LTspice Tutorial - how to use this program

A short introduction into LTspice circuit simulation program

The Interface

LTspice IV is a very simple and accurate tool to provide circuit simulation. The system is totally free, it can work in Windows, Mac OS X or Linux using Wine. There is one very interesting feature in this program - the result of simulation can be written into a wav file, so you can play this file to hear the result.

Download LTspice IV here: or here (a direct link): LTspiceIV.exe (15 MB). Additional libraries can be downloaded from here and here. (registration required)

After install, click on the program icon and you'll see the main program window:

The main window of LTspice program for circuit simulation

Now you have to create a new schematic file (from menu File --> New schematic), it will activate almost all icons in the top toolbar:

Icons in the top toolbar of the program LTspice

Apart from icons in the top toolbar, there is some useful function keys:

  • R - place a new Resistor on the schematic;
  • C - place a new Capacitor on the schematic;
  • L - place a new Inductor on the schematic;
  • D - place a new Diode on the schematic;
  • G - place a GND symbol on the schematic;
  • T - place a new text on the schematic;
  • S - place a SPICE directive on the schematic;
  • F2 - place a new component on the schematic;
  • F3 - Draft Wires;
  • F4 - Label a node;
  • F5 - Delete;
  • F6 - Duplicate (Copy a section of a schematic);
  • F7 - Move a section of the schematic;
  • F8 - Drag a section of the schematic;

All this functions also accessible via the Edit menu.

Example: how to create an op-amp based relaxation oscillator.

Press the key F2, it will show the window that allows you to choose a component, then select [opamps] (use double click), and choose an op-amp you want, in this example we will use LT1013:

The window with selection of components in LTspice circuit simulator

How to choose an opamp in the components window of the program LTspice

Now click somewhere on the schematic, in a place you want to put the opamp:

Placing the op-amp on the schematic

After the opamp is placed on the schematic, press ESC key to quit the current component selection mode. Now again press F2 key and in the component selection window go to the root directory. Select there the voltage component - this is the power supply, put it on the schematic in two places - click there twice - above and below of the op-amp:

Creating a circuit diagram in the LTspice simulator program

While the cursor has the shape of a component, it is possible to rotate it using the key combination Ctrl+R (see the hint in the bottom status bar of the main window). If a component is already placed on the schematic, press the key F7 (or use the Move button from the top toolbar), click on the component and press the key combination Ctrl+R.

Now put all other components on the schematic:

Adding components to the schematic in the LTspice circuit simulator

Use the key F3 to draw wires and the key F5 to delete a wire:

Drawing wires in the LTspice schematic

Now we need to enter component values for the capacitor C1, resistors R1, R2, R3 and power supply V2, V3. Move the cursor to a component, then press the right mouse button, here it the example for the capacitor C1:

How to enter a component value in the LTspice program

The capacitor C1 value is 1n, i.e. 1000 pF, because symbol n means "Nano" prefix, it is equal to 10-9. There is another prefixes:

  • m - milli = 10-3
  • u (or μ) - micro = 10-6
  • n - nano = 10-9
  • p - pico = 10-12
  • f - femto = 10-15
  • K - kilo = 103
  • MEG - mega = 106
  • G - giga = 109
  • T - tera = 1012

For the capacitance value of, for example, 100 pF, use designation of 100p, for 0.1 μF - 0.1u, for 1 Farad - 1 (just 1, with no prefix). The decimal point (".") is used as a decimal symbol. The lower and uppercase are treated the same way (you can use 1n or 1N, it's the same). The E notation can be used instead of decimal form, for example, 1n9 = 1900 pF.

Next, enter values for resistors, they are all of 100 Kohms:

Enter value for a resistor in the LTspice schematic

Instead of 100k you can use 0.1meg, it's the same.

For voltage sources enter 10 volts for each one:

Setting up a power supply source in the LTspice schematic

At the end, when all component values are entered, we will have this schematic:

The completed schematic in the circuit simulator LTspice

And now we have to set up a simulation mode. Select the Edit simulation Cmd from the menu Simulate, and fill the three upper fields of the first tab (Transient) for transient analysis:

Edit simulation Command in the LTspice program

Let's explain what it means:

0.01 - this is the full simulation time;
0 - the start time for a data to display;
1u - the maximum time step (the less it is, the more accurate plot we get, but it takes more time).

The lower field (.tran 0 0.01 0 1u) is filled automatically, it has all the parameters described above.

Now close the window Edit simulation Cmd, and place the text command somewhere on the schematic:

The simulation command placed on the schematic

And save the schematic (select from the menu File --> Save As).

To start the simulation, press the "Run" button from the top toolbar or select the command Run from the Simulate menu. You'll see the blank window of simulation. Hover the cursor over a node of the schematic (the cursor will change to a probe), and press the left mouse button. Now you'll see a voltage plot in the simulation window.

The main window of the LTspice with a voltage plot

To add a plot to the plot pane, click on the other wire while pressing the Ctrl key. Hover the cursor over a component, the cursor will change to a current clamp, and if you click, you'll see on the plot pane a current, flowing through the component.

To remove a plot from the plot pane, use Delete tool (press the key F5), you'll see the scissors shaped cursor.

How to write the signal into a file.

You have to label a node for the wire, from which the signal will be taken. Press the key F4 or select the command Label Net from the Edit menu:

How to add a label for a node in the LTspice simulator program

Name the node with a name, in this case it is named out, and put it on the schematic (on a wire):

The marked node on the LTspice schematic

Next, press the key S (or select the command Spice directive from the Edit menu), and type there this line:

.wave ./file.wav 8 11025 V(out)

How to write a signal into a file in the LTspice circuit simulator program

Be sure that the switch Spice directive is on.

