www.kxcad.net Home > Electronic Index > Altium(Protel) Index
A Transient analysis generates output similar to that normally shown on an oscilloscope, computing the transient output variables (voltage or current) as a function of time, over the user-specified time interval. An Operating Point analysis is automatically performed prior to a Transient analysis to determine the DC bias of the circuit, unless the Use Initial Conditions parameter is enabled.
Transient analysis is set up on the Transient/Fourier Analysis Setup page of the Analyses Setup dialog (after the dialog appears, simply click the Transient/Fourier Analysis entry in the Analyses/Options list). The default setup for this analysis type is shown in the image below:
Transient Stat Time - the value for the start of the required time interval for analysis (in seconds)
Transient Stop Time - the value for the end of the required time interval for analysis (in seconds)
Transient Step Time - the nominal time increment used in the analysis.
Transient Max Step Time - the maximum variation in size of the time step that can be used by the Simulator when calculating the transient data. By default, the value used is either
Transient Step Time or
(Transient Stop Time - Transient Start Time) / 50,
whichever is the smaller.
Use Initial Conditions - when enabled, the Transient analysis begins from the initial conditions defined in the schematic, bypassing the Operating Point analysis. Use this option when you wish to perform a transient analysis starting from other than the quiescent operating point.
Use Transient Defaults - when enabled, parameters are automatically calculated before each simulation run, overriding any manually set values.
Default Cycles Displayed - the default number of periods of a sinusoidal waveform to display. This value is used in the automatic calculation of the Transient Stop Time, when the Set Defaults button is pressed.
Default Points Per Cycle - the number of data points per sinusoidal waveform period. This value is used in the automatic calculation of the Transient Step Time when the Set Defaults button is pressed.
A Transient analysis always begins at time zero. In the time interval between zero and Transient Start Time, the circuit is analyzed but the results are not stored. In the time interval between Transient Start Time and Transient Stop Time, results are stored for display.
Although Transient Step Time is the nominal time increment used in the analysis, the actual time step is varied automatically to achieve convergence.
Typically Transient Step Time and Transient Max Step Time are set to the same value. As a starting point set both of these parameters to
(Transient Stop Time - Transient Start Time) / 1000.
Transient Start Time is set to zero
Transient Stop Time, Transient Step Time and Transient Max Step Time are calculated based on the values entered for the Default Cycles Displayed and Default Points Per Cycle parameters, as well as the lowest frequency source in the circuit (with frequency FL). The formulae used for the calculations are as follows:
Transient Stop Time = (1/FL) * Default Cycles Displayed
Transient Step Time = (1/FL) / Default Points Per Cycle
Transient Max Step Time = Transient Step Time
Data is saved for all signals in the Available Signals list, on the General Setup page of the Analyses Setup dialog.
The simulation results are displayed on the Transient Analysis tab of the Waveform Analysis window.
Transient Start Time = 0.000
Transient Stop Time = 100.0u
Transient Step Time = 500.0n
Transient Max Step Time = 1.000u
Default Cycles Displayed = 5
Default Points Per Cycle = 50
Use Initial Conditions and Use Transient Defaults parameters are both disabled.
The entry in the SPICE netlist will be:
*Selected Circuit Analyses:
.TRAN 5E-7 0.0001 0 1E-6
and running the simulation will yield the output waveforms shown in the image below:
Operating Point Analysis