PSpice Application Notes

PSpice App Note_Modeling Potentiometers and Variable Resistors

Issue link: https://resources.pcb.cadence.com/i/1480198

Contents of this Issue

Navigation

Page 1 of 12

APPLICATION NOTE 1 Introduction In this application note, we will model potentiometers and variable resistors using OrCAD Capture and simulate the example circuits, which include models of potientiometer and variable resistors, using PSpice. Electrically, a potentiometer consists of two resistors connected in series. The specification for the potentiometer consists of: 1. The total resistance (R), and 2. The pot's setting (SET). That is, where the center tap is set. A convenient way to describe this is to define SET to be 0 when the tap is all the way at the bottom and 1 when it is all the way at the top. Modeling Potentiometer A potentiometer can be implemented by the following subcircuit: .SUBCKT POT 1 T 2 PARAMS: VALUE=1K SET=0.5 RT 1 T {VALUE*(1-SET)+.001} RB T 2 {VALUE*SET+.001} .ENDS The values 1.001 (instead of 1) and .001 (instead of 0) are used to prevent the resistors from having 0 ohms at the extremes. So far, the setting of the pot has been static. That is, it does not change with time. This is appropriate for almost all applications, since the time required for the movement of the pot is much longer than the electrical time constants of the circuit. In other words, there is no loss of information by running several transient analyses and varying the pot's setting with a .STEP command. A typical usage would be: .PARAM SET=.5 .STEP PARAM(SET) 0, 1, .2 X1 3 5 17 POT PARAMS: R=10K SET={SET} Here a 10k pot is used in 6 runs, having the settings 0, .2, .4, .6, .8, and 1. In schematics there is a symbol for a potentiometer located in breakout.olb. The following example circuit shows that how a pot may be used with an adjustable regulator. Note: The pot R1 is swept to show the adjustment range of the regulator. Figure 1: Linear potentiometer test circuit

Articles in this issue

view archives of PSpice Application Notes - PSpice App Note_Modeling Potentiometers and Variable Resistors