a practical consideration.
Depends how the term "trace impedance" is being used. It may be used to mean the series impedance (primarily resistance) of the trace, which is important at high current.
Or it may be synonymous with characteristic impedance.
Context may help.
If the "impedance" is a fraction of an ohm, or the context is high DC currents, or you're working on a buck converter or motor driver, it means the trace resistance (thicker the trace, the lower the impedance). Nobody thinks about transmission line characteristics in a PSU; you usually want the lowest possible trace resistance - and inductance in switching circuits.
If the "impedance" is 50 or 75 ohms or close to these, or the context is an antenna input or an RF filter, then characteristic impedance (in which case the actual trace resistance will appear not as"impedance" but as transmission line "loss".)
Now, you haven't given us any of the context, so...
A PCB trace is a transmission line.
An ideal transmission line has a resistive impedance. A transmission line with loss will have an impedance so close to resistive that few people would treat it as anything but resistive.
On a real substrate, say FR4, the impedance of a real PCB trace will vary with frequency due to the dielectric constant and loss of the dielectric varying, and the resistance of the copper varying with frequency. In addition, if the trace is microstrip, then the amount of field in air and in the board will vary with frequency causing speed and impedance variations.
PCB trace impedance doesn't seem to take into account frequency
That’s not true at all. What about high speed circuits? Any interface with a differential pair, like PCIe or USB, will consider frequency for designing a trace.
I’m not a believer of “pure resistance”. As long as electromagnetism exists, there will always be impedance, even if the imaginary (e.g. inductance/capacitance) part of it is extremely tiny.
I think what you’re looking for is a microstrip, which is a type of transmission line for PCB board. They contain a trace, ground plane, and a dielectric substrate.
Altium has their own design guides specifically for traces and frequency.
PCB traces have resistance, and they have impedance. That is, a trace can act as a resistor, an inductor, and a capacitor. They are all three at once.
Resistance is independent of the frequency of the signals. The inductance and the capacitance of the trace are also (largely) independent of the frequency.
Resistance depends on the length and the cross section area of the trace.
Inductance depends on the length of the trace an how it is routed (curlicues make higher impedances.)
Capacitance depends on the length and the surface area of the trace, as well as the area of adjacent conductors - a wide trace over a ground plane has more capacitance to ground than a narrow trace crossing a narrow ground trace at right angles.
For a given trace, resistance, inductance, and capacitance are pretty well fixed and don't greatly change with the frequency of the signal.
Impedance, however, is frequency dependent.
That is inherent in the definitions of impedance for inductors and capacitors:
$$ Z_C = -\frac{j}{2 \pi fC}$$
$$ X_L = 2 \pi fL$$
The impedance of a trace is therefore dependent on the frequency of the signal traveling through it.
Any time you want to know the impedance of a trace, you must know the frequency of the signal.
Transmission lines (strip lines, microstrip lines, and all their other PCB relatives) play the inductance and the capacitance against one another to achieve an impedance that is mostly independent of the frequency of the signal. That's thevsame as the characteristic impedance of a coax cable, except you can design it to an impedance of your liking rather than what the cable manufacturer delivered.
If you look into the (simplified) equations used to design striplines, you will see that there are no frequencies involved.
This Analog Devices paper on striplines has a lot of examples.
There are no frequencies involved, just the dimensions and properties of the materials used.
The impedances designed into a PCB will be indepedent of the frequency to the extent that the material properties and the precision of the making allow it.
At extremely high frequencies, you do have to use different materials and probably different tooling. The principles remain the same, though.
