SlideShare a Scribd company logo

LTspice.ppt

Download as PPT, PDF
D
DrVikasMahor

LTspice IV is a free SPICE circuit simulator developed by Linear Technologies. It allows users to schematically capture circuits and perform DC and transient analyses. While more advanced than simulators with schematic capture, LTspice requires knowledge of SPICE directives and has limited component libraries. However, it is widely used due to being free, fast, and powerful. The document provides guidance on using LTspice's interface and features such as adding models, performing analyses, and viewing waveforms.

Engineering
1 of 90
Downloaded 13 times
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53
54
55
56
57
58
59
60
61
62
63
64
65
66
67
68
69
70
71
72
73
74
75
76
77
78
79
80
81
82
Most read
83
84
85
86
Most read
87
88
89
90
Most read
1 Electronics Principles & Applications 8th Edition Dr. Vikas Mahor LTspice IV
2 LTspice IV • A freeware SPICE circuit simulator written by Mike Engelhardt at Linear Technologies http://www.linear.com/ – SPICE I and SPICE II were written using the FORTRAN programming language. SPICE III was written using the C programming language (U.C. Berkeley, 1985). http://bwrc.eecs.berkeley.edu/Classes/IcBook/SPICE/) • LTspice was written to support circuit designers who evaluate or use Linear Technology products. – It includes an extensive library of Linear Technology devices. • It has schematic capture and is much easier to use than traditional text-based SPICE. – Traditional SPICE requires a text file called a netlist that describes the circuit to be simulated. – With schematic capture, the user can enter a circuit using schematic symbols via a graphical user interface.
3 LTspice IV • Is powerful and fast, but is not as intuitive for beginners as simulators such as Multisim – Requires more knowledge about SPICE directives and terminology – Has a limited (mostly proprietary) device library – LTspice has only basic behavioral gates for digital circuits. It is expandable, but this requires knowledge about SPICE and device behavior. • Is worth learning about – Since it is free, fast, and powerful, it is one of the most widely used circuit simulators at this time. – Many professionals consider it to be superior to some commercial simulators.
4 LTspice IV is a free download and can be found on the Linear Technology website: http://www.linear.com/designtools/software/switchercad.jsp
5 Get started by clicking File and then New Schematic, or hold down the Control key and then press the “N” key (Ctrl+N). It’s easy to “draw” a circuit.
6 Drawing a circuit … is easier if the grid is active. Click on View and then Show Grid. Or, you can type Ctrl+G.
7 Delete tool It is easy to place grounds and basic components. Click on the desired component and then move the mouse to position it and then left click to place it. You will find that the connectors (square blue boxes above) snap to the nearest grid points. To place another component of the same type, move to the next location and click the left mouse button again. To cancel or quit a component type, click the right mouse button. It is often more time efficient to place all of the resistors, then the capacitors, and so on. Use the scissors (delete tool) to remove components and wires.
8 After a component has been selected, it can be rotated by holding down the Control key and then pressing the R key. Here, D1 was placed first (by left-clicking in the desired location on the schematic) followed by Control+R and then D2 was placed followed by Control+R again and so on.
9 Control+E was used here before placing Q2 on the above schematic. Note that Q2 is the mirror image of Q1. Control+E is the mirror command. Control+R and Control+E are keyboard shortcuts. Rotated components Mirrored components Rotated and mirrored
10 The menu command Tools→Control Panel→Drafting Options→Hot Keys allows you to define your own keyboard shortcuts.
11 Additional components are available by clicking on the gate symbol or by pressing the F2 key. Suppose you need a voltage source. Choose “voltage” from the component symbol list and then place the source on the drawing area with a left click. Right click the source to specify the voltage. To specify a sinusoidal voltage source, select Advanced after right clicking. or
12 Specifying a SINE ac voltage source Amplitude and Frequency (V1, as shown here, is a 44-V dc source.)
13 Use the pencil tool to connect the components. Left click a terminal (blue box) and then move the mouse to the connecting terminal and left click again. The crosshairs below are positioned to connect R4 to R5. The blue boxes disappear after they are connected. Unconnected nodes can cause Netlist errors.
14 Tool Bar Summary Place Circuit Element Draw Wire Place Ground Label Node Place Resistor Place Capacitor Place Inductor Place Diode Move Drag Undo Redo Rotate Mirror Place Comment Place SPICE Directive Zoom In Pan Zoom Out Auto Scale Delete Copy Paste Find Simulate
15 Or, click Select Resistor to view a Standard list. Place a resistor and right click it to enter its values. You must specify component values.
16 Right click the resistor label to enter a new reference designator. You can specify vertical text.
17 Models are required. • Missing models will generate error messages. – The next slide shows an example. – LTspice does not have a model for the 1N4001 diode. • There are several ways to add models.
18
19 You can expand the component data base (add models). • For example, suppose that you want to simulate a circuit using a BFR540 transistor and that you have the SPICE model saved in text format via Windows Notepad (go to Start, Programs, Accessories to launch this basic text editor). – Load the SPICE model into Windows Notepad and then Copy it to the clipboard using Control+A followed by Control+C. – Use Windows Notepad with File Type set to All Files to open the file C:Program FilesLTCSWCADIVlibcmpstandard.bjt, scroll to the end of that file, and then paste the model from the clipboard (Control+V) and then Save the file. – The next time that you run LTspice, the BFR540 will be available as a choice when selecting an NPN BJT transistor as shown on the next slide.
20 CMRR Here it is!
21 A SPICE model for the BFR540 .MODEL BFR540 NPN + IS = 1.04516E-015 + BF = 1.84359E+002 + NF = 9.81774E-001 + VAF = 4.16981E+001 + IKF = 1.00000E+001 + ISE = 2.32436E-013 + NE = 2.02825E+000 + BR = 4.39917E+001 + NR = 9.92532E-001 + VAR = 2.09773E+000 + IKR = 1.66296E-001 + ISC = 1.29849E-016 + NC = 1.06486E+000 + RB = 5.00000E+000 + IRB = 1.00000E-006 + RBM = 5.00000E+000 + RE = 3.53552E-001 + RC = 1.34000E+000 + EG = 1.11000E+000 + XTI = 3.00000E+000 + CJE = 1.97895E-012 + VJE = 6.00000E-001 + MJE = 3.32695E-001 + TF = 7.45719E-012 + XTF = 1.14072E+001 + VTF = 3.15854E+000 + ITF = 1.56917E-001 + CJC = 7.93745E-013 + VJC = 1.85522E-001 + MJC = 8.41656E-002 .ENDS
22 Also, a SPICE model can be added directly to the schematic.
23 • Copy the model to the clipboard. – Left click and hold and drag over the model and then capture it with Control+C. e.g. .MODEL 1N4001 D IS=29.5E-9 RS=73.5E- 3 N=1.96 CJO=34.6P VJ=0.627 +M=0.461 BV=60 IBV=10U • Click on .op on the toolbar • Paste the model into the window. – Control+V. • Click OK. • Place the model on your schematic with a left click. • This method is often preferred when sharing circuits with others. – The necessary model or models are imbedded in the circuit file. Adding a model to a schematic
24 Including a model from a file 1/ Click on .op. 2/ Enter the following text: .include filename.txt (where filename is the name of your model file, such as zener6, or 2N3055 and has been saved as a .txt file). 3/ Click OK. 4/ Place the SPICE-directive on your schematic where you want it to appear with a left-click. Note: It is advisable to save the model file to the same folder as your circuit file. The same applies for model files including sub-circuits.
