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
83
84
85
86
87
88
89
90
91
92
93
94
95
96
97
98
99
100
101
102
103
104
105
106
107
108
109
110
111
112
113
114
115
116
117
118
119
120
121
122
123
124
125
126
127
128
129
130
131
132
133
134
135
136
137
138
139
140
141
142
143
144
145
146
147
148
149
150
151
152
153
154
155
156
157
158
159
160
161
162
163
164
165
166
167
168
169
170
171
172
173
174
175
176
177
178
179
180
|
%$Id: dc.tex,v 1.1 96/03/24 11:12:52 al Exp $
% man commands dc .
%------------------------------------------------------------------------
\section{{\tt DC} command}
\index{dc command}
\index{transfer characteristics}
\index{nonlinear transfer analysis}
%------------------------------------------------------------------------
\subsection{Syntax}
\begin{verse}
{\tt DC} {\it start stop stepsize} \{{\it options} ...\}\\
{\tt DC} {\it label start stop stepsize} \{{\it options} ...\}
\end{verse}
%------------------------------------------------------------------------
\subsection{Purpose}
Performs a nonlinear DC steady state analysis, and sweeps the signal input,
or a component value.
%------------------------------------------------------------------------
\subsection{Status}
Nesting of sweeps is not supported. (SPICE supports two
levels of nesting.)
%------------------------------------------------------------------------
\subsection{Comments}
The nodes to look at must have been previously selected by the {\tt print} or
{\tt plot} command.
If there are numeric arguments, without a part label, they represent a ramp
from the {\tt generator} function. They are the start value, stop value
and step size, in order. They are saved between commands, so no arguments
will repeat the previous sweep.
A single parameter represents a single input voltage. Two parameters
instruct the computer to analyze for those two points only.
In some cases, you will get one more step outside the specified range of
inputs due to internal rounding errors. The last input may be beyond the end
point.
This command also sets up a movable operating point for subsequent {\tt AC}
analysis, which can be helpful in distortion analysis.
The program will sweep any simple component, including resistors,
capacitors, and controlled sources. SPICE sweeps only fixed sources (types
{\tt V} and {\tt I}).
%------------------------------------------------------------------------
\subsection{Options}
\begin{description}
\item[{\tt *} {\it multiplier}] Log sweep. Multiply the
input by {\it multiplier} to get the next step. Do not
pass zero volts!!
\item[{\tt >} {\it file}] Send results of analysis to {\it file}.
\item[{\tt >>} {\it file}] Append results to {\it file}.
%%%\item[{\tt ACMAx}] Use worst case max values, per last
%%%{\tt AC} analysis.
%%%\item[{\tt ACMIn}] Use worst case min values, per last
%%%{\tt AC} analysis.
\item[{\tt BY} {\it stepsize}] Linear sweep. Add {\it
stepsize} to get the next step.
\item[{\tt Continue}] Use the last step of a {\tt OP},
{\tt DC} or {\tt Transient} analysis as the first guess.
%%%\item[{\tt DCMAx}] Use worst case max values, per last
%%%{\tt DC} or {\tt OP} analysis.
%%%\item[{\tt DCMIn}] Use worst case min values, per last
%%%{\tt DC} or {\tt OP} analysis.
\item[{\tt Decade} {\it steps}] Log sweep. Use {\it
steps} steps per decade.
%%%\item[{\tt Input} {\it volts}] Apply {\it volts} input to
%%%the circuit, instead of the sweep. It will not forget the
%%%old sweep parameters.
%%%\item[{\tt LAg}] Use worst case values, for lagging phase,
%%% per {\tt AC} analysis.
%%%\item[{\tt LEad}] Use worst case values, for leading
%%% phase, per {\tt AC} analysis.
\item[{\tt LOop}] Repeat the sweep, backwards.
%%%\item[{\tt MAx}] Use worst case max values, per same type
%%%({\tt OP} or {\tt DC}) analysis. (Same as {\tt DCMAx},
%%% here.)
%%%\item[{\tt MIn}] Use worst case min values, per same type
%%%({\tt OP} or {\tt DC}) analysis. (Same as {\tt DCMIn},
%%% here.)
%%%\item[{\tt MCarlo} {\it trials}] Monte-Carlo analysis.
%%% Simulate {\it trials} circuits; compile statistics. Hide
%%% individual trials.
\item[{\tt NOPlot}] Suppress plotting.
\item[{\tt PLot}] Graphic output, when plotting is
normally off.
\item[{\tt Print}] Send results to printer.
\item[{\tt Quiet}] Suppress console output.
%%%\item[{\tt Random} {\it trials}] Simulate {\it trials}
%%% circuits using random values.
\item[{\tt REverse}] Sweep in the opposite direction.
%%%\item[{\tt TAble}] Tabular output. Override default plot.
\item[{\tt TEmperature} {\it degrees}] Temperature,
degrees C.
\item[{\tt Times} {\it multiplier}] Log sweep. Multiply
the input by {\it multiplier} to get the next step. Do
not pass zero volts!!
\item[{\tt TRace} {\it n}] Show extended information during solution.
\begin{description}
\item[4] Show every iteration.
\item[5] Show extended diagnostics.
\end{description}
%%%\item[{\tt WOrstcase} {\it probe}] Worst case analysis, at
%%%{\it probe}.
\end{description}
%------------------------------------------------------------------------
\subsection{Examples}
\begin{description}
\item[{\tt dc 1}] Do a single point DC signal simulation, with {`1 volt'}
input.
\item[{\tt dc -10 15 1}] Sweep the circuit input from -10 to +15 in steps of
1. (usually volts.) Do a DC transfer simulation at each step.
\item[{\tt dc}] With no parameters, it uses the same ones as the last time.
In this case, from -10 to 15 in 1\ volt steps.
\item[{\tt dc 20 0 -2}] You can sweep downward, by asking for a negative
increment. Sometimes, this will result in better convergence, or even
different results! (For example, in the case of a bi-stable circuit.)
%%%\item[{\tt dc input 2.3}] Apply an input to the circuit of 2.3 volts. This
%%%overrides the sweep, for now. It isn't remembered for next time. Also,
%%%since it is a single point, you will get a table, rather than a plot.
\item[{\tt dc}] Since the last time used the {\tt input} option, go back one
more to find what the sweep parameters were. In this case, downward from 20
to 0 in steps of 2. (Because we did it 2 commands ago.)
\item[{\tt dc -2 2 .1 loop}] After the sweep, do it again in the opposite
direction. In this case, the sweep is -2 to +2 in steps of .1. After it
gets to +2, it will go back, and sweep from +2 to -2 in steps of -.1. The
plot will be superimposed on the up sweep. This way, you can see hysteresis
in the circuit.
\item[{\tt dc temperature 75}] Simulate at 75 degrees, this time. Since we
didn't specify new sweep parameters, do the same as last time. (Without the
loop.)
%%%\item[{\tt dc 1 worstcase v r12}] A worst case analysis
%%% for voltage across the resistor {\tt R12}, with input of 1.
\end{description}
%------------------------------------------------------------------------
%------------------------------------------------------------------------
|
