PCB high-voltage meltdown

[Winfield Hill]

After experiencing a PCB high-voltage meltdown, I am
driven to ask for advice from experienced folks here
on s.e.d. s/n 19 of my new +/-1100-volt amplifier
suffered a severe insulation breakdown between two
BNC output-connector-mounting holes and pads, spaced
only 0.10-inch apart. A carbon path is now clearly
visible on the bottom of the PCB. The HV breakdown
is so severe that after being exposed to 500V, 3mA
pumped into the output can't raise the voltage more
than 100 volts (implying a 33k short).

It's possible the carbon pathway first began forming
in an uncleaned solder-flux region between the two
pads. The carbonization eats well into the interior
of the PCB, obscuring evidence of the initial path.

The guilty pc-mounting BNC connector (not my choice,
BTW), with its two holes and pads, is not being used.
The high-voltage hole is needed for an output wire.
The guilty ground hole 0.1" next to it was also used,
but the ground connection can be made elsewhere.

My solution for now is to completely drill out the
dangerous ground hole, leaving only surface conduction
to a ground plane 0.1" away. (The rest of the board
has healthy clearances for the up to 2.5kV voltages
seen, but sadly I didn't give the PCB design of the
output-connector region, with its 1.1kV potential,
the same attention.)

I wonder if we can count on about 0.1" of PCB
insulation to maintain a low-leakage (over 500M)
over time. Perhaps we should spray or coat this
region of the PCB with a conformal-coating sealant,
after a careful cleaning.

We have made 160 of these rather complex amplifiers,
and now we're seeking advice for a robust, but we
hope not too painful, solution to this problem.

 

[Phil Allison]

"Winfield Hill"

After experiencing a PCB high-voltage meltdown, I am
driven to ask for advice from experienced folks here
on s.e.d. s/n 19 of my new +/-1100-volt amplifier
suffered a severe insulation breakdown between two
BNC output-connector-mounting holes and pads, spaced
only 0.10-inch apart. A carbon path is now clearly
visible on the bottom of the PCB. The HV breakdown
is so severe that after being exposed to 500V, 3mA
pumped into the output can't raise the voltage more
than 100 volts (implying a 33k short).

It's possible the carbon pathway first began forming
in an uncleaned solder-flux region between the two
pads. The carbonization eats well into the interior
of the PCB, obscuring evidence of the initial path.

The guilty pc-mounting BNC connector (not my choice,
BTW), with its two holes and pads, is not being used.
The high-voltage hole is needed for an output wire.
The guilty ground hole 0.1" next to it was also used,
but the ground connection can be made elsewhere.

My solution for now is to completely drill out the
dangerous ground hole, leaving only surface conduction
to a ground plane 0.1" away. (The rest of the board
has healthy clearances for the up to 2.5kV voltages
seen, but sadly I didn't give the PCB design of the
output-connector region, with its 1.1kV potential,
the same attention.)

I wonder if we can count on about 0.1" of PCB
insulation to maintain a low-leakage (over 500M)
over time. Perhaps we should spray or coat this
region of the PCB with a conformal-coating sealant,
after a careful cleaning.

We have made 160 of these rather complex amplifiers,
and now we're seeking advice for a robust, but we
hope not too painful, solution to this problem.

** Suround the BNC with a ring of Ivory.

I'm sure you have just loads of that stuff where you hang out.

With all the other bats.





....... Phil

 

[Michael A. Terrell]

After experiencing a PCB high-voltage meltdown, I am
driven to ask for advice from experienced folks here
on s.e.d. s/n 19 of my new +/-1100-volt amplifier
suffered a severe insulation breakdown between two
BNC output-connector-mounting holes and pads, spaced
only 0.10-inch apart. A carbon path is now clearly
visible on the bottom of the PCB. The HV breakdown
is so severe that after being exposed to 500V, 3mA
pumped into the output can't raise the voltage more
than 100 volts (implying a 33k short).

It's possible the carbon pathway first began forming
in an uncleaned solder-flux region between the two
pads. The carbonization eats well into the interior
of the PCB, obscuring evidence of the initial path.

The guilty pc-mounting BNC connector (not my choice,
BTW), with its two holes and pads, is not being used.
The high-voltage hole is needed for an output wire.
The guilty ground hole 0.1" next to it was also used,
but the ground connection can be made elsewhere.

My solution for now is to completely drill out the
dangerous ground hole, leaving only surface conduction
to a ground plane 0.1" away. (The rest of the board
has healthy clearances for the up to 2.5kV voltages
seen, but sadly I didn't give the PