Home » Blog » Projects » Electronics Projects » LTSpice FFT Spectrum Analyzer for Amplifiers

LTSpice FFT Spectrum Analyzer for Amplifiers

ltspice fft

You can use an LTSpice FFT to check expected performance from an amplifier, and compare simulated results to the data sheet specifications. 

Although it took me a while to figure out, the LTSpice FFT feature is quite useful. In the pictures above, I am simulating the dynamic performance of the AD8067 op amp in my wideband loop base amplifier. The AD8067 is a high gain bandwidth FET amplifier that provides substantial gain up to about 54 MHz.

With a 5 volt single supply, I expect to get spurious free dynamic range (SFDR) between 75 – 85 dB reference to the carrier. On the right side above, the LTSpice FFT shows overall dynamic range at around 120 dBc, and SFDR of 80 dBc, which is reasonable.

I also checked out the two-tone dynamic range. This involved feeding two signals into the amplifier, with 20 kHz spacing. On the left side above, you can see that the nearest spurious responses are about 60 dB down from the actual signals. By running this test with signals at different strength, you can estimate the dynamic performance of the amplifier under different conditions.

You can also use the Fourier Transform to estimate total harmonic distortion of the amplifier at various frequencies. For this op amp, THD was 0.03% at 5 MHz.

The challenge is that out of the box, it’s not obvious how to do Fourier analysis with LTSpice.

LTSpice FFT Spectrum Analysis – How To Do

Basically, you run a Transient Analysis on your simulation to collect samples for the LTSpice FFT. The main relationship is between Simulation Time and FFT Frequency Resolution. Essentially, Frequency Resolution is 1/Simulation Time.

The simulated Sample Rate depends on the Maximum Time Step you set in the Transient Analysis. I usually set my Maximum Time Step to 4 or 10 nS (nano seconds).

Sample rate should be at least twice the highest frequency. So, to create a 30 MHz FFT, you want to sample at 60 Mhz. This, in turn, requires a maximum time step of 16.7 nano seconds.

If you want your LTSpice FFT to have a resolution of 1 kHz, you need to run the Transient Analysis for 1/1000 = 1 millisecond. This should provide around 100,000 simulated samples, which will provide a great FFT display.

LTSpice lets you apply different Windows to your analysis. Once you figure out the basic formulas, doing LTSpice FFT is easy:

  • Transient Analysis Simulation Time = 1 / Desired FFT Frequency Resolution
  • Minimum FFT Sample Rate = 1 / Maximum Time Step in Transient Analysis
  • Number of Simulated Samples = Transient Analysis Simulation Time / Maximum Time Step

Leave a Reply

This site uses Akismet to reduce spam. Learn how your comment data is processed.