Hi,

I am doing a project on Buck converter. I tried to simulate the power stage of a buck converter. I tried with asynchronous Buck converter with PMOS switch. But I faced problem in the switching section of the buck converter which is performed by an NMOS/PMOS. Later I tried to simulate just a single MOSFET and the switched output is as desired but if I use it in the Buck circuit, the Vsw(switched voltage) is not as desired.

The LT-spice files and the waveforms are attached. Please guide me to use proper MOSFET switch for the buck converter for both synchronous and asynchronous buck converter.

The designed values are for the specifications

Vin= 12 V
VOUT= 5 volts
ILOAD= 2 amps
Fsw= 400 KHz

 

I just looked at the one marked buck. Looks ok to me. What don't you like. I would make pulse +/- 10 volts to make the fet turn on hard.
If you post just the .asc file more people will look than the php file.

 

You should also attach the pure circuit not the *.asc file, using *.asc will limiting the members to see the circuit.

 

A few things in buck.asc:

As Ronv noted you need minus 10V gate-source voltage to fully turn on the MOSFET. Set the pulse to -10v to 0V. Alternately you can connect the gate to ground to turn it on.

What is the purpose of R2? It just wastes power. If you are using that to suppress ringing then you should add a small capacitor in series with R2.

D1 should be a Schottky diode, not a zener.

 

Hi,

Thank you for your quick responses. Sorry, as this is my first post I didn't know people don't prefer *.asc files. However, as per the above suggestions, I have modified the circuit and there are 2 versions I have attached, one with the gate pulse voltage source connected between the gate to source and the other with gate to ground. As you can see, still the switched voltage, inductor current and output voltage are not as expected. Can you please help me with the successfully simulated *.asc file?

 

Sorry, here are the attachements.

 

It's good to post the .asc files so those with LTspice can simulate it if desired. You just need to also add a picture of the circuit in some other common format so anyone can see the circuit.

Several things on your simulation:

When you drive the MOSFET with the voltage source connected to ground as in buck1, the pulse voltage should go between 0V (MOSFET on) and +12V (MOSFET off).

For Buck_2 --

To minimize the initial large startup transient and allow faster settling I:

Changed the pulse from -10V and 0 to 0V and -10V so the transistor is initially off when the simulation starts.

Set the output voltage to near its final output value using the .ic command.

Set the VPULSE rise and fall times to 10ns. Setting them to 0 (a practical impossibility) is actually the same as leaving the values blank, and the rise and fall times default to a rather large value.

Perhaps your outputs look odd because the inductor is operating in the discontinuous mode (inductor current goes to zero between pulses). If you increase the inductor value to at least 400μH, then the inductor operates in the continuous mode and the waveforms may look more like you expected. Alternately increasing the load current by reducing the value of R1 to 15 ohms or less with your original inductor value also works.

Why do you use non-standard values for your caps? Their values are non-critical so you just pick the larger standard value.

Does the waveforms below look better to you now?

 

Hi,

Thanks again (crutschow). Ur inputs were of greater help. U know, I had read at least 10 to 15 references, but I didn't get as much as your guidance. Accordingly my simulations are as attached. Additionally, I have also simulated a synchronous Buck converter as in buck_3. The reason I chose the non-standard capacitor value is, I wanted to simulate for the calculated value, so as to simplify further layout considerations.

Now, here are my new questions.
1. Is the synchronous buck_3 connections are ok w.r.to the gate pulse connections?
2. You used the initial condition statement. If at all the layout of the buck converter is being done, how the initial condition is met. Is it kind of including startup circuit in the output?
3. How did you choose 400μH for the inductor?
4. When I simulated in Cadence (180nm), I get a warning message saying the gate voltage exceeds Tox limits. Is it because the Tox for the 180nm MOSFET is thin and the gate voltage cannot exceed 5V or something? So, we cannot fabricate buck converter for 12V in 180nm? Of coarse my specs are low power.
5. How to give initial condition in cadence?
6. Can we not control the switches (PMOS) by small voltage pulses?
7. What are the Width Length design considerations for the switch MOSFET in synchronous buck converter?

Awaiting you valuable responses.

 

Hi,

Thanks again (crutschow). Ur inputs were of greater help. U know, I had read at least 10 to 15 references, but I didn't get as much as your guidance. Accordingly my simulations are as attached. Additionally, I have also simulated a synchronous Buck converter as in buck_3. The reason I chose the non-standard capacitor value is, I wanted to simulate for the calculated value, so as to simplify further layout considerations.

Now, here are my new questions.
1. Is the synchronous buck_3 connections are ok w.r.to the gate pulse connections?
2. You used the initial condition statement. If at all the layout of the buck converter is being done, how the initial condition is met. Is it kind of including startup circuit in the output?
3. How did you choose 400μH for the inductor?
4. When I simulated in Cadence (180nm), I get a warning message saying the gate voltage exceeds Tox limits. Is it because the Tox for the 180nm MOSFET is thin and the gate voltage cannot exceed 5V or something? So, we cannot fabricate buck converter for 12V in 180nm? Of coarse my specs are low power.
5. How to give initial condition in cadence?
6. Can we not control the switches (PMOS) by small voltage pulses?
7. What are the Width Length design considerations for the switch MOSFET in synchronous buck converter?

Awaiting you valuable responses.

 

Here are the remaining attachments.

 

1. You cannot use a floating source to drive the gate pulses with one driver. You need to use two drivers, one for M1 and the other for M2 with each driver connected either to ground or vin.

Note that M2 is often an N-MOSFET since it's easier to drive a grounded-source configuration. (Edit: To drive the M2 P-MOSFET fully ON in this configuration, the gate must go to a negative voltage, with magnitude well above Vth.)

2. The .ic initial condition is just to speed up the simulation. It has nothing to do with the operation of the real circuit.

3. I experimentally kept increasing the inductor until it no longer was operating in the discontinuous mode. You can calculate the value but it's easier to experimentally determine it in simulation. Note that with a 2.5 ohm load you can go back to your original inductor value or even smaller and it will still operate in the continuous mode. The inductor size for continuous operation is inversely related to the load current.

4.I cannot answer questions about 180nM design as I'm not familiar with that.

5. Not familiar with that either. Have you tried using a .ic command?

6. The pulse voltage needed to switch a MOSFET depends upon it's maximum threshold voltage. The gate-source voltage needs to be high enough over that value to insure that the MOSFET is well turned on, typically at least a few volts over the max threshold.

7. Afraid I'm not very familiar with width-length considerations in IC design either. I know that in general you use more width for a lower ON resistance, and a longer length for higher voltage operation.