[SOLVED] LT spice Simulation AD8220 shows some weird results and I don't know why

[wogoos]

Hi Analog engineers
First something info about the circuit. I'm designing a Current control for a switched mode oversupply with a feedback (FB) voltage of 1.215 Volt ( the U5 reference has a little more 1.23V but for the simulation that doesn't matter). The current control is done by a microcontroller using a 12bit DAC. The idea is that the DAC sets the set point of the current and when the set point is reached by the increasing current the SMPS FB will start reducing it's duty cycle till it is equal or below the set point again. The circuit is based on a AD8220 Differential amplifier with a G=62.5 where the Uin+ input voltage generated by the Current of a Rs=0.004Ohm is subtracted with the Uin- voltage with is the DAC voltage divided by 62.5 using a resistor divider till the output reaches 1.215Volt (here 1.23V)..

I have simulated all this in LTSpice and no problem with simulation. When I match the specs of the AD8220 with the simulation results, I see some weird things. For example, the data sheet specifies an output swing way better than what the simulation shows. The Voltage swing is between 0.15V and 4.85V with Vcc=5V with a 10K load. The simulation show that after 3.10Volts output the amplification curve knees and continues with a very different gain compared with the calculated gain of 62.5. This knee point you see at 7.59A or at 0.42 seconds. I simulated the same circuit in Multisim with the same results.

Can anyone tell me what I'm doing wrong here or if there is some kind of error in the spice model of this AD8220.
What is your experience with LTspice, does it normally simulate close to reality.
Can you comment on the schematic, any better ideas here?.

Hope you can help thanks

 

[barry]

Nothing looks wrong to me. Maybe it has something to do with the Impedance of the reference? Try replacing it with a voltage source.

 

[KlausST]

Hi,

Output voltage swing:
Generally I don't think that the simulation models are optimized to show realistic values.
Besides this your circuit differs regarding test conditions. The datasheet conditions are:
* RLoad = 10k ... usually this is against (VS+ + VS-) /2 = (+5V + 0V) / 2 = +2.5V.
* Gain = 1
* And it mentiones: "The AD8220 can operate up to a diode drop below the negative supply but the bias current increases sharply. The input voltage range reflects the maximum allowable voltage where the input bias current is within the specification." ... which may explain the knee.

Generally I believe more in datasheet values than simulation values.

Klaus

 

[wogoos]

Nothing looks wrong to me. Maybe it has something to do with the Impedance of the reference? Try replacing it with a voltage source.

Thanks for your commend Klaus

--- Updated Jun 25, 2021 ---

Nothing looks wrong to me. Maybe it has something to do with the Impedance of the reference? Try replacing it with a voltage source.

Thanks for your commend Barry

--- Updated Jun 25, 2021 ---

forgot to add the LT-Spice file. Here is the file for the ones who like to give it a try

 

[FvM]

Maybe it has something to do with the Impedance of the reference?

Apparently not. Vref is constant in the simulation.

--- Updated Jun 25, 2021 ---

Problem is limited input common mode range and its dependence on gain, output and reference voltage.

For example, the data sheet specifies an output swing way better than what the simulation shows.

There's no thing like an unconditional output swing of this component. Data sheet shows relation of input common mode voltage, gain, reference voltage and output swing only for some combination of values, not for the settings you apply. I'm not sure if the SPICE model exactly matches the behaviour of the real component, but a similar behavior seems plausible.

--- Updated Jun 25, 2021 ---

To understand the behavior, you can add internal model nodes V(u4:n003) and V(u4:n012) to the plot, they correspond to NODE C and D of the internal circuit. You see that Node D is clipping a 0V.

 

[wogoos]

I found the solution. The U4 negative voltage Vs- should be -1...-5 Volt. The specification does show this simulation test with U4 Vs- at zero volt but they have the reference at 2.5V. In that station it works too. The problem is solved.