Transcript Computer Aided Design

Computer Aided Design
Course 2
Setting up Analyses
In order to measure a circuit performance, it
is necessary to simulate its behavior. PSpice A/D
is a simulation program that models the behavior
of a circuit containing any mix of analog and
digital devices. Used with Schematics for design
entry, you can think of PSpice A/D as a softwarebased breadboard of your circuit that you can
use to test and refine your design before ever
touching a piece of hardware.
For the circuit to be simulated you need to
setup the analyses first. Certain analyses
(such
as
noise,
Monte
Carlo,
sensitivity/worst-case,
DC
sensitivity,
Fourier, and small-signal DC transfer
function) require you to specify output
variables for voltages and currents at
specific points on the schematic.
1. DC Analyses
In order to set up and run DC analyses, you will
have to go through a sequence of several steps.
A typical example of such a sequence is given
below:
• Applying an appropriate DC Stimulus
• Setting up Initial Bias Point Condition (for
some DC sweep analyses)
• Enabling Bias Point Detail analysis
• Performing DC Sweep analysis
• Setting up Small-Signal DC Transfer analysis
• Selecting DC Sensitivity analysis
• Selecting Options
1. DC stimulus
To run a DC sweep ( with swept variable a V or I
source) or small-signal DC transfer analysis,
you need to place and connect one or more
independent sources and then set the DC
voltage or current level for each source.
Adding and Defining Stimulus
To simulate your circuit, you need to connect one
or more source symbols that describe the input
signal that the circuit must respond to.
The PSpice libraries supply several source
symbols that are described in the tables that
follow. These symbols depend on:
• the kind of analysis you are running,
• whether you are connecting to the analog or
digital portion of your circuit, and
• how you want to define the stimulus: using the
Stimulus Editor, using a file specification, or
by defining symbol attribute values.
The analog stimuli symbols available in
Schematics are presented on the following chart:
stimulus.doc
2. Initial Bias Point Condition
There are three options for simulation initial
conditions setting:
• Save and Load Bias Point
• Setpoints
• Setting Initial Conditions
Save and Load Bias Point
Save Bias Point and Load Bias Point are used to
save and restore bias point calculations in
successive PSpice A/D simulations. Saving and
restoring bias point calculations can decrease
simulation times when large circuits are run
multiple times and can aid convergence.
Save/Load Bias Point affect the following types of
analyses:
– transient
– DC
– AC
Setpoints
Pseudo components that specify initial conditions are called
setpoints. These apply to the analog portion of your circuit.
IC1 is a one-pin symbol that allows you to set the initial
condition on a net for both small-signal and transient bias
points
IC2 is a two-pin symbol that allows you to set initial
condition between two nets
Using IC symbols sets the initial conditions for the bias
point only. It affect only initial condition for transient
analysis. It is necessary for oscillators. It does not affect
the DC sweep. If the circuit contains both an IC symbol
and a NODESET symbol for the same net, the NODESET
symbol is ignored.
NODESET1 is a one-pin symbol which helps calculate the
bias point by providing a initial guess for some net.
NODESET2 is a two-pin symbol which helps calculate the
bias point between two nets. Some or all of the circuit nets
may be given an initial guess.
NODESET symbols are effective for the bias point (both
small-signal and transient bias points) and for the first step
of the DC sweep. It is used for DC sweep of bistable
circuits. It has no effect during the rest of the DC sweep or
during the transient analysis itself.
• Setting Initial Conditions
The IC attribute allows initial conditions to be set on
capacitors ( initial voltage on C) and inductors ( initial current
by L). These conditions are applied during all bias point
calculations. However, if you select (•) the Skip Initial
Transient Solution check box in the Transient Analysis Setup
dialog box, the bias point calculation is skipped and the
simulation proceeds directly with transient analysis at
TIME=0. Devices with the IC attribute defined start with the
specified voltage or current value; however, all other such
devices have an initial voltage or current of 0.
3. Bias (Operating) Point Detail
The bias point is calculated for any analysis
whether or not the Bias Point Detail analysis is
enabled in the Analysis Setup dialog box. When
Bias Point Detail analysis is not enabled, only
analog node voltages and digital node states are
reported to the output file.
When the Bias Point Detail analysis is enabled,
the following information is reported to the
output file:
SMALL SIGNAL BIAS SOLUTION
• A list of all analog node voltages;
• A list of all digital node states;
• The currents of all voltage sources and their
total power.
OPERATING POINT INFORMATION ( for OP )
• Currents, terminal voltages
• A list of the small-signal parameters for all
nonlinear devices.
At the final of Operating Point analysis
nonlinear circuit elements are ready.
the linearizing
Convergence problems:
The best aid for problems in calculating the bias point is the
NODESET statement.
It is rare to have a convergence problem in the bias point
calculation; this because PSpice contains an algorithm for
automatically scaling the power supplies if it ts having trouble
finding a solution.
Example:
Determine the OP for CS JFET amplifier.
