The transient analysis portion of DR. SPICE computes the transient output variables as a function of time over a user-specified time interval. The initial conditions are automatically determined by a DC analysis. All sources that are not time dependent (for example, power supplies) are set to their DC value. The transient time interval is specified on a .TRAN control line.
| Entry | Description |
| Print Interval | Required entry, but is used only when printing data to the .out file. |
| Final Analysis Time | The time at which simulation will stop. |
| Starting Save Time | Time at which printing and plotting waveforms will begin. Default is 0. |
| Maximum Step Size | The largest time step DR. SPICE is allowed
to take. The default is unlimited. |
| Skip Operating Point Calculation (UIC) | DR. SPICE uses the initial conditions
placed on elements as the starting solution at time zero. |
| Title | Tile which will appear within the Simulation menu |
The Transient Analysis dialog box is analogous to the .TRAN analysis command found in the circuit file. The syntax is:
.TRAN TSTEP TSTOP [TSTART [TMAX]] [UIC]
Examples:
.TRAN 1NS 100NS .TRAN 1NS 1000NS 500NS
TSTEP is the printing or plotting increment for line-printer output. TSTEP is the suggested computing increment for use with the post-processor. TSTOP is the final time, and TSTART is the initial time. If TSTART is omitted, it is assumed to be zero. The transient analysis always begins at time zero. In the interval <zero, TSTART>, the circuit is analyzed (to reach a steady state), but no outputs are stored.
In the interval <TSTART, TSTOP>, the circuit is analyzed and outputs are stored. TMAX is the maximum stepsize that DR. SPICE will use [for default, the program chooses either TSTEP or (TSTOP-TSTART)/50.0, whichever is smaller]. TMAX can be used to guarantee a computing interval that is smaller than the printer increment, TSTEP.
The optional keyword UIC (use initial conditions) indicates that the user does not want DR. SPICE to solve for the quiescent operating point before beginning the transient analysis. If this keyword is specified, DR. SPICE uses the values specified using IC=... on the various elements (C, L, D, ...) as the initial transient condition and proceeds with the analysis. If the .IC statement has been specified, then the node voltages on the .IC statement are used to compute the initial conditions for the devices. Refer to the description on the .IC statement for its interpretation when UIC is not specified.
Example Transient Circuit Analysis: Class B Output Stage
This is one of the example circuits provided with DR. SPICE. You can run the simulation and view the results. In the following example, DR. SPICE computes the transient response of a class B output stage from 0 ms to 100 ms.
The circuit schematic looks like this:
Transient Analysis Example Circuit Schematic
The SPICE file created from the schematic is available in the examples directory as ckt1.cir. The file looks like this:
SIMPLE CLASS B OUTPUT STAGE VIN IN 0 SIN(0 5 10K) VCC VCC 0 12V VEE VEE 0 -12V Q1 VCC IN OUT MODN Q2 VEE IN OUT MODP RLOAD OUT 0 10K .MODEL MODN NPN .MODEL MODP PNP .TRAN 1U 100U .END
If you open the SPICE file and run it now, the output should look like:
Transient Analysis Output File
You can see the effect of crossover distortion.