Gap, Creepage and Clearance for HF HV

oops..Need to rewrite..

Aside from gap width, voltage and gas mix, does breakdown in air also depend on frequency?

D from BC

Hello D from BC,

There are three things; Creepage, corona and distance through air. According to "Reference data for Engineers" (Newnes):

Break down voltage for uniform E-field in air at sea level and room temperature is 75kVp/inch, 30kVp/cm. Valid up to 300 MHz, use a safety margin.

So you should evaluate the worst-case field strength for your application. Highest field strength will probably occur at an air/ insulation transition on thin wire.

Corona discharge When corona discharge occurs at an air/insulation transition, frequency comes in play. High frequency will give higher corona effect and erosion of the insulation will go faster. When the insulation finally breaks down (under emission of material), the eroded material helps to lower the air breakdown voltage significantly. A nice smooth sounding arc will occur with nice smoke and color effects (I played many times with that [with plenty of water nearby in case of fire]).

Also with high frequency, the zero voltage transition is too short to extinguish the arc.

I use an RF receiver with high pass filter to search for corona discharge in HV circuits.

Creepage is another thing. An arc is formed by miniscule discharges over a (polluted) surface. Here evaporated material also helps the ionization process to establish and maintain the arc. 300Vp requires about 1.1mm insulation between traces on an uncoated PCB (functional insulation, not safety insulation).

When breakdown of a barrier involves a safety hazard, there are minimum requirements for distance trough air (clearance) and distance over surface (creepage). Here transient over voltage must also be taken into account (4kV for 230V mains building installation equipment) and the type of insulation system (basic or double/ reinforced). To read more for free, go to

Go to ECMA287 it is like IEC950, but then for free.

300V/ 700 kHz does not arc that fast (I used same frequency in a power circuit). Are you sure that there are no higher transient voltages present in that waveform? Did you clean the board after soldering, etc?

Best regards,

Wim PA3DJS

How long did it run before the failure mode occurred?

If it ran for a long period, then the solution is to conformally coat the assembly (while it is new, of course).

Air ionization will eventually lead to carbon trail forming.

This is one reason why the long ceramic insulators on high tension lines need to be changed out periodically. They eventually form carbon trails on their surface, and all the creepage distance in the world wont stop that resistor from conducting.

I did a speed read of that and the only mention of frequency was that corona can generate an audible or radio frequency noise. The arcing I witnessed on my PCB did "sing" for about 2 seconds before parts started blowing. My arcing HF smps design probably got so chaotic that it managed to produce spectrum in the audio range. D from BC

As the frequency rises the needed gap also increases. A sharp edge and RF frequencies are a bad combination. Both make it easier for the electrons in the metal to get into the air and start trouble.

The corona effect creates ions and is bad in two ways. Firstly, these ions can be the ones that start the spark. Secondly, these ions are very reactive things and they eat the epoxy of the PCB. They slowly turn the PCB into something that is conductive.

Since this is a new design you are working on, there could be another problem. Did you forget to wash and dry the PCB before you applied power? The drying step is very important. It is hard to wait while you latest invention dries in the hot box but wait you must.

300 volts peak isn't really "high voltage" and is unlikely to cause corona or arcing in air. I suppose it's possible, but just barely, that dielectric losses heated up a spot on the pcb, and cooked the epoxy to failure.

But likely something else went wrong.

What sorts of clearances do you have in the regions where you have the

300 volts? Post a pic if you can; schematic too.

John

Errr...noooo... I didn't clean the board...Doh! :( I used a flux pen on the pcb for better soldering and then used flux core solder. There's visible rosin between the HV and gnd traces spaced 15mil to

20mil apart..

Your post should help. Thanks. D from BC

1 to 2 seconds. Probably closer to 1 second. The arc started when I switched on the power.

It's probably a combo of traces too close together with flux on the pcb.

But from I've read so far, it looks like I have to do my trace spacing not only to prevent arcing but also to prevent eventual arcing.

More complications for the pcb layout. Arrrghhh :( D from BC

Our multiplier stages had either fully buried traces where the only thing exposed was the via/component mount hole, or they were all on one side, and the assembly was vacuum potted.

You may want to bake your assembly at approx 60C for an hour, and even place it under a vacuum for about ten minutes. PCB material is hygroscopic (soaks up water). Both FR4 and G10 are hygroscopic.

The way we cleaned our boards, we could detect more moisture trapped in a masked PCB than in the unmasked multiplier areas of our designs. The unmasked area was also more receptive of the potting primer, and thereby caused less potting detachment issues. Definitely the way to go with potted HV assemblies. We even grit blasted the glassy finish off our dipped capacitors to get superior potting adhesion. One fingerprint blows the whole multiplier though.

You should watch out for sharp corners in your traces too. We even used arced (sp) traces when it yielded a benefit.

Rosin, RMA, Aqueous?

Line-op stuff I see often has wide spacing (>0.2", I guess) and notches punched out of the board to eliminate creepage as such entirely. At least, the better stuff.

True, you may not have the luxury of that much space.

Tim

-- Deep Fryer: A very philosophical monk. Website @

Ohhh..there's ooddles of flux I didn't clean off.. oops... And I have to review the trace-trace separation with respect to frequency, corona and voltage. All new stuff for me. The posts are helping.

Now I'm wondering about something...

I'm using a power mosfet in a TO220 package. It's got a 600Vds rating. (IIRC ..That's a DC spec.) Could there be a frequency restriction due to the TO220 lead spacing? In other words.. Could a mosfet be driven at such a frequency and voltage to get TO220 package lead to lead arcing? Even worse... I make fat PCB pads for TO220 leads. Now there's even less spacing.

D from BC

I've seen (and have, I think) some TO-220's rated to 1500Vcbo. Most such devices extend epoxy around the center pin (collector), but still. Makes ya wonder...

(On the other hand, I have some deflection transistors that are TO-247 sized, ISO-TO-220 shaped (i.e. covered in black plastic), and the center pin has extended plastic. Now that I would trust. Uh, 2SC5041 or something like that.)

Tim

-- Deep Fryer: A very philosophical monk. Website @

It's quite common in HV PCB designs to route out a slot in your PCB to separate high voltage traces. Also commonly used for low leakages designs too.

Dave.

Well, don't make fat pads! You can bend the leads before mounting to give you a staggered pin spacing which increases the pin spacing a lot.

Dave.

Are you saying that it's possible for the epoxy between traces (top side trace to top side trace or top trace to bottom ground plane) to get fried like too much current through a lossy capacitor? Cool! A possible headache but still cool. :) But dunno yet if that's the case.. Working on it..

I have the 300Vpk at 700Khz between two top traces separated by 20mil. Beneath these traces is the ground plane separated by 40mil of FR4. I've yet to do the math if this is ok at this voltage and frequency.

I'll try to prep a pcb layout and schematic for my website. Both need some spiffing up first for presentation for less confusion and quicker viewing.. I'll let you know when it's uploaded and provide a link. D from BC

Kester flux pen # 951 low solids no clean and then I used Multicore solder which I believe contains rosin.

I haven't looked it up yet but I bet the breakdown voltage of this flux combo is probably much less than air for a 20mil separation between two top pcb traces with a potential diff of 300vpeak.. And I'm thinking about the frequency and square waveform making it easier to arc through the flux too.. D from BC

So that's what that's for... I saw that many years ago on a pcb..I don't recall where the pcb came from (a tv?) but I do remember those mystery slots. Mystery no more. :) D from BC