Micro-Cap v7.1.6 / RM
.PDF
Capacitor
SPICE format
Syntax
C<name> <plus> <minus> [model name] <value> [IC=<initial voltage>]
Examples
C1 2 3 1U
C2 7 8 110P IC=2
<plus> and <minus> are the positive and negative node numbers. The polarity references are used to apply the initial condition.
Schematic format
PART attribute <name>
Examples
C5
XC16
VALUE attribute
<value> [IC=<initial voltage>]
Examples 1U
110P IC=3 50U*(1+V(6)/100)
FREQ attribute [fexpr]
Examples 1.2+10m*log(F)
MODEL attribute [model name]
Examples
CMOD
MICA
377
VALUE attribute
<value> may be a simple number or an expression involving time-domain variables. It is evaluated in the time domain only. Consider the following expression:
1n+V(10)*2n
V(10) refers to the value of the voltage on node 10 during a transient analysis, a DC operating point calculation prior to an AC analysis, or during a DC analysis. It does not mean the AC small signal voltage on node 10. If the DC operating point value for node 10 was 2, the capacitance would be evaluated as 1n + 2*2n = 5n. The constant value, 5n, would be used in AC analysis.
FREQ attribute
If <fexpr> is used, it replaces the value determined during the operating point. <fexpr> may be a simple number or an expression involving frequency domain variables. The expression is evaluated during AC analysis as the frequency changes. For example, suppose the <fexpr> attribute is this:
1n + 1E-9*V(1,2)*(1+10m*log(f))
In this expression F refers to the AC analysis frequency variable and V(1,2) refers to the AC small signal voltage between nodes 1 and 2. Note that there is no time-domain equivalent to <fexpr>. Even if <fexpr> is present, <value> will be used in transient analysis.
Initial conditions
The initial condition assigns an initial voltage across the capacitor.
Stepping effects
The VALUE attribute and all of the model parameters may be stepped. If VALUE is stepped, it replaces <value>, even if it is an expression. The stepped value may be further modified by the quadratic and temperature effects.
Quadratic effects
If [model name] is used, <value> is multiplied by a factor, QF, a quadratic function of the time-domain voltage, V, across the capacitor.
QF = 1+ VC1•V + VC2•V2
This is intended to provide a subset of the old SPICE 2G POLY keyword, which is no longer supported.
378 Chapter 22: Analog Devices
Temperature effects
The temperature factor is computed as follows:
If [model name] is used, <value> is multiplied by a temperature factor, TF.
TF = 1+TC1•(T-Tnom)+TC2•(T-Tnom)2
TC1 is the linear temperature coefficient and is sometimes given in data sheets as parts per million per degree C. To convert ppm specs to TC1 divide by 1E6. For example, a spec of 1500 ppm/degree C would produce a TC1 value of 1.5E-3.
T is the device operating temperature and Tnom is the temperature at which the nominal capacitance was measured. T is set to the analysis temperature from the Analysis Limits dialog box. TNOM is determined by the Global Settings TNOM value, which can be overridden with a .OPTIONS statement. T and Tnom may be changed for each model by specifying values for T_MEASURED, T_ABS, T_REL_GLOBAL, and T_REL_LOCAL. See the .MODEL section of Chapter 20, "Command Statements", for more information on how device operating temperatures and Tnom temperatures are calculated.
Monte Carlo effects
LOT and DEV Monte Carlo tolerances, available only when [model name] is used, are obtained from the model statement. They are expressed as either a percentage or as an absolute value and are available for all of the model parameters except the T_parameters. Both forms are converted to an equivalent tolerance percentage and produce their effect by increasing or decreasing the Monte Carlo factor, MF, which ultimately multiplies the final value.
MF = 1 ± tolerance percentage /100
If tolerance percentage is zero or Monte Carlo is not in use, then the MF factor is set to 1.0 and has no effect on the final value.
The final capacitance used in the analysis, cvalue, is calculated as follows:
cvalue = value * C * QF * TF * MF
Model statement form
.MODEL <model name> CAP ([model parameters])
Examples
.MODEL CMOD CAP (C=2.0 LOT=10% VC1=2E-3 VC2=.0015)
.MODEL CEL CAP (C=1.0 LOT=5% DEV=.5% T_ABS=37)
379
Model parameters |
|
|
|
Name |
Parameter |
Units |
Default |
C |
Capacitance multiplier |
|
1 |
VC1 |
Linear voltage coefficient |
V-1 |
0 |
VC2 |
Quadratic voltage coefficient |
V-2 |
0 |
TC1 |
Linear temperature coefficient |
°C-1 |
0 |
TC2 |
Quadratic temperature coefficient |
°C-2 |
0 |
T_MEASURED |
Measured temperature |
°C |
|
T_ABS |
Absolute temperature |
°C |
|
T_REL_GLOBAL |
Relative to current temperature |
°C |
|
T_REL_LOCAL |
Relative to AKO temperature |
°C |
|
Noise effects
There are no noise effects included in the capacitor model.
