LTspice Tutorial: Part 1
The LTspice Tutorial below will take
through how to get started with LTspice®, the free
circuit simulation package from Linear Technology.
download LTspice, go to the
Home Page and click on the LTspice Download
icon. You can either register to get notifications
of updates, or just download the package anyway. If
you do not register, you can still update the
package as often as you like.
recommend you download LTspice XVII and not LTspice
IV. LTspice IV is not updated
Download the .exe file to a directory of your
the .exe file, accept the license agreement and
LTspice should start automatically and place an icon
on your desktop.
in LTspice, click on Tools-> Sync Release to ensure
you have the latest updates. It is worth repeating
this step every time you use LTspice to ensure you
have the latest models loaded.
LTspice has models of most of the LTC analogue part
numbers as well as 'jigs' to get you started. 'Jigs'
are ready made circuits including the desired
component and all of the surrounding resistors,
capacitors and inductors to enable you to
immediately start evaluating it without having to
place all the passives.
It is advisable to
create a separate directory to store your LTspice files so you do not overwrite the original
start, we are going to design a non inverting
amplifier with a gain of 10 and a 1kHz 1V sinewave
input and a load of 10k Ohms, based on the LT1012 op
Double clicking on the
desktop icon brings up the page shown in FIG 1.
Click on File -> Open
and navigate to C:\Program Files\LTC\LTspiceIV\Examples\jigs
and open up the 'jig' associated with the LT1012,
called 1012.asc. It should look like FIG 2
Save this file to your
bring up the 'jig' select File -> New Schematic then
icon and navigate to the component you need, then
click 'Open this macromodel's test fixture', as
shown in FIG 2a
Then save the jig to
your chosen directory.
To open the datasheet
for the part, right click on the part and Select 'Go
to Linear website for datasheet'.
Incidentally, I prefer
a white background instead of grey. To change this
go to Tools -> Control Panel then click on the
Waveforms tab, select Color Scheme, click on the
Schematics tab, then next to Select Items choose
Background from the drop down menu. You can then
move the Red Green and Blue sliders to pick a colour
of your choice.
We are going to edit
this schematic to get a non inverting amplifier as
The following shortcut
allow you to edit any schematic in LTspice:
move component without wires attached
move components with wires attached
rotates component (once it has been selected using
mirrors component (once it has been selected using
In addition to the
commands above, the LTspice toolbar shown in FIG 3,
allows us to insert components
In the schematic
above, V1 and V2 are the +/-15V supply to the
LT1012, so we will keep these. We also want to keep
V4, the input signal as well as the op amp.
Using the shortcut
keys and the toolbar construct the schematic shown
in FIG 4. It is worth noting that large areas of
circuit can be deleted/moved/copied by selecting the
appropriate <F> key, holding down the left hand
mouse button and highlighting that part of the
Note that R1 and R2
are generic resistors with no value. To change the
value of any component in LTspice, right click over
the component to bring up the basic component
properties. Holding down the <CTRL> key and right
clicking brings up a more comprehensive list of
properties. To change the values of R1 and R2, right click over these components and type 10k
into the Resistance box.
We now need to modify
V4 to give us a sinewave of 1kHz. Right click over
V4 and it will bring up the box shown in FIG 5
This dialogue box
allows us to choose whether V4 is a dc voltage,
Pulse, Sinewave, Exponential, Single Frequency FM or
Piece Wise Linear waveform. The only parameters we
need to modify are Amplitude (change this to 1) and
Freq (change this to 1k).
recognises 'M' to mean 'milli' so setting the
frequency to 1M will produce a sinewave of
1milliHertz. If a frequency of 1MHz is desired,
either use 1000k or 1MEG.
Click OK to return to
We now need to add
some labels to the circuit. This makes probing much
easier. Click on the Label icon and add IN to the
input and OUT to the output. Your circuit should
look like FIG 6
To set the simulation
conditions, click on Simulate -> Edit Simulation cmd
and enter 10ms in the Stop Time box as shown in FIG
We are now ready to
simulate the circuit. Save the file first.
Click on the Running
Man symbol in the toolbar as shown in FIG 8
The screen will divide
showing the schematic in one half and the simulation
window in the other. Click the mouse anywhere in the
schematic window. Moving the mouse over certain
parts of the circuit will highlight either a voltage
probe or current probe.
Hover the mouse over the
output of the op amp and click when the probe
appears to show the voltage at the output of the op
amp. Repeating this process at the input of the op
amp shows the input voltage. The resultant waveform
screen should look like FIG 9
LTspice Tutorial 1: Other Tips and
All circuits must have
Drawing a wire
straight through several components is an easy way
of connecting the components in series.
If you need to plot a
differential voltage, move the mouse to the positive
node of the voltage to be measured and once the
probe symbol has appeared, left click the mouse then
drag the probe to the negative node. The probe
colour will change from red to black. Release the
mouse and the differential voltage will be
If you want to plot
multiple waveforms with respect to a node other than
ground, navigate to that node, right click the mouse
and the following list of options will appear:
Reference'. Thereafter all plots will be referenced
with respect to that node.
Sometimes it is
convenient to have 2 plot panes, especially when
comparing 2 voltages of very different amplitudes.
To create multiple plot panes, move the mouse to the
plot pane, right click and select Add Plot Pane.
Left clicking on a specific pane loads the probe
results into that pane. Left clicking on the
waveform icon (eg V(out)) and dragging the icon to
the other pane, moves the waveform to the other pane.
To remove a waveform
from the plot pane, hit the <F5> key and delete the
appropriate waveform logo at the top of the plot
pane. As with the schematic editor, the <F9> key
undoes the last action performed in the plot pane.
Holding down the ALT
key and left clicking over a wire plots the current
in the wire.
Holding down the ALT
key and left clicking over a components displays the
instantaneous power in that component.
The latest version of
LTspice (LTspice XVII) allows the use of multiple
monitors, so the schematic can be displayed on one
monitor, while the plot results are displayed on a
second monitor. Right click in the Schematic Window
and select 'Float Window'. The Schematic Window can
now be moved between screens. The same can be done
with the Plot Window.
The toolbar can,
however, only address non floating windows, so the
Running Man symbol is greyed out when windows are
floating. To run the simulation, select the
Schematic Window, right click then select 'Run'.
Want to know more?
Tutorial: Part 2
LTspice is a registered trademark of Linear