ltspice basic practice.pptx

©2019 Analog Devices, Inc. All rights reserved.
JOE WEADICK (FAE, ILLINOIS & WISCONSIN)
JOE.WEADICK@ANALOG.COM
(847) 612-7983
LTspice XVII Basic Lab Class
1

2
Why Use LTspice?
► Stable SPICE circuit simulation with:
 Unlimited number of nodes
 Schematic/symbol editor
 Waveform viewer
 Library of passive devices
► Fast simulation of switch mode power supplies
 Steady state detection
 Turn on transient
 Step response
 Efficiency / power computations
► Advanced analysis and simulation options
 Not covered in this lab class (sort of)
► Outperforms or as powerful as pay-for tools
 In other words LTspice is free!
► Automatically builds syntax for common tasks
 2500+ macromodels of Legacy Linear
Technology products
 1500+ power products
 300+ Legacy ADI Products (power and amps)
LTspice is also a great schematic capture / BOM tool
SPICE = Simulation Program with
Integrated Circuit Emphasis

3
How Do I Get LTspice and Documentation?
 Go to http://www.analog.com/LTspice
 Left-Click on Download LTspice for Windows 7, 8 and 10
 Follow the instructions to install
 LTspice is a standalone application that runs on your computer
 At this link, you will also find:
 LTspice Download Links
 LTspice Demo Circuits
 LTspice Documentation
 LTspice Technical Articles & Videos
 SPICE Models

4
How Do I Get Started using LTspice?

5
How Do I Get Started Using LTspice?
► Demo Circuits: Use one of the 100’s of demo circuits available at analog.com
 Designed and Reviewed by Factory Apps Group
 Go to http://www.analog.com/LTspice or browse through the part’s webpage for LTspice simulation information
► JIG Files: Use a pre-drafted test fixture (JIG)
 Provides a good starting point, but is not production-ready
 Used to prove out part models, and are not complete designs
 Components are typically “ideal” components and will need to be modified based on your operating conditions
► Use simulation circuits posted on the LTspice Yahoo! User’s Group
 URL = https://groups.yahoo.com/neo/groups/LTspice/info
 Also contains many very helpful discussion threads and tutorials
► Use the schematic editor to create your own design
 LTspice contains models for most LTC power devices, opamps, and many more
 ADI opamp models are being added to the LTspice library (nearly 100 ADI models to date)
 LTspice can be used to simulate any analog circuit you can think of!

6
Demo Circuits at analog.com
► Go to http://www.analog.com/LTspice and scroll down to the demo circuits section:
What if I’m browsing the part’s webpage?

7
Demo Circuits at analog.com (cont.)
► Go to the part’s webpage (LT8641 example):
► Click on “Tools & Simulations” to find reference LTspice circuit(s)
http://www.analog.com/LT8641

8
What are Demo Circuits ?
► LTspice demo circuits are designed and reviewed by the LTC factory apps group
It remains the customer’s responsibility to verify proper and reliable operation in the actual application.
Printed circuit board layout may significantly affect circuit performance and reliability.
What if I cannot find a LTspice demo circuit ?

9
 Go to http://www.analog.com/LTspice or browse through the part’s webpage (right column)

10
Pre-drafted Test Fixture
► These simulations / designs are not production-ready, but are a great starting point!
► Used to prove out part models, and are not complete designs
► Components are typically “ideal” components and will need to be modified based on your operating
conditions
It remains the customer’s responsibility to verify proper and reliable operation in the actual application.
Printed circuit board layout may significantly affect circuit performance and reliability.

11
Opening a Test Fixture
1. Edit menu, select
“Component”
2. Search for
macromodel
(ex. LTC3412A)
3. Click Here

12
Opening a Test Fixture
Voilà !

13
New Components in LTspice Library With AD, ADP, ADM, and ADuM Prefixes

14

15
LTspice Yahoo! User’s Group
https://groups.yahoo.com/neo/groups/LTspice/info
Join the group here.
As of March 2019,
there are over 69,000
members!
Several hundred
message posts a
month!

