3
\$\begingroup\$

How to measure the input impedance (shown in the figure below) of this differential amplifier with BJTs in LTspice? enter image description here

\$\endgroup\$
5
  • 1
    \$\begingroup\$ Set v3 as an ac source, plot v(vin)/I(v3) \$\endgroup\$
    – sstobbe
    Aug 26 '17 at 22:00
  • \$\begingroup\$ I had done this before, but it did not work. I used an AC source of amplitude 1. I believe that the problem may be in the parameters of AC Analysis simulation. What parameters to use in AC Analysis? \$\endgroup\$ Aug 26 '17 at 22:13
  • \$\begingroup\$ As long as the DC operating point was solved correctly Ic(q1)=Ic(q2), the results should be valid. Without feedback on Q2 the input impedance isn't going to be that high. \$\endgroup\$
    – sstobbe
    Aug 26 '17 at 22:26
  • 1
    \$\begingroup\$ You call this a differential amplifier, but you drive it with a single-ended input. Do you want the single-ended input impedance, or do you want the differential input impedance? \$\endgroup\$
    – The Photon
    Aug 26 '17 at 23:24
  • \$\begingroup\$ Why is the current through R6 so high? Couldn't you improve efficiency by increasing R6 so we don't burn 4mA through R6 and the diodes? \$\endgroup\$
    – nuggethead
    Oct 12 '20 at 18:43
1
\$\begingroup\$

There are two principal ways to use a simulator to measure the input impedance of an amplifier - the direct way, and the indirect way.

The direct way is to measure the input voltage, and current, and take the ratio.

The indirect way is to put a resistor in series with the input, and note the drop in output of the amplifier, and do the sums from that.

With a differential amplifier, take care that you're driving it in the right way. If you ground one input and drive the other, you'll be seeing a mix of both the differential and the common mode input impedance. To see the pure differential input impedance, you have to drive the two inputs differentially.

\$\endgroup\$
0
\$\begingroup\$

There are two ways to do this.

The "simple" method is to insert a resistor in series with the input (let's call it Rin) and make it's value very small like 0.001m. Then do an AC analysis and click on the Rin to plot the I(Rin). Then hover of the base of the transistor and look at the status bar to get the name of that net (let's call it V(n001)). Now right-click on the plot label for Rin to launch the series editor and change the expression to V(n001)/I(Rin). Finally, select Plot Settings > Manual Limits and change the plot type form Decibel to Linear. That will automatically change the units to ohms. Now you have a plot of impedance over the AC range.

The less simple but more official way, is to use an AC current source as the input (in place of the usual voltage source) and then do the same as above but use V(n001)/I(I1). If you search "ltspice measure impedance" you'll find examples of this.

But the "simple" method should work equally well and you don't have to trash your schem too much. Ohms law says that R = V/I so you can measure the impedance of anything that has a voltage drop across (although if the device is in the middle of a circuit you will need to adjust the expression to compute the voltage drop and then divide that by the current through it like (V(n011)-V(n003))/I(C8)).

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.