LTspice Simulation vs Hand Calculation

Question

I am new to electrical engineering and am building a boost converter project, which takes 2.4-3 V input to 5 V output. I simulated my results in LTspice to check if it works. My hand calculated duty cycle of 0.616, considering 80% efficiency, results in around 7.2-7.3 V. After playing around with the simulator, I found that a duty cycle of 0.4375 yields approximately 5 V. The inputs are two AA alkaline batteries in series, since min and max voltage is 1.2/1.5 V each then Vin(min) is 2.4 V and Vin(max) is 3 V: the equation I used to calculate the duty cycle used Vin(min), found from TI's website: https://www.ti.com/lit/an/slva372d/slva372d.pdf?ts=1729356262259

QUESTION:

Why are the results different? Which value of duty cycle will give me the closest real-life approximation? I understand that LTspice probably doesn't incorporate efficiency but I don't want to blow anything up after I assemble the circuit in real life (the output will go to a USB-A port converter, which takes a 5 V input). Screenshots of my simulation are shown below; the first is trial and error duty cycle (~5 V), the second is with hand calculated duty cycle (~7.4 V).

Answer 1

The answer to your asked question is that your results differ because the equation you do the calculation with and the math LTspice does for the simulation aren't both accounting for all the same variables such as the efficiency you mentioned.

If you plan to build this unregulated boost circuit purely for learning purposes, you will probably learn a lot, particularly how variables such as input voltage and output load can shift the unregulated output voltage. If you want to build a real world robust circuit, however, you've gone too far down an assumed design path and are asking the wrong question.

Most real world circuits like you describe incorporate a feedback loop to keep them regulating the output voltage to a fixed amount regardless of variables like input voltage, output load, and efficiency. You want to look in to boost regulator chips that include this feedback loop mechanism. This is how such things are typically done in boost converter designs where output voltage needs to be regulated. Basically, the chip will sample the output voltage, and constantly adjust the duty-cycle to keep the output voltage at whatever you set it to regardless of the operating condition variables.

Answer 2

Guessing an arbitrary efficiency number will get you within a gross ballpark number, but it shouldn't be relied upon.

Caveat: The simulation results are only as good as the models.
The diode, and presumably the FET (can't tell what that box is, but I'll guess it's a power FET) have resonable models associated with them - a good start. The inductor and capacitors need help and there are models in LTspice's library that attempt to model actual parts. Battery series resistance can be a factor as well as wiring parasitics.

You want to use a realistic efficiency number for the equation given in TI's literature. Fortunately, LTspice has a nifty power graphing and integration tools that allows you to calculate the efficiency of the circuit.

• Run the simulation and start recording data when the waveform stabilizes (.tran card, Time to start saving data). Alternately, you can select a steady-state portion of the waveform after the simulation has run.
• Alt+LMB on the power source, V1. This will show a plot of the input power. LMB = left mouse button.
• Alt+LMB on the load resistor, R1. This will show a plot of the load power.
• Ctrl+LMB on the input power graph. This will bring up a window showing the Average input power. Record this number and close the dialog box.
• Ctrl+LMB on the output power graph. This will bring up a window showing the Average output power. Record this number and close the dialog box.
• Efficiency: \$ \eta = {P_{out} \over P_{in}} \$

Beyond this study, to make a useful circuit, you need feedback to regulate the output voltage. There are a number of switching regulator controllers out there that provide a stable output voltage and current limiting.