I'm now going on an amplifier project, I can simulate the ferquency responds, offset, overshort, and so on but distortion via a dos version pspice (5.0).
Can anyboday tell me how to simulate distortion in this version of pspice?
Is there any better choice for distortion simulation?
Definition of THD
-----------------
Total Harmonic Distortion (THD) is the ratio of the harmonic power to the power at the measured peek. In the following equation, v1 is the RMS value at the peek frequency and v2, v3, …, vn are RMS values at the harmonics.
THD = sqrt (v2^2 + v3^2 + … + vn^2) / v1
Definition of THD with noise
----------------------------
Total Harmonic Distorsion + Noise (THD + N) is the ratio of the harmonic power plus noise to the power of the measured peek. THD + N values will almost always be greater than the THD values for the same signal.
THD + N = sqrt (sum of squares of RMS values excluding measured peek) / (RMS value of measured peek)
Spice is not so good for low distortion. You will have to use the .option type statement to make the tolerances smaller. You will also have to specify smaller time steps. Make the time duration of the analysis a large interger multiple of the period of the input signal. Once all of this is done you should get better results. Do not expect to see distortion terms lower than 60 or 80 dB down. This is a shortcoming of spice.
The main source of error in the simulation is amplitude errors at each point. Decreasing the tolerance parameters will make spice spend more time at each point getting a better value. The main error in the FFT is that it uses evenly spaced time points. Spice does not do even points. A straight line interpolation is used to get the value at the points. When the spice time points are closer together there is less error in the interpolations.