I would like to design a boost converter using LM3481 from texas instruments. To de the job, I have selected TINA TI circuit simulator, where the average model of LM3481 is given. So I have used this model to get the open loop bode plot of the power stage without the compensator.My objective is to get a plot that will help me to decide where to put poles and zeros of the compensator. The circuit is given bellow with (L=6uH, Rsense=20m, Fsw=227kHz)

enter image description here

My probleme is that I do not know how to built a circuit for AC simulation, for exmample, I do not know how to isolate the COMPENSATION PIN or where to connect it.

*If I connect it the compensator circuit, I will not get the open loop graphs, but I will get the closed ones, am I right ?

*If I connect it to the ground, I get a strange graphs that are not convinient to me.

What are the techniques that I should use to get the bode plot of the power stage without the compensator?


1 Answer 1


The circuit shown is ready for the open-loop analysis you want: \$L_1\$ and \$C_2\$ close the loop in dc and open it in ac analysis. This is an old trick and I traced it back to the Vince Bello times when he first published his average models.

When you run the ac analysis, SPICE computes a bias point to know where all the elements operate. During this moment, inductors are shorted and capacitors are opened. The loop of your converter is thus physically closed by \$L_1\$ and the simulator calculates the correct operating point set by the resistive divider.

When the ac analysis starts, the extremely-low cutoff frequency of \$L_1C_2\$ filter isolates/opens the return path and the converter runs in ac open-loop conditions. Should you change operating conditions (input voltage, load current...), the correct operating point will be computed each time you run the .AC analysis and parameter sweeping is easy.

Now, if you want the power stage transfer function, probe the output voltage and the voltage at the COMP pin. When plotting the ratio of these two variables you'll obtain the control-to-output transfer function you want and decide what strategy to adopt with the compensation elements. Once compensation elements are calculated, probe \$V_{out}\$ only and you'll have the loop gain from which you can infer the 0-dB crossover and various margins. If you now want to test the transient response, reduce both \$L_1C_2\$ to a 1-p value and the loop is now closed in dc and ac. More information in this book.

  • \$\begingroup\$ Your answer is very helpful. But I still I don't understant how I can plot Vout/Verr. What should I do to COMP pin, how can I plot (Vout/Verr), how can I make it in the circuit?? \$\endgroup\$ Sep 14, 2019 at 12:13
  • \$\begingroup\$ It depends on the tool you use. With OrCAD's probe, you would plot Vdb(V(out)V(comp)) but with TINA I don't know. For the phase, Vp(out)-Vp(comp). \$\endgroup\$ Sep 14, 2019 at 12:27

This site is temporarily in read-only mode and not accepting new answers.

Not the answer you're looking for? Browse other questions tagged .