LTSPICE AC analysis amplitude

[szszjdb]

Dear all,
I am trying the MeasureBW example in the educational folder. I notice that when changing the AC amplitude in the small signal AC analysis dialog of the AC source, from the original 1 to 50m, the gain will change from 44dB to 16dB.  As in the transient analysis , the 1V input will saturate the output. So I change the AC amplitude in the AC analysis. 
What is the correct AC amplitude should be?

Best Regards,
James

[Ian.M]

LTspice (like all other SPICE3 compatible simulators) does a .AC analysis by replacing all nonlinear components with linear equivalent models calculated at the DC operating point, to derive a linear equivalent circuit that can be solved in the frequency domain.   Saturation, clipping and other non-linear effects are not modelled during .AC analyses.

Therefore the only effect of setting non-unit amplitude for a current or voltage source used as the signal input is to shift the reference level of the resulting plot.  e.g. set AC 10 and 20dB will be added to all amplitude result curves, set AC 0.1 and 20dB will be subtracted, etc.  Its therefore usual to simply use AC 1 for the source or sources that are inputs and leave it blank for all other sources.

Your source with AC 50m simply subtracts 26dB across the whole frequency range, as 20*log(50mV/1V)=-26dB, with no other effect (except confusing you)!

[szszjdb]

Hi,Ian.M,
Many Thanks!

That is to say , the more accurate way to evaluate the gain is to calculate the gain by the Vin and Vout in the transient analysis, as the clipping and saturation is involved?

BTW, could you give me some advice on how to measure the input and output impedance of the circuit above?

Best Regards,
James

[Kleinstein]

One can directly measure the input impedance (actually the inverse) by looking at the current flow from the source. So no extra simulation needed.

Output impedance is a bit more effort. I use a extra current source at the ouput in AC mode and than have the other AC sources off. This simulates a load with an external 1 A AC current (in the linear model, so no problem to use this with small parts). So the voltage for the output gives the output impedance. So 0 dB for the voltage would correspond to 1 ohms output impedance.

[Ian.M]

That is to say , the more accurate way to evaluate the gain is to calculate the gain by the Vin and Vout in the transient analysis, as the clipping and saturation is involved?

You can do that, but if there's significant nonlinearity with respect to input amplitude, the result isn't something you could call gain.  Also there are other complexities e.g. the need to filter out harmonics before calculating the gain.

BTW, could you give me some advice on how to measure the input and output impedance of the circuit above?

In addition to the method Kleinstein suggested, you can use the .NET command with a .AC analysis, but its a bit of a PITA to set up correctly.  See the help file (Dot Commands =>.NET) for details.

[iMo]

The schematics looks weird, but the principle of measuring in/out impedance seems to be ok..

[iMo]

Example:

[szszjdb]

Hi,Kleinstein ,Ian.M, and imo，

Many Thanks!
All of you help much!

Best Regards,
James

[Kleinstein]

For the test of the output impedance one sould still keep the input source connected, or at least have a short instead of the original test source at the input.
depending on the circuit this can make a difference for the ouput impedance.

[szszjdb]

Hi,Kleinstein，

Many Thanks!
I am simulating some RF circuit. Some old part like MMBFJ310 ,2SC3358, 2SC3357, are hard to find the manufactory LTspice model .
Could you give me some advice on where to find the the model?

Further more, it is possible to emulate the distortion performance like the OIP3 of the amplifier? By the FFT analysis?

Best Regards,
James