====== Course A Power Electronics ======
Within this course, you will investigate the behavior of a buck converter through simulation and real measurements. Simulations will be carried out using LTSpice, which you can download at [[https://www.analog.com/en/resources/design-tools-and-calculators/ltspice-simulator.html|Analog Devices]]. For the measurements, you will receive our DIY power electronics evaluation board, equipped with three separately configurable half-bridges. The hardware is controlled using a Simulink experiment. \\
One main goal of the lab course is to train the usage of measurement tools such as oscilloscopes, current clamps, differential voltage probes, and more.
===== Simulation =====
The problem often arises that electronic assemblies such as microcontrollers, sensors, small actuators or motors have to be supplied with 5V from a higher-level voltage source, e.g. 20V.
Since linear regulators, which are nothing more than variable series resistors, generate excessive losses, buck converters are often used. With the use of modern semiconductors, efficiencies of > 98% can be achieved. \\
For our first experiment, we design a buck converter with the following properties:\\
Input voltage range: 15V ... 24V, nominal 20V\\
Regulated output voltage: 5V\\
Rated output power: 25W\\
==== Ideal World ====
Unfortunately, a simulation is often very similar to installing real hardware: soldering everything together and applying voltage in the hope that it will work is utopian. Or in a simulation: parameterize all components, connect them and press the run button usually doesn't work :-( \\
This usually doesn't work even if we only use ideal components. We have to gradually start approaching the matter and build up the simulation step by step. And each step must confirm the results we expected at the beginning. If this is not the case, the simulation should be reduced or simplified again until the result meets our expectations in order to achieve a trustworthy result. Don't let a simulation lie to you.
It is just as important as the simulation itself to check whether the results are plausible. If, for example, currents > 100A or voltages in the MS range occur in the simulation, you should not trust the result under any circumstances.
**Task 1a)**
Create the circuit diagram of a buck converter consisting of a switching element, diode, coil, capacitor and load. Determine the load resistance so that the required power is set at the output.
Use LTSpice to create a simulation of a buck converter with the boundary conditions described above, consisting of an ideal switch, an ideal diode, coil and output capacitor. \\
**Task 1b)**
Create a table and sketch the voltage and current curves. Calculate the expected voltage and current values for each component at the nominal input voltage.\\
**Task 1c)**
Use LTSpice to create a simulation of a buck converter with the boundary conditions described above, consisting of an ideal switch, an ideal diode, coil and output capacitor. \\
**Task 1d)**
Compare the simulation result with the expected results. What do you notice? What explains the deviations? \\
**Task 1e)**
You may have noticed that although we asked LTSpice to use an ideal diode, it was not chosen as ideal. Use the simulation to calculate the efficiency of your buck converter.
For the simulation/calculation please use the following parameters: \\
Switching frequency: Last two digits of your Matrikelnummer in kHz ((if the value is less than 20, it is doubled until it is greater)\\
Inductor: Last three digits of your Matrikelnummer in µH (if the value is less than 40, it is doubled until it is greater) \\
Capacitor: Use a 330µF electrolyte capacitor.
Note: Within LTSpice you have to configure the switch parameters first:
{{ :professoren_webseiten:rebholz:simple_switch.png?400 |}}
Diodes always incur power loss, primarily caused by the voltage drop across the device. Thus, the freewheeling diode is often replaced by a second power switch, leading to the commonly used half-bridge topology. This is a clever solution, especially when using MOSFETs as switches. MOSFETs always come with an intrinsic diode, known as the body diode. Therefore, even if the MOSFET is not activated, the body diode can serve as the freewheeling diode. The body diode, of course, exhibits the same poor power loss characteristics as the previously used diode. Therefore, we activate the MOSFET to allow the current to flow through the MOSFET instead of the diode.The rule to avoid short circuits is as follows: whenever the high-side MOSFET is turned off, the low-side MOSFET is turned on. However, this introduces another problem. Since the switching speed of the devices is not infinite, a certain amount of delay is required before turning on the low-side MOSFET after the high-side MOSFET is turned off, and vice versa. This delay is referred to as dead time. With ideal switches, we do not need any deadtime. However, you can equip the PWM generator with a deadtime function, as we will need it later
**Task 2a)**
Replace the diode in your simulation with an additional ideal switch and run the simulation again. Now, the calculated current values should match the simulated ones pretty well.\\
**Task 2a)**
Once again, compare the simulation results with your expected values. Ensure that your simulation produces reasonable results, as values in the range of kA or MV are outside the expected scope!
Note: Dead time can be generated by shifting the comparator values with a negative or positive offset. In the following example, Qn is the inverse PWM signal of Q, with variable dead time.
{{ :professoren_webseiten:rebholz:pwm_deadtime.png?400 |}}
==== Real Components ====
==== Adding Mosfets ====
LTSpice, like any network simulation program, is capable of accounting for the real behavior of MOSFETs. However, as we know, the parasitic elements of almost all semiconductors are strongly dependent on temperature. For MOSFETs, parasitics such as the parasitic capacitance are even dependent on the current voltage value.
Nevertheless, having a simple, realistic behavioral model is better than having none at all. The models can normally be downloaded from the manufacturer's website.
Here {{ :professoren_webseiten:rebholz:irf3205s.zip |}} you can find the model for your IRF320 MOSFET. \\
Datasheet: {{ :professoren_webseiten:rebholz:irf320.pdf |}}
**Task 3a)**
Replace the ideal switches with the MOSFET model. Be sure to set the correct gate-source voltages.\\
**Task 3b)**
Determine the required dead time for the MOSFETs to ensure safe operation. Observe and document what happens if the dead time is too short. Take a screenshot for your documentation. \\
**Task 3c)**
Adjust the duty cycle so that the output is set to 5V again.
