VPULSE - Pulse Voltage Source Model

Old Content - visit altium.com/documentation

Modified by Admin on Sep 13, 2017

Model Kind

Voltage Source

Model Sub-Kind

Pulse

SPICE Prefix

SPICE Netlist Template Format

@DESIGNATOR %1 %2 ?"DC MAGNITUDE"|DC @"DC MAGNITUDE"| PULSE(?"INITIAL VALUE"/&"INITIAL VALUE"//0/ ?"PULSED VALUE"/&"PULSED VALUE"//5/ ?"TIME DELAY"/&"TIME DELAY"//0/ ?"RISE TIME"/&"RISE TIME"//4U/ ?"FALL TIME"/&"FALL TIME"//1U/ ?"PULSE WIDTH"/&"PULSE WIDTH"//0/ ?PERIOD/&PERIOD//5U/ &PHASE) #"AC MAGNITUDE"|AC @"AC MAGNITUDE"| @"AC PHASE"

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.

DC Magnitude	DC offset used in an Operating Point Analysis. (Default = 0).
AC Magnitude	the magnitude of the source when used in an AC Small Signal Analysis. (Default = 1).
AC Phase	the phase of the source when used in an AC Small Signal Analysis. (Default = 0).
Initial Value	voltage amplitude at time zero (in Volts). (Default = 0).
Pulsed Value	maximum amplitude of the output swing (in Volts). (Default = 5).
Time Delay	delay before the source changes from Initial voltage value to Pulsed voltage value (in seconds).
Rise Time	the time it takes to rise from Initial voltage value to Pulsed voltage value (in seconds). Must be > 0. (Default = 4u).
Fall Time	the time it takes to fall from Pulsed voltage value back to the Initial voltage value (in seconds). Must be > 0. (Default = 1u).
Pulse Width	the time that the source remains at the Pulsed voltage amplitude (in seconds). (Default = 0).
Period	the time between the start of the first pulse and the start of the second pulse (in seconds). (Default = 5u).
Phase	phase shift of the waveform at time zero (in Degrees).

Notes

The image below shows an example waveform produced by a periodic-pulse voltage source (connected to a 1Ohm load). The Pulse Width has been set to 5u, the Period has been set to 20u. All other parameters have been left at their default values:

The shape of the waveform is described as follows:

V(t ₀ ) = V_IV

V(t _TD ) = V_IV

V(t_TD + t_RT) = V_PV

V(t_TD + t_RT + t_PW) = V_PV

V(t_TD + t_RT + t_PW + t_FT) = V_IV

V(t_STOP) = V_IV

where,

t is an instance of time
V_IV is the initial value of the voltage
V_PV is the pulsed value of the voltage
t_TD is the Time Delay
t_RT is the Rise Time
t_PW is the Pulse Width and
t_FT is the Fall Time.

The value for the voltage at intermediate values of time is calculated using linear interpolation.
The simulation-ready pulse voltage source component (VPULSE) can be found in the Simulation Sources integrated library (\Library\Simulation\Simulation Sources.IntLib).

Examples

Consider the pulse voltage source in the above image, with the following characteristics:

Pin1 (positive) is connected to net CP
Pin2 (negative) is connected to net GND
Designator is VCP
Time Delay = 0
Rise Time = 1u
Pulse Width = 500u
Period = 1000u
All other parameters for the model are left at their default values.

The entry in the SPICE netlist would be:

*Schematic Netlist: VCP CP 0 DC 0 PULSE(0 5 0 1u 1u 500u 1000u) AC 1 0