1. Skip to navigation
  2. Skip to content
  3. Skip to sidebar

LTspice: Speed Up Your Simulations

Gabino Alonso - Strategic Marketing Engineer Jul 20th 2015

LTspice is designed from the ground up to produce fast circuit simulations, but there is margin in some simulations to increase the speed. Note, there may be trade-offs in accuracy using the methods described here. For further details on any of these approaches, please refer to the LTspice Help File (F1). To measure the effects of your changes, review the simulation time in the LTspice error log (Ctrl + L).

Reduce Power Supply Start-Up Time

Reduce the time required for switch mode power supply (SMPS) simulation by shortening the voltage ramp of the output by changing the value of the soft-start capacitor. Before doing so, make sure you have a good understanding of the power supply’s start-up performance. Then, reduce the soft-start capacitor value—using 0.001μF instead of the of the 0.1μF default—to quickly ramp to the desired output voltage.

Note that the soft-start capacitor should not be decreased to the point where the rising output allows the VC/ITH pin to ramp well beyond its nominal control point and slew further down to stop overshoot.

Delay the Application of the Load to a Power Supply

Another effective technique to speed up simulation of an SMPS is to delay application of the load via a voltage controlled switch (SW). By using a switch that turns on the main load when the output voltage is near regulation (or at a known time), all the SMPS output energy goes into charging up the large output capacitors prior to the load being applied. The startup and the main load resistance can also be encapsulated in Ron and Roff of the SW model statement rather than using seperate resistors.

Delay the Application of the Load to a Power Supply with Switch

A simpler approach can be achieved using a current load configured with a pulse function.

Delay the Application of the Load to a Power Supply with Current Load

Set the Initial Conditions

Similarly, it might be effective to use the .ic spice directive to set initial conditions for selected nodes. For example, specify the initial voltage on the output so that it is close to regulation when the simulation starts. Likewise, you can specify the voltage at the compensation node to eliminate the initial droop at start-up.

.ic V(out)=11 V(vc)=1

Reduce the Amount of Transient Analysis Data

Normally, LTspice transient analysis starts at time = 0. You can edit the .trans simulation command’s “Time to start saving data” to delay saving until a later time of interest, thus decreasing your overall simulation time. Of course this assumes you do not need the initial data points, which are not saved.

Reduce the Amount of Transient Analysis Data

Alternately, if you are only interested in a few node voltages and device currents, you can restrict the quantity of saved data by using the .save directive to save only those specific node voltages and device currents. In the directive, add the “dialogbox” option to display all available nodes and currents so you can choose to save additional data of interest.

.save V(out) I(L1) V(in) dialogbox

Skip the Initial Operating Point Solution

Occasionally you will notice that a simulation stays in “Damped Pseudo-Transient Analysis” for a long period of time (see the lower left corner of the window for simulation status information). This usually occurs when a DC solution is sought in order to find the operating point of the circuit. If it is acceptable in your simulation, you can select Esc to skip finding the initial operating point and continue with the simulation. Likewise you can also “Skip initial operating point solution” by editing the simulation command.

Skip the Initial Operating Point Solution

If you prefer to save a difficult to solve DC operating point, you can use the .savebias command to save the preferred solution to a file in the initial simulation, and then in subsequent simulations, use the .loadbias command to quickly find the DC solution before proceeding with the rest of the simulation.

Use .savebias directive in initial simulation:

.savebias filename.txt internal time=10m

Used .loadbias in subsequent simulations:

.loadbias filename.txt

Convert to Fast Access Format When Viewing Waveforms

To maintain fast simulation speed, LTspice uses a compressed binary file format that allows additional simulation data to be quickly appended on the fly. However, once the simulation has completed, this format is non-optimal for waveform viewing. To speed up waveform plotting after the simulation is complete, convert the file to an alternate, “Fast Access,” format. Click in the waveform window and choose Files > Convert to Fast Access. This can also be implemented using the .option fastaccess directive:

.option fastaccess

It is important to note that in some simulations this conversion may take longer than the actual simulation.

 


Software

LTspice

LTspice® software is a powerful, fast and free simulation tool, schematic capture and waveform viewer with enhancements and models for improving the simulation of switching regulators. Click here to download LTspice

To launch a ready to run LTspice demonstration circuit for this part:

To explore other ready to run LTspice demonstration circuits, please visit our Demo Circuits Collection.