0
\$\begingroup\$

I have a problem witht the AC analysis of a circuit. The circuit is a voltage driven constant current driver: enter image description here It is intended to drive a constant current into L1 (R1 being the series resistance of the inductor). R2 is the resistor to sense the current passing through the coil. U2, U3 and associated resistors are just there to rescale the voltage so that a variation of 1V on V3 will lead to a variation of 1A in L1.

The AC analysis give the following response: enter image description here We can see that at 1kHz, the gain is still more or less the same as at 10 or 100Hz: -20dB represent 100mV across R2 wich is then 1A. When I do the transient response with V3 at 1V/10Hz I see the 1A passing through R2, but when I do it at 1kHz I only see 500mA through R2.

That is actually normal because at 1kHz, the coil reactance is R=wL=31 Ohms. The power supply being +/-15V the current passing through the coil and through R2 cannot be higher than 500mA (15V/~30 Ohms) meaning at 1kHz the amplitude is actually divided by 2 so the gain should not be the same at 10Hz and 1kHz.

This information is not visible on the AC analysis so my question is: Is LTSPICE ignoring any power supply limitation of an OPAMP when it does AC analysis?

| improve this question | |
\$\endgroup\$
1
\$\begingroup\$

Your circuit is a feedback system that sets the voltage at node8 to produce a constant current through the inductor. That is exactly what it is doing. When the inductive reactance rises, the circuit compensates and drives a higher voltage at the top of R1 to maintain node8 voltage as constant as possible.

AC analysis does not take account of power supply limits - if you want power supply limits to be taken into account do a transient response test. AC analysis is a small signal analysis.

| improve this answer | |
\$\endgroup\$
  • \$\begingroup\$ I know the circuit is doing exactl what it should, my question is not about the circuit it is about the simulation in LTSPICE. I though that during the AC analysis LTSPICE would still take ito account the value of V3 but it apparently does not. \$\endgroup\$ – damien Jun 12 '18 at 10:18
  • \$\begingroup\$ As I put in my answer - AC analysis never does this because it does a small signal analysis then scales up the result accounting for the stimulus level you specified. It ignores DC limitations such as power rails because that would cloud what AC analysis is intended for. \$\endgroup\$ – Andy aka Jun 12 '18 at 10:20
  • \$\begingroup\$ SPICE first computes the dc operating point and linearizes the circuit around it. Then ac analysis is launched. What is always important to check is that operating points are correctly evaluated: ask LTspice to display them and you will know if the circuit is correctly operated. If you want to see the effects you mentioned (op-amp railing up or down, saturation mechanisms of all sorts), you will have to resort to a piece-wise linear simulator such as SIMPLIS, PSIM or NL5. These programs consider perfect elements and can deliver a small-signal response from a switching circuit. \$\endgroup\$ – Verbal Kint Jun 12 '18 at 11:01
  • \$\begingroup\$ Thanks for the answer. Then what is the "AC amplitude" (in the AC small signal analysis ) used for? because indeed I checked and the operating point is 0V. But I though this field was the value of the amplitude I wanted for the small signal \$\endgroup\$ – damien Jun 12 '18 at 12:02

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.