Post Go back to editing

# LTC3811 power stage transconductance - exponential behaviour

Hi,

I'm trying to determine the power stage transconductance of an LTC3811 regulator circuit so I can design the compensation network. I made some measurements on an LTSpice simulation by applying various load steps and looking at the resulting voltage step on the COMP pin, and the results are showing that the transconductance is exponentially related to the value of the sense resistor. The graph shows my measurements, and I was able to fit an exponential curve to it and predict the transconductance at any sense resistor value reliably. This behaviour also seems to be very consistent regardless of load current.

Can anyone confirm if this is the expected behavior and not just a simulation artifact, because I would have expected a simple inverse linear curve? I do intend to verify this on a dev board at some point but I figured it was worth asking before I go buying hardware.

Thanks,

Tom

Parents
• Hello Tom,

The power stage transconductance vs sense resistor value curve is equal to the slope of the current sense threshold vs COMP voltage curve (page 9 of the D/S, first plot, top row) divided by the value of the current sense resistor. Therefore, the curve should be of the form A/x as you stated, not an exponential curve. I do not have an explanation for the shape of your curve. You can send me the simulation to my email address for further analysis if you wish.

Best regards,

Mike

• Hi Mike,

Thank you, that would be very helpful. What's you email address so I can send you the simulation?

Thanks,

Tom

• Hello Tom,

Michael.shriver@analog.com

Thank you,

Mike

• Hi Mike,

I think I've tracked down the issue. I was including some series inductance in my sense resistor in an attempt to make the simulation more realistic (and model the behavior of the sense filter properly). Turns out LTSpice gives all inductors a 1mR ESR by default. So my 1mR sense resistors were actually becoming 2mR, 2mR was becoming 3mR etc. When I manually set the ESR to 0R I get the expected response.

Thanks,

Tom

• Hi Mike,

I think I've tracked down the issue. I was including some series inductance in my sense resistor in an attempt to make the simulation more realistic (and model the behavior of the sense filter properly). Turns out LTSpice gives all inductors a 1mR ESR by default. So my 1mR sense resistors were actually becoming 2mR, 2mR was becoming 3mR etc. When I manually set the ESR to 0R I get the expected response.

Thanks,

Tom

Children
• Hello Tom,

Thank you for letting me know. Your explanation makes sense. Overlooking the 1mOhm default DCR is easy to do when using a discrete inductor to model the sense resistor's ESL. It has happened before.

Best regards,

Mike