Tackling efficiency and thermal behavior of SMPS with SPICE
Analog designers rely on datasheets provided by component manufacturers to define the specification of their circuit design. Although datasheets include the specifications of individual components and remain an indispensable resource for the designer, yet they lack some information of how parts will behave within different design configurations. This is why circuit simulation is a good complementing design tool to datasheets that provides such insight.
Semiconductor manufacturers work on providing SPICE models within different simulation environments to facilitate the simulation task for their customers. SPICE technology is commonly used to model discrete components such as BJTs, Op-Amps, and MOSFETs. However, integrated systems that require a higher level of sophistication are getting more and more accurately modeled. Integrated power converters and switching controllers are examples of these parts where the capabilities of SPICE simulation could be leveraged for the evaluation of system performance parameters such as power efficiency, conduction and switching losses, and overall thermal behavior.
The example presented here addresses Switch Mode Power Supplies (SMPS) modeling and simulation, an area where manufacturers have been focusing a lot of their modeling efforts and where SPICE is capable of yielding accurate results. Simulation in the Multisim SPICE environment of the new low VCEsat BJTs by NXP, used for medium power switching converter applications, is chosen as a use-case highlighting different performance attributes. The design of the BJT-based converter shows how to properly drive it and meet ripple and efficiency requirements, while determining power dissipation of the switching elements helped better understand the contributors to the losses and the implications on the thermal design.
This suggests an overall effective approach of designing SMPS by relying on advanced modeling and simulation capabilities. The resulting outcome is getting to an optimized design before leaving the desktop simulation stage of the design flow.
Medium Power DC-DC Buck Converter Using the Improved Technology of low VCEsat Transistors
This example demonstrates how designers could benefit from the NXP simulation models in the Multisim environment designing the power stage of a DC-to-DC buck converter. The simulation helps in taking accurate design decisions that directly impact the circuit performance such as:
- Choosing capacitor and inductor values to meet ripple requirements
- Choosing gate driver components to ensure that the BJT is driven optimally
- Calculating the efficiency of the converter
- Calculating power dissipation to gain insight about the thermal behavior
Design Specifications
Design specifications and constraints are defined to provide explicit information about the requirements for the circuit and how the circuit topology is to be put together. The design needs to meet the following conditions and design requirements:
Design Specification |
Value |
Input voltage |
10V |
Equivalent load resistance |
2Ω |
Switching Frequency |
50kHz |
Output voltage |
3.3V |
Inductor current ripple |
<400mA |
Output voltage ripple |
<60mV |
Efficiency |
>80% |
Such an application is suitable for the low VCEsat products by NXP because it is optimized for high-speed switching. The high and constant current gain, the low saturation voltage and the good switching performance of NXP BISS-4 transistors allow the use of a bipolar transistor for the described circuit of medium-power DC-to-DC converter instead of a P-channel MOSFET. The BISS transistor proposed in the example is optimized for minimized switching times. The storage and switching times are much reduced compared to types optimized for an ultra-low VCEsat.
Circuit Set-up
As a first pass, based solely on the operating voltage and current (10V, 1.65A), we chose the PBSS4032PD PNP transistor (30V, 2.7A) as the main switch and the PMEG3020BEP Schottky diode (30V, 2A) as the freewheeling diode.
To help manage and choose values for the various components in the circuit, global Circuit Parameters are added in Multisim to define key parameters such as the switching frequency, Vin, and Vout. These parameters are hard-coded throughout the design process while some other parameters have variable dependencies such as the duty cycle, the filter inductance L, and capacitance C.
The formulas for these parameters are based on fundamental equations of an ideal buck converter and provide a reasonable starting point for choosing values. The Preview column provides the numerical evaluation of the expression. Certain circuit parameters, including L and C, are directly applied to values of component parameters in the buck converter circuit.
Simulation and Analysis
A 1ms transient analysis simulation quickly generates the following waveforms for the output voltage and inductor current.
Note that the output voltage, at 3.7V, is inconsistent with expectations from theoretical calculations. As a result of the various voltage drops across the BJT and the diode, the expectation is to see a voltage slightly lower than 3.3V, not higher. An inspection of the BJT waveforms with respect to the drive signal reveals the cause.
The actual BJT turn-on and turn-off events lag significantly those commanded by the gate drive signal. The turn-off lag is greater than the turn-on lag, explaining the higher-than-expected output voltage. A far more serious problem indicated by the above waveforms is that the BJT spends a significant amount of time in the active region where it consumes a large amount of power. As expected, probing the average power dissipation in the BJT, results in 2.5W of power dissipation. This implies not only that the efficiency of the converter is likely below 50% but also that the transistor will probably be destroyed without an impractically large heat-sink.