380 Chapter 22: Analog Devices
Dependent sources (SPICE E, F, G, H devices)
Standard SPICE formats:
Syntax of the voltage-controlled voltage source
E<name> <plusout> <minusout> [POLY(<k>)] n1p n1m
+ [n2p n2m...nkp nkm] p0 [p1...pk] [IC=c1[,c2[,c3...[,ck]]]]
Syntax of the current-controlled current source
F<name> <plusout> <minusout> [POLY(<k>)] v1 [v2...vk] + p0 [p1...pk] [IC=c1[,c2[,c3...[,ck]]]]
Syntax of the voltage-controlled current source G<name> <plusout> <minusout> [POLY(<k>)] +n1p n1m [n2p n2m...nkp nkm] p0 [p1...pk] [IC=c1[,c2[,c3...[,ck]]]]
Syntax of the current-controlled voltage source
H<name> <plusout> <minusout> [POLY(<k>)] v1 [v2...vk] + p0 [p1...pk] [IC=c1[,c2[,c3...[,ck]]]]
Standard PSpice supported formats:
Extended syntax of the voltage-controlled voltage source
[E | G]<name> <plusout> <minusout> VALUE = {<expression>}
[E | G]<name> <plusout> <minusout> TABLE{<expression>} = + <<input value>,<output value>>*
[E | G]<name> <plusout> <minusout> LAPLACE {<expression>} = + {<Laplace transfer function>}
[E | G]<name> <plusout> <minusout> FREQ + {<expression>} = [KEYWORD]
+<<frequency value>,<magnitude value>,<phase value>>*
n1p is the first positive controlling node. n1m is the first negative controlling node. nkp is the k'th positive controlling node. nkm is the k'th negative controlling node. p0 is the first polynomial coefficient.
pk is the k'th polynomial coefficient.
v1 is the voltage source whose current is the first controlling variable.
382 Chapter 22: Analog Devices
vk is the voltage source whose current is the k'th controlling variable. c1 is the 1'st initial condition.
ck is the k'th initial condition.
SPICE Examples
E2 7 4 POLY(2) 10 15 20 25 1.0 2.0 10.0 20.0
G2 7 4 POLY(3) 10 15 20 25 30 35 1.0 2.0 3.0 10.0 20.0 30.0 F2 7 4 POLY(2) V1 V2 1.0 2.0 10.0 20.0
H2 7 4 POLY(3) V1 V2 V3 1.0 2.0 3.0 10.0 20.0 30.0 E1 10 20 FREQ {V(1,2)} = (0,0,0) (1K,0,0) (10K,0.001,0)
L1 10 20 TABLE{V(5,6)*V(3)} = {(0,0,0) (1K,0,0) (2K,-20,0)} L2 10 20 LAPLACE {V(5,6)} = {1/(1+.001*S+1E-8*S*S)}
Schematic format
The schematic attributes are similar to the standard SPICE format without the <plusout> and <minusout> node numbers. The TABLE, VALUE, LAPLACE, and FREQ features are not supported in the schematic versions of the E, F, G, and H devices. These features are supported in the Function and Laplace devices, described later in this chapter.
PART attribute <name>
Example
G1
VALUE attribute
[POLY(<k>)] n1p n1m [n2p n2m...nkp nkm] p0 [p1...pk] + [IC=c1[,c2[,c3...[,ck]]]]
[POLY(<k>)] n1p n1m [n2p n2m...nkp nkm] p0 [p1...pk] + [IC=c1[,c2[,c3...[,ck]]]]
[POLY(<k>)] v1 [v2...vk] p0 [p1...pk] [IC=c1[,c2[,c3...[,ck]]]]
[POLY(<k>)] v1 [v2...vk] p0 [p1...pk] [IC=c1[,c2[,c3...[,ck]]]]
Examples
POLY(2) 10 15 20 25 1.0 2.0 10.0 20.0
POLY(3) 10 15 20 25 30 35 1.0 2.0 3.0 10.0 20.0 30.0
POLY(2) V1 V2 1.0 2.0 10.0 20.0
POLY(3) V1 V2 V3 1.0 2.0 3.0 10.0 20.0 30.0
383
The lightly shaded parts of the table mark the coefficients used for summing the input variables. The heavily shaded portions of the table mark the coefficients used for forming a product of the input variables. Other combinations of polynomial products are shown in the rest of the table.
For example, to create a voltage source whose value equals the sum of three input voltages, use this:
E1 4 0 POLY(3) 1 0 2 0 3 0 0 1 1 1
This creates a voltage source whose output is a third-order polynomial function of three sets of differential voltages.
Input variable 1 = V(1) - V(0)= V(1)= voltage on node 1
Input variable 2 = V(2) - V(0)= V(2)= voltage on node 2
Input variable 3 = V(3) - V(0)= V(3)= voltage on node 3
The exponents E1=1, E2=1, and E3=1 are chosen from the p1, p2, and p3 rows, respectively, of the 3'rd order column. The output of this source is:
V =p0•V10•V20•V30+ p1•V11•V20•V30+ p2•V10•V21•V30+ p3•V10•V20•V31
V = p0+ p1•V1+p2•V2+p3•V3
V =0 + 1•V1+1•V2+1•V3
V =V1+V2+V3
To create a current source whose value equals the product of the current flowing in two sources, use this:
F1 3 0 POLY(2) V1 V2 0 0 0 0 1
This creates a current source whose output is a second order polynomial function of the current flowing in the sources V1 and V2.
Input variable 1 = I1= current flowing through V1
Input variable 2 = I2 = current flowing through V2
The exponents E1=1 and E2=1 are chosen from the p4 row and second order col- |
|||||||||||||||||||
umn. The output of this source is: |
|
|
|
|
|
|
|
||||||||||||
I = p |
•I |
0•I 0+ p |
•I 1•I |
0+ p •I 0 |
•I |
1+ p |
•I |
2•I |
0+ p •I 1•I 1 |
||||||||||
0 |
1 |
|
2 |
1 |
1 |
2 |
|
2 |
1 |
2 |
|
3 |
1 |
|
2 |
|
4 |
1 |
2 |
I = 0•I |
0•I 0+ 0•I |
1•I 0+ 0•I 0•I 1+ 0•I |
2•I 0+ 1•I 1•I |
1 |
|
|
|
||||||||||||
1 |
2 |
1 |
|
2 |
|
1 |
2 |
|
|
1 |
2 |
|
1 |
2 |
|
|
|
||
I = I1•I2 |
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
386 Chapter 22: Analog Devices