VDD
VDD
RG1
RI
C1
V2
RD
5k
1.4MEG
J1
20V
C2
1u
100k
VI
0.022u
RL
BF256B
RG2
0
RS
0.6MEG
0
10k
VTO=-2.3V
C3
3.5k
0
0
6.83u
.OP
** SMALL SIGNAL BIAS SOLUTION
NODE VOLTAGE
NODE VOLTAGE
TEMPERATURE = 27.000 DEG C
NODE VOLTAGE
( VDD) 20.0000 (N00021)
6.0000 (N00057)
(N00088)
9.8023 (N000390)
0.0000 (N00155)
NODE VOLTAGE
0.0000 (N00060)
7.1384
0.0000
VOLTAGE SOURCE CURRENTS
NAME
CURRENT
V_VI
0.000E+00
V_V2
-2.050E-03
TOTAL POWER DISSIPATION 4.10E-02 WATTS
** OPERATING POINT INFORMATION
NAME
MODEL
ID
J_J1
BF256B
2.04E-03
VGS
-1.14E+00
VDS
2.66E+00
GM
3.52E-03
GDS
8.47E-06
CGS
1.60E-12
CGD
1.21E-12
TEMPERATURE = 27.000 DEG **** JFETS
4. DC Sweep
The DC sweep analysis causes a DC sweep to be
performed on the circuit. DC sweep allows you to sweep a
source (voltage or current), a global parameter, a model
parameter, or the temperature through a range of values. The
bias point of the circuit is calculated for each value of the
sweep. This is useful for finding the transfer function of an
amplifier, the high and low thresholds of a logic gate, and so
on.
To calculate the DC response of an analog circuit, PSpice
A/D removes time from the circuit. This is done by treating all
capacitors as open circuits, all inductors as shorts, and using
only the DC values of voltage and current sources. A similar
approach is used for digital devices: all propagation delays
are set to zero, and all stimulus generators are set to their
time-zero
values.
Nested DC Sweep
A second sweep variable can be selected once a primary
sweep value has been specified in the DC Sweep dialog box.
When you specify a secondary sweep variable, it forms the
outer loop for the analysis. That is, for every increment of the
second sweep variable, the first sweep variable is stepped
through its entire range of values.
val_var2=start2
for ( val_var2  stop2, val_var2(i+1)=val_var2(i)+pas2)
val_var1=start1
for(val_var1  stop, val_var1(j+1)=val_var1(j)+pas1)
out_var=f(val_var1, val_var2)
Minimum Circuit Design Requirements:
•Swept Variable
Convergence problems:
The most common cause of failure of the DC sweep analysis is an attempt to
analize a circuit with regenerative feedback, for instance a Schmitt trigger.
There is an easy solution for this problem: don’t do this. The DC sweep is
not appropriate for calculating the hysteresis of such circuits because it is
required to jump discontinously from one solution to another at the crossover
point. Instead, use transient analysis.
Settings of secondary variable
Settings of primary variable
5. Small-Signal DC Transfer
The Small-signal DC transfer analysis causes the smallsignal transfer function to be calculated by linearizing the circuit
around the bias point. The small-signal gain (dVout/dVin),
(dIout/dIin), (dIout/dVin) sau (dVout/dIin) , input resistance
(dVin/dIin), and output resistance (dVout/dIout) are calculated
and reported.
Minimum circuit design requirements
•The circuit should contain an input source, such as VDC.
Minimum program setup requirements
In the Transfer Function dialog box, specify:
•the name of the input source
•the output variable
Example 1: Consider the CE BJT amplifier. Compute the small-signal
parameters when the input small-signal is I1.
v(out)/I_I 1  
R
2 βR
1
R r
2 π
R r
Rin  2 π
R r
2 π
R r
Rout  1 CE
R r
1 CE
r  β
π g
m
GM
5.81E+01
4.89E-02
V1
+5V
R2
R1
1k
out
200k
0
Q1
Q2N3011
I1
0A
0
Simulation results are:
BETADC
VCC
VCC
.OP
.TF V([out]) I_I1
0
SMALL-SIGNAL CHARACTERISTICS
V(OUT)/I_I1 = -1.173E+05
INPUT RESISTANCE AT I_I1 = 1.239E+03
OUTPUT RESISTANCE AT V(OUT) = 1.951E+03
6. DC Sensitivity
The sensitivity is calculated by linearizing all devices
around the bias point. DC sensitivity analysis calculates
and reports the sensitivity of one node voltage: absolute
sensitivity () and relative sensitivity , to each device
parameter for the following device types:
•resistors
•independent voltage and current sources
•voltage and current-controlled switches
•diodes
•bipolar transistors
Minimum program setup requirements:
In the Sensitivity Analysis dialog box, enter the output variable
desired.
Example 1: Consider the BJT cascode amplifier (CE-CB). Compute the
sensitivity of IC(Q2).
VCC
RC
R1
VCC
6k
18k
V1
15V
VSENS
C4
0
Q2
1u
C3
10u
0
RS
RL
4k
Q2N3904
R2
C1
4k
0
Q1
.SENS I(VSENS)
4k
VS
1u
Q2N3904
R3
RE
8k
0
C2
3.3k
0
0
10u
****
DC SENSITIVITY ANALYSIS
TEMPERATURE = 27.000 DEG C
DC SENSITIVITIES OF OUTPUT I(V_VSENS)
ELEMENT
NAME
ELEMENT
VALUE
ELEMENT
SENSITIVITY
NORMALIZED
SENSITIVITY
(AMPS/UNIT) (AMPS/PERCENT)
R_RE
3.300E+03
-2.869E-07
-9.466E-06
R_R3
8.000E+03
1.044E-07
8.352E-06
R_R2
4.000E+03
-3.847E-08
-1.539E-06
R_R1
1.800E+04
-3.909E-08
-7.036E-06
R_RC
6.000E+03
-1.850E-10
-1.110E-08
R_RS
4.000E+03
0.000E+00
0.000E+00
R_RL
4.000E+03
0.000E+00
0.000E+00
0.000E+00
-1.901E-07
0.000E+00
V_V1
1.500E+01
7.763E-05
1.164E-05
V_VS
0.000E+00
0.000E+00
V_VSENS
0.000E+00
7. Options
The Options is used to set all the options, limits, and control parameters for the
simulator.