Help with VCO circuit simulation

Schematic Simulation (Ngspice)
1

Hello,
I am a beginner with simulation in KiCAD and NGSPICE. This is a request for help with a VCO circuit that I have imported from LTSPICE where it works, but I’d like to learn how to do the simulation in KiCAD.
I have replaced all the symbols that pointed to an LTSPICE library with generic KiCAD symbols and run an ERC check, which now passes with 2 exclusions (for 2 hierarchical labels).
I have included the text .model statements for the transistors and Zener diode in the schematic. The model for the BB105B varicap diode can’t be found, but I have included an example. This example is from a post on the LTSPICE groups.io forum.
I need to get the potentiometer working on the schematic, and I have NOT run the simulation yet. I need to take this step by step. Can someone help? Thanks.
JLH_TUNER_VCO.kicad_sch (91.1 KB)

PS I’m using KiCAD 8.05 on Windows 10. Should I be using resistor/capacitor symbols from a simulation library? If so, I will upload again later with an actual DC power supply included.

2

Please post the LTSPICE project here as a reference and post the missing potentiometer.lib used by your KiCad/ngspice circuit.

Some tentative action points:

Annotate the schematic.

Oscillators often do not start oscillation automatically. You need to add a start-up helper. For example use a pulse source as power supply and give it a single, small dip from 12 to 10 V for a few ns (see https://www.youtube.com/watch?v=dMuMCdSWAGk)

Add a load resistor to the RFOUT output (10Meg or so). Never leave a capacitor node unconnected.

Remove all .model statements from the canvas, put them into a file.

Put also a suitable potentiometer model (a subcircuit model) into this file.

There is a BB105A model available in standard.dio.

Attach all models to their symbols.

Check the diodes’ pin sequences. They seem to be inverted.

Remove the .tran statement from the canvas.

Add suitable analyses from the ‘Spice Simulator’ window (operating point and transient).

The .step command is not available in ngspice.

My tutorial at KiCad Eeschema as GUI for ngspice, tutorial for setting up the simulation or the introductory videos at https://www.youtube.com/@holger8105/videos may answer some more questions.

Often starting with some single elements (e.g. just checking out the potentiometer) is much more awarding than starting with a complete circuit.

.

3

Thanks holger,
Please find attached the LTspice file.
I will give your suggestions a try.
linearized_frequency_varicap_VCO.asc (4.5 KB)

4

Potentiometer subcircuit

* This is the potentiometer
*      _____
*  1--|_____|--2
*        |
*        3
*
.SUBCKT potentiometer 1 2 3
.param w=limit(wiper,1m,.999)
R0 1 3 {R*(1-w)}
R1 3 2 {R*(w)}
.ENDS
5

More information on this project is found here: Varactor Linearization techniques - Page 1

I have edited my post from above.

6

This does not conform to ngspice syntax, even if it may be working (see ngspice manual chapter 2.9.1, here missing ’ ’ or { } ).

And what is ‘wiper’?

You may find some potentiometer models at Simulation examples for KiCad8/Eeschema/ngspice.

Edit: Have not heard from you for some time. Attached you will find my vco project
VCO_briscoe.7z (14.6 KB).