1. SPICE
Simulation Program with Integrated-Circuit Emphasis, Originated in Berkeley, 1972
Commercial versions are $$, limited free demos are available (OrCAD).
LTspice is freeware offered by Linear Technology, a producer of analog IC's: op-amps, regulators, ADCs.
Includes 1100 models for their devices and 100's of switch-mode supply circuit models
Not node or component limited
External models and subcircuits may be added
Includes waveform viewer
Limitations? No automated optimization (Monte Carlo analysis? See example file MonteCarlo.asc)

2. SPICE Demonstration - LTspice
What is LTspice and what can you do with it?
Circuit simulation: extendable parts libraries; built-in diode and transistor behavioral models
Draw a circuit (schematic capture)
Create a BOM
Where to get a free copy of Ltspice?
Go to
Left click on “Download LTspice IV”
How to learn to use it: LTspice IV Getting Started Guide

3. SPICE Text Listing
SPICE originally required a text based input. Remember punch cards anyone?
Now, the graphical capture front end automatically creates the necessary node
and command lists. Listing here is from the simple linear supply design.
Each circuit node in your design is automatically numbered and can be renamed.
Example syntax for transistor: Qxxx Collector Base Emitter [Substrate Node] model
* C:\Users\Steve\Desktop\SPICE Demonstration\SimpleSupply.asc
Q1 N001 N003 Vout 0 2N3055
R1 N003 N002 {10k-Pres}
R4 0 N003 {Pres}
R2 N001 N
R3 Vout 0 {Rload}
C3 Vout 0 470µF
V1 N001 N004 20
D1 0 N002 BZX84C15L
I1 Vout 0 PULSE(1mA 50mA 10ms 10ns 10ns 100ms 500ms 1)
C2 Vout N pf
V2 N004 0 SINE( )
.model D D
.lib C:\PROGRA~2\LTC\LTSPIC~1\lib\cmp\standard.dio
.model NPN NPN
.model PNP PNP
.lib C:\PROGRA~2\LTC\LTSPIC~1\lib\cmp\standard.bjt
.PARAM Rload=970
.dc I1 10mA 100mA 2mA
;tran 0 200ms 0
.step param Pres 1k 9k 1k
* .step temp
.param Pres=5k
.backanno
.end

4. SPICE Prefixes and Suffixes
Leading Character
Type of line *
Comment 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 X
Subcircuit Invocation +
A continuation of the previous line. The "+" is removed and the remainder of the line is considered part of the prior line.
From Ltspice Help
Suffix
Multiplier T
1e12 G
1e9
Meg
1e6 K
1e3
mil
25.4e-6 m
1e-3
u(or μ)
1e-6 n
1e-9 p
1e-12 f
1e-15

5. Power Supply Example
20V
2N3055
60Vceo
10A
15V
*My assumptions in Blue

6. Simulation Types Transient Analysis (.tran)
User sets starting conditions and runs the simulation for a specified time.
Output graphs show voltages/currents as a function of time
DC Analysis (.dc)
Shows the DC operating point while a voltage or current source is stepped through the specified range.
AC Analysis (.ac)
A voltage or current symbol is the source for the circuit exitation specified as a frequency range.
Output graphs are a log scale (dB) voltage or current function of frequency.
There is also “Noise”, “DC Operating Point”, and “DC Transfer Function”

7. LTspice Simulation
Demo capture of the following design: SimpleSupply.asc
To simplify, the transformer and rectifier are replaced with a voltage source V1.
Represent a potentiometer with two resistors and use of a “parameter”.

8. What makes a good power supply?
An ideal supply is a voltage source with zero Output Resistance
The output voltage should be stable as Temperature changes
The output voltage should be stable if the Output Current changes suddenly.
The output voltage should be independent of Input Power Fluctuations
Are all supply components operating within their limits for voltage, current, and power dissipation?
This really is true for any design...