25 Where does one obtain SPICE models? • Search the Internet … many are available as free downloads or can be copied to the clipboard and then pasted into Windows Notepad (or onto your schematic via .op on the toolbar). Some links are provided at the end of this presentation. • Search device manufacturers’ websites. • Modify an existing model. • Create your own. – Software is available. http://www.intusoft.com/spicemod.htm • Or, you can use a subcircuit.
26 Subcircuits (.SBCKT) • Are often used when repetition occurs. – Better than cluttering the schematic with redundant information • Also can be used to replace a complicated device such as an OP-AMP, a DIAC or a TRIAC. • The next slide shows a common dimmer circuit where the DIAC and TRIAC functions are defined by subcircuits. – LTspice has pre-defined schematic symbols for DIACS and TRIACS, but no corresponding models.
27
28 More about models and subcircuits Models given as .MODEL statements are for intrinsic SPICE devices such as diodes and transistors. The .MODEL statement gives the parameters for the specific component. The general behavior of the device is already known by SPICE … only the parameters need to be given to finish specifying the component's electrical characteristics. On the other hand, models given by .SUBCKT statements define the modeled component by a collection of intrinsic SPICE devices. For example, the SPICE model of an opamp would be given as a subcircuit. In the previous slide, the SPICE models of a DIAC and a TRIAC were specified as subcircuits.
29 LTspice is useful for analyzing circuits designed by others. • It is sometimes only necessary to use it to review and experiment with circuit files that have already been created. – Many can be found in the LTspice subdirectories. – Some examples are available for download. This is an outstanding example: http://cmosedu.com/cmos1/book.htm
30 How to run an existing circuit file • From the File menu, select Open. Make sure the file type is set to Schematics. • Some good examples are available in C:ProgramFilesLTCSwCADIVexamplesEducational (created on your hard drive when you install LTspice). • Some appropriate examples for the McGraw-Hill basic skills series are available on the website: http://highered.mcgraw- hill.com/sites/0073106941/student_view0/lt_spice_instru ctions_and_support_files.html (You probably have these files if you obtained this presentation from the McGraw- Hill site.) • The next slide shows a circuit from Schuler’s book. To view the dc voltages and currents, a dc analysis is selected by first clicking on Simulate, then Edit Simulation Cmd. – The SPICE directive is .op.
31 CMRR SPICE directive for dc analysis
32 The DC operating point selection provides all node voltages and device currents. When you click OK, the SPICE directive .op is placed on the schematic.
33 A ground is required for simulation.
34 -24V -12V 40W 28.8W 9.6W 1.2W 12W -88W -3.6W After a DC operating point analysis, moving the cursor over the schematic reveals the various node voltages, currents, and the dissipations in each component. These values are displayed in the lower left portion of the screen. DC operating point (I(R5) = 200 mA Dissipation = 1.2 W Placing the cursor here shows the current and the dissipation in R5, as shown below. Summing the dissipations in this circuit produces zero. The negative signs at V1 and V2 indicate that they are power sources.
35 It is also possible to display the dc voltage at one or more nodes on the schematic. Run the simulation and then right-click any empty area on the schematic and select View Place .op Data Label as shown below.
36 Then, move the rectangular cursor to the desired node and click it. The dc voltage at that node will be displayed on the schematic. Repeat the procedure to add nodes.
37 After you have one or more nodes selected, you can change circuit values and re- run the simulation to see the effect on the selected dc node voltages. R2 has been changed from 20 ohms to 10 ohms.
38 You can choose horizontal orientation for voltage labels by placing the small square at the bottom of the selection rectangle on a horizontal wire.
39 Waveforms • Waveforms are what one sees on an oscilloscope (graphs of instantaneous voltages versus time). • Waveforms can be viewed via the transient analysis option. Click on Simulate, Edit Sim Command, and then select the Transient tab. • The next three slides show the procedure.
40 Load the circuit from the file menu. Then, click run. Reference: Schuler, 7th edition, page 247 … the stiff current source has been replaced with a resistor. Probe both the base and the collector of Q2. Without the stiff current source, the CMRR is notably poorer.
41 Move the cursor to the desired node. When the cursor changes to a probe, click the left mouse button to view the waveform. A small differential signal plus a large common-mode signal
42 Move the cursor to the collector. Left click and now two waveforms are shown. Can you see the 60 Hz common-mode component at the collector of Q2?
43 The next slide demonstrates the value of simulation when evaluating circuit performance. • The differential amplifier circuit is much improved with a stiff current source. • The common-mode rejection ratio (CMRR) is remarkably better. – The common mode signal cannot be seen in the output. • Circuit simulators make it easy and fun to investigate issues such as this.
44 Stiff current source The 60 Hz common-mode signal is too small to be seen here.
45 Remember, waveforms are available via transient analysis. • You must specify the time duration of a transient analysis by specifying a Stop Time. – Often, this is all that is required. • You can also specify the Time to Start Saving Data. – Useful in circuits where the start-up period is not important. • You can also specify the Maximum Timestep.
46 CMRR Go to Simulate and then click on Edit Simulation Cmd. The time duration of a transient analysis is like choosing the time base setting on an oscilloscope.
47 For a basic analysis, this is often all that needs to be specified.
48 In this circuit, the common-mode signal is 60 Hz. A 60 Hz signal has a period of roughly 17 milliseconds. Thus, a Stop Time of 20 milliseconds is a reasonable choice.
49 Expanded waveform measurements are easy. Hold the left mouse button down and drag a box around the area of interest. Before you release the button, the measurements are available here: dx = 500 us (2 kHz) dy = 4.7 V Box
50 When you release the mouse button, the area inside the box will be zoomed to fill the waveform display. Restore the original waveform by right-clicking in the waveform area and then selecting Zoom to Fit or simply press Ctrl+E.
51 To obtain an accurate frequency measurement, draw a box around several cycles and then draw a second box to capture one cycle.
52 1.572 kHz This box captures one cycle. (The peaks are easier to identify than the zero crossings.) The output frequency of this Wien bridge oscillator is predicted by 1/(2πRC), thus we can expect an output at 1.59 kHz.
53 To obtain the voltage difference across two nodes, move the cursor to the first node and left click when it changes to a red voltage probe and then without releasing the mouse button, move to the second node and when the cursor changes to a black voltage probe, release the mouse button.
54 To determine the Average and RMS values of a waveform, hold down the Control key and left click the waveform’s label. Ctrl+Left Click here
55 The Fourier transform • Converts from the time domain to the frequency domain (the signal spectrum) – Schuler, 7th edition, page 500 • The FFT (fast Fourier transform) is available in LTspice. – After a waveform is plotted, right click in the waveform window and select FFT. Choose the node of interest and then click OK. Left click the node label in the FFT window and then use the keyboard arrow keys to make accurate measurements of frequency and amplitude for the various spectral components. Left click and hold to draw a box around a part of the graph to expand it.
56 FFT (frequency domain) display Time domain display
