# How can I simulate an RF signal as received by an antenna in LTspice?

How can I simulate an RF signal as received by an antenna in LTspice?

I am designing a simple HF RF receiver and want to test it via LTspice. Can I simulate an RF signal as:

1. A pure voltage source, with an amplitude ranging from 1uV (weak amateur signal) to 1 mV (strong amateur signal) to 100 mV (strong broadcast signal)
2. Feeding through a 50 ohm resistor (to account for the 50 ohm source impedance of a typical antenna and transmission line)
3. Connect multiple sources and resistors to account for multiple signals (necessary to simulate the receiver's ability to handle such cases)
4. Modulate any of the voltage sources according to signal modulation

Is that an accurate LTspice representation of an HF RF antenna and transmission line? If not, what is?

• That has been my approach for similar projects. Note that for LTspice input/output impedance simulations, the AC 1 voltage source should not have a series resistor. Commented Jul 15 at 22:12

Yes, to all, with the caveat that (4) will take a very long time as transient simulation proceeds incrementally, as discussed in another recent question. And consequently might not be very accurate (small numerical errors compounding over hundreds of cycles, etc.).

Note that (1) isn't very meaningful by itself, but you combine it with (2) to model the Thevenin or Norton equivalent source. In general, the antenna has a complex network equivalent, impedance and gain both varying with frequency, of course you can simply assume a given amplitude at any given frequency; the importance of impedance modeling, however, depends on what it's connected to.

(You can put the source almost anywhere in the antenna equivalent network, as long as it isn't changing the impedance thereof -- it can be a voltage source in series with any one component, or a current source between any two nodes.)

At some point, you should probably develop an understanding of what an RF port is, what incident and reflected waves are, impedance matching, tuning and all that. This will not come quickly, it's a deep topic, take it patiently -- but the value is immediate and huge: being able to break down a general N-component network into halves, joined by a port, through which current and voltage flow.

For example, if your receiver has a tuned input, and the tuning range is fairly wide, then it's probably safe to connect it to a narrower antenna, but do check that image bands haven't been created (resonances between antenna and receiver reactances, and the transmission line joining them, that don't exist otherwise), and which aren't rejected elsewhere in the system (because the antenna doesn't pick up those frequencies, or the receiver isn't sensitive to them). Doing this, requires modeling these sections themselves: SPICE provides a transmission line element which can be used, but the antenna you will likely have to measure yourself, and thus theory must be supported by practice: for example, use a signal generator and directional or reflectance bridge to measure the antenna's impedance.

Then apply the same definitions and principles, to build up a test jig in the simulator, and use that to match the impedance and gain of real networks you build.

Example:

I built this circuit in ye olde vacuum tubes for fun:
(leaving as links as this is an optional section, and to maintain copyright)
https://www.seventransistorlabs.com/Images/FMRadio3.jpg (note middle-bottom coils by the BNC connector)