Physics 536 - Electronic Techniques for Research

Physics 536 - Spring 2008

Electronic Techniques for Research

Using Berkeley SPICE with nanoHUB

Introduction

SPICE is a general-purpose circuit simulation program for nonlinear DC, nonlinear transient, and linear AC analysis. It was developed at the University of California, Berkeley. Circuits may contain resistors, capacitors, inductors, mutual inductors, independent voltage and current sources, four types of dependent sources, transmission lines, and the four most common semiconductor devices: diodes, BJT's, JFET's, and MOSFET's.

SPICE is freely available and can be installed on most UNIX-like platforms and can be downloaded from
ftp://sunsite.unc.edu/pub/Linux/apps/circuits/spice3f5sfix.tar.gz
but it is not trivial to run this under Windows. Instead, for Physics 536 we will use a web-based interface to SPICE using nanoHUB. To use this you will need to follow these instructions:

Visit nanoHUB and click on 'Register' near the top of the page.
Pick a user name and password and fill in your login and contact information. The personal information you are asked for is used to collect statistics for reports to the funding agencies that support nanoHUB.
Once your account is created, log in and go the the page for the SPICE simulation tool: http://www.nanohub.org/tools/spice3f4/
On that page is a link to a demonstration
It may be helpful to allow pop-ups from the www.nanohub.org in your web browser.
You may wish to print out the manual.
Work through the example below:

Example of a simple DC analysis

Consider the circuit shown below:

In which the components have the following values:

Component	Value
V₁	5 V
V₂	10 V
R₁	10 Ω
R₂	20 Ω
R₃	5 Ω

The goal is to determine the current flowing through each resistor.

Step 1

Simulating this circuit using SPICE requires translating the schematic into a representation that can be interpreted by the SPICE program. This representation is called a netlist and is constructed by the following sequence of steps.
First, number the nodes in the circuit, with ground always assigned '0'. A node is any point in the circuit that is electrically equivalent. Two parts of the circuit are electrically equivalent if there are no components between them through which current must flow (except, of course, an idealized wire). The result might look like this:

Step 2

The netlist lists the components in the circuit and specifies which nodes they are connected to. In this case, the circuit contains only resistors and voltage sources. In their simplest form, these are represented in the netlist by lines of the form

  Rxxxxxx N1 N2 <VALUE>

and

  Vxxxxxx N+ N- DC <VALUE>

where N1 and N2 are the nodes on each end of the resistor and N+ and N- are the nodes at the positive and negative end of a voltage source, respectively. Following these examples, the circuit is completely described by a netlist that looks like this:

  
   V1 1 0 DC 5V
   V2 2 0 DC 10V
   R1 2 3 10
   R2 1 3 20
   R3 3 0 5

Step 3

Although the netlist is the basis for simulating the circuit, SPICE requires some minor additions including a title line, lines to indicate what simulation is to be performed, and a line to indicate the end of the input file. In this case the .OP line indicates that the DC operating point of the circuit will be determined. The complete input file that is needed to simulate this circuit using SPICE would look like this:

  
   PHYSICS 536 EXAMPLE CIRCUIT
   V1 1 0 DC 5V
   V2 2 0 DC 10V
   R1 2 3 10
   R2 1 3 20
   R3 3 0 5
   .OP
   .END

Step 4

Go to the nanoHUB SPICE web page. Make sure to log in and click on the 'Launch Tool' button on the right.
Type the SPICE input file into the input window and click on the 'Simulate' button:

Step 5

Fix any errors... read the error messages carefully, consult the manual to make sure the syntax is correct, check that the netlist is a correct representation of the circuit you are analyzing, etc...

Step 6

Examine the output:

Circuit: PHYSICS 536 EXAMPLE CIRCUIT
--------------------------------------------------------------------------
PHYSICS 536 EXAMPLE CIRCUIT
V1 1 0 DC 5V
V2 2 0 DC 10V
R1 2 3 10
R2 1 3 20
R3 3 0 5
.OP
.options nopage
.END

--------------------------------------------------------------------------
Note: no resource usage information for 'space',
	or no active circuit available

Circuit: PHYSICS 536 EXAMPLE CIRCUIT

Circuit: PHYSICS 536 EXAMPLE CIRCUIT
Date: Tue Dec 18 10:40:31  2007



Operating point information:

	Node	Voltage
	----	-------
	V(3)	3.571429e+00
	V(2)	1.000000e+01
	V(1)	5.000000e+00

	Source	Current
	------	-------

	v1#branch	-7.14286e-02
	v2#branch	-6.42857e-01

 Resistor models (Simple linear resistor)
 model             R

       rsh         0
    narrow         0
       tc1         0
       tc2         0
      defw     1e-05

 Resistor: Simple linear resistor
 device           r3        r2        r1
 model             R         R         R
resistance         5        20        10
         i     0.714    0.0714     0.643
         p      2.55     0.102      4.13

 Vsource: Independent voltage source
 device           v2        v1
        dc        10         5
     acmag         0         0
         i    -0.643   -0.0714
         p      6.43     0.357

CPU time since last call: 0.006 seconds.

Total CPU time: 0.006 seconds.

Step 7

Think about what it means... In this case the output indicates that the following currents flow from the voltage sources and through the resistors:

Component	Value	Current
V₁	5 V	71.4 mA
V₂	10 V	643 mA
R₁	10 Ω	643 mA
R₂	20 Ω	71.4 mA
R₃	5 Ω	714 mA

This should make sense because all the current flowing out of V₁ must pass through R₂ and all the current flowing out of V₂ must pass through R₁. The current flowing through R₃ must be the sum of these two currents (and you can check that it is). Note that currents flowing through voltage sources are presented as current flowing into the positive terminal and hence are listed as negative quantities in the SPICE output in this case.