Why do some JFETs oscillate and others don't?

Question

Below is a simple JFET Clapp Oscillator, which works quite well. It starts oscillating at around 40us and gets into clean, stable oscillation by 100us:

When I replace the J309 JFET with a more modern MMBF4416A, which says "Designed for RF Amplifiers", the oscillation stops completely, and I get close to 0 gate voltage. Why?

I looked at several different JFET data sheets and have had trouble deciphering which characteristics are needed for a (good, clean, stable) oscillator - or for any oscillation at all.

Which characteristics of the JFET enable it to function as an oscillator in this case? What should I look for when selecting a JFET in my circuit? Is there a modern SMD JFET that will work as well (or better) than a J309?

---

Update

Thank you for the responses. To answer the questions that were raised:

1. This is an LTspice simulation, with JFET models coming from http://bordodynov.ltwiki.org/
2. My question is: What parameters of the JFET on the datasheet are relevant to making a good oscillator? Looking at different datasheets, what should I look for when building an oscillator? What characteristics cause one to oscillate well and one not to?

Answer 1

models and datasheets

The MMBF4416A datasheet you provided is terrible. There are no charts given. Nothing to examine. However, my eye is drawn to this:

If you now set this up in LTspice where \$V_{_\text{CC}}=15\:\text{V}\$ (per datasheet spec):

Note that I downloaded the PSpice model from OnSemi and included its text, as well, adding an X to the model name. This demonstrates that the model from OnSemi for PSpice appears to be the same as the model included in the LTspice library of parts.

Also note that the value of about \$14\:\mu\text{A}\$ is nothing like what the datasheet says.

It turns out that the 2N4416/2N4416A/SST4416 is very much better and does include curves. First, let's look at the \$I_{_\text{DSS}}\$ value:

That matches up with the OnSemi datasheet.

And here's the chart curve of interest:

This definitely disagrees with the results in LTspice using both the internal model as well as the downloaded PSpice model I got from OnSemi.

So this is a problem. If the models are accurate (and the only way to tell is to buy some parts and measure them) then this device won't be useful. It's \$\beta\$ value is simply way too small. If the models are not accurate, then perhaps the device will work fine (you still need to buy some and verify) and somehow a very bad Spice model has been propagated (cargo cult-like.)

I don't know the reality here. But I can see problems, already. The Spice models won't support the circuit. But the real device may do fine. I just can't tell without having some to test.

simulating your circuit

The first thing I need to do is to figure out what to expect from the circuit, by theory. Here's what I find:

solve(Eq(1/I/omega/470e-12 + 1/I/omega/470e-12 + 1/I/omega/(47e-12+18.5e-12)+I*omega*10e-6,0),omega)
[-44184267.2469006, 44184267.2469006]
(44184267.2469006/2/pi).n()
7032144.53923756

So I'm expecting to see about \$7\:\text{MHz}\$ as the oscillation frequency.

The impedance, looking into the \$C_1\$/\$C_2\$ node of your circuit is:

Freq or omega (add 'j'): 7e6
470pF|(470pF+47pF+18.5pF+10uH)
-j46.6668025, 46.6668025 < -90

Which tells me that the impedance of the remaining inductor (\$L_1\$ in your circuit) needs to be about \$10\times\$ that much, which at this frequency means \$10\:\mu\text{H}\$. That's quite a bit smaller than what you used. By a rule of thumb that also means \$R_1=470\:\Omega\$. (You aren't far from it, there.)

I will use my values for your \$R_1\$ and \$L_1\$, not your values. I'm also adding a semi-necessary diode (and eliminating your grid/gate leak self-bias resistor):

The indicated \$f\approx 6.95\:\text{MHz}\$ is very close to my calculations above. I'm calling it good.

Now, I'll apply the PSpice model, which we already know won't work well. However, since I already know that the \$\beta\$ is way way too low, the impedance of \$L_1\$ (your circuit, not mine) and \$R_1\$ does need to be increased a lot. I'll multiply both of them by about 50 to get the inductor value back to where you had it. But your \$R_1\$ will be higher than you used:

The frequency is still about the same. But the signal's peak-to-peak is almost non-existent. The PSpice model's \$\beta\$ is just pathetic.

I'll change that, now, while returning your \$R_1\$ and \$L_1\$ back to the values I calculated earlier:

So, it is the \$\beta\$ parameter that is the problem. And as I wrote before, without parts in hand I cannot tell you much about the reality of using that part. I don't know whether the models provided are wrong or the datasheet is wrong. (Probably the model. But I don't know.)

Answer 2

Made with microcap v12, interactive mode "Stability" analysis.

Just change your C1. It will start to oscillate within 250 us ...

Tried until 420 MHz.

Answer 3

JFETs have very spready DC characteristics .I have not used them in any high volume products due to fear of a production disaster. Sure people do and seem to get away with it .Try reducing R1 to get more gain so it will start.I always place a reverse 1n4148 gate to ground to help stabilise amplitude on low volume car radio local oscillator because you want good starting but not too much overall gain because this will distort the output waveform and give bad stability .The diode allows more room for spreads in gain.