9. Output Resistance?
Use .DC Analysis with a current source to vary the load
Attach 2 cursors to the output voltage trace and measure the change in voltage and current.
Up/Down cursor keys moves between traces. Right click on cursor to display step information.
Rout = deltaV / delta I
Test at multiple output voltage settings (“.step” with parameters)
Why is the output resistance worse (higher) in the middle of the pot travel?

10. Temperature Effect on Output?
Use .temp or “.step temp” with .DC Analysis to see how the output voltage changes with temperature
From -40C to +80C, the output shifts about 0.4V, or about 3.3mV per degree C.
What is causing this? (hint:PN junctions)
+80C -4
-40C
-40F

11. Stable with Output Current Changes?
Add a Current Source in “Pulse” mode to vary load current
Use .tran Analysis
Curves show the effect of a short (90ms) spike of 50mA in output current.
Aside from voltage droop due to non-zero output resistance, no sign of ringing or other instability.

12. Input Source Rejection?
We know that the AC source (transformer and rectifier) will produce a 120Hz ripple on the input to the series transistor.
Add a second voltage source to simulate 120 Hz ripple, set to 4Vp-p (just a guess).
Use .tran to measure effect on output. (.AC analysis could be used, too).
Worst rejection 40dB (top) high output voltage and large load current (50mA).
Best rejection 65dB (bottom) low output voltage and low load current (1mA).
39mVp-p
2.2mVp-p

13. Waveform Viewer
Click any node to display voltage waveform (cursor is a red voltage probe)
Click and hold any node (red probe appears) then drag to another node and release when black probe appears. Displays voltage difference between the selected nodes.
Hover over any symbol lead until current probe appears and Click. Current waveform is displayed.
Hold Alt key and hover over a component. Click the thermometer symbol for power waveform display.
On Waveform Display
Cursor position appears in bottom frame.
Drag a box and hold – Box limits appear in bottom frame.
Drag a box and click – display zooms.
Left click on node name – select # of cursors
Right click on node name – cursor is attached to waveform and info box appears. Drag cursors as desired.
Hold Ctrl key and right click node name – Average value for displayed range is calculated and appears.
The FFT of any signal can be displayed: under VIEW menu
Many more... The help is actually rather helpful!

14. Modified Circuit #1
Reduce resistance “seen” by Q1 Base by adding Q2 emitter follower.
Output resistance now <1.5 ohms (was 37 ohms)
Still stable with output current change.
Input source rejection is much better: now 55dB worst case vs. 40dB, but...
Larger temperature sensitivity: 5.1mV/C vs. 3.3mV/C
Likely worth the trade-off!

15. What about the Transformer and Rectifier??
The simulation runs faster as demonstrated with fewer components.
Transformer model parameters would have to be measured for accuracy - not given in datasheets.
Nevertheless, to model a transformer:
draw multiple inductors, set inductance and series resistance. Note: inductance ratio is square of turns ratio.
Link inductors with Mutual Inductance SPICE directive, eg. “K L1 L2 0.98” links L1 and L2 with a 0.98 coupling coefficient.
Note the appearance of phasing dots.
See Model: Transformer and Rectifier.asc

16. One Last Improved Version
Circuit Source: Bob Pease, Troubleshooting Analog Circuits, 1991
Output resistance is 72 micro-ohms!
Stable with output current change +50mA.
Input source rejection is better: now 58dB worst case
Temperature sensitivity virtually undetectable: 5mV TOTAL!
R1 sets the output current limit, ~300mA.
Lack of output capacitor protects circuit under test - low discharge energy

17. .AC Frequency Analysis
To demonstrate .AC analysis, the following model shows 2 independent filters
Source: Hayward et al. Experimental
Methods in RF DESIGN, 2009 pg 8.14

18. Last Word LTspice is a very useful tool.
See “LTC/LTspiceIV/examples/Educational” folder for useful examples
Most Linear Technology components provide “test fixtures”, ready to run macromodels.
Like any tool, results are only as good as the inputs (models).
In SPICE, wires have zero resistance, capacitors, inductors, and resistors are ideal.
Real components (even passives) have stray capacitance and inductance, as well as non-linear behavior.
Any circuit design must be built and tested on the bench to verify function.