57 Expanded FFT display Note: you can increase the simulation time for better frequency resolution. Resolution = 1/Time
58 Simulation time = 0.001 seconds Resolution = 1 kHz Simulation time = 0.01 seconds Resolution = 100 Hz
59 In addition to increasing the simulation time, you can turn off data compression for better resolution (Tools  Control Panel  Compression). The next slide shows a significant improvement in dynamic range with data compression turned off. Default data compression No data compression
60 FFT with default data compression (90 dB range) FFT with no data compression (approaching a 120 dB range)
61 The option plotwinsize determines the number of data points to compress in one window. Set plotwinsize to zero to disable compression. Data compression will always be turned off, regardless of the control panel settings (an advantage when sharing circuits with others).
62 Individual waveforms can be placed onto different plot panes. • Right click in the waveform pane and then select Add Plot Pane. • The next slide shows the usefulness of this feature. – With all five waveforms on one plot pane, the display is confusing. – Separate plot panes make it easy to see the divide-by-two action of each flip-flop.
63
64 There are three important waveforms here. Three plot panes add clarity. 555 one-shot Input (TRIG) Threshold waveform Output
65 A dc offset is also available. • The next slide shows a D/A converter. • The input waveforms were separated by right- clicking on the node name, e.g. V(b1), as shown below, and adding a dc offset of +2 volts. • It also shows how colors can be chosen by using Tools→Color→Preferences→Selected Item→Waveform→Background→Grid→Axis dc offset V(b1)+2
66 0 dc offset +2 dc offset +4 dc offset +6 dc offset Separate plot plane
67 Current waveforms • Moving the cursor to the inside area of a component, after a transient analysis has been run, displays the current waveform in that component. • When the cursor morphs to a current probe: – left click to see the current waveform. • This is illustrated in the next slide.
68 Current waveforms can be obtained after a transient analysis by moving the cursor to the inside of a device. When the cursor changes to a current probe, left click the mouse to obtain the current waveform. To display the current in a wire, Alt-left click the wire. The current probe, like the voltage probe, shows time variations after a transient analysis. Here, the current in R1 averages 2 mA (which was measured earlier in a dc analysis) and the current fluctuations in R1 are easy to see. Current probe icon
69 The current in Q1 is constant. The constant current source is doing its job!
70 To display a power waveform (instantaneous power), hold down the Alt key and left click on the component of interest (after the cursor has changed to a thermometer). e.g., Alt+click here.
71 To determine the average power dissipation, Control+left-click on the label. Ctrl+left-click
72 AC Analysis • Provides the frequency response of a circuit – Both the amplitude and the phase angle are graphed as a function of frequency (Bode plot). • Go to Simulate, Edit Simulation CMD, and then click on the AC Analysis tab. – You must enter the Number of points per sweep interval, the Start Frequency and a Stop Frequency. – You can also choose various sweep intervals. • Octave, Decade, or Linear
73 Output Input AC Analysis provides the frequency response of a circuit. One of the signal sources must be designated as the input by specifying an AC Amplitude for Small signal AC analysis. Run the simulation and then probe the output for the Bode plot. Amplitude Phase Spice directive
74 Ctrl+left-click the label to measure bandwidth.
75 Here, the only change is the transistors. This illustrates the need for proper SPICE models when investigating issues such as bandwidth. The BFR540 is a high-frequency transistor. BFR540 2N3904
76 The .measure directive • Is useful to find instantaneous values and values over intervals • The next slide shows an example of an instantaneous measurement. Keyword Operation performed over interval AVG Compute the average value of <expr> MAX Find the maximum value of <expr> MIN Find the minimum value of <expr> PP Find the peak-to-peak value of <expr> RMS Compute the root mean square value of <expr> INTEG Integrate <expr>
77 vi: v(exponential_a)=0.632013 at 0.001 Run->View->View SPICE Error Log will show the instantaneous value at 1 ms.
78 The SPICE .STEP directive has been added to show the charge and discharge curves for capacitor values from 0.2 microfarads to 1.2 microfarads in 0.2 microfarad steps.
79 Here, bandwidth is measured. (8.5 Hz to 2.8 MHz)
80 Configuring LTspice • There are many user options. – SPICE options (e.g. integration method) – Drafting options including font properties – Data saving defaults – Compression • Hint: turn compression off for the least distortion for analog circuit simulations. – Most options are available via the control panel. • The next two slides illustrate some configuration choices.
81 Tools  Control Panel  Operation LTspice generates several kinds of files. To save disk space and avoid clutter, these files can be deleted automatically.
82 Tools  Color Preferences LTspice allows color choices for waveform plots and the background on which they are plotted. Also, the axes and grid colors are selectable
83 Support for LTspice • The next slide shows an example of the built-in help system. • The help file is a downloadable and printable document: http://ltspice.linear.com/software/scad3.pdf • There are numerous other resources. Check the Links slide at the end of this presentation.
84 Press F1 for the Help System. You can download the User’s Manual from: http://ltspice.linear. com/software/scad 3.pdf
85 The help files explain many things: for example, how to model transformers.
86 Some “gotchas” and hints • “M” and “m” are interpreted the same by SPICE. Thus, a resistor value of 10M is the same as 10m (ten milliohms or 10-3). – Use 10MEG (or 10E6) to specify ten megohms. • Do not enter “1F” or “1f” as the capacitance for a one- farad capacitor (enter “1”). “F” and “f” designate the prefix femto (10-15). • SPICE will not allow voltage sources in parallel, even when of the same value. – Add series resistances. • SPICE will not allow current sources in series, even when of the same value. – Add parallel resistances.
87 Prefixes are case insensitive: T = t, G = g, and so on • T = terra = 1012 • G = giga = 109 • MEG = meg = 106 • K = kilo = 103 • M = milli = 10-3 • U = micro = 10-6 • N = nano = 10-9 • P = pico = 10-12 • F = femto = 10-15
88 LTspice leading characters • A special functions device • B arbitrary behavioral source • C capacitor • D diode • E voltage dependent voltage source • F current dependent current source • G voltage dependent current source • H current dependent voltage source • I independent current source • J JFET transistor • K mutual inductance • L inductor • M MOSFET transistor • O lossy transmission line • Q bipolar transistor • R resistor • S voltage controlled switch • T lossless transmission line • U uniform RC-line • V independent voltage source • W current controlled switch • X subcircuit invocation • Z MESFET transistor • * comment • + continuation of prior line • . simulation directive
89 LTspice IV final notes • Like many modern software tools – it is relatively easy to begin using but one must spend some time to discover and then master the most powerful features. • As freeware goes, it is outstanding! – It is relatively bug-free. – It is compact and very fast. – It is regularly updated. • A tip for students: – Knowing how to use a professional level circuit simulator looks great on your resume!
90 Links http://www.intusoft.com/models.htm#freemodels http://www.penzar.com/links.htm http://ee.cleversoul.com/simulation.html http://cmosedu.com/videos/videos.htm http://cmosedu.com/cmos1/book.htm http://www.onsemi.com/site/support/models http://www.coilcraft.com/modelsswcad.cfm http://tech.groups.yahoo.com/group/LTspice/ http://ltspice.linear.com/software/scad3.pdf