The line .wave ./file.wav 8 11025 V(out) means that the signal will be written into the file with the name file.wav that will be created in the same directory as the schematic file. This wav file will have 8 sampling bits per channel and a sample rate of 11025 Hz. You have to use standard audio parameters for the signal, or else you will need to resample the wav file to listen it on your computer. You can write this file in any other directory, just change the path to the file: .wave c:/file.wav 8 11025 V(out).

To make the playing time longer we have to increase the simulation time, and increase the maximum timestep to accelerate the simulation:

Increasing simulation time in the LTspice

Here is one important note: the amplitude of a signal has to be in the range -1..+1 volts or amperes, or the signal will be distorted.

Let's change the circuit by adding a three stage RC filter and a voltage divider R7, R8:

Circuit diagram of the relaxation oscillator with a three stage RC filter in the LTspice

Now in the node out the signal is almost sine wave:

Sine wave signal at the output of the oscillator with the three stage RC filter in LTspice modelling program

Note, that if you are zooming the plot between two points with the spatial period, in the bottom status panel you'll see the signal frequency, in this example it is 1.35 KHz (the accuracy depends on the cursor positioning).

The audio file converted into MP3 format can be listen here: ltspice.mp3.

The file with the last schematic can be downloaded here.

How to use libraries in the LTspice.

Warning! By default, there is no CD4000 library in LTspice program, you have to download it here: Copy whole the directory CD4000 into LTspiceIV\lib\sym\CD4000, copy files CD4066B.lib and CD4000.lib into LTspiceIV\lib\sub directory.

Let's draw the schematic of the Schmitt trigger oscillator:

Circuit diagram of the Schmitt trigger oscillator based on the logic gate 40106

The logic gate CD40106B can be found in the [CD4000] directory (press the key F2 to go there):

CMOS CD4000 library in the LTspice circuit simulator

Set the time and Maximum Timestep of the simulation (0.001 and 100u):

Setting up simulation parameters for the Schmitt trigger oscillator in the LTspice

But when you'll try to run the simulation, you'll get the error message of "Unknown subcircuit":

The error message about an unknown subcircuit in LTspice

This means that the library with the gate CD40106B is not found. We have to include the library in the schematic. To do this, press the key S (or use the menu File --> Spice directive), in the Edit window enter the command .lib cd4000.lib:

How to use CD4000 library in the LTspice program

Be sure that the switch Spice .lib directive is on.

Now run the simulation and click the output of the logic gate, you'll set the result of the simulation:

Modeling the oscillator circuit in LTspice

The file with the Schmitt trigger can be downloaded here.

How to start the simulation of an astable multivibrator circuit in the LTspice.

Let's draw the classic astable multivibrator circuit, it is based on bipolar transistors, we can use here, for example, 2N2222.

Circuit diagram of the astable multivibrator drew in the LTspice

Note, that there is a text OUT on the wire at the right side of the schematic - this is the label of the node, press the key F4 to create it (or use the menu Edit-->Label Net) and place it on a wire you want to label:

How to place a label on a wire in LTspice

Just type the word OUT in the field and close the form (and press the button OK), you don't need to do anything more.

Now we have to setup a simulation command (in the menu Simulate --> Edit Simulation Cmd): .tran 0 0.01 10n (Stop Time - 0.01, Time to Start Saving Data - 10n)

If we will try to start the simulation (click the key Run in the top toolbar), there will be no oscillation. It fails because the circuit is symmetric - all components from the left side of the schematic (except the voltage source V1) are the same as all components at its right side, so parameters of transistor Q1, Q2 are the same and so on. In real circuits it's never happen.

There is some ways to solve this problem. Let's see the first one. We can change a component (any one) value just a little bit:

The value of resistor R2 is changed to allow to start the simulation

As we can see, the value of the resistor R2 is increased to 100.01 kΩ. But this is not enough, oscillations will not start. We need to add the startup directive to the simulation parameters - in the menu Simulate --> Edit Simulation Cmd check the option Start external DC supply voltages at 0V:

Changing simulation parameters to run the circuit in the LTspice

Now the line with simulation parameters will look like this: .tran 0 0.01 10n startup.

The directive startup means that independent sources will be ramped on during the first 20 microseconds of the simulation (check out the voltage across the voltage source V1 to see the voltage ramp). Now the astable multivibrator works:

The waveform at the output of the astable multivibrator

The second way to start oscillations. Lets' change the resistor R2 value back to 100 kohms and uncheck the startup option. Now place the SPICE directive .ic V(OUT)=5 on the schematic. This directive sets initial conditions of simulations, in our case it sets the voltage of 5 volts at the node OUT on startup. To add this directive, press the key T or select the Text item from the menu Edit:

Setting initial conditions for the schematic of the astable multivibrator

Make sure that the option SPICE directive is checked, then the text text will be treated as a directive! Press the button OK, and place the text somewhere on the schematic:

The circuit schematic with the SPICE directive that determines the initial conditions

The directive .ic V(OUT)=5 sets the initial voltage of 5 volts at the point OUT in the moment when the power supply voltage is applied to the circuit. After that, when the DC analysis is completed, the initial voltage went off. And now the astable multivibrator works:

The astable multivibrator oscillates

The circuit schematic of the astable multivibrator can be downloaded here: multivibrator.asc.

See also LTSpice: how to use the Current Controlled Switch