obtaining open-loop bode plot

Thread Starter

myil

Joined May 2, 2020
124
Hi Everyone,

I would like to obtain an open-loop bode plot of a boost converter with my siglent scope and signal generator.
I have a injection transformer but I don't know where to place it to measure the open-loop gain and phase of the converter.
Can anybody help me with this or maybe share a simple schematics?

Thank you & Regards
 

Papabravo

Joined Feb 24, 2006
18,978
This is how I would do it.
1660165079172.png
Notice how the results get squirrelly as the stepped frequency approaches the Ramp Frequency. D=0.48, output voltage should be Vi/(1-D) ≈ 19.23V
If you want the simulation file, I can package it up for you. Alternatively tell me what components you are using, and I'll make you a custom one.
 

Thread Starter

myil

Joined May 2, 2020
124
Hi Papabravo,

Sorry for late notice. Can you please explain the gate side of the mosfet? You used many different voltage sources ( sine, Vduty and Vsw) and U1. I couldn't quite understand what is happening there. And how can I do this test in real life with bode plotter?

Greetings
 

Papabravo

Joined Feb 24, 2006
18,978
Vduty outputs a constant voltage of 4.8 Volts DC, which sets the average duty cycle at 4.8/10 = 0.48 = 48%
Vsin outputs a sine wave that swings from -1V to +1V, which changes the actual duty cycle from 38% to 58% at a fixed frequency for each of 34 simulations.
Vsw generates a sawtooth waveform which goes from 0 VDC to 10VDC with a rise time of 4.8 usec and a fall time 0.2 usec for a total of 5 usec for the period. The sawtooth frequency is 1/5 usec = 200 kHz. U1 is a comparator which generates the PWM signal.

E1 is a voltage-controlled voltage source that replicates the PWM voltage. It represents the sort of driver you should use on a MOSFET gate to ensure fast and clean switching waveforms. There is a dotted line connection from U1 to E1 because an actual wire is not required in the simulation

U1 is just a generic comparator. The output is high when the + input is greater than the - input

V1 is the input voltage source of +10 VDC with a turn on ramp time of 5 msec.

The purpose if the simulation is to characterize the transfer function of the output voltage with respect to the input voltage which sets the duty cycle.

Actual circuits to duplicate the functional blocks of the simulation are basic design tasks that can be dealt with easily.

Your original question was: "How can I do this"? The simulation provides a road map.
 

Thread Starter

myil

Joined May 2, 2020
124
I almost draw the same schematic in pspice. But couldn't get any significant result. I don't know where I did wrong. You measure dB(out/in) to get the gain of open loop, right? Sorry I am new to this. Need your help :)
 

Papabravo

Joined Feb 24, 2006
18,978
I'm not familiar with pspice, so I don't think I will be much help. The plot I got came from the twelve .meas(ure) statements which is the collection of spice directives in the black text. The data being plotted came from 34 separate simulation runs at frequencies from 100 Hz to 200KHz with 10 frequencies per decade. This is NOT the same thing as running an AC analysis where you change the frequency of the AC over a range in a single simulation. That technique won't work for an AC source that is controlling the duty cycle, when doing a .tran (transient) analysis.

The method used was introduced by Middlebrook

R. David Middlebrook, "Measurement of Loop Gain in Feedback Systems", International Journal of Electronics (vol 38, no. 4, pages 485-512, April 1975).
Below the schematic is the excerpt from the LTspice helpfile in PDF format on the method.
This version of the schematic might be easier for you to read:

1660348257598.png
 

Attachments

Last edited:

ronsimpson

Joined Oct 7, 2019
2,250
Hi Papabravo ,

Please attach your "Boost_Bodie.asc" file. I have tried to make one just like yours and failed. It is slightly over my head.
You clearly have put lots of work in this.

Thankyou,
RonSimpson
 

Papabravo

Joined Feb 24, 2006
18,978
Hi Papabravo ,

Please attach your "Boost_Bodie.asc" file. I have tried to make one just like yours and failed. It is slightly over my head.
You clearly have put lots of work in this.

Thankyou,
RonSimpson
Happy to oblige. I did verify that the diode and the MOSFET are part of the standard LTspice distribution. The generic comparator symbol and subcircuit are also included. There is 1 simulation per frequency between 100 Hz. and 200 KHz.

Getting the data plotted requires the following steps after the 34 simulations are complete.
  1. Select "View | Spice Error Log"
  2. In the Spice Error Log Window, right-Click and select "Plot .step'ed .meas data"
  3. A dialog box will appear that says:
    "This file has real data with names that can be combined to be complex data.
    Shall I write these as complex data?"
  4. Click "YES"
  5. A new plot window will open up with the saved data.
 

Attachments

Top