More Related Content

PDF
VLSI Technology Trends
Usha Mehta
 
PPT
basic-electronics
ATTO RATHORE
 
PDF
Power Amplifier
Jason J Pulikkottil
 
PDF
Design of FIR filters
op205
 
PDF
Amorphous Materials: Structural Principles and Characterization
University of Wisconsin MRSEC
 
PPTX
Crystal Defects
Vikash Prasad
 
DOCX
Eut 440-2013-2014-sem-1-final-exam-answer-scheme
Shahril Majid
 
PPT
Aterramento
FRANCESCO GALGANO
 
VLSI Technology Trends
Usha Mehta
 
basic-electronics
ATTO RATHORE
 
Power Amplifier
Jason J Pulikkottil
 
Design of FIR filters
op205
 
Amorphous Materials: Structural Principles and Characterization
University of Wisconsin MRSEC
 
Crystal Defects
Vikash Prasad
 
Eut 440-2013-2014-sem-1-final-exam-answer-scheme
Shahril Majid
 
Aterramento
FRANCESCO GALGANO
 

What's hot (20)

PPTX
Introduction to LTspice iv
Hoopeer Hoopeer
 
PPTX
Bcd to 7 segment display
Maulik Sanchela
 
PDF
343logic-design-lab-manual-10 esl38-3rd-sem-2011
e11ie
 
PPTX
gate level modeling
VandanaBR2
 
PPTX
Current mirror
Hossam Moghrabi
 
PDF
Architectural Level Techniques
GargiKhanna1
 
PDF
Code conversion using verilog code VHDL
Bharti Airtel Ltd.
 
PPTX
Pll
katamthreveni
 
PPTX
Latches and flip flop
Shuaib Hotak
 
PPTX
Latch & Flip-Flop.pptx
GargiKhanna1
 
PDF
Electronics Lab Manual by Er. Swapnil V. Kaware
Prof. Swapnil V. Kaware
 
PPT
Verilog hdl
Muhammad Uzair Rasheed
 
PPTX
Verilog Test Bench
Dr.YNM
 
PPTX
7 Segment Decoder
Kamal Acharya
 
PPTX
Diode
Seti Saiman
 
PPTX
Flip flops, counters &amp; registers
Dharit Unadkat
 
PPTX
Latch and flip flop
GargiKhanna1
 
PPTX
Programmable logic devices
ISMT College
 
PPTX
Tuned amplifire
Abdulla Al jubayr
 
PPTX
bandgap ppt
lingadhar reddy
 
Introduction to LTspice iv
Hoopeer Hoopeer
 
Bcd to 7 segment display
Maulik Sanchela
 
343logic-design-lab-manual-10 esl38-3rd-sem-2011
e11ie
 
gate level modeling
VandanaBR2
 
Current mirror
Hossam Moghrabi
 
Architectural Level Techniques
GargiKhanna1
 
Code conversion using verilog code VHDL
Bharti Airtel Ltd.
 
Pll
katamthreveni
 
Latches and flip flop
Shuaib Hotak
 
Latch & Flip-Flop.pptx
GargiKhanna1
 
Electronics Lab Manual by Er. Swapnil V. Kaware
Prof. Swapnil V. Kaware
 
Verilog hdl
Muhammad Uzair Rasheed
 
Verilog Test Bench
Dr.YNM
 
7 Segment Decoder
Kamal Acharya
 
Diode
Seti Saiman
 
Flip flops, counters &amp; registers
Dharit Unadkat
 
Latch and flip flop
GargiKhanna1
 
Programmable logic devices
ISMT College
 
Tuned amplifire
Abdulla Al jubayr
 
bandgap ppt
lingadhar reddy
 
Ad

Similar to LTspice.ppt (20)

PPTX
LTspice_lecture electronic circuit Modeling.pptx
wgntbq9h6j
 
PDF
Express pcb tutorial
awazapki
 
DOCX
EELE 5331 Digital ASIC DesignLab ManualDr. Yushi Zhou.docx
toltonkendal
 
DOCX
Dtmf robot
ARCHANA S
 
PPT
Pspice software+ presentation
RAhul Soni
 
PDF
Cadence manual
Hoopeer Hoopeer
 
PDF
Ads
Saravana Selvan
 
PPT
Project_PPT_Presentation.ppt
BIPLABNAYAK10
 
DOCX
Arduino PAPER ABOUT INTRODUCTION
NAGASAI547
 
PPT
PCB DESIGN - Introduction to PCB Design Library Creation
Vibrant Technologies & Computers
 
PPTX
ORCAD pcb design
JHALAKNIHALANI
 
PDF
Magazine awr-ims-3
Sam Sambala
 
PDF
Kpsi User Guide Model 500
TAMUK
 
DOC
Express sch r
rajeev911
 
PDF
LTSpiceIntro.pdf
BalajiDhanabal
 
PDF
Magic Tutorial by IIIT Hyderabad professor
ssuser58c997
 
PDF
Ug10 2
Moez Ansary
 
PDF
Eagle tut
parisalitopan
 
DOCX
ECET 380 Entire Course NEW
shyamuopuop
 
PDF
Programming the ARM CORTEX M3 based STM32F100RBT6 Value Line Discovery Board
Gaurav Verma
 
LTspice_lecture electronic circuit Modeling.pptx
wgntbq9h6j
 
Express pcb tutorial
awazapki
 
EELE 5331 Digital ASIC DesignLab ManualDr. Yushi Zhou.docx
toltonkendal
 
Dtmf robot
ARCHANA S
 
Pspice software+ presentation
RAhul Soni
 
Cadence manual
Hoopeer Hoopeer
 
Ads
Saravana Selvan
 
Project_PPT_Presentation.ppt
BIPLABNAYAK10
 
Arduino PAPER ABOUT INTRODUCTION
NAGASAI547
 
PCB DESIGN - Introduction to PCB Design Library Creation
Vibrant Technologies & Computers
 
ORCAD pcb design
JHALAKNIHALANI
 
Magazine awr-ims-3
Sam Sambala
 
Kpsi User Guide Model 500
TAMUK
 
Express sch r
rajeev911
 
LTSpiceIntro.pdf
BalajiDhanabal
 
Magic Tutorial by IIIT Hyderabad professor
ssuser58c997
 
Ug10 2
Moez Ansary
 
Eagle tut
parisalitopan
 
ECET 380 Entire Course NEW
shyamuopuop
 
Programming the ARM CORTEX M3 based STM32F100RBT6 Value Line Discovery Board
Gaurav Verma
 
Ad

More from DrVikasMahor (20)