16
 ADI part models are actively being added to the LTspice library (nearly 100 ADI models to date)

17
Start With a New Schematic
► To open up a blank schematic screen select “File” Menu and “New Schematic”
Blank schematic
a.k.a.
MasterPiece in progress

18
Using the Schematic Editor in LTspice

19
How to Wire up a Simple RC Circuit
►The completed exercise:

20
Toolbar and Keyboard Shortcuts
Place Circuit Element [F2]
Place Diode [D]
Draw Wire [F3]
Place Ground [G]
Label Node [F4]
Place Resistor [R]
Place Capacitor [C]
Place Inductor [L]
Zoom In
Pan
Zoom Out
Autoscale
Paste b/t Schematics [Ctrl+V]
Duplicate [Ctrl+C]
Find [Ctrl+F]
Delete [Del]
Place SPICE directive [S]
Place Comment/text [T]
Mirror [Ctrl+E]
Rotate [Ctrl+R]
Redo [Shift+F9]
Undo [F9]
Drag [F8]
Move [F7]

21
► Step 1: Open up a blank schematic screen
 Select “File” Menu and “New Schematic”

22
► Step 2: Add the passives and grounds
 Using the toolbar, select Resistor, Capacitor and Ground. Place these symbols on the schematic as shown below. Use
Ctrl+R to rotate before placement.
Select and place
res, cap & GND, or
use keyboard keys
R, C, and G
Tip: Ctrl+R to rotate
before placement

23
► Step 3: Add the voltage source
 Select “Edit” Menu and “Component”. From the component window, start typing “voltage” in the dialog box,
and click “OK”
1. Edit menu, select
“Component”
2. Type
“Voltage”
3. Click “OK”

24
How to Wire up a Simple RC Circuit (cont.)
►Step 4: Wire up the circuit
 Using the toolbar, select Wire, or, press F3
1. Select
“Wire” button

25
► Step 4: Wire up the circuit (cont.)
Left-Click ground
“Pull” wire up through the source
Left-Click here to anchor
“Pull” wire through the resistor
Left-Click here to anchor
“Pull” wire down through the capacitor
Left-Click here to anchor & finish
Hint: Press the ESC key at any time to clean up the schematic

26
► Step 5: Add net labels
 Using the toolbar, select Label Net (or press F4). Label the input/output nodes as shown below
1. Select “Label
Net”
2. Enter net
name
3. Place on wire

27
► Step 6a: Component values
 Right-Click on each component symbol to change its value as shown below
Right-click on
symbol
Or Right-click on
value

28
Using Labels to Specify Units for Component Attributes
► K = k = kilo = 103
► MEG = meg = 106
► G = g = giga = 109
► T = t = tera = 1012
► M = m = milli = 10-3
► U = u = micro = 10-6
► N = n = nano = 10-9
► P = p = pico = 10-12
► F = f = femto = 10-15
Hints
 Use MEG (or meg) to specify 106, not M
 Enter 1 for 1 Farad, not 1F

29
Editing Components
► You can also edit the visible attribute and label by pointing at the text with the mouse and
then right-clicking
► Mouse cursor will turn into a text caret
► Right-Click on the component to edit attributes

30
Component Database
► Resistors, capacitors, inductors, diodes, Bipolar transistors, MOSFET transistors, JFET transistors,
Independent voltage and current sources
► You can access a database of known devices

31
► Step 6b: Source parameters
 Right-Click on the voltage source and enter the parameters shown below under the “Advanced” tab.
Right-click source
Click
“Advanced”

32
► Step 6b: Source parameters
 Select the PULSE button and enter the parameters shown below:

33
Running and Probing a Circuit in LTspice

34
Summary of Hotlinks Used in This Presentation
►The following hotlinks are used in this presentation for opening up LTspice
simulation files
Note: Presentation Mode must be used for the hotlinks to work
Class exercise
Solution to exercise
Circuits to explore at your leisure

35
Running the RC Circuit Simulation – Transient Analysis
► With the RC circuit in the active window, click on the RUN button on the toolbar
► The Edit Simulation Command window will appear. Set the Stop Time to 60m and click OK.
► Using the mouse, click on the IN node and OUT node to display the input and output voltage
waveforms.
Run
Click here for
output
waveform
RCFilterTimeDomain.asc

36
► To add a measurement cursor to the waveform window, left+click the mouse on the waveform name.
Click to display
measurement
cursor. Click
and drag cursor
position.
► To add a second
measurement cursor
(paired cursors), just
left+click on the
waveform name again.