To determine the required deadtime you can delete the load and increase the deadtime as long as there are short circuit pulses. Due to the parasitic mosfet capacities which are continuously charged and discharged, a remaining current can be seen even with sufficient dead time. In reality, however, this is not as large as in our almost ideal simulation environment, due to additional damping lead resistances or the internal resistance of the source.
==== Adding Gate Driver ====
In a simulation, it is very easy to generate an isolated voltage source that is independent of the common ground. In reality, generating isolated sources requires significant effort, as transformers are typically needed to decouple the grounding. The problem arises with the gate supply of the high-side MOSFET, as the drain potential continuously switches between the reference ground and the input voltage. A commonly used solution is the use of a so-called bootstrap circuit. Put simply, the circuit charges a capacitor which is then connected to the mosfet independently of the ground potential. Integrated circuits such as the IRS2890DS driver we use perform this task for us and can control one half-bridge at a time.
{{ :professoren_webseiten:rebholz:irs2890.png?200 |}}
Gate drivers are often equipped with additional features. Our driver can detect overcurrents and if necessary, will turn off all MOSFETs for safety. Since overcurrents in a simulation tool will not damage your PC or notebook, you can ignore this feature in the simulation. Pull up the RFE output and connect ITRIP to ground. \\
Datasheet: {{ :professoren_webseiten:rebholz:infineon-irs2890ds-ds-v01_00-en.pdf |}}
**Task 4a)**
Add the driver circuit to your simulation and check the functionality. The general behavior should be the same as before! The simulation time now might significantly increases depending on how fast your computer is. Use the datasheed to complete the circuit.\\
**Task 4b)**
Now you can determine the switching time of the drive and the MOSFETs. Measure the required time to turn the MOSFETs on respectively off for every MOSFET.\\
**Task 4c)**
Since we cannot turn the switch off before it has fully turned on, a minimum on-time for the switch is required, which will define the maximum frequency. Calculate the maximum frequency we can use for this setup if we want to use a minimum duty cycle of 10%. \\
Check if the gate-source voltage of the MOSFETs can reach the full desired value to ensure the device turns on safely
As a rule of thumb, the bootstrap capacitor is selected in the range of the input capacitance Ciss of the MOSFET to be driven. However, many developers start with a 100nF capacitor and check the function in the design. During the turn on phase the voltage at the gate should be as constant as possible. What do you think? \\
Is a 100nF capacitor enough? Gate series resistors are used either to reduce the switching speed of the mosfets or to dampen unwanted oscillations. A value between 1 and 10 ohms is often used as the starting value.
==== Estimat Parasitics ====
Now we have a pretty good simulation of the buck converter to calculate the operation point and get a feeling for the losses. Simulation however ist getting slower and slower. To get even closer to the real behavior of ourbuck converter we have to consider the parasitic elements of the components. \\
* For the inductor we can add the series resistance given within the Datasheet: {{ :professoren_webseiten:rebholz:74437429203101_100u.pdf |}}
* The frequency behavior of the capcaitor can be calculated from the measured Z(f) plot {{ :professoren_webseiten:rebholz:z_f_330uf.png?linkonly |}}. Many manufacturers, such as Würth, offer the data for download on their homepage. [[https://redexpert.we-online.com/we-redexpert/en/#/home|Würth]]
* All PCB traces that carry a high current must be included in the overall consideration. The following values can be assumed as a rule of thumb. Inductance 1µH/m for supply lines or 10nH/cm for conductor tracks.The resistance can be estimated as 0,5mOhm/cm for a 35µm track with 1cm width.
**Task 5a)**
Add parasitic elements to the inductor, capacitor and pcb traces. Estimate a trace length to connect the MOSFET leads of about 1cm.
**Task 5b)**
Run the simulation again and describe the effect of the parasitic elements.\\
**Task 5c)**
Every trace and wire represents an inductor. Distinguish between good and bad parasitic inductors. Mark all critical inductors within a sketch or the schematic.\\
It might now be clear that the final output voltage does not depend solely on the duty cycle. In a real system, many parameters influence its behavior. This is one of the reasons why we need a control loop, which we will implement later in the lab.\\
===== Reactive Current =====
When we think of reactive currents or reactive power, we usually think of AC voltage systems but not of a step-down converter. But let's imagine the following scenario: The load resistor increases, or the load is lost— for example, because you turned it off or due to a broken connection. The DC-DC converter still attempts to regulate the output voltage to 5V with a constant duty cycle. In the half-bridge configuration, the high-side MOSFET will charge the output capacitor, while the low-side MOSFET discharges the capacitor within the same cycle. This creates a circulating current between the output capacitor and the power supply. You can easily demonstrate this behavior with a simulation. However, in the lab, it might be dangerous. Why? During the discharge of the capacitor, the circuit behaves like a boost converter. If the input voltage source cannot handle negative currents, it might get damaged. In many cases, however, the reactive current generates losses, and the bulk capacitor at the input of the buck converter can absorb the reverse current.
**Task 6a)**
Run the simulation with verly light load respectively a very high ohmic load resistor e.g. 100kOhms. Observe the capacitor current and the current through the MOSFETs. What is bad about this mode of operation? \\
**Task 6b)**
Find a solution how to prevent the drawbacks you have observed in task a) and run the simulation again. Please check the desired output voltage!\\
**Task 6c)**
How can you implement your solution within a microcontroller regulated buck converter?\\
===== DIY Board =====
=== Additional Components ===
{{ :professoren_webseiten:rebholz:parts_l_c.png?400 |}}