Developer Help

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.

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.

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.

Cut the connection between EN and VIN.

Move the Voltage Source V1 from VIN to EN.

Place a second voltage source to supply VIN.

Run the simulation to observe the start-up response.

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.

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

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.

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

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, as seen below.

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

Edit the Bode plot probe according to the figure below.

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.

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.

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.

Datasheets:

• MCP1703A
• MCP1700
• MIC29300
• MIC5235

Evaluation boards

• SOT-23-3 Evaluation board for LDOs and Voltage Supervisors