PPTX
Consumer_Electronics_Detailed_Presentation.pptx
DrVikasMahor
 
PPTX
Wireless communication UNIT 1 PPt.pptx
DrVikasMahor
 
PPTX
introduction to telcomm. new for BTech.pptx
DrVikasMahor
 
PPTX
television ppt new for BTech consumer.pptx
DrVikasMahor
 
PPTX
LEcture 3 on Loudspeaket and sound technology.pptx
DrVikasMahor
 
PPTX
Audio Compression technology for BTech.pptx
DrVikasMahor
 
PPTX
8279 Co Processor for integrating with main processor.pptx
DrVikasMahor
 
PPTX
NEP_2020_Summary_Slides_new_Institues.pptx
DrVikasMahor
 
PPTX
8087 co processor for 8086 and other.pptx
DrVikasMahor
 
PPTX
sp34 Introduction to 8086 Microprocessor.pptx
DrVikasMahor
 
PPT
color models new for multimedia communication.ppt
DrVikasMahor
 
PPT
PCB_Design_Process for BTech students.ppt
DrVikasMahor
 
PPTX
PCB_Designing_Tutorial_with_Images -new.pptx
DrVikasMahor
 
PPTX
proximity sensors for integration new.pptx
DrVikasMahor
 
PPTX
Sound Sensor new presentation for Electronics.pptx
DrVikasMahor
 
PPTX
E-Waste_Management_Presentation_Engineering.pptx
DrVikasMahor
 
PPTX
Plastic_Waste_Management_Presentation.pptx
DrVikasMahor
 
PPTX
Internship Report of a BTech Student.pptx
DrVikasMahor
 
PPTX
Midterm Presentation _ASHISH RATHORE.pptx
DrVikasMahor
 
PPT
Introduction to VHDL language VHDL_Intro.ppt
DrVikasMahor
 
Consumer_Electronics_Detailed_Presentation.pptx
DrVikasMahor
 
Wireless communication UNIT 1 PPt.pptx
DrVikasMahor
 
introduction to telcomm. new for BTech.pptx
DrVikasMahor
 
television ppt new for BTech consumer.pptx
DrVikasMahor
 
LEcture 3 on Loudspeaket and sound technology.pptx
DrVikasMahor
 
Audio Compression technology for BTech.pptx
DrVikasMahor
 
8279 Co Processor for integrating with main processor.pptx
DrVikasMahor
 
NEP_2020_Summary_Slides_new_Institues.pptx
DrVikasMahor
 
8087 co processor for 8086 and other.pptx
DrVikasMahor
 
sp34 Introduction to 8086 Microprocessor.pptx
DrVikasMahor
 
color models new for multimedia communication.ppt
DrVikasMahor
 
PCB_Design_Process for BTech students.ppt
DrVikasMahor
 
PCB_Designing_Tutorial_with_Images -new.pptx
DrVikasMahor
 
proximity sensors for integration new.pptx
DrVikasMahor
 
Sound Sensor new presentation for Electronics.pptx
DrVikasMahor
 
E-Waste_Management_Presentation_Engineering.pptx
DrVikasMahor
 
Plastic_Waste_Management_Presentation.pptx
DrVikasMahor
 
Internship Report of a BTech Student.pptx
DrVikasMahor
 
Midterm Presentation _ASHISH RATHORE.pptx
DrVikasMahor
 
Introduction to VHDL language VHDL_Intro.ppt
DrVikasMahor
 

Recently uploaded (20)

PPTX
Construction Project Organization Group 2.pptx
vj5agdales
 
PDF
composite construction of structures.pdf
AinieButt1
 
PDF
Enhancing Cyber Defense Against Zero-Day Attacks using Ensemble Neural Networks
IJCNCJournal
 
PPTX
additive manufacturing of ss316l using mig welding
premcdr7799
 
PPTX
M Tech Sem 1 Civil Engineering Environmental Sciences.pptx
ShriNRPrasad
 
PDF
Automation-in-Manufacturing-Chapter-Introduction.pdf
pcmth867
 
PPTX
Engineering Ethics, Safety and Environment [Autosaved] (1).pptx
MehrabTaseenTalukder
 
PPTX
Internet of Things (IOT) - A guide to understanding
Davies Chacko
 
DOCX
573137875-Attendance-Management-System-original
AYUSHMANAV
 
PPTX
UNIT-1 - COAL BASED THERMAL POWER PLANTS
Chandra Kumar S
 
PDF
July 2025 - Top 10 Read Articles in International Journal of Software Enginee...
sebastianku31
 
PDF
Well-logging-methods_new................
ZafriFarid
 
PPTX
web development for engineering and engineering
keshriji700
 
PPTX
CARTOGRAPHY AND GEOINFORMATION VISUALIZATION chapter1 NPTE (2).pptx
abhi1361yadav
 
PDF
Mitigating Risks through Effective Management for Enhancing Organizational Pe...
IJAEMSJORNAL
 
PPTX
CH1 Production IntroductoryConcepts.pptx
RacemMellouli1
 
PPTX
MET 305 2019 SCHEME MODULE 2 COMPLETE.pptx
VinayB68
 
PDF
Digital Logic Computer Design lecture notes
CHINNASUNKAIAH1
 
PDF
The CXO Playbook 2025 – Future-Ready Strategies for C-Suite Leaders Cerebrai...
Cerebraix Technologies
 
PPTX
Lecture Notes Electrical Wiring System Components
eedgecbhojpur
 
Construction Project Organization Group 2.pptx
vj5agdales
 
composite construction of structures.pdf
AinieButt1
 
Enhancing Cyber Defense Against Zero-Day Attacks using Ensemble Neural Networks
IJCNCJournal
 
additive manufacturing of ss316l using mig welding
premcdr7799
 
M Tech Sem 1 Civil Engineering Environmental Sciences.pptx
ShriNRPrasad
 
Automation-in-Manufacturing-Chapter-Introduction.pdf
pcmth867
 
Engineering Ethics, Safety and Environment [Autosaved] (1).pptx
MehrabTaseenTalukder
 
Internet of Things (IOT) - A guide to understanding
Davies Chacko
 
573137875-Attendance-Management-System-original
AYUSHMANAV
 
UNIT-1 - COAL BASED THERMAL POWER PLANTS
Chandra Kumar S
 
July 2025 - Top 10 Read Articles in International Journal of Software Enginee...
sebastianku31
 
Well-logging-methods_new................
ZafriFarid
 
web development for engineering and engineering
keshriji700
 
CARTOGRAPHY AND GEOINFORMATION VISUALIZATION chapter1 NPTE (2).pptx
abhi1361yadav
 
Mitigating Risks through Effective Management for Enhancing Organizational Pe...
IJAEMSJORNAL
 
CH1 Production IntroductoryConcepts.pptx
RacemMellouli1
 
MET 305 2019 SCHEME MODULE 2 COMPLETE.pptx
VinayB68
 
Digital Logic Computer Design lecture notes
CHINNASUNKAIAH1
 
The CXO Playbook 2025 – Future-Ready Strategies for C-Suite Leaders Cerebrai...
Cerebraix Technologies
 
