Designing a regulated 120kV power supply

[Aerogight]

Hey everyone,

I'm looking to put together an adjustable HV supply for driving x-ray tubes, aiming for 60-120 kV at 2 mA. Right now, I've been deep into simulations but haven't started building yet.

I'm trying to implement a regulated output voltage by driving the ZVS inverter with a buck converter.

I've been tinkering with a setup where M3, D11, and L3 form a buck converter without output smoothing. This setup adjusts the input voltage of the ZVS inverter. The duty cycle at the gate of M3 flips between two fixed values depending on how the output high voltage compares to the setpoint voltage.

R6 acts as an output current limiting resistor, and G1 is there as the test load. The feedback network, made up of R8/R9, attenuates the output voltage, which is then scaled by U4 so that 150 kV is around 4.9V. U5 compares this feedback voltage to the setpoint and outputs either ~0.5V or ~4.5V. Then, this voltage is compared to a triangle wave to create the PWM signal for the buck converter.

Check out the attached pictures for the schematic and simulation results.

I've got a few questions:
- Has anyone ever put together regulated inverter and voltage-multiplier supplies or know of some good resources for more info?
- Anyone have experience regulating a ZVS inverter's output voltage using some kind of switching topology, or know where to find more info?
- Are there any glaring problems or difficulties with building this design that I might be overlooking?

[davekni]

I've been tinkering with a setup where M3, D11, and L3 form a buck converter without output smoothing.

Yes, that works well.  Great idea.  BTW, I suspect L3 could be much smaller value.

The duty cycle at the gate of M3 flips between two fixed values depending on how the output high voltage compares to the setpoint voltage.

I think it would function fine with the two fixed duty cycles being 0% and 100%.  Would simplify circuit considerably.
Either way, if the flipping frequency is within audible range, may make some audible noise (vibration of magnetic components).  May not be enough to annoying.

R6 acts as an output current limiting resistor,

Do you expect sudden discharges such as an arc from HV to ground?  Probably a good idea to include the resistor just in case, even if intended load has no sudden shorts.

The feedback network, made up of R8/R9, attenuates the output voltage, which is then scaled by U4 so that 150 kV is around 4.9V. U5 compares this feedback voltage to the setpoint and outputs either ~0.5V or ~4.5V. Then, this voltage is compared to a triangle wave to create the PWM signal for the buck converter.

If you do keep the ramp generator (PWM other than 0% and 100%), why not linear feedback (duty cycle proportional to error voltage)?

Check out the attached pictures for the schematic and simulation results.

Great simulation.  Kudos for simulating before constructing.

Are there any glaring problems or difficulties with building this design that I might be overlooking?

Just make sure V2 turns on before V6.  Then verify experimentally that power from V2 through R3 and R4 is sufficient to start low-amplitude oscillation.  If V6 turns on first or simultaneously, ZVS oscillator may not start, resulting in very high V6 current and fried FETs.
Of course, all the normal HV insulation requirements (oil immersion or whatever).

Great project!  Looking forward to seeing your progress.

[huntergroundmind]

Looks all right, but i would add an capacitor (1-10nf) parallel with R9 for protection of opamp input. You may also add transil. Voltage spike can appear with sudden output voltage change (for example in case of accidental or intended discharge), because parasitic capacitance of R8 6Gohm resistor.

I made power supply in almost the same topology, and I had no issues with it for few years.
https://highvoltageforum.net/index.php?topic=1775.msg13467#msg13467
I used TL494 for controlling buck, and modified gate drive in ZVS, and other solution of hv part but concept of topology was essentially the same.

[davekni]

Looks all right, but i would add an capacitor (1-10nf) parallel with R9 for protection of opamp input. You may also add transil. Voltage spike can appear with sudden output voltage change (for example in case of accidental or intended discharge), because parasitic capacitance of R8 6Gohm resistor.

Small-signal schottky diodes (ie. BAT54) to 0V and 5V (opamp supply rails) should suffice.  10nF might be fine, but does change control loop response, which might make it unstable depending on existing phase margin.

A couple other thoughts:
Series connection of diodes is sometimes problematic.  If diode reverse recovery times aren't well matched, one diode of the pair recovers first, then goes into avalanche breakdown (over-voltage) until other diode recovers.  I've had more trouble with strings of lower voltage (1kV) diodes than with 20kV diodes, but it is still a concern.
What type of capacitors are you using?  HV ceramic caps sometimes have extreme reduction in capacity with voltage.
Voltage multipliers like this (not intended for rapid discharge) are more efficient with larger cap values at the start and lower values at the end of the ladder.  Uniform 500pF may be fine, but lower stages will have a bit more voltage than upper stages due to cumulative current.
BTW, stray capacitance between the two sides of multiplier ladder can reduce output noticeably.  May be worth estimating capacitance and including in simulation.

