Chapter 02 - MPLAB® Mindi™ Analog Simulator - Linear and LDO Regulator Models

Last modified by Microchip on 2023/11/10 10:59

This chapter introduces the simulation and analysis of Low Dropout (LDO) Regulators. In order to showcase the functionality of the parts, the MPLAB® Mindi analog simulator tool will be used.

2.1 Prerequisites

2.2 LDO regulator model experiments

The main objective of the following section is to study the behavior of linear regulators with the emphasis being on the dynamic response.

2.3 Case Study: The LDO Start-Up

2.3.1 Start-up from Vin

Download and open the “MIC5235-ADJ Startup” example schematic from the MIC5235 Analog Simulation software library.

Place a voltage probe on the net going to the VIN and EN pins, then double-click it.

voltage probe

Set the Curve Label to VIN and the Graph name to StartUp from VIN as seen on the image above.

Also change the Graph name and Curve label for the VOUT net probe, so that this waveform appears on the same graph.

Configure the voltage source, V1, as a single pulse with a width longer than the start-up time of the part, as seen in the figure below. Adding a delay for the pulse will make it easier to see the rising edge of the input voltage and the response of the LDO.

configure voltage source

Adjust the Stop time parameter for the transient analysis to be longer than the start-up time, and then run the simulation to observe the response.

2.3.2 Start-up from Enable

The existing setup can easily be changed to measure the Start-Up from Enable behavior.

Cut the connection between EN and VIN.

Move the Voltage Source V1 from VIN to EN.

Place a second voltage source to supply VIN.

startup from enable

Run the simulation to observe the start-up response.

2.4 Case Study: Line transient response

The main objective of this section is to show the dynamic response of the LDO and experiment with different test conditions. The setup used for the Start-Up from VIN can be changed in order to simulate the line transient response of the part.

Change the minimum value of the pulse to a value equal to the output voltage + 1 V and the maximum to the stepped value (no more than the max input voltage parameter from the datasheet). Also, the pulse needs to occur after the part has entered into regulation, thus a delay higher than the start-up time is required.

The load current can be set by using a resistor. The resistor value can be replaced by the following syntax: { VOUT / IOUT } , where IOUT is the desired output current.

Run the simulation and select the waveform window with VIN and VOUT. Stacking the curves and zooming into the relevant section should produce the image below.

Vin and Vout waveforms

Change the values for load current and slopes for the input voltage. Analyze the differences between fast and slow slopes.

2.5 Case Study: Load transient response

Analyze the load transient response of a MIC5235-ADJ LDO.

Download and open the “MIC5235-ADJ Transient Load Step” example schematic from the MIC5235 Analog Simulation software library.

For this simulation, a current probe needs to be added before the load.

As seen in the figures below, cut the wire and insert an inline current probe. Label the curve as "IOUT", and make sure that it plots on the same separate graph as VOUT.

current probe1

Current Probe

Run the simulation, stack the curves, and zoom to better analyze the response. Press C to activate cursors to measure the undershoot and overshoot.

undershoot overshoot

2.6 Case Study: Power Supply Rejection Ratio (PSRR)

Analyze the PSRR of the MCP1700 LDO.

Navigate to the MCP1700 Analog Simulation library, download, and open the MCP1700-12 Startup example schematic.

Add a second voltage source in series with the existing one and set it as an AC voltage source with an AC Voltage of 200 mV.

Add a Bode plot probe and connect it between the VIN and VOUT pins of the part.

psrr simulation

Edit the Bode plot probe according to the figure below.

bode edit

Configure the analysis type to AC Analysis, setting the desired start frequency to 1 Hz and stop frequency to 1 MHz.

Run the simulation and observe the resulting frequency response.

psrr frequency response

2.7 Case Study: Bode plots

Analyze the frequency response using the Bode Plot Probe.

For adjustable parts, the frequency response (gain and phase) can be measured. This can be achieved by inserting an AC Voltage Source between the VOUT and top resistor of the feedback loop as shown below.

bode plot simulation

Make sure to have gain and phase measurements enabled inside the 'Bode Plot Probe – with Measurements' probe. Also, for the PSRR measurement, you need to run an AC simulation.

Bode plot - gain and phase

2.8 References


Evaluation boards

Back to Top

​Learn More

Back to Top