Issue link: https://resources.pcb.cadence.com/i/1180526
PSpice User Guide DC analyses October 2019 473 Product Version 17.4-2019 © 1999-2019 All Rights Reserved. The Simulation Settings dialog box appears. 2. Under Analysis Type, select DC Sweep. 3. For the Primary Sweep option, enter the necessary parameter values and select the appropriate check boxes to complete the analysis specifications. 4. Click OK to save the simulation profile. 5. Select Run under the PSpice menu to start the simulation. Note: Do not specify a DC sweep and a parametric analysis for the same variable. Overview of DC sweep The DC sweep analysis causes a DC sweep to be performed on the circuit. DC sweep allows you to sweep a source (voltage or current), a global parameter, a model parameter, or the temperature through a range of values. The bias point of the circuit is calculated for each value of the sweep. This is useful for finding the transfer function of an amplifier, the high and low thresholds of a logic gate, and so on. For the DC sweep analysis specified in Figure 9-1, the voltage source V1 is swept from -0.125 volts to 0.125 volts by steps of 0.005. This means that the output has (0.125 + 0.125)/0.005 +1 = 51 steps or simulation points. A source with a DC specification (such as VDC or IDC) must be used if the swept variable is to be a voltage type or current source. To set the DC value, select Properties from the Edit menu, then click on the cell under the DC column and type in its value. The default DC value of V1 is overridden during the DC sweep analysis and is made to be the swept value. All of the other sources retain their values. 1. In this guide, design entry tool is used for both OrCAD Capture and Design Entry HDL. Any differences between the two tools is mentioned if necessary. Depending on the license available, you will access either PSpice or PSpice Simulator.