Hi all,
First time posting in the forum, and a relative newbie with electronics. One of my friends is working on a mass spectrometer at school and needs help with the power supply (PS). We managed to get our hands on an older PS but it doesnt seem to work, so we are taking it apart to understand it and see if we can fabricate our own.

The circuit I have attached is what is currently in the PS, it is some type of oscillator that uses a comparator in a positive feedback configuration to generate oscillations. I was reading a bit about relaxation oscillators, which I suspect it may be, but I am a little out of my depth.

Does anyone have any ideas about the operation of this circuit? Or please let me know if I should clarify any points.

 

What more can you tell us about those inductors?

Are they wound on a form? Or are they air coils? (nothing in between)
Or are they wound on a toroidal core, or other type of core possibly made of ferrite?
If it's a transformer wound on a toroid, what color is the toroid?

What is the approximate diameter and length of each coil?

The coil with 20 turns - it's not connected to anything on either end? It would produce a pretty high voltage.

 

Yes, the "main" inductor, which has approximately 20 coils, is wound around what looks like a solid plastic cylinder approximately 1 inch in diameter.

The "red" coil, which I believe is initiating the oscillation, and is connected to the output of the comparator, is slightly thicker and is wrapped once around the "main" inductor.

Finally, the "blue" coil is wrapped twice around the "main" inductor.

And the voltage produced is supposed to be pretty high, approximately 500 volts peak to peak.

I should mention that there are actually two "main" coils, and I believe that they are configured in a way such that one is 180 degrees out of phase with the other. The "main" coils are what is connected to the output, and where we want to see a high voltage oscillation. The output consists of a quadrupole, essentially two pairs of metal bars which give off RF.

I know the explanation isnt the greatest, this very short video clip below might explain what the final output is... those 4 rods are giving off RF that trap particles depending on their masses and ionic charges... depending on frequency and amplitude of the RF you can select which charges make it to the detector at the end.
http://www.youtube.com/watch?v=445HGbcUWEw&feature=related

 

OK, I'm guessing that the 20 turn blue coil is 1.5" long. Am I at least close?

 

Yea, thats about right.

 

Well, this is what I have so far, but there are lots of unknowns.

I don't know what your reference voltage is for the center of the 20 turn coil. Before when I thought it was just one coil, and you didn't have it shown connected to anything - I was just rectifying the output using D1 and C4 in the attached schematic.

Anyway, with the guesses I've made at the coil's inductance, you probably have a frequency range of perhaps 2MHz to 7 MHz or so.

But, I don't know what you're doing with the "white" coil - it's not in the photos, I don't know what it's supposed to be connected to...

Anyway, have a look at the attached. The out1,out2 is the voltage across the 20 turn blue coil; I'm getting about 500 volts peak to peak out.

 

Wow, that's really great! Yes, the frequency we would expect would be in the 2 to 3 Mhz range so that's pretty good. I am downloading this LTSpice tool, as I would really like to simulate this circuit as well.
The "white" coil leads to another little circuit that feeds into a small multimeter-on-pcb which displays the output voltage.
The reference voltage just leads to a BNC connector on the power supply, so the user can use whatever dc offset voltage he/she wants.

I was wondering, could you sort of summarize the action of the components, like give a walkthrough of this oscillator and driver circuit so I can understand its function a little bit?

Thanks alot, you've made my day

 

You like that, eh?

OK, I've added more labels to the nodes on the simulation to make it easier to connect the signal plots to the schematic. The downside is that the schematic looks more cluttered, but it's "good" clutter.

BTW, I used the diameter of your core (reportedly 1"), length of the inductors, number of turns and plugged that into an Excel spreadsheet I wrote a few years ago to calculate the inductance of those coils.

Refer to the attached schematic and simulation.
I've "zoomed in" on just the part where the MOSFET just begins to conduct; from 40uS to 80uS. When the simulation first starts, the gate (see red plot) is at 0v. R3, the level adjust pot on the right, brings the gate voltage up until the MOSFET threshold voltage is reached (if R3 isn't set right, it won't start), and the MOSFET starts conducting via the drain, which causes current to start flowing through L3.

L3 is coupled via L2 and L4, back to L1. That signal on L1 gets coupled to +in via C3, which allows the +in (noninverting input) of the comparator to have an average voltage equal to ground (0v). This feedback to the comparator causes its' output to change states, turning off the MOSFET, causing the current through L3 to begin to decay, inducing a current in L2/L4, which is coupled back to L1, back through C3 to +in to toggle the comparator again. The process continues until something breaks or the power is turned off.

Your center-tapped 20-turn blue coil having that tune-able C6 in there is a "resonant tank" circuit; it wants to resonate as a function of the combined L of L2/L4 and the capacitance of C6. The resonant tank provides the phase shift so that the circuit will continue to oscillate.

The LT1016 is an extremely fast comparator; response time is 10nS typical.

I'm uploading the simulation .asc file, but you'll need a few more pieces before you can run it on a fresh LTSpice install. The default doesn't come with the pot or the IRF610.

 

Oops, forgot the attachments; here they are.

[eta]
Added pots.zip and irffets.zip.

Pot.zip contains two files:
pot.asy - goes in \Program Files\LTC\SwCad\lib\sym
pot.sub - goes in \Program Files\LTC\SwCad\lib\sub

irffets.zip contains two files:
Irf_nmosfets.lib goes in \Program Files\LTC\SwCad\lib\sub
IRFFETS.asy goes in \Program Files\LTC\SwCad\lib\sym\MOSFETs\N-ch

Now, your installation won't have the MOSFETs nor the N-ch directory; you'll need to make them yourself. I got tired of having so much stuff in the Misc subdirectory and started sorting things out.

 

Perfect!
I substituted the IRF610 with the generic n-channel mosfet that LTSPICE has, and the pot with two resistors, and my simulation is up and running!
I will tackle trying to find a specific model (or making one?) of the IRF610 and the pot at another time.
Thanks again for your help.

 

Ahh - thanks for those too!

 

We cross-posted - just go ahead and download the .zip files that I provided.

 

OK, with the "nmos.asy" that comes with LTSpice, you need to right-click and select a decent MOSFET model from the list. The default MOSFET is pretty wimpy.

The IRFFETS.asy that I uploaded works differently than the supplied LTSpice nmos.asy; the irf_nmosfets.lib has fets described using .subckt's instead of .model statements.

It's a different way of defining them. The .model statements for MOSFETs can actually be added to LTSpices' default library so they will come up in the list when you right-click on the nmos.asy in your schematic.

You can't add MOSFETs described as .subckt's to the LTSpice MOSFET list menu. However, I've defined IRFFETS.asy so that you can right-click on it, and then double-click on the SpiceModel line; it'll show a down-arrow on the right end of the box. Click the down-arrow, and you'll have a scrolling list of the parts in the irf_nmosfets.lib.

If you don't choose a MOSFET from that list, the default "irf_nmosfets" will cause an error when you run the simulation.

 

Well, the IRF610's gate signal really looks quite pitiful, and I discovered that it was dissipating 10 Watts of power, which is a lot. Also, the adjustment on pot R3 seems to be rather critical; if set too low, the MOSFET dissipates a LOT more power as heat, and if set too high the oscillations become erratic and then quit altogether, but there will still be current flow through L3 and the MOSFET. If R3 is set too high, the oscillator won't start.