# How to calculate impedance of a PCB trace Antenna in Altium w.r.t. a given frequency?

I am keeping things abstract as I intend to learn and not just copy another design.

So, suppose I am trying to design an antenna of impedance Z and frequency f. Now, in Altium 18, there is a feature that suggests trace widths for a specified impedance. Now, what I fail to understand is :

1. how is that the impedance is not dependent on trace length and only on trace widths ?

2. how can Altium suggest a trace width without me specifying the frequency ?

I mean to calculate trace width from Impedance , one surely needs to know the working frequency . I guess, it is only taking resistance in consideration but then , that would depend on the length too?

3. Is there a way I can calculate Impedance between any two given points on a trace for a given frequency ? I want both the resistance and reactance to design matching .

4. If there is no such way in Altium(which I suspect), then how do people design Antennas these days ?

• I bet the answer to this question fills textbooks because it's too general. You might want to choose a simple antenna type and find a design guide or ask questions relative to it. PCB trace antenna narrows it down some but I bet there are still multiple shapes. Also is the feature you describe suggesting trace widths for antennas or just in general? If they're just looking at trace width and not frequency they might be estimating resistive impedance. – K H Jan 28 at 5:17
• I think the Altium feature you describe is related to transmission line impedance which is Independent of trace length. There surely are better design tools for antenna design, e.g. keysight ADS where you can perform simulations. – Lars Hankeln Jan 28 at 5:35
• Thanks @KH ! If you will focus on the questions that are in the body and not in the title, I guess the answer will be a bit shorter. I am more interested in the impedance, reactance and resistance of traces in my question for given frequencies in pcbcad softwares for a given layer stackup than the antenna shapes. i guess that will narrow down the answer a bit too. Also, the feature is for trace widths in general. – Curious Cosmopolitan Jan 28 at 5:44
• Thanks @LarsHankeln ! Does the tool you mention takes care of the layer stackup, crosstalk etc. too ? I mean , does it import the pcb layout ? If not, then is it a general practice to design antenna in some antenna design tool and then use the design in a pcbcad software ? – Curious Cosmopolitan Jan 28 at 5:53
• Question 1 was previously addressed here: Should each trace carrying RF be 50Ohm in characteristic impedance? How? – The Photon Jan 28 at 6:24

how is that the impedance is not dependent on trace length and only on trace widths ?

This question has previously been asked and answered several times. For example:

How can PCB trace have 50 ohm impedance regardless of length and signal frequency?

Should each trace carrying RF be 50Ohm in characteristic impedance? How?

How is xΩ impedance cable defined?

The key point is you should not confuse characteristic impedance (the ratio of voltage to current for a propagating signal on a trace) with the impedance of a circuit branch (the ratio of voltage to current flowing through that branch).

how can Altium suggest a trace width without me specifying the frequency ?

The characteristic impedance depends on the balance between inductance and capacitance per unit length of trace. Therefore it doesn't change (to a first order approximation) at different frequencies.

Is there a way I can calculate Impedance between any two given points on a trace for a given frequency ?

The characteristic impedance of a trace is not the same as the impedance between two points on the trace. It is the ratio of voltage to current that is required for a signal to propagate along the trace.

If the trace is long enough that the charcteristic impedance matters, then you can't actually define the "impedance between any two points on a trace" because there will be a delay between when a current signal is applied at one point and when a voltage is developed at the other point. Further the voltage won't depend only on the positions on the trace but also on what else is connected to the trace ends.

Instead you can define a scattering matrix (or S-matrix or S parameters) for the piece of trace. Or you can define Z, Y, or ABCD parameters, which are all equivalent.

If there is no such way in Altium(which I suspect), then how do people design Antennas these days ?

In any case, you do not want to use the Altium estimate for the trace width to achieve a given impedance to design an antenna. Altium will assume you want to confine the signal to your trace (and ground plane), rather than cause radiation. If you are designing an antenna you want a radiated signal, not a confined signal.

You can use a tool like HFSS to design an antenna.

Or you can use various more ad hoc methods that are known to RF engineers (for example, you could simply design an antenna that you know is too long for your desired frequency, and trim it back until it resonates at the desired frequency)

• Many thanks to you @ThePhoton ! Great Explanation ! I will surely follow your advise not to use Altium for Antenna design. – Curious Cosmopolitan Jan 28 at 6:54

1. how is that the impedance is not dependent on trace length and only on trace widths ?

There are two kinds of impedance: The (usual) resistive impedance is only dependent on trace length. The travelling wave impedance is only dependent on trace widths (The wave only "sees" what is beside its propagation direction, not what's ahead).

2. how can Altium suggest a trace width without me specifying the frequency?...

The wave impedance is almost not dependent on frequency. Think of light rays of different colors (frequency) which propagate the same way in air. Wave impedance is only dependent on geometry.

3. Is there a way I can calculate Impedance between any two given points on a trace for a given frequency ? I want both the resistance and reactance to design matching .

Impedances between any two points in the world can be calculated. When dealing with (high frequency) waves, you may want to calculate scattering parameters and reflection coefficients instead of resistances and reactances.

4. If there is no such way in Altium(which I suspect), then how do people design Antennas these days?

Altium Designer does not provide antenna design tools. But it can calculate the wave impedance of a trace that feeds an antenna structure.

• @stefenwyss ! Thanks for the insight. – Curious Cosmopolitan Jan 28 at 7:21