LTspice Tutorial: Part 2
have learned how to enter a schematic in LTspice®.
This LTspice tutorial will explain how to modify the circuit and apply
some different signals to it.
To save you
constructing a new schematic, download this file:
2nd order Butterworth low pass filter. The
shown in FIG 1
Note the voltage
source is missing. To test the frequency response of
the filter we could apply a sinewave input to the
circuit and measure the amplitude of the output,
then change the frequency of the sinewave and repeat
the process. Or we could apply an ac sweep to the
input and get a plot in the frequency domain instead
of the time domain.
To add a generic
voltage source go to 'Add Component' by clicking on
the symbol and
this should bring up the menu as shown in FIG 2
Scroll to the far
right and add a 'voltage' and place it in the
To implement an ac
sweep, right click over the voltage source and
select advanced to display the following:
Keeping the Function
selections as 'None' enter a voltage in the Small
Signal AC analysis box. Enter an amplitude of 1V
then click OK.
We now need to
configure the simulator to perform the ac sweep.
In the schematic
editor, click on Simulate -> Edit Simulation cmd
then click on the ac analysis tab. Enter the
parameters as shown in FIG 4
This sets the number
of steps to be displayed per octave, with a start
frequency at 10Hz and a stop frequency of 100kHz.
Click OK and put the simulation statement anywhere
on the schematic. The final circuit is shown in FIG
Save the file.
Clicking on the
running man symbol will run the simulation. Probing
the OUT node will plot the frequency response of the
filter, clearly showing roll of above 1kHz. The
phase response of the output with respect to the ac
signal source is also plotted on the right hand
If we want to magnify
a certain area of the plot, move the crosshairs to
the desired part of the plot, left click the mouse
and, holding it down, drag it over the area to be
magnified. The plot will then zoom into that area.
The coordinates of the crosshairs are shown in the
bottom left hand corner of the screen and when a box
is selected, these coordinates show the differential
values of the box. Since this example is plotted in
the frequency domain, the x-axis displays frequency.
If the x-axis shows the time domain, the coordinates
show time and when a box is selected the coordinates
show differential time and frequency.
Hitting the <F9> key
undoes this action.
If you want to zoom in
or out when in the schematic window, use the Zoom In
and Zoom Out symbols on the menu bar. Alternatively
the jog wheel on your mouse performs the same
function. Holding down the left mouse button and
moving it over the schematic allows you to pan over
Hitting the space bar
auto-sizes the schematic window.
The x-axis and y-axis
settings can be changed by moving the crosshairs
over the desired axis and left clicking the mouse.
To check the roll off
characteristics of the filter, we need to display
the cursors. Move the mouse to the 'Vout' logo at
the top of the plot pane and right click. This
brings up a menu to enable us to select between 1
cursor or 2. Selecting a single cursor results in
(the shortcut for
displaying the single cursor is to left click on the
waveform icon V(out)). To select 2 cursors, double
click on the Vout icon.
Moving the crosshairs
over the cursor and left clicking the mouse enables
us to move the cursor and measure the magnitude and
phase response of the circuit in the results box.
Closing the results box removes the cursors. If 2
cursors are selected differential voltages and
phases can be displayed.
We are now going to
change the input signal from an ac sweep to a
piecewise linear waveform. A piecewise linear
voltage source consists of a series of voltages
specified at certain instances in time with a linear
change in voltage between them.
Firstly, delete the
Simulation command (.ac OCT 10 10 100k)
Right click over the
input voltage source to bring up the parameters
dialogue box. Delete the ac amplitude and change the
function button from (none) to PWL (piecewise
The setting box should
look like FIG 7
The waveform above
starts at 0V, stays at 0V until 1m after which it
rises to 1V in 0.001ms. It stays at 1V until 2ms,
then falls to 0V in 0.001ms.
In the schematic
editors, click on Simulate -> Edit Simulation cmd
and click on the Transient tab. Set the transient
analysis to have a stop time of 5ms and click OK.
Clicking the running
man symbol brings up the plot pane as shown in FIG 8
Probing the IN and OUT
nodes shows that although the Butterworth filter has
excellent pass band performance, it is a poor filter
to use if trying to maintain the shape of a pulse.
A word of warning: If
the PWL input starts at a non zero voltage, the Y
axis of the plot pane will start at a non zero
Run this simulation:
LT1761 with Vin starting at 3.5V
The input to this 3v3
linear regulator starts at 3.5V and ramps to 5V.
Plot the output voltage. The Y axis of the plot pane
starts at 3.2V, not 0V
In the simulation
below, the PWL input voltage has been changed to
start at 0V instead of 3.5V. Now the Y axis of the
plot pane starts at 0V:
with Vin starting at 0V
Want to know more?
Tutorial: Part 3
If you want to learn
about noise measurements see this article:
Op Amp Noise Analysis
LTspice is a registered trademark of Linear