PSpice Notes PSpice Analysis Types and Common Signal Sources http://www.csee.ogi.edu/support/tut/pspice.notes.txt John Hunt 10/10/2006 ****************************************************** DC Nodal Analysis (also known as "Bias Point Detail") The DC Nodal Analysis is performed before any other analysis to determine the initial DC voltages throughout the circuit. ****************************************************** DC Sweep DC Sweep steps the source through a range of DC values that you specify and calculates the DC voltages throughout the circuit. Use the Analysis Setup, DC Sweep window to select the voltage source you want to sweep and the sweep parameters. Signal Sources for DC Sweep or DC Nodal Analysis: VDC default unit DC= none volt required (you have to set the value of "DC" or the netlist will not be generated) VSRC, VAC, VSIN, VPULSE default unit DC= 0 volt "DC" defaults to 0V for these sources ****************************************************** AC Sweep AC Sweep performs frequency domain analysis. It finds the magnitude and phases of voltages and currents throughout your circuit. Use it for Bode plots, gain and phase plots, phasor analysis. PSpice first calculates the DC bias points then runs a small-signal analysis at the bias points. This process is repeated at each AC frequency you specified in your sweep parameter settings. AC Sweep will not show signal clipping or other distortion: it assumes that the signal you are applying (of any amplitude) is a "small signal" applied to a perfect linear system linearized about the DC bias points. You need to run Transient Analysis to observe time domain signal distortion. Use the Analysis Setup window to select AC Sweep Type and Sweep Parameters. This is also where you select the optional Noise Analysis which runs in conjunction with AC Sweep. ****************************************************** Noise Analysis Noise Analysis can be selected in the AC Sweep setup window. If enabled, Noise Analysis is performed at each frequency step in the AC sweep interval. Two output noise variables are created which can be selected as traces in probe: V(ONOISE) is the output noise with units of volts/rt Hz V(INOISE) is the equivalent input noise (volts/rt Hz) A noise value is produced at each frequency step in the AC sweep. The noise values can also optionally be reported in the output file. (If your schematic file is called mycircuit.sch pspice will produce mycircuit.out as its output file). To setup Noise Analysis you need to click on "Noise Enabled" in the AC Sweep setup box and specify: Output Voltage: This is the node from which the output noise is to be calculated. For example, V(vout) Input I or V source: For example, v1 To calculate the equivalent input noise PSpice needs to know where you want to consider the input to be. It needs to know the "Reference Designator" for the input source. For example, if your signal source is a VSIN shown as v1 on the schematic, specify v1 . Interval: for example, 10 This is the "print interval". Noise analysis is performed at each of the frequency steps you specify for the AC sweep. "Interval" determines which of the frequency steps will produce an entry in the output file. If you choose 10, then every 10th step is reported. If you choose 1, then every step is reported. 0 is the default which results in no noise reports in the output file. ****************************************************** Signal Sources for AC Sweep: VAC default unit DC= 0 volt ACMAG= 0 volt (peak amplitude) Other Signal Sources: VSIN or VPULSE or VSRC are normally meant for Transient Analysis. However, you can also use them to set the AC sweep amplitude. For further confusion, the AC sweep amplitude attribute is called "AC" for those sources (not "ACMAG" as used in the VAC source). Note: AC sweep uses the "ACMAG" or "AC" attribute. These attributes are ignored for DC Sweep or Transient Analysis. ****************************************************** Transient Analysis Transient Analysis calculates the time domain response of your circuit and optionally performs a Fourier and distortion analysis. Within the Transient Analysis setup window you specify: Print Step: time between steps in the output data file (needs to be < final time or Pspice won't run) Final Time: last time value in the output file (total transient run time) No Print Delay: optional, skips generation of output data for print and probe for specified initial time Step Ceiling: maximum time between steps, default is Final Time/50. Reduce this value to improve the accuracy of your probe plots. PSpice adjusts its internal time steps to maintain sufficient accuracy yet save simulation time. During static intervals the time steps will be increased (up to the limit of the Step Ceiling you specify). During transient events it will be reduced to until adequate accuracy is achieved. Specifying the values in the Transient setup requires some judgment. In the two extremes you can specify either: 1. small time steps for good accuracy for your plotted waveforms (but long simulation times and big data files). 2. large time steps for short simulation times (but possibly missing important time response details). The individual plotted points at each time step will be accurate, but the plot can be misleading because the data points are connected by straight lines. ****************************************************** Signal Sources for Transient Analysis: VSIN default unit DC= 0 volt only used for DC sweep AC= 0 volt only used for AC sweep VOFF= none volt DC offset voltage (required) VAMPL= none volt AC peak amplitude (required) FREQ= none Hz (required) VPULSE DC= 0 volt only used for DC sweep AC= 0 volt only used for AC sweep V1= none volt initial voltage (required) V2= none volt peak voltage (required) TD= 0 sec initial time delay TR= Pstep sec rise time (default is "Print Step" from Transient Analysis setup) TF= Pstep sec fall time (default is "Print Step" from Transient Analysis setup) PW= Tfinal sec pulse width (default is "Final Time" from Transient Analysis setup) PER= Tfinal sec period (default is "Final Time" from Transient Analysis setup) ****************************************************** Fourier Analysis and Harmonic Distortion Fourier Analysis can be selected in the Transient setup window. Center Frequency: This is the fundamental frequency to be used in the Fourier Analysis. Normally you want to set this equal to your source frequency. Number of Harmonics: (optional, default is 9) Output Vars: the waveform to be analyzed, for example: V(vout) The last portion in the transient output data (one period of the fundamental) is used for the analysis. Take care to have the fundamental match your source frequency so the harmonic analysis is performed over a full period. If you want an FFT of the entire waveform you can run an FFT from within Probe. The result of the Fourier Analysis is attached as a table at the end of the output file. (If your schematic file is called mycircuit.sch pspice will produce mycircuit.out as its output file). The Total Harmonic Distortion is also printed as part of Fourier Analysis table.