[huntergroundmind]

10nF might be fine, but does change control loop response, which might make it unstable depending on existing phase margin.

It would be worth to simulate circuit with it, and play around with component values and feedback loop modifications

BTW, stray capacitance between the two sides of multiplier ladder can reduce output noticeably.  May be worth estimating capacitance and including in simulation.

Especially in case using metal tank for containing hv things in oil.
     Some thoughts about above mentioned oil type of insulation:
 If you have two points with high voltage between them close to each other add a mylar, plexiglas or other good insulating plastic barrier between them. Oil can hold off f.e. 30kV/mm depending on electrode geometry and other factors like moisture, and gas content but particles, dust, impurities like this in oil can charge and be attractedin high field region to form a bridge between points that will cause breakdown. Barrier will mitigate this bridging. If you will solder things, try to make blobs from solder on joints, eliminating sharp egdes, as it will reduce field at them. If you will mount multiplier on pcb try to cut slots between neighboring points with hv on them. By use of dremel tool for example. Filling container in vacuum to get rid of bubbles will be a good thing too. Its most important for transformer winding, as it has many of closet air pockets inside its winding. The best is to create vacuum first, and then slowly introduce oil.

[Aerogight]

Thank you for all the helpful replies.

If you do keep the ramp generator (PWM other than 0% and 100%), why not linear feedback (duty cycle proportional to error voltage)?

I tried using a linear feedback loop with a difference amplifier but couldn't get any performance that was even close to the two-point controller, Im probably just bad a tuning it. I have now simplified even further using just one comparator and 0/100% duty cycle as suggested. This does work a lot better than I expected. Very similar performance to the previous configuration.

I'm still working out a proper amount of hysteresis for the comparator. My thinking is that low hysteresis will produce better output regulation but cause more switching and power loss in M3. But the average loss in M3 was only around 3W at its worst using around 300V of hysteresis, so maybe the right amount of hysteresis is zero. Seems to work fine with zero hysteresis in the simulator, might this cause some problem in practice?

Looks all right, but i would add an capacitor (1-10nf) parallel with R9 for protection of opamp input. You may also add transil. Voltage spike can appear with sudden output voltage change (for example in case of accidental or intended discharge), because parasitic capacitance of R8 6Gohm resistor.

Adding a capacitor across R9 sounds like a good idea. I was unable to get the control loop working with 10nF (See result2.png with 60kV setpoint). Lowering it to 1nF, however, did not cause any problems. I also added protection diodes and a series resistor.

What type of capacitors are you using?  HV ceramic caps sometimes have extreme reduction in capacity with voltage.

I was thinking of using two 20kV 1nF ceramics in series because they seemed cheap and available on AliExpress. Looking into it, the capacitance change with voltage in ceramic capacitors seems a lot more significant than I had previously realized. Obviously, these Chinese caps don't have a specification on capacitance with increasing voltage or even what dielectric is used, so it seems safe to assume it's pretty bad. Even getting 500pF using 2x1nF seems very optimistic now. Increasing the multiplier capacitance would decrease output ripple and increase maximum output current, while decreasing response time and increasing cost. Are there any other considerations here? Increasing the capacitances to 1nF in the simulation significantly reduced the output ripple (See result3.png). Considering the potentially large loss of capacitance due to voltage, I might go for two 4.7nF caps in series.

Voltage multipliers like this (not intended for rapid discharge) are more efficient with larger cap values at the start and lower values at the end of the ladder.  Uniform 500pF may be fine, but lower stages will have a bit more voltage than upper stages due to cumulative current.

I tried doubling the first stage caps (C3, C5) to 2nF in the simulator and saw a little better ripple under load (See result4.png). Since doubling C3 is cheaper since it is only exposed to half the voltage, I might go for double the capacitance in the first stage.

Series connection of diodes is sometimes problematic.  If diode reverse recovery times aren't well matched, one diode of the pair recovers first, then goes into avalanche breakdown (over-voltage) until other diode recovers.  I've had more trouble with strings of lower voltage (1kV) diodes than with 20kV diodes, but it is still a concern.

Using multiple diodes in series seems like the only option if I want 120kV using a four-stage multiplier. I was unable to find any diodes with a higher voltage rating than 20kV. Does anybody know of some that arent extremly expensive?

Of course, all the normal HV insulation requirements (oil immersion or whatever).

Also, I think running the transformer + multiplier under oil is the smartest choice. Will make sure to degas it properly.

