Help calculating and simulating buck converter

Question

I want to simulate a DCDC buck converter to go from 6V to 3.3V, with a max. output current of 100mA.

I'm using this buck converter online calculator to find out the values I need. This is the results I obtain:

It doesn't mention the capacitor I need, but it does calculate the required inductor and duty cycle.

I have plugged these values into a CircuitLab buck converter example, but I don't obtain the desired output:

You can simulate the circuit here.

What do I need to do to achieve an output of 100mA @ 3.3V? (I'm not concerned about the ripple at this point)

Answer 1

I'm not sure what the original simulation got wrong since I didn't check it - that's on you. But this one works as you expect:

^{simulate this circuit – Schematic created using CircuitLab}

The input current envelope:

The input and inductor currents in steady-state:

Things to keep in mind:

1. Run the simulation for a number of complete PWM cycles. Set "Stop Time" to, say, 500 PWM cycles. That is 500/20k. One PWM cycle lasts, by definition, 1/20kHz = 50μs. Writing 500/20k is clearer IMHO than writing 500*50E-6. CircuitLab allows expressions most everywhere.

2. Have an integer number of time steps within each PWM cycle. In this case we set 100 steps/cycle, that is 1/100/20k.

3. Set "Skip Initial" to Yes, since the steady state solution for this circuit is useless.

   

4. When using PWSREPEAT here, the output voltage can be just 0/1V since VCVS1 then steps that voltage up times VCC. The PWM duty cycle and frequency can be entered easily like this:

   

   • 0,1 means "1V at t=0"
   • 0.6/20k,0 means "0V at \$t=0.6\times{\rm period}\$"
   • 1/20k,0 means "keep 0V till end of the period, the period length \$T=(1/(20\cdot10^3)){\rm\ s}\$"
   • the PWS[REPEAT] source keeps the voltage constant until the next line in the CVS field. So, it outputs 1V from t=0 to t=30μs, then 0V until t=50μs and loops back to t=0.

5. It takes a long time for the output voltage to stabilize after power-up. That is normal. You need to be patient and wait :)

6. Use real components - most simulators have less trouble with them. A simulator that uses ideal components - say ideal diodes - is much harder to make. This means:

   • the diode must be non-ideal,
   • the inductor must have some series resistance,
   • the capacitor must have some series resistance,
   • the switching transistor should resemble a real part.

7. Connect the voltage source that controls the gate between Gate and Source of the mosfet. V(GS) is what controls the mosfet, not V(G0).

Answer 2

What do I need to do to achieve an output of 100mA @ 3.3V?

• Ensure that the P channel MOSFET is ideal i.e. doesn't drop any volts between drain and source when activated
• Ensure that the P channel MOSFET is ideal in that when deactivated it is fully open circuit
• Ensure that the MOSFET is full activated and deactivated by the control signal
• Ensure that the diode is ideal (zero volt drop when conducting and full open-circuit when not conducting)

Alternatively use a slightly higher value of duty cycle to accommodate those losses and hopefully, you should see a constant 3.3 volt output. Better still use a feedback loop that controls the duty cycle based on the output hitting the required level of 3.3 volts.