Luckily this problem can be easily mitigated by placing a small capacitor in parallel with the base resistor.
This capacitor provides extra current during the turn-on and turn-off transients. A simple parameter sweep analysis in Multisim can be used to determine a good value for the capacitor. We have chosen the power dissipated by the transistor as the metric for evaluating the effectiveness of various capacitor values. The graph below in Figure 6 shows the average power dissipation of the transistor for various values of the capacitor.
From a range of 1pF to 1uF, a value of 10nF appears to provide turn-on/turn-off characteristics which result in the lowest power dissipation. A more standard value for the capacitor, 4.7nF, yields the following results for the output voltage and inductor current.
The output voltage, at 3.1V, is now much more in-line with the expected performance. In practice this converter would be operated at a duty cycle higher than 33% to compensate for the various voltage drops which push the output voltage below the value expected from the ideal relationship, Duty*Vin.
The inductor current ripple is 298mA, which matches well our estimate from the ripple formula, and is below the required maximum. The voltage ripple is 60mV, which is higher than that expected according to the ripple formula; it is also just at the limit of the requirement. The excess ripple is a result of the output capacitor’s ESR. It is preferable to reduce it.
SPICE simulation provides an interesting insight into the sensitivities of the ripple. For instance, simulation shows that increasing the capacitance value from 9.4uF to 100uF reduces the ripple only by 5mV. However it also shows that decreasing the ESR from 200mΩ to 100mΩ reduces the ripple by 15mV. Therefore it may be more effective for the designer to focus on decreasing the ESR rather than increasing capacitance.
Efficiency and thermal behavior
Now that we are able to properly drive the BJT and have met the ripple requirements, we can turn our attention to the efficiency of the converter and its thermal behavior.
The efficiency of the converter is calculated by setting up a mathematical expression in Multisim averaging the consumed power by the resistive load divided the supplied power by the input DC source over a period of 60us. The following plot (Figure 8) shows the result of this expression along with the major contributions to the overall power dissipation coming from the Diode and the BJT.
An efficiency of 87% meets the requirements. However it should be possible to improve the efficiency of the converter by, for instance, selecting different BJT and Diode components. Since many other fully functional NXP components are readily available in the Multisim database, attempting to optimize the design by swapping in and out different components is simple.
The average power dissipation provides insight about the thermal behavior of the components, the junction temperature in particular. For instance, from the datasheet of the PBSS4031PD, we note that the thermal resistance from junction to ambient for a BJT mounted on an FR4 board on a 6cm2 mounting pad is 160°/W. With an average power dissipation of 204mW, the average junction temperature rise above ambient is 32.8°. Therefore, there is plenty of headroom before the junction temperature reaches the maximum temperature of 150°.
Conclusion
This quick example showed how Multisim could be used to determine key parameters of a DC-DC converter. The converter is based on the new low VCEsat transistor models and diode parts from NXP. The design of the BJT-based converter is properly driven and meets ripple and efficiency requirements, while determining power dissipation of the switching elements helped better understand the contributors to the losses and the implications on the thermal design.
NI and NXP continue to offer circuit designers a complete library of accurate component models and a simulation environment that enables them to evaluate their circuit performance resulting in a more efficient flow and improved prototype designs.
Mahmoud Wahby
Product Manager
I’ve been part of the product marketing team at National Instrument since 2011. My responsibilities include defining product positioning and marketing strategy, working on launch campaigns of new product releases, and driving awareness and relationships with partner companies for the circuit design tools at the company. I have a background in RF applications having worked with Ericsson Egypt approximately 2 years and Transradio Sender System in Berlin, Germany. I hold a Masters of Science degree from Queen’s University in Canada, my research focus was on the synthesis and analysis of RF passive components. About National Instruments: Since 1976, National Instruments has equipped engineers and scientists with tools that accelerate productivity, innovation, and discovery. NI’s graphical system design approach provides an integrated software and hardware platform that simplifies development of any system that needs measurement and control. Engineers and scientists use this platform from design to production in multiple industries, advanced research, and academia. The company’s long-term vision and focus on improving society through its technology has led to strong, consistent company growth and success of its customers, employees, suppliers, and shareholders.
Credits
This article is co-authored by Oleg Stepanov from National Instruments R&D. The author would also like to thank Bjoern Scheffler and Burkhard Laue from NXP Semiconductor for their assistance with this work.