Micro-Cap v7.1.6 / RM

.PARAMETERS

General Form (Schematics only)

.PARAMETERS (<parameter[=<value>]> [, <parameter[=<value>]>]*)

Examples

.parameters(GBW, Slew, Iscp, F1=1K, F2=1.1K)

.Parameters(Gain,ROUT=50)

The .PARAMETERS statement is placed in a macro circuit as grid text or in the text area and declares the names of parameters to be passed to it from the calling circuit. A parameter is a numeric value that you pass to a macro circuit from the macro's VALUE attribute (or an equivalent .MACRO statement). It can be used in the macro circuit as, for example, the VALUE attribute of a resistor, or as a model parameter value, such as the BF of a BJT transistor.

The optional default [=<value>] specifies a parameter's default value. This value is assigned to the parameter when the part is placed in the schematic. The value can be edited from the Attribute dialog box. If the parameter's default value is not specified in the .PARAMETERS statement within the macro, its value must be specified when the macro is placed in a circuit.

See the macro circuits SCR, XTAL, PUT, or TRIAC for examples of this command.

317

.PLOT

General Form (SPICE files only)

.PLOT <analysis type> [<output variable>]* + ([<lower limit value>,<upper limit value>])*

Examples

.PLOT AC V(10) V(1,2) (0,10)

.PLOT TRAN V(1) D(2)

This statement specifies what is to be plotted in the analysis plot. It enters the specified variables as simple waveform expressions in the Analysis Limits Y expression fields. <analysis type> is one of the following AC, DC, NOISE, or TRAN. Output variables can be any valid node voltage, source current, or digital state.

318 Chapter 20: Command Statements

.PRINT

General Form (SPICE files only)

.PRINT <analysis type> [<output variable>]*

Examples

.PRINT AC V(1) V(3)

.PRINT TRAN V(1) D(10)

This statement specifies what is to be printed in the Numeric Output window. It enters the specified variables as simple waveform expressions in the Analysis Limits Y expression fields. <analysis type> is one of the following: AC, DC, NOISE, or TRAN. Output variables include node voltages, source currents, and digital states. Numeric Output window contents are also saved in one of the followingfiles:

319

.SENS

General Form (SPICE files only)

.SENS <output expression> [<output expression>]*

Examples

.SENS V(1) V(3)

.SENS V(D1)*I(D1)

This statement controls the sensitivity analysis feature. It tells the program to calculate the DC sensitivity of each specified <output expression> to the default parameters. Default parameters include a subset of all possible model parameters. These can be changed from the Sensitivity analysis dialog box.

320 Chapter 20: Command Statements

.SUBCKT

General Form (SPICE files and schematic text areas only)

.SUBCKT <subcircuit name> [<node>]*

+[OPTIONAL:<<node>=<default value>>*]

+[PARAMS:<<parameter name>=<parameter default value>>*]

+[TEXT:<<text name>=<text default value>>*]

Examples

.SUBCKT LT1037 1 2 3 50 99

.SUBCKT CLIP IN OUT PARAMS: LOW=0 HIGH=10

.SUBCKT 7400 D1 D2 Y1

+ OPTIONAL: DPWR=44 DGND=55

This statement marks the beginning of a subcircuit definition. The subcircuit definition ends with the .ENDS statement. All statements between the .SUBCKT and the .ENDS statements are included in the subcircuit definition.

<subcircuit name> is the name of the subcircuit and is the name used when the subcircuit is called or used by another circuit.

[<node>]* are the node numbers passed from the subcircuit to the calling circuit. The number of nodes in the subcircuit call must be the same as the number of nodes in the .SUBCKT statement. When the subcircuit is called, the nodes in the call are substituted for the nodes in the body of the subcircuit in the same order as in the .SUBCKT statement. Consider this example:

X1 1 2 BLOCK

.SUBCKT BLOCK 10 20 R1 10 0 1K

R2 20 0 2K

.ENDS

In this example, the resistor R1 is connected between node 1 and node 0 and R2 is connected between node 2 and node 0.

The OPTIONAL keyword lets you add one or more nodes to the subcircuit call. If the nodes are added, they override the default node values. This option is often used to override the default digital global power pins. In the subcircuit call, you may specify one or more of the optional nodes in the call, but you must specify all

321

.TEMP

General Form (SPICE files only)

.TEMP <temperature value>

Examples

.TEMP 50

.TEMP 0 50 100

The .TEMP statement specifies the operating temperature at which the circuit will be analyzed. The default value is 27 ° Centigrade. Temperature dependent parameters are a function of the difference between the operating temperature and the measurement temperature.

The temperature at which device parameters are assumed to have been measured is called the measurement temperature or TNOM. It is obtained from a

.OPTIONS TNOM=XX statement. If this statement is not present in the circuit, the Global Settings TNOM value is used instead.

323

.TF

General Form (SPICE files only)

.TF <output expression> <input source name>

Examples

.TF V(OUT) V1

.TF VBE(Q1)*IB(Q1) VIN

In this type of analysis, the program calculates the small-signal DC transfer function from the specified <input source name> to the specified <output expression>. It also calculates the small-signal DC input and output resistances.

324 Chapter 20: Command Statements

.TIE

General Form (Schematics)

.TIE <part name> <pin name>

Examples

.TIE JKFF CLKB

.TIE LF155 VCC

The .TIE statement connects together all of the specified <pin name> pins of the specified <part name> parts. This is a convenient way of simultaneously connecting many common pins. It is normally used for power, clock, reset, and preset pins. The first example above specifies that the CLKB pins of all JKFF parts are to be connected together.

Note that <part name> is the general part name from the Component library, not a schematic part name. For example, in a circuit with three JKFF parts, named U1, U2, and U3, the CLKB pins would be connected with .TIE JKFF CLKB.

325

.TR

General Form (Schematics)

.TR <s1 t1> [s2 t2...sn-1 tn-1 sn tn]

The .TR statement lets you set the maximum time step during different parts of transient analysis.

Examples

.TR 1n 100n .1n 200n 10n 1u

In this example the time step is limited to 1n from tmin to 100n. Between 100ns and 200ns it is limited to .1n. Between 200ns and 1us it is limited to 10n.

The purpose of this command is to provide some flexibility in simulating difficult circuits. It is mainly used when the circuit needs a more conservative (smaller) maximum time step during a critical part of the simulation but would have a very long run time if the smaller maximum time step were specified for the entire run.

Without this command, the Maximum Time Step parameter specified in the Analysis Limits dialog box controls the time step for the entire run.

326 Chapter 20: Command Statements