37
► To display the current in the resistor, just left+click on the resistor.
Click here for
resistor current
waveform

38
► Split the plot pane by selecting “Add Plot Pane” under the Plot Settings pull-down menu.
► Drag and drop the I(R1) waveform title into the new plot pane

39
Summary of the Waveform Viewer
► LTspice integrated waveform viewer:
 Plot the voltage on any wire by a simple point and click
 Plot the current through any component by clicking
on the body of the component
► When using the current probe, the convention of
positive current is from netlist pin #1 to pin #2.
► Add a waveform measurement cursor by left+clicking on
the waveform name. Add a second measurement cursor
by left+clicking on the waveform name again.
Voltage probe cursor
Current probe cursor

40
AC Analysis

41
AC Analysis Overview
►Performs small signal AC analysis linearized about the DC operating point
►Useful for analysis of filters, networks, stability analysis, and noise considerations

42
Simulating AC Analysis – RC Filter
► Single pole filter using RC network
► Syntax: .ac <oct, dec, lin> <Nsteps> <StartFreq> <EndFreq>
► Example: RC network and .ac dec 100 .01 1MEG
-3dB point:
1/(2*pi*R*C) = 159Hz
Right-click on .tran
command and select
“AC Analysis”
AC amplitude of 1 sets
magnitude to 0dB

43
Simulating AC Analysis – RC Filter
►Right-click on the .tran command
►Select AC Analysis tab
►Enter the following parameters:

44
Simulating AC Analysis – RC Result
Click here for
Bode plot

45
Simulating AC Analysis – Active Filter
► Single pole active filter using an opamp (AD8672)
Click here for
Bode plot
ActiveFilterACSweep.asc

46
Defining a Component Value as a Variable
(a taste of intermediate & advanced topics)

47
Defining a Component Value as a Variable (Using Parameters)
► The .param SPICE directive allows the creation of user-defined variables.
► To define a component value as a variable, replace the component value with a variable name
enclosed in curly braces. Example: {X}
Right+click to
change the
component
value to {X}
Add the
.param SPICE
directive (press
S on the keyboard)
RCFilterACAnalysis_Param.asc

48
Defining a Component Value as a Variable (Using Parameters)
► The simulation results are the same as when the component value was defined as 10K.
Click here for
Bode plot
RCFilterACAnalysis_Param.asc

49
Defining a Component Value as a Variable (Stepping Parameters)
► The .STEP command can be used to vary a component variable over a range of values to plot a
family of curves.
► This is very powerful and can be used for sensitivity and Monte Carlo Analysis.
Right+click to
change SPICE
directive to the
.step command
RCFilterACAnalysis_Step Command.asc

50
Defining a Component Value as a Variable (Stepping Parameters)
► For this AC analysis example, the simulation result includes three Bode plots, one each for R = 10K,
20K, and 30K
Click here for
Bode plot
RCFilterACAnalysis_StepCommand.asc

51
Running a DC/DC Converter Simulation
and Analyzing Circuit Performance

52
Running a DC/DC Converter Simulation
► Access the LTC3412A circuit
 Click File ---> Open, and navigate to the LTspice Lab folder on your desktop. Look for the file titled
“LTC3412A_DC_Load.asc”
 Or click “c” symbol on the right
LTC3412A_DC_Load.asc

53
Viewing Voltage Waveforms
► Plot the voltage on any wire by Left-Clicking it
 Tip: All Demo Circuits have INs and OUTs clearly labeled to help you quickly select them
Click here for
output
waveform

54
Viewing Current Waveforms
► Plot the current through any component by Left-Clicking on the body of the component
 Current flowing into a node is defined as being positive
Click here for
inductor current
waveform