Lecture Notes Electrical Wiring System Components
eedgecbhojpur
 

LTspice.ppt

  • 1. 1 Electronics Principles & Applications 8th Edition Dr. Vikas Mahor LTspice IV
  • 2. 2 LTspice IV • A freeware SPICE circuit simulator written by Mike Engelhardt at Linear Technologies http://www.linear.com/ – SPICE I and SPICE II were written using the FORTRAN programming language. SPICE III was written using the C programming language (U.C. Berkeley, 1985). http://bwrc.eecs.berkeley.edu/Classes/IcBook/SPICE/) • LTspice was written to support circuit designers who evaluate or use Linear Technology products. – It includes an extensive library of Linear Technology devices. • It has schematic capture and is much easier to use than traditional text-based SPICE. – Traditional SPICE requires a text file called a netlist that describes the circuit to be simulated. – With schematic capture, the user can enter a circuit using schematic symbols via a graphical user interface.
  • 3. 3 LTspice IV • Is powerful and fast, but is not as intuitive for beginners as simulators such as Multisim – Requires more knowledge about SPICE directives and terminology – Has a limited (mostly proprietary) device library – LTspice has only basic behavioral gates for digital circuits. It is expandable, but this requires knowledge about SPICE and device behavior. • Is worth learning about – Since it is free, fast, and powerful, it is one of the most widely used circuit simulators at this time. – Many professionals consider it to be superior to some commercial simulators.
  • 4. 4 LTspice IV is a free download and can be found on the Linear Technology website: http://www.linear.com/designtools/software/switchercad.jsp
  • 5. 5 Get started by clicking File and then New Schematic, or hold down the Control key and then press the “N” key (Ctrl+N). It’s easy to “draw” a circuit.
  • 6. 6 Drawing a circuit … is easier if the grid is active. Click on View and then Show Grid. Or, you can type Ctrl+G.
  • 7. 7 Delete tool It is easy to place grounds and basic components. Click on the desired component and then move the mouse to position it and then left click to place it. You will find that the connectors (square blue boxes above) snap to the nearest grid points. To place another component of the same type, move to the next location and click the left mouse button again. To cancel or quit a component type, click the right mouse button. It is often more time efficient to place all of the resistors, then the capacitors, and so on. Use the scissors (delete tool) to remove components and wires.
  • 8. 8 After a component has been selected, it can be rotated by holding down the Control key and then pressing the R key. Here, D1 was placed first (by left-clicking in the desired location on the schematic) followed by Control+R and then D2 was placed followed by Control+R again and so on.
  • 9. 9 Control+E was used here before placing Q2 on the above schematic. Note that Q2 is the mirror image of Q1. Control+E is the mirror command. Control+R and Control+E are keyboard shortcuts. Rotated components Mirrored components Rotated and mirrored
  • 10. 10 The menu command Tools→Control Panel→Drafting Options→Hot Keys allows you to define your own keyboard shortcuts.
  • 11. 11 Additional components are available by clicking on the gate symbol or by pressing the F2 key. Suppose you need a voltage source. Choose “voltage” from the component symbol list and then place the source on the drawing area with a left click. Right click the source to specify the voltage. To specify a sinusoidal voltage source, select Advanced after right clicking. or
  • 12. 12 Specifying a SINE ac voltage source Amplitude and Frequency (V1, as shown here, is a 44-V dc source.)
  • 13. 13 Use the pencil tool to connect the components. Left click a terminal (blue box) and then move the mouse to the connecting terminal and left click again. The crosshairs below are positioned to connect R4 to R5. The blue boxes disappear after they are connected. Unconnected nodes can cause Netlist errors.
  • 14. 14 Tool Bar Summary Place Circuit Element Draw Wire Place Ground Label Node Place Resistor Place Capacitor Place Inductor Place Diode Move Drag Undo Redo Rotate Mirror Place Comment Place SPICE Directive Zoom In Pan Zoom Out Auto Scale Delete Copy Paste Find Simulate
  • 15. 15 Or, click Select Resistor to view a Standard list. Place a resistor and right click it to enter its values. You must specify component values.
  • 16. 16 Right click the resistor label to enter a new reference designator. You can specify vertical text.
  • 17. 17 Models are required. • Missing models will generate error messages. – The next slide shows an example. – LTspice does not have a model for the 1N4001 diode. • There are several ways to add models.
  • 18. 18
  • 19. 19 You can expand the component data base (add models). • For example, suppose that you want to simulate a circuit using a BFR540 transistor and that you have the SPICE model saved in text format via Windows Notepad (go to Start, Programs, Accessories to launch this basic text editor). – Load the SPICE model into Windows Notepad and then Copy it to the clipboard using Control+A followed by Control+C. – Use Windows Notepad with File Type set to All Files to open the file C:Program FilesLTCSWCADIVlibcmpstandard.bjt, scroll to the end of that file, and then paste the model from the clipboard (Control+V) and then Save the file. – The next time that you run LTspice, the BFR540 will be available as a choice when selecting an NPN BJT transistor as shown on the next slide.
  • 21. 21 A SPICE model for the BFR540 .MODEL BFR540 NPN + IS = 1.04516E-015 + BF = 1.84359E+002 + NF = 9.81774E-001 + VAF = 4.16981E+001 + IKF = 1.00000E+001 + ISE = 2.32436E-013 + NE = 2.02825E+000 + BR = 4.39917E+001 + NR = 9.92532E-001 + VAR = 2.09773E+000 + IKR = 1.66296E-001 + ISC = 1.29849E-016 + NC = 1.06486E+000 + RB = 5.00000E+000 + IRB = 1.00000E-006 + RBM = 5.00000E+000 + RE = 3.53552E-001 + RC = 1.34000E+000 + EG = 1.11000E+000 + XTI = 3.00000E+000 + CJE = 1.97895E-012 + VJE = 6.00000E-001 + MJE = 3.32695E-001 + TF = 7.45719E-012 + XTF = 1.14072E+001 + VTF = 3.15854E+000 + ITF = 1.56917E-001 + CJC = 7.93745E-013 + VJC = 1.85522E-001 + MJC = 8.41656E-002 .ENDS
  • 22. 22 Also, a SPICE model can be added directly to the schematic.
  • 23. 23 • Copy the model to the clipboard. – Left click and hold and drag over the model and then capture it with Control+C. e.g. .MODEL 1N4001 D IS=29.5E-9 RS=73.5E- 3 N=1.96 CJO=34.6P VJ=0.627 +M=0.461 BV=60 IBV=10U • Click on .op on the toolbar • Paste the model into the window. – Control+V. • Click OK. • Place the model on your schematic with a left click. • This method is often preferred when sharing circuits with others. – The necessary model or models are imbedded in the circuit file. Adding a model to a schematic
  • 24. 24 Including a model from a file 1/ Click on .op. 2/ Enter the following text: .include filename.txt (where filename is the name of your model file, such as zener6, or 2N3055 and has been saved as a .txt file). 3/ Click OK. 4/ Place the SPICE-directive on your schematic where you want it to appear with a left-click. Note: It is advisable to save the model file to the same folder as your circuit file. The same applies for model files including sub-circuits.
  • 25. 25 Where does one obtain SPICE models? • Search the Internet … many are available as free downloads or can be copied to the clipboard and then pasted into Windows Notepad (or onto your schematic via .op on the toolbar). Some links are provided at the end of this presentation. • Search device manufacturers’ websites. • Modify an existing model. • Create your own. – Software is available. http://www.intusoft.com/spicemod.htm • Or, you can use a subcircuit.
