voltage to current converter

Hi experts!

I'm designing a voltage to current converter that should have the following specifications:
Vin = 0 V  to 10 V
Iout = -15 mA to 15 mA
load: inductive load: R= 206 Ohm, L=2.2H

I searched for answered questions on this forum and I didn't find a symmetric converter.

The first design that I made (using LTspice), that I was expecting to work properly (as you can see below - and file voltageCurrent_1.asc attached) is limited to only |5 mA|. Can you explain me why?
In this design the output, during the transient, oscillates a lot, how could I stabilize it?

The second design has an addictional resistor which "extends" the current to |10 mA| (as you can see below - and file voltageCurrent_2.asc attached), but I can't increase it more. How should I do?
In this case the output is much more damped

One more: I couldn't find the output current in the op amp DS, how could I be sure that the part that I selected works properly? and how should I select the part without this info from the DS?

Attached the circuit filesFile:



Kind regards,


  • is someone knows why this topic fallen here in ADC while I wrote it in operational amplifier section? I already deleted twice and rewrote it..but it is still here in ADC drivers...

  • 0
    •  Analog Employees 
    on Jan 19, 2021 5:44 PM 1 month ago in reply to aga

    Hi aga,

    Your circuit is oscillating because with that large an inductor in the feedback (2.2H), you run out of phase margin. That's because you're encountering too much phase shift around the loop through the inductor.

    You can check your loop gain using this technique in LTspice:


    I've done that here and it shows that you have near 0deg phase margin (phase angle when magnitude shown is 0dB):

    Your circuit needs some compensation. I tried an RC across the inductor but that did not help much.

    Maybe you can experiment with this simulation file to see what you can do to help increase your phase margin:

    OP213 voltage_Current loop gain EZ 1_19_21.asc

    Sorry if I've not really solved your issue. But may be this is of some help anyway.

    Also, don't know why you had some posting troubles.



  • Hi Hooman,

    many thanks for your reply.

    Many thanks to point me to the AC, I didn't know how to do it with LTspice.

    After one day I had the following idea:

    • move to another op amp (high current) since this is not designed for this kind of use, then the model could be wrong when "high" current is sinked.
    • the inductance is a pole a very low frequency, very far from the op amp band and since this circuit will run up to only 100 Hz, this shouldn't represent a problem for the stability.

    I'll try to switch to a new high current op amp and then I'll report my sim.

    Kind regards,


  • 0
    •  Analog Employees 
    on Jan 20, 2021 10:51 PM 1 month ago in reply to aga

    Hi AGA,

    I found an RC combination (R3, C1) across your 2.2H inductor which gives a stable response, as shown below:

    AC simulation looking for Loop Gain confirms adequate Phase Margin with this modification:

    I don't think output current capability of OP213 is an issue here as you're only needing +/-5mA from its output which it can supply as shown as I(R7) above.

    Here I've increased the output current demand to +/-10mA. You can see that the V(out) is at its limit (-11V) with -12V supply. So, it's a little marginal but simulates fine:

    Here is the simulation file:

    Op213 Voltage to Current +-10mA EZ 1_20_21.asc



  • Hi Hooman,

    many thanks to been on this again.

    Since the current should be -15 mA, +15 mA I decided to move to another op amp: LT1497 capable to source up to 125 mA.

    I run the simulations and results look quite similar to the previous one, so now I'm ready to make it and test it.

    I let you know next week.

    Kind regards,