55
Zooming In and Out on a Waveform
► In the waveform window, use the mouse to zoom in and out. Click and drag a box about the region
you wish to see drawn larger
► Using the toolbar, click on “Zoom full extents”, to zoom back out
Zoom Full Extents

56
Measuring V, I and Time in the Waveform
(Measurement Using Cursors)
► Right-Click on the waveform name in the waveform window
► For “Attached Cursor”, select “1st & 2nd”
► Position cursors to make desired measurements
1. 2. 3.
Result

57
Measuring V, I and Time in the Waveform
(Measurement Using Zoom Window)
► Drag a box about the region you wish to measure
 Left-Click, drag, and hold
► View the lower left corner of the window for the status bar. The dx and dy measurement data is
displayed here.
► Use Undo from the File menu or press “F9”

58
Viewing Differential Voltage Waveforms
► Left-Click on one node and drag the mouse to another node
 Red voltage probe at the first node
 Black probe on the second

59
Viewing Differential Voltage Waveforms
► To create a measurement reference node, Right-Click on the desired node and select “Mark
Reference”
 A black voltage probe is anchored to the selected node
► All measurements in the circuit are now referenced to the node with the black probe
► Hit the ESC key to remove the reference mark

60
Viewing Wire Current Waveforms
► Plot the current through any wire by Alt+Left-Clicking on the wire
 An ammeter will appear to indicate that the wire current will be displayed

61
Average & RMS Calculations
► Average & RMS Current, Voltage, or Power Dissipation
 Calculated only for the visible area of the plot window
► Click on inductor L1 to display the inductor current waveform
 Ctrl+Left-Click the I(L1) trace label in the waveform view
Example:
Measure average and RMS
current for inductor in
LTC3412A circuit. Zoom in
as shown for this
waveform.

62
Instantaneous & Average Power Dissipation
► Instantaneous Power Dissipation
 Alt+Left-Click on the symbol of the LTC3412A
 Waveform is displayed in units of Watts
► Average Power Dissipation
 Click, hold, and drag in the waveform window to
display waveform at steady state
 Ctrl+Left-Click on the Power Dissipation Trace
Label in the waveform view
 Waveform summary window will appear which
shows power dissipation in the IC
Example:
Measure the power dissipation in the
LTC3412A IC

63
Deleting Waveforms
► Method #1: Right-Click on a trace label to be deleted
 Select “Delete this Trace”
 Deletes only the selected trace

64
Deleting Waveforms
►Method #2: If the plot window is active hotkey F5 is equivalent
 Cursor turns into scissors
 Left-Click on one or more trace labels to delete. ESC to quit

65
Deleting Waveforms
►Method #3: Plot the same waveform twice in succession
 Deletes all but that waveform
Click,
click

66
Net Labeling

67
Advantages of Labeling
► Replaces the default SPICE node names with node names and waveform titles that are easy to
understand and remember
► Allows LTspice circuit nodes to match those on your production schematic, i.e. “TP15”
Without With

68
Labeling - Trick
► Highlight net from waveform viewer
 Alt-Left-Click on the label in the waveform viewer (i.e. V(n006)) and it will now highlight that particular net on
the schematic. You can also use the search function ( )
Net
Highlighted
Alt-Left-
Click

69
Generating a BOM and Efficiency Report

70
BOM
► Under View select Bill of Material
 Displayed on Diagram
 Paste to Clipboard

71
Steps to Computing Efficiency
► Note: Efficiency will only be calculated in the steady state condition
► 1.) Right-Click the .tran statement on the schematic to bring up the Edit Simulation Command
dialog box
► 2.) Check the box “Stop simulating if steady state is detected” …
1. Simulate menu,
select “Edit
simulation Cmd”
2. Check
Box

72
► 3.) Load must be a current source or a resistor labeled Rload**
4.) Run the simulation …
The Good The Bad
This will be treated
just like any other
resistor – efficiency
will read ZERO

73
► 5.) Upon completion select the View dropdown menu, Efficiency Report, then Show on Schematic
► 6.) Efficiency report will be pasted under the schematic