  • 26. 26 Subcircuits (.SBCKT) • Are often used when repetition occurs. – Better than cluttering the schematic with redundant information • Also can be used to replace a complicated device such as an OP-AMP, a DIAC or a TRIAC. • The next slide shows a common dimmer circuit where the DIAC and TRIAC functions are defined by subcircuits. – LTspice has pre-defined schematic symbols for DIACS and TRIACS, but no corresponding models.
  • 27. 27
  • 28. 28 More about models and subcircuits Models given as .MODEL statements are for intrinsic SPICE devices such as diodes and transistors. The .MODEL statement gives the parameters for the specific component. The general behavior of the device is already known by SPICE … only the parameters need to be given to finish specifying the component's electrical characteristics. On the other hand, models given by .SUBCKT statements define the modeled component by a collection of intrinsic SPICE devices. For example, the SPICE model of an opamp would be given as a subcircuit. In the previous slide, the SPICE models of a DIAC and a TRIAC were specified as subcircuits.
  • 29. 29 LTspice is useful for analyzing circuits designed by others. • It is sometimes only necessary to use it to review and experiment with circuit files that have already been created. – Many can be found in the LTspice subdirectories. – Some examples are available for download. This is an outstanding example: http://cmosedu.com/cmos1/book.htm
  • 30. 30 How to run an existing circuit file • From the File menu, select Open. Make sure the file type is set to Schematics. • Some good examples are available in C:ProgramFilesLTCSwCADIVexamplesEducational (created on your hard drive when you install LTspice). • Some appropriate examples for the McGraw-Hill basic skills series are available on the website: http://highered.mcgraw- hill.com/sites/0073106941/student_view0/lt_spice_instru ctions_and_support_files.html (You probably have these files if you obtained this presentation from the McGraw- Hill site.) • The next slide shows a circuit from Schuler’s book. To view the dc voltages and currents, a dc analysis is selected by first clicking on Simulate, then Edit Simulation Cmd. – The SPICE directive is .op.
  • 32. 32 The DC operating point selection provides all node voltages and device currents. When you click OK, the SPICE directive .op is placed on the schematic.
  • 33. 33 A ground is required for simulation.
  • 34. 34 -24V -12V 40W 28.8W 9.6W 1.2W 12W -88W -3.6W After a DC operating point analysis, moving the cursor over the schematic reveals the various node voltages, currents, and the dissipations in each component. These values are displayed in the lower left portion of the screen. DC operating point (I(R5) = 200 mA Dissipation = 1.2 W Placing the cursor here shows the current and the dissipation in R5, as shown below. Summing the dissipations in this circuit produces zero. The negative signs at V1 and V2 indicate that they are power sources.
  • 35. 35 It is also possible to display the dc voltage at one or more nodes on the schematic. Run the simulation and then right-click any empty area on the schematic and select View Place .op Data Label as shown below.
  • 36. 36 Then, move the rectangular cursor to the desired node and click it. The dc voltage at that node will be displayed on the schematic. Repeat the procedure to add nodes.
  • 37. 37 After you have one or more nodes selected, you can change circuit values and re- run the simulation to see the effect on the selected dc node voltages. R2 has been changed from 20 ohms to 10 ohms.
  • 38. 38 You can choose horizontal orientation for voltage labels by placing the small square at the bottom of the selection rectangle on a horizontal wire.
  • 39. 39 Waveforms • Waveforms are what one sees on an oscilloscope (graphs of instantaneous voltages versus time). • Waveforms can be viewed via the transient analysis option. Click on Simulate, Edit Sim Command, and then select the Transient tab. • The next three slides show the procedure.
  • 40. 40 Load the circuit from the file menu. Then, click run. Reference: Schuler, 7th edition, page 247 … the stiff current source has been replaced with a resistor. Probe both the base and the collector of Q2. Without the stiff current source, the CMRR is notably poorer.
  • 41. 41 Move the cursor to the desired node. When the cursor changes to a probe, click the left mouse button to view the waveform. A small differential signal plus a large common-mode signal
  • 42. 42 Move the cursor to the collector. Left click and now two waveforms are shown. Can you see the 60 Hz common-mode component at the collector of Q2?
  • 43. 43 The next slide demonstrates the value of simulation when evaluating circuit performance. • The differential amplifier circuit is much improved with a stiff current source. • The common-mode rejection ratio (CMRR) is remarkably better. – The common mode signal cannot be seen in the output. • Circuit simulators make it easy and fun to investigate issues such as this.
  • 44. 44 Stiff current source The 60 Hz common-mode signal is too small to be seen here.
  • 45. 45 Remember, waveforms are available via transient analysis. • You must specify the time duration of a transient analysis by specifying a Stop Time. – Often, this is all that is required. • You can also specify the Time to Start Saving Data. – Useful in circuits where the start-up period is not important. • You can also specify the Maximum Timestep.
  • 46. 46 CMRR Go to Simulate and then click on Edit Simulation Cmd. The time duration of a transient analysis is like choosing the time base setting on an oscilloscope.
  • 47. 47 For a basic analysis, this is often all that needs to be specified.
  • 48. 48 In this circuit, the common-mode signal is 60 Hz. A 60 Hz signal has a period of roughly 17 milliseconds. Thus, a Stop Time of 20 milliseconds is a reasonable choice.
  • 49. 49 Expanded waveform measurements are easy. Hold the left mouse button down and drag a box around the area of interest. Before you release the button, the measurements are available here: dx = 500 us (2 kHz) dy = 4.7 V Box
  • 50. 50 When you release the mouse button, the area inside the box will be zoomed to fill the waveform display. Restore the original waveform by right-clicking in the waveform area and then selecting Zoom to Fit or simply press Ctrl+E.
  • 51. 51 To obtain an accurate frequency measurement, draw a box around several cycles and then draw a second box to capture one cycle.
  • 52. 52 1.572 kHz This box captures one cycle. (The peaks are easier to identify than the zero crossings.) The output frequency of this Wien bridge oscillator is predicted by 1/(2πRC), thus we can expect an output at 1.59 kHz.
  • 53. 53 To obtain the voltage difference across two nodes, move the cursor to the first node and left click when it changes to a red voltage probe and then without releasing the mouse button, move to the second node and when the cursor changes to a black voltage probe, release the mouse button.
  • 54. 54 To determine the Average and RMS values of a waveform, hold down the Control key and left click the waveform’s label. Ctrl+Left Click here
  • 55. 55 The Fourier transform • Converts from the time domain to the frequency domain (the signal spectrum) – Schuler, 7th edition, page 500 • The FFT (fast Fourier transform) is available in LTspice. – After a waveform is plotted, right click in the waveform window and select FFT. Choose the node of interest and then click OK. Left click the node label in the FFT window and then use the keyboard arrow keys to make accurate measurements of frequency and amplitude for the various spectral components. Left click and hold to draw a box around a part of the graph to expand it.
  • 56. 56 FFT (frequency domain) display Time domain display
