DC analysis defines 1 or 2 DC transfer curve sources and sweeps their values.
| Entry | Description |
| First Source Name | The first independent voltage or current source name. |
| Start Value | When ramping the source, start at this value. |
| End Value | The final value the source is ramped to. |
| Number of Points | Number of point between the starting and ending values. |
| Increment | The delta voltage (current) between each simulation in the analysis. |
| Has Second Sweep | Enables the Second Source Name entry boxes. |
| Second Source Name | The second independent voltage or current source name. The first source will be ramped for each value of the second source. |
| New Title | Tile which will appear within the Simulation menu. |
The DC Analysis dialog box is analogous to the .DC analysis command found in the circuit file. The syntax is:
.DC SRCNAM VSTART VSTOP VINCR [SRC2 START2 STOP2 + INCR2]
Examples:
.DC VIN 0.25 5.0 0.25 .DC VDS 0 10 .5 VGS 0 5 1 .DC VCE 0 10 .25 IB 0 10U 1U
SRCNAM is the name of an independent voltage or current source. VSTART, VSTOP, and VINCR are the starting, final, and incrementing values respectively. The first example will cause the value of the voltage source VIN to be swept from 0.25 V to 5.0 V in increments of 0.25 V.
A second source (SRC2) may optionally be specified with associated sweep parameters. In this case, the first source will be swept over its range for each value of the second source. This option can be useful for obtaining semiconductor device output characteristics.
Example .DC Circuit Analysis: Simple Class B Amplifier
This is one of the example circuits provided with DR. SPICE. You can run the simulation and view the results.
The circuit schematic looks like this:
DC 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 DC 0 AC 1 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 .DC VIN -12 12 0.5 .end
If you open the SPICE file and run it now, the output should look like this:
DC Analysis Output File
You can clearly see the effects of crossover distortion in this circuit.
DC Sweep Analysis Example
Input File, sweepm.cir:
Project sweep: DR. SPICE Curve Trace Model Test for RB N5 N22 1K VCE VCE 0 DC 0 VIC VCE N34 DC 0 IB 0 N5 DC 0 Q1 N34 N22 0 q2n2222 .DC VCE 0 10 .02 IB .01m 10m 1m .PROBE/CSDF DC I(VIC) .model q2n2222 npn(is=28.2f xti=3 eg=1.11 vaf=101.8 bf=224.1 ne=1.327 ise=28.2f + ikf=.5699 xtb=1.5 br=3.374 nc=2 isc=0 ikr=0 rc=0 cjc=12.14p vjc=.75 + mjc=.3333 fc=.5 cje=23.71p vje=.75 mje=.3333 tr=113.7n tf=340.7p itf=0 vtf=0 + xtf=0) .END
Waveforms in DR. SPICE:
BJT I-V Characteristics