74
SMPS Efficiency Tips
► LTspice will not always be able to determine steady state, but this is rare!
 Workaround: Alt+Left-Click on individual component and integrate waveform
► Probe the various nodes and verify the circuit is stabilized
 If not, edit the .tran statement and increase the Stop Time parameter. Re-run simulation
► For multiple output and/or multiple input supplies, efficiency must be determined partially by hand
from the efficiency report
 Alternatively use behavioral models
► Right-Click any component will report power dissipation if steady state has been detected or Mark
Start/End has been used
► If circuit has stabilized for a long time and LTspice still hasn’t detected the steady-state
 Use Mark Start/End (Simulate pull-down menu ---> Efficiency Calculation ---> Select Mark Start/End)
 Only steady-state data is displayed before Mark End

75
Simulating a Transient Response

76
Current Load and Pulse Function
► You can simulate a load with a Resistor or Current (active) load
► In particular, the Pulse function with a current load is helpful for transient response analysis
 Steps a current load from one load value to another load value
LTC3412APulseLoadSolution.asc

77
Edit the Current Load to a Pulse Function
► Edit the .tran directive in the LTC3412A simulation to disable steady state detection
► Right-Click on the current load
 Select “Pulse”
 Modify the attributes (see below). Click “OK”
*
Forces current
to be zero when
voltage is zero

78
Run the Simulation for Transient Response
► Run the simulation
► Click on the OUT node to display Vout
► Click on the output current load to
display Iout
► Notice the presence of the pulse load
► Use the application of the pulse load /
transient response to verify stability
and modify the compensation
components as necessary.
LTC3412APulseLoadSolution.asc

79
Importing Third Party SPICE Models

80
Steps for importing a third-party SPICE model:
1.) Download the SPICE model file from the manufacturer’s website
2.) Place the SPICE model file in the same directory as the LTspice simulation file
(simplest). It can be placed in another folder on your computer or even on a network
drive.
3.) Open up the SPICE model file and note the device name
4.) Add the following SPICE directive to the LTspice simulation schematic (Edit pull-
down menu ---> SPICE Directive):
.include spice_model_file_name.abc
5.) Modify the device name on the LTspice schematic to match the device name
listed in the SPICE model file (Right+Click on the device name on the simulation
schematic and modify accordingly).

81
The following items are CRITICAL!
1.) The file name in the .include statement must match the SPICE model file name
identically! The file name syntax is can be anything, just make sure that all of the
characters match.
2.) The device name on the LTspice simulation schematic must match the device
name in the SPICE model file identically! The device name syntax can be
anything, just make sure that all of the characters match.

82
SPICE Model
Example #1:
File name = 1N5244B.mod
Model name = 1N5244B1
SPICE Model
Example #2:
File name = Joe.txt
Model name = Everest
Summary: The file and device
names are irrelevant. Just make
sure that the LTspice simulation
device name and .include file name
match those of the SPICE model file.

83
Hands-on Exercise:
1.) Navigate to the LTspice Training Files folder
2.) Open up the simulation file titled “Zener Import
Example.asc”
3.) Open up the SPICE model file titled
“1N5244B.mod” and note the device name.
4.) Modify the simulation file so that it uses the
1N5244B third-party SPICE model based on the
instructions provide on the previous slides
5.) Run the simulation and probe the IN and OUT
nodes

84
Solution:
1.) Zener name changed to 1N5244B1
to match device name in the SPICE
model file. Right+Click on the diode
name text to change.
2.) .include SPICE directive added to link
to the SPICE model file. Use the Edit
pulldown menu ---> SPICE Directive to
add this SPICE directive to your
simulation.
3.) Result after clicking on the Running
Person symbol on the toolbar and
probing the IN and OUT nodes.

