2
\$\begingroup\$

I need to have several base current values on the same graph with the output characteristics of the NPN transistor, which I set using Rb.

How can I make them on the same graph?

enter image description here

\$\endgroup\$
1
  • \$\begingroup\$ Plot the base current on the x-axis? Is that what you mean? \$\endgroup\$
    – tobalt
    Commented Nov 20, 2023 at 14:11

4 Answers 4

2
\$\begingroup\$

Use the "STEP PARAM" command:

.step param RX list A B C D E F G

If you change R6's resistance value (1000) to something like {RX} (just a name and can be anything) and add the LTSpice directive above to your simulation, the simulation will run each time with the next (A, B, C ...) RX value applied to R6. I put 7 values as example but can be 2, 3, or 10.

For example, if you want to run the simulation for R6 = 1k, 1k2, 1k3 and 1k5, add the following command:

.step param RX list 1000 1200 1300 1500

This will run the simulation for each value and plot the curves on the same waveform. For details, see here and here.

\$\endgroup\$
2
  • 1
    \$\begingroup\$ As a result, you will get different graphs for the various R values - but they will not be equally spaced (as in data books) \$\endgroup\$
    – LvW
    Commented Nov 20, 2023 at 11:55
  • \$\begingroup\$ If you get any error message, place another SPICE statement ".param RX 10k". Your .step will override it. I still haven't figured out why it's sometimes needed. \$\endgroup\$
    – winny
    Commented Nov 20, 2023 at 12:15
2
\$\begingroup\$

If you would like to have in your diagram equally spaced base currents I recommend to use not a voltage source with a resistor at the base but instead a current source which can be stepped through different values (use param feature of the program).

\$\endgroup\$
2
\$\begingroup\$

In CircuitLab you can Run a DC Sweep with a Second Parameter

schematic

simulate this circuit – Schematic created using CircuitLab

enter image description here

You can click on the simulate this circuit link above to enter the CircuitLab simulator.

\$\endgroup\$
2
\$\begingroup\$

You can .dc a current source into the base and plot the collector current:

enter image description here

\$\endgroup\$
2
  • \$\begingroup\$ I think this is the best solution, but it sounds like the questioner wants the BJT output characteristics so V1 also needs to be sweeped (and be first in the list)…and also maybe linear sweep is more appropriate?? \$\endgroup\$
    – Ste Kulov
    Commented Nov 21, 2023 at 6:57
  • 1
    \$\begingroup\$ @SteKulov Perhaps.. The question is a bit unclear. But I guess all the answers taken together provide enough suggestions to find a solution ;) \$\endgroup\$
    – tobalt
    Commented Nov 21, 2023 at 7:13

Your Answer

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

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