All content Copyright 2022 Parallel Systems Ltd.

 

1. Create a new PSpice project, named Zener, based upon the empty project template.

 

2. Use the parts VDC, 0, R and D1N750, to create the circuit pictured below.

 

3. Set up a DC sweep analysis that sweeps the voltage of V1 from 0 to 10 in 10m steps.

The graphic that follows shows the suggested profile settings for this simulation.

 

 

4. Place a current marker on the cathode of the diode, the upper Pin.

 

5. Run the simulation.

 

6. Examine the results in the Probe window.

Notice the diode begins conducting between 4 and 5 volts.

 

7. Move the mouse to the diode and left-click to select it.

 

8. Choose Edit>PSpice Model from the top menu.

Or, right-click>Edit PSpice Model to start the Model Editor.

 

9. Find Bv in the list of parameters.

 

10. Change the value of Bv to 8.0.

 

11. Save the file.

 

12. Return to Capture.

 

13. Rerun the simulation and examine the results. You will see that the diode begins conducting at about 8V.

 

14. Edit the PSpice model again and select the text for the model, starts at the .model and then include the two lines that start with”+” using a mouse drag and the use Control+C to copy the text to the clipboard, then close the Model Editor.

 

15. In the Capture window, select Place>Text from the top menu and use Control+V to paste the text from the Model Editor into the text window.

 

16. Left-click to the left of the “.” in “.model” and type:

@PSpice:

then use Control+Enter to add an embedded new line, just Enter will close the text window.

 

17. Move through the text and locate the Bv= parameter, change the 8.0 value from the copied text to 6.8 and left-click>OK to add the text.

@Pspice:

.model D1N750 D(Is=880.5E-18 Rs=.25 Ikf=0 N=1 Xti=3 Eg=1.11 Cjo=175p M=.5516

+ Vj=.75 Fc=.5 Isr=1.859n Nr=2 Bv=6.8 Ibv=20.245m Nbv=1.6989

+ Ibvl=1.9556m Nbvl=14.976 Tbv1=-21.277u)

 

18. Rerun the simulation again and note that the diode now conducts between 6 and 7 volts.

This is an alternative method to add PSpice objects to the design.

 

 

End of Lab

 

 

All content Copyright 2022 Parallel Systems Ltd.