While simulating with LTSpice I discovered the simulator gives milliamps of inverting and non-inverting terminal current in op amps and also the same thing for MOSFETs, milliamps into gates. Here is a simple circuit demonstrating the current into a non-inverting terminal with an op amp. I will also put down that I measured only nanoamps of current into op amp inverting and non inverting terminals and also MOSFET gates in Multisim to verify that LTspice is incorrectly giving results, which leads me to believe LTSpice is seriously flawed and this should be reported to developers. Is this normal or is it a bug which should be reported to developers? Simple Circuit

Output current for non-inverting terminal

Another circuit With 2 inputs

Inverting terminal current

  • \$\begingroup\$ So what's your question? \$\endgroup\$
    – Matt Young
    Jan 30, 2018 at 1:46
  • 3
    \$\begingroup\$ @user33915 Why would you imagine that an opamp has zero (very low) input current when the voltage difference between the inputs is 3 V???? Try arranging things so that both inputs are at 3 V and THEN check the input currents. \$\endgroup\$
    – jonk
    Jan 30, 2018 at 1:49
  • 2
    \$\begingroup\$ @user33915 1 V is still just as bad. Linear Technology's LT1001 and LT1002 are bipolar opamps. I suppose you have no idea how a bipolar opamp is designed to work? If you want low currents, you MUST keep the differential between the two inputs well under 100 mV and preferably only a few mV, if possible. Try a 30 mV difference, for example. \$\endgroup\$
    – jonk
    Jan 30, 2018 at 2:20
  • 1
    \$\begingroup\$ @user33915 These things use diff-pairs. Examine Figure from page 167 of a book by Abraham Pressman. Note the range of differences allowed for? And if you look over that nice picture, you'll see that \$\pm \:30\:\text{mV}\$ is about all you want to allow. This is not a problem with LTspice. This is a user problem. Totally different kind of bug. \$\endgroup\$
    – jonk
    Jan 30, 2018 at 2:25
  • 1
    \$\begingroup\$ AFAIK LTSpice has realistic device models. A theoretical ideal op-amp draws no current but it is not simulating a theoretical ideal op-amp, it's simulating a LT1002. \$\endgroup\$
    – user253751
    Jan 30, 2018 at 3:25

1 Answer 1


As mentioned in comments, opamps don't like their inputs to be as widely different potentials. That said, I believe LT Spice might be telling the truth. Take a look at the LT1002 schematic. Notice the series R and protection diodes between the two inputs. If the two inputs differ by more than 2 diode drops or about 1.2V, the current will be limited by the two 500 series resistors.

The current into the higher potential input and out of the lower potential input will then be equal to the difference between the two Vin sources, minus 1.2V, all divided by 1k ohms (sorry, no math fonts on my phone). snipped LT1002 schematic

  • \$\begingroup\$ What you did not take into consideration is the fact that LTspice does the same high currents even with FET input op amps, and also milliamps into MOSFET gates. However I do appriciate the elaboration for the LT1002 IC, I am posting this only because I saw nanoamps in Multisim so I thought I might as well put it here that I saw LTspice put milliamps into MOSFET gates. \$\endgroup\$
    – user33915
    Jan 30, 2018 at 6:13

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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