Post Go back to editing

SPICE Model for AD8610 does not work

I'm using the AD8610 in a simple buffer application. AD8627 and ADA4622 are working as expected but in the prototype i am bound to the AD8610. See the part of the simulation below.

Followup: I tried also to eliminate R1, R2, C1 and C2, same result

AGND is just a virtual GND for the single supplied circuit and should have a voltage of 2.5V. The right side is a square voltage generator with the AGND as offset. The pp-voltage is 400mV and the AD8610 acts as buffer. Here is what the waves should look like (simulated with AD8627):

v(generator) and v(generator_out) are congruent... v(agnd) is 2.5V

Now the waves with original AD8610 spice model:

v(generator_out) is wrong.

I compared both models and found a way to make the circuit run, but I have no idea what the changed parameter does actually or where I can find it in the datasheet. Hope anyone can help me.

Left: AD8627 / right: AD8610

If I change V3 to 5 or something the circuit works correct. What is V2 and V3 for? Are the values correct?

Thanks in advance and best regards


  • Hi Fabian,

    V2 and V3 are part of the voltage limiting or clamping function of the model together with D1 and D2. Looking at the spice models of AD8627 and AD8610, there is some difference between the two in terms of how V2/V3/D1/D2 (clamping) are connected on the second stage and pole.

    I assumed you are putting 5V supply to your AVDD, is that correct? But I wonder why you need to put 100 ohms in series with AVDD? I tried to remove this resistor and AD8610 works fine without modifying the model. 

    Let me know if you have further questions.



  • Hi Arthur,

    thx for your quick reply.

    Please take the 100 Ohms and the two caps as history :-) they are part of an existing circuit and they were used as input filter for the supply voltage.

    I forgot the supply voltage, sorry. It is 12V and not 5V. The AD8610 with ±13V dual supply should work with a 12V single supply I guess?

    For comparing the circuit with your test I made a new simulation including only the discussed parts.

    You're right, with a 5V supply voltage and SPICE Algorithm "normal" it works fine (pictures above). With 12V supply voltage instead, I never get any result with LTSpice (Made a try with ±12V supply too). Perhaps the algorithm is the problem. With 7V there are weird result as pictured in my first question or in the picture below.

    Do you have any suggestions?

    If not I will do the simulation with another type..

    Thank you and have a nice day.
    Best regards


  • Hi Fabian,

    I tried to emulate your circuit and I noticed that the voltage reference LT6656-5 is affecting the LTspice simulation with AD8610 causing slow convergence or at times non-convergence and incorrect output voltage. Even if you change V2 and V3 to 5 in the AD8610 spice model as what you mentioned on your first post, this will only solve the problem on certain values of supply voltage for example it will work on 12V but if you try 7 or 8V, still the error is present. I tried replacing the LT6656-5 with an ideal voltage source and output voltage is correct for AD8610 for single supply voltages from 0 to 26V. Please see attached image.

    You could use AD8627 or ADA4622 for now since its already working fine with LT6656-5 in this circuit without problem.

  • Hi Arthur

    Oh dear. I should have find out that for myself sorry.

    Thank you so much for your help. I will use a ideal voltage source instead if the LT6656-5, cause its not that important in the circuit.

    Thx again and have a nice day.

    Best regards


  • This question has been assumed as answered either offline via email or with a multi-part answer. This question has now been closed out. If you have an inquiry related to this topic please post a new question in the applicable product forum.

    Thank you,
    EZ Admin