This thread will show some LTspice techniques I use for simulating circuits.
I started from @LarryDee 's circuit here: https://www.theradioboard.org/forum/main/comment/6fec3991-140b-4f9f-b18f-d437c65622ab?postId=6268d23aea895900167700d1
I modified this a bit as follows.
The main changes I made were:
Removed units suffixes on all component values. For example, you specify an inductor's value as "10u", and LTspice knows this means 10uH, so you don't have to specify the "H" (Henries) unit.
Added the potentiometer component. To use this, copy the attached files "potentiometer.sub" and "potentiometer 2.asy" into the same folder as the main simulation file "larry-regen-with-preamp.asc".
Added some ballpark guesses of resistance to simulate resistive losses in the choke L1 and in the tank inductor L2.
Added a pulse voltage source V2, which provides a small kick of voltage at the start of the simulation to encourage oscillation of the oscillator circuit.
Added a .tran statement to run a "transient" (time-domain) simulation, to examine the oscillator waveforms and if oscillation is possible. You can also run .ac (frequency-domain) simulations, for example to check the bandwidth of tuned circuits -- including checking the bandwidth of a regenerated tank. That might be a topic for a future article.
The next video shows a typical simulation session inside of LTspice. Unfortunately, my video capture software captured only the main LTspice window, and not any popup windows. During the video, I right click on some components, which brings up a popup window (not visible in the video) where you can alter the component value. After closing the popup window (not visible in the video), the changed values are then shown in the main schematic (which is visible in the video).
The goal of this simulation session is to check if the circuit oscillates, and to alter the circuit parameters until it oscillates.
Here's what's happening in the video:
Time 0:00: file is opened.
Time 0:04: "Run" button is clicked to start simulation. The simulation result window opens. Windows are rearranged to be tiled vertically, with schematic on the left and results on the right.
Time 0:11: Mouse is clicked on the "tank" label at the top of the L2 tank inductor, to check the voltage at the top of the tank. The simulation window shows a decaying voltage, indicating the circuit is not oscillating.
Time 0:34: Based on trial and error, I discovered that I had to increase C5 and C6 to 4700 pF for oscillation to occur.
Time 0:38: Simulation is re-run with 4700 pF capacitors. Results window shows an exponentially-increasing waveform until amplitude limiting occurs. In other words, we have oscillation. There is some brief and strange secondary oscillation at a different frequency from 0-80 uS, which must be caused by some other secondary resonance, almost certainly due to the choke L1. Understanding this secondary oscillation requires correctly characterising the choke L1, including its equivalent series resistance (ESR) and self-resonant frequency (SRF). In this simulation, we just use R4 to damp the choke L1, to represent some hopefully plausible value of ESR.
Time 1:12: We zoom in to the waveforms and check that they look reasonable. They are smooth sinusoidal curves, so this is reasonable. To get this result, it is important to turn off waveform compression (by unchecking all three compression options) in LTspice, in the settings window (accessible via the hammer icon).
Time 1:31: We zoom into a subset of the results starting from 690 uS up until 990 uS, therefore omitting the initial part of the data (from 0-80 uS) that contained the unwanted secondary oscillation. We right-click on the results window and select the View > FFT menu (not visible in the video), and generate an FFT based only on the currently-visible subset of the data.
Time 1:51: The FFT window is displayed, showing the oscillation frequency, about 2.625 MHz. Clicking the window and dragging the cursor shows a popup window (not visible in the video) with the measured frequency at the cursor. Greater accuracy can be had by running the simulation with smaller timesteps, and by running the FFT with more points.
Time 2:20: The pot wiper is increased to 1.0, increasing the source resistance. Re-running the simulation shows that the tank energy dies down over time. We are now below the oscillation threshold.
Time 2:42-5:55: The pot wiper is gradually adjusted to find the value just below oscillation, re-running the simulation after each change. A value of 0.22 is found to be below the oscillation threshold, while 0.21 is found to be above the oscillation threshold. Therefore, with the pot wiper at 0.22 (22% of its travel) we are very near, but still below, the oscillation threshold. This adjustment was done in minimum increments of 1%, which for a 270-degree potentiometer assumes that the pot can be physically manipulated in increments of 2.7 degrees, which is physically plausible. If you have a ten-turn pot, or a large knob on the pot, you might want to adjust the simulated wiper value in smaller increments like 0.001, which will allow you to bring the simulation very close to the oscillation threshold, and allow you to achieve very high tank Q values.
Simulation files are attached as text files. To use these files, you should rename them as follows:
The last filename has a space between the word "potentiometer" and the numeral "2".
Put all files in the same directory, and then you should be able to open the file larry-regen-with-preamp.asc in LTspice.