85
Steps:
1.) Download the AD8237 SPICE model from the ADI website
2.) Open up the AD8237 SPICE model using LTspice
3.) Use LTspice to autogenerate the schematic symbol (right-click on the .SUBCKT statement)
4.) Wire up the circuit
Importing Third Party SPICE Models: Practical Example Using AD8237

86
Autogenerated Schematic Symbol:

87
Final Implementation:

88
More Information and Support

89
ADI / LTC Design Tools That Autogenerate LTspice Simulation Circuits
1.) LTpowerCAD
http://www.analog.com/LTpowerCAD
2.) Analog Filter Wizard
http://www.analog.com/designtools/en/filterwizard/
3.) Photodiode Circuit Design Wizard
http://www.analog.com/designtools/en/photodiode/

90
Reminder to Periodically Sync Release
►It is important to sync your release of LTspice periodically to get the latest updates
 Software updates and bug fixes
 Models
 Sample circuits and examples
Tools pull-down menu ----> Sync Release
**May need to run LTspice as administrator or run “Elevated”

91
Reminder to Periodically Sync Release (Windows)
► Vista, Win7, and Win8 users (any UAC-enabled OS)
 You must “Run as administrator” LTspice.exe or its shortcut even if you are logged in as an administrator

92
Reminder to Periodically Sync Release (Mac)
1. Open
“Control Panel”
2. Under
“Operation”
3. “Sync
Release”
for Mac

93
Built-in Help System

94
Appendices

95
Other Resources
► LTspice forum: Use simulation circuits posted on LTspice Yahoo! User’s Group
 Go to https://groups.yahoo.com/neo/groups/LTspice/info
 Also contains many very helpful discussion threads
► Educational Files: Check out LTspice capabilities using the education examples
 Available on C:Program FilesLTCLTspiceXVIIexamplesEducational
► LTspice videos: Video tutorials by Linear’s technical staff
 LTspice Videos at www.analog.com
► LTspice Videos on YouTube!
 https://www.youtube.com/results?search_query=ltspice
► LTwiki: Undocumented features …
 http://ltwiki.org/
► Wurth LTspice Book – available at Amazon, or, contact your local Wurth field sales engineer

96
Other Resources – Educational Files
Design examples
demonstrating LTspice
capabilities

97
Other Resources – LTwiki
► http://ltwiki.org/

98
Other Resources – LTspice Book
Other Resources – LTspice Book

99
Appendix - Steps to Calculate Power Supply Efficiency
► Efficiency will only be calculated in the steady state condition
► Right-Click the .tran statement on the schematic to bring up the Edit Simulation Command dialog
box
► Check the box “Stop simulating if steady state is detected”
► Load must be a current source or resistor labeled Rload
► Run the simulation
► Upon completion select the View dropdown menu, then Efficiency Report, then Show on
Schematic
► Efficiency report will be pasted under the schematic

100
Appendix – Summary of Special Mouse and Keyboard Commands
► Schematic-Based Special Commands
 Alt-Left-Click on a wire
 This will display the waveform for the current flowing in the wire
 Alt-Left-Click on a component
 This will display the instantaneous power dissipation in the component
 Ctrl-Right-Click on a component
 Allows you to edit embedded component attributes
► Waveform-Based Special Commands
 Ctrl-Left-Click on a waveform title
 Displays the average and RMS values for the waveform
 Left-Click on node and drag to another node
 Displays differential voltage
 Alt-Left-Click on the label in the waveform viewer (i.e. V(n006))
 Particular net on the schematic is highlighted

101
Appendix – Summary of Additional Features
► Pause a simulation
 “Simulate” pull down menu ---> Pause
 There is no toolbar button for this function
► Zoom in/out using the schematic editor:
 Just use the wheel on your mouse
► Pan around a schematic
 Left-Click-Hold the mouse, then drag
 Tilt wheel to move right and left
► Move a window to another monitor (new to LTspice XVII)
 Right-Click on window contents, then from the context menu check box “Float Window”
 Left-Click-Hold the window title bar to drag to another monitor

102
Thank you for attending, and happy simulating!
Homework: Once you return to the office, go back over
the training materials within a week!

ltspice basic practice.pptx

Recommended

Recommended

More Related Content

What's hot

What's hot (20)

Similar to ltspice basic practice.pptx

Similar to ltspice basic practice.pptx (20)

More from HabyarimanaProjecte

More from HabyarimanaProjecte (9)

Recently uploaded

Recently uploaded (20)

ltspice basic practice.pptx