BVSRC - Non-Linear Dependent Voltage Source Model

Old Content - visit altium.com/documentation

Modified by Admin on Sep 13, 2017

Model Kind

Voltage Source

Model Sub-Kind

Equation

SPICE Prefix

SPICE Netlist Template Format

@DESIGNATOR %1 %2 V=@EQUATION

Parameters (definable at component level)

The following component-level parameters are definable for this model type and are listed on the Parameters tab of the Sim Model dialog. To access this dialog, simply double-click on the entry for the simulation model link in the Models region of the Component Properties dialog.

Equation

expression defining the source waveform.

Notes

Standard SPICE non-linear dependant voltage source. This source is sometimes called an Equation-defined source, as the output is defined by a user-defined equation, often referencing voltages at other nodes in the circuit.
The voltage waveform is described by:

V = expression

where,

expression is the user-defined equation entered in the corresponding Equation parameter field.

The following standard functions can be used to create the expression:

ABS()	absolute value function. ABS(x) returns the value of \|x\|.
LN()	natural logarithm function, where LN(e) = 1.
SQRT()	square root function.
LOG()	log base 10 function.
EXP()	exponential function. EXP(x) returns the value of 'e raised to the power of x', where e is the base of the natural logarithms.
SIN()	sine function.
ASIN()	arc sine function.
ASINH()	hyperbolic arc sine function.
SINH()	hyperbolic sine function.
COS()	cosine function.
ACOS()	arc cosine function.
ACOSH()	hyperbolic arc cosine function.
COSH()	hyperbolic cosine function.
TAN()	tangent function.
ATAN()	arc tangent function.
ATANH()	hyperbolic arc tangent function.
U()	unit step function. Returns a value of 1 for arguments greater than 0 and a value of 0 for arguments less than 0.
URAMP()	unit ramp function. Integral of the unit step: for an input x, the value is 0 if x is less than 0, or if x is greater than 0, the value is x.

The following standard operators are supported:

+	addition operator.
-	subtraction operator.
*	multiplication operator.
/	division operator.
^	power operator. y^x returns the value of 'y raised to the power of x'.
unary -	unary minus operator. unary -x returns -x.

To reference in an equation the voltage at a node in your circuit, you must first name the node in the schematic using a Net Label. You then use the name defined in the Net field of the Net Label's properties to reference the node using the following syntax:

V(Net) - references the voltage at node Net

For example, if you have a node in your circuit labeled with a Net Label called IN, then the following would be valid entries in the Equation parameter field of the source:

V(IN)^3 COS(V(IN))

By default, the node is referenced to the Spice Reference Net Name, specified on the Spice Options page of the Analyses Setup dialog. This is GND by default. You can include a different reference node directly in the equation using the following syntax:

V(netlabel1, netlabel2)

For example:

LN(COS(LOG(V(NetLabel1,NetLabel2)^2)))- V(NetLabel2)^V(NetLabel1)

If the argument of a LOG(), LN(), or SQRT() function becomes less than zero, the absolute value of the argument is used.
If a divisor becomes zero or the argument of log or ln becomes zero, an error will result. Other problems may occur when the argument for a function in a partial derivative enters a region where that function is undefined.
The simulation-ready non-linear dependent voltage source component (BVSRC) can be found in the Simulation Sources integrated library (\Library\Simulation\Simulation Sources.IntLib).

Examples

Consider the non-linear dependent voltage source in the above image, with the following characteristics:

Pin1 (positive) is connected to net N9
Pin2 (negative) is connected to net GND
Designator is BGND
Equation = V(VCC).5+V(VEE).5

The entry in the SPICE netlist would be:

*Schematic Netlist: BGND N9 0 V=V(VCC).5+V(VEE).5