BTW, stray capacitance between the two sides of multiplier ladder can reduce output noticeably.  May be worth estimating capacitance and including in simulation.

I tried first with 2pF of capacitance parallel to the diodes and the output couldn't even reach 65kV. Estimating the capacitance as two parallel wires 5cm apart, 2cm long, and 1mm in diameter using a Relative Permittivity of 2.2 for mineral oil comes out to ~268fF. The diodes claim a Max Virtual Junction Capacitance of 1pF, but the Diode model already includes that. I decided to add another 1pF parallel to the Diodes just to be on the safe side, and it didn't cause any problems even at 125% load (See result5.png).

Yes, that works well.  Great idea.  BTW, I suspect L3 could be much smaller value.

Lowering the value of L3 did work but increased the current spikes when M3 was switching, so I decided to keep it at this value to reduce the filtering needed on the DC power supply.

Just make sure V2 turns on before V6.  Then verify experimentally that power from V2 through R3 and R4 is sufficient to start low-amplitude oscillation.  If V6 turns on first or simultaneously, ZVS oscillator may not start, resulting in very high V6 current and fried FETs.

Verified that oscillations keep going in the ZVS inverter with around 22Vp even with M3 totally off.

Attached current schematic as Schematic_LT2.png.

Thanks again for all the great help.

[davekni]

Seems to work fine with zero hysteresis in the simulator, might this cause some problem in practice?

Likely fine in practice.  Same as infinite gain linear feedback.  Resulting buck converter frequency is controlled by total delay around loop.

Looking into it, the capacitance change with voltage in ceramic capacitors seems a lot more significant than I had previously realized. Obviously, these Chinese caps don't have a specification on capacitance with increasing voltage or even what dielectric is used, so it seems safe to assume it's pretty bad.

Capacitance vs. voltage specifications are rare for almost all ceramic capacitor manufacturers.  Some of the larger well-known companies have started publishing typical curves for their parts.  Varies widely, even for the relatively cheap ones.  One supplier's parts may drop by 90%.  Another similar-looking part from another supplier may drop only 30%.  I saw one report here saying the Y5V dielectric parts they'd purchased measured as only -30% at rated voltage.
I'd suggest using 40kV caps rather than series-connected 20kV caps.  With series pairs, bleed resistors are needed across caps to keep charge equal.  Oil circulation currents can be significant, causing the imbalance.  As was suggested by huntergroundmind, insulating baffles will reduce oil circulation, but probably not enough to avoid need for resistors.
Only Y5V 40kV cap I see on EBay is 10nF:
    https://www.ebay.com/itm/204483870595
Another option to consider is film capacitors such as these polystyrene dielectric parts:
    https://www.ebay.com/itm/225014970693
I've purchased some of these before.  They should work quite well for voltage multiplier use.  Capacitance is constant over voltage.  They are not good for repeated sudden discharge such as Marx generator, but that doesn't matter for you.

Are there any other considerations here? Increasing the capacitances to 1nF in the simulation significantly reduced the output ripple (See result3.png).

Increasing early-stage capacitance will increase output voltage for a given input voltage due to lower ripple.  Will be more pronounced at high load and with high parasitic capacitance.  I think the optimum distribution for 4 stages is 4x, 3x, 2x, 1x for the stages, where x is capacitance of final stage.  Of course, no need to hit exact ratios.  Any change to increase capacitance of early stages helps.

Using multiple diodes in series seems like the only option if I want 120kV using a four-stage multiplier. I was unable to find any diodes with a higher voltage rating than 20kV. Does anybody know of some that arent extremly expensive?

May work fine.  On Ebay there are 30kV and 40kV diodes available.
    http://www.hvgtsemi.com/picv_994.html
is one 40kV part available from a couple Chinese EBay stores.  No personal experience with these parts.

I tried first with 2pF of capacitance parallel to the diodes and the output couldn't even reach 65kV. Estimating the capacitance as two parallel wires 5cm apart, 2cm long, and 1mm in diameter using a Relative Permittivity of 2.2 for mineral oil comes out to ~268fF. The diodes claim a Max Virtual Junction Capacitance of 1pF, but the Diode model already includes that. I decided to add another 1pF parallel to the Diodes just to be on the safe side, and it didn't cause any problems even at 125% load (See result5.png).

Actual stray capacitance depends on geometry.  For a crude guess, something like 0.5pF/cm (50pF/m) of multiplier length presuming in oil in a plastic (insulating) housing.  A metal housing will add capacitance.  If that ends up being closer to 2pF per diode, higher early-stage capacitance will help get voltage back up.

Good luck with your build!