I would like to ask if anyone can help me with the following problem. I would like to print the output characteristics of the JFET-transistor in PSpice. This is PMBFJ309, here is the datasheet. My test setup looks like this.enter image description hereenter image description hereenter image description here

And here is the output.

enter image description here

The values of Vgs goes from top to bottom, starting from 0V to -4V, the increment is 0.25V. But when you compare this result to a datasheet, it's completely different.

enter image description here

So my question is, is there any way to get the same graph as from the datasheet.

There are .model characteristics.

+             VTO = -2.3973E+000
+            BETA = 3.81468E-003
+          LAMBDA = 3.80761E-002
+              RD = 2.33008E+000
+              RS = 2.33008E+000
+              IS = 3.02702E-016
+            CGS  = 6.50000E-012
+            CGD  = 5.70000E-012
+              PB = 6.83767E-001
+              FC = 5.00000E-001

Thank you in advance.

  • \$\begingroup\$ Also, the chart you shared does not come from the datasheet you linked. \$V_{GS}\$ for an n-channel JFET should be negative, and it is shown as negative in the linked datasheet. The chart you used probably comes from a p-channel JFET's datasheet. \$\endgroup\$
    – The Photon
    May 21, 2021 at 15:09
  • \$\begingroup\$ It comes from the same datasheet -- see the OP's link to it. For some reason the minus signs are not showing but you can tell there is space for them. \$\endgroup\$
    – ErikR
    May 21, 2021 at 15:13

2 Answers 2


You can try to adjust various parameters in the .model, but in the end you have to remember that a SPICE element is only an approximation of the real-life counterpart. You can clearly see that the saturation region is a straight line in the simulation, and the knee points are rather abrupt. Getting a perfect match with the datasheet is quite impossible. Besides, the JFETs are known to have very large variations even compared to their own datasheets. It's one of the reasons you don't see constant current generators with JFETs everyhere. BTW, you used 0...-4 for the Vgs, but in the datasheet it's shown as 0...-1. For this case, you could try adjusting the beta parameter. In LTspice, beta=3.5m seems to come closer to what's shown (the default value is 4.682m).

  • \$\begingroup\$ Where could I find the .model properties of the transistor in PSpice? \$\endgroup\$ May 21, 2021 at 15:25
  • \$\begingroup\$ @TomášMacháček It looks like you already found the .model definition, so you could try to tinker with the variables, see if you will get a better match. \$\endgroup\$ May 21, 2021 at 17:23

If you want to get just the graphs for those specific voltages try using the .STEP directive, e.g.:

.STEP VGG 0V -.25V -.5V -.75V -1V

  • \$\begingroup\$ This doesn't explain why the datasheet shows ~16 mA current at 0 V Vgs while the simulation shows ~30 mA. \$\endgroup\$
    – The Photon
    May 21, 2021 at 15:07
  • \$\begingroup\$ @ThePhoton - There is a large spread - the max is about 30mA for IDSS. \$\endgroup\$ May 21, 2021 at 16:09

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge that you have read and understand our privacy policy and code of conduct.

Not the answer you're looking for? Browse other questions tagged or ask your own question.