  • 57. 57 Expanded FFT display Note: you can increase the simulation time for better frequency resolution. Resolution = 1/Time
  • 58. 58 Simulation time = 0.001 seconds Resolution = 1 kHz Simulation time = 0.01 seconds Resolution = 100 Hz
  • 59. 59 In addition to increasing the simulation time, you can turn off data compression for better resolution (Tools  Control Panel  Compression). The next slide shows a significant improvement in dynamic range with data compression turned off. Default data compression No data compression
  • 60. 60 FFT with default data compression (90 dB range) FFT with no data compression (approaching a 120 dB range)
  • 61. 61 The option plotwinsize determines the number of data points to compress in one window. Set plotwinsize to zero to disable compression. Data compression will always be turned off, regardless of the control panel settings (an advantage when sharing circuits with others).
  • 62. 62 Individual waveforms can be placed onto different plot panes. • Right click in the waveform pane and then select Add Plot Pane. • The next slide shows the usefulness of this feature. – With all five waveforms on one plot pane, the display is confusing. – Separate plot panes make it easy to see the divide-by-two action of each flip-flop.
  • 63. 63
  • 64. 64 There are three important waveforms here. Three plot panes add clarity. 555 one-shot Input (TRIG) Threshold waveform Output
  • 65. 65 A dc offset is also available. • The next slide shows a D/A converter. • The input waveforms were separated by right- clicking on the node name, e.g. V(b1), as shown below, and adding a dc offset of +2 volts. • It also shows how colors can be chosen by using Tools→Color→Preferences→Selected Item→Waveform→Background→Grid→Axis dc offset V(b1)+2
  • 66. 66 0 dc offset +2 dc offset +4 dc offset +6 dc offset Separate plot plane
  • 67. 67 Current waveforms • Moving the cursor to the inside area of a component, after a transient analysis has been run, displays the current waveform in that component. • When the cursor morphs to a current probe: – left click to see the current waveform. • This is illustrated in the next slide.
  • 68. 68 Current waveforms can be obtained after a transient analysis by moving the cursor to the inside of a device. When the cursor changes to a current probe, left click the mouse to obtain the current waveform. To display the current in a wire, Alt-left click the wire. The current probe, like the voltage probe, shows time variations after a transient analysis. Here, the current in R1 averages 2 mA (which was measured earlier in a dc analysis) and the current fluctuations in R1 are easy to see. Current probe icon
  • 69. 69 The current in Q1 is constant. The constant current source is doing its job!
  • 70. 70 To display a power waveform (instantaneous power), hold down the Alt key and left click on the component of interest (after the cursor has changed to a thermometer). e.g., Alt+click here.
  • 71. 71 To determine the average power dissipation, Control+left-click on the label. Ctrl+left-click
  • 72. 72 AC Analysis • Provides the frequency response of a circuit – Both the amplitude and the phase angle are graphed as a function of frequency (Bode plot). • Go to Simulate, Edit Simulation CMD, and then click on the AC Analysis tab. – You must enter the Number of points per sweep interval, the Start Frequency and a Stop Frequency. – You can also choose various sweep intervals. • Octave, Decade, or Linear
  • 73. 73 Output Input AC Analysis provides the frequency response of a circuit. One of the signal sources must be designated as the input by specifying an AC Amplitude for Small signal AC analysis. Run the simulation and then probe the output for the Bode plot. Amplitude Phase Spice directive
  • 74. 74 Ctrl+left-click the label to measure bandwidth.
  • 75. 75 Here, the only change is the transistors. This illustrates the need for proper SPICE models when investigating issues such as bandwidth. The BFR540 is a high-frequency transistor. BFR540 2N3904
  • 76. 76 The .measure directive • Is useful to find instantaneous values and values over intervals • The next slide shows an example of an instantaneous measurement. Keyword Operation performed over interval AVG Compute the average value of <expr> MAX Find the maximum value of <expr> MIN Find the minimum value of <expr> PP Find the peak-to-peak value of <expr> RMS Compute the root mean square value of <expr> INTEG Integrate <expr>
  • 77. 77 vi: v(exponential_a)=0.632013 at 0.001 Run->View->View SPICE Error Log will show the instantaneous value at 1 ms.
  • 78. 78 The SPICE .STEP directive has been added to show the charge and discharge curves for capacitor values from 0.2 microfarads to 1.2 microfarads in 0.2 microfarad steps.
  • 80. 80 Configuring LTspice • There are many user options. – SPICE options (e.g. integration method) – Drafting options including font properties – Data saving defaults – Compression • Hint: turn compression off for the least distortion for analog circuit simulations. – Most options are available via the control panel. • The next two slides illustrate some configuration choices.
  • 81. 81 Tools  Control Panel  Operation LTspice generates several kinds of files. To save disk space and avoid clutter, these files can be deleted automatically.
  • 82. 82 Tools  Color Preferences LTspice allows color choices for waveform plots and the background on which they are plotted. Also, the axes and grid colors are selectable
  • 83. 83 Support for LTspice • The next slide shows an example of the built-in help system. • The help file is a downloadable and printable document: http://ltspice.linear.com/software/scad3.pdf • There are numerous other resources. Check the Links slide at the end of this presentation.
  • 84. 84 Press F1 for the Help System. You can download the User’s Manual from: http://ltspice.linear. com/software/scad 3.pdf
  • 85. 85 The help files explain many things: for example, how to model transformers.
  • 86. 86 Some “gotchas” and hints • “M” and “m” are interpreted the same by SPICE. Thus, a resistor value of 10M is the same as 10m (ten milliohms or 10-3). – Use 10MEG (or 10E6) to specify ten megohms. • Do not enter “1F” or “1f” as the capacitance for a one- farad capacitor (enter “1”). “F” and “f” designate the prefix femto (10-15). • SPICE will not allow voltage sources in parallel, even when of the same value. – Add series resistances. • SPICE will not allow current sources in series, even when of the same value. – Add parallel resistances.
  • 87. 87 Prefixes are case insensitive: T = t, G = g, and so on • T = terra = 1012 • G = giga = 109 • MEG = meg = 106 • K = kilo = 103 • M = milli = 10-3 • U = micro = 10-6 • N = nano = 10-9 • P = pico = 10-12 • F = femto = 10-15
  • 88. 88 LTspice leading characters • A special functions device • B arbitrary behavioral source • C capacitor • D diode • E voltage dependent voltage source • F current dependent current source • G voltage dependent current source • H current dependent voltage source • I independent current source • J JFET transistor • K mutual inductance • L inductor • M MOSFET transistor • O lossy transmission line • Q bipolar transistor • R resistor • S voltage controlled switch • T lossless transmission line • U uniform RC-line • V independent voltage source • W current controlled switch • X subcircuit invocation • Z MESFET transistor • * comment • + continuation of prior line • . simulation directive
  • 89. 89 LTspice IV final notes • Like many modern software tools – it is relatively easy to begin using but one must spend some time to discover and then master the most powerful features. • As freeware goes, it is outstanding! – It is relatively bug-free. – It is compact and very fast. – It is regularly updated. • A tip for students: – Knowing how to use a professional level circuit simulator looks great on your resume!