Temperature in Simulations

The default simulation Temperature used by PSpice, TNOM, is 27C (300K), close enough to the nominal datasheet value of 25C.

Devices with Temperature coefficients are: GaAsFETs; Capacitors; Diodes; JFETs; Inductors; MOSFETS; Bipolar Transistors; Resistors; Voltage and Current Switches (for noise calculations only)

The simulation temperature can be set from the TNOM in Options in the Simulation Profile, sweep the temperature in a DC Sweep, sweep the temperature in a Parametric sweep. Temperature units are degrees Celsius.

Temperature in Models

Semi-conductor devices get their temperature behaviour modelled from temperature in the device equations, see the PSpice Reference manual for more details.

Passive components get their temperature behaviour modelled from Temperature co-efficient Property Values attached to the Parts (Or models for the breakout parts).

Sub-circuits don’t exhibit any temperature dependent behaviour unless this has been added to the component models that the sub-circuit uses.

Temperature attributes are: T_MEASURED, the temperature at which the parameters are extracted; T_ABS, the absolute temperature of the component, overrides TNOM; T_REL_GLOBAL, the temperature of the component is relative to the global temperature, TNOM + T_REL_GLOBAL; T_REL_LOCAL, the component is modelled as an AKO, “another kind of” derived from another model, and the temperature of the component is the T_ABS of the component that it is derived from plus the T_REL_LOCAL value. Only one of the T_ABS, T_REL_GLOBAL or T_REL_LOCAL parameters can be combined with T_MEASURED (See the PSpice Reference Manual for more details).

It will be more accurate to derive a new model at the required operating temperature from the datasheet than to assume that changing the simulation temperature will alter the model parameters. The PSpice libraries contain some temperature specific and radiated models.

Temperature in Resistors

As a specific example, the temperature coefficients for resistors are used as follows:

If TCE is not defined, TC1, the linear temperature coefficient, and TC2, the quadratic temperature co-efficient are used according to this equation:

Resistance = <value>*R*(1+TC1(T-TNOM)+TC2(T-TNOM)**2)

<value> is from the Value property, R is usually 1 and T is the simulation temperature

If TCE is defined:

Resistance = <value>*R*1.01**(TCE*(T-TNOM))

For a Resistor with a datasheet temperature coefficient of 20ppm, set the TC1 property value to 20u

All content Copyright 2022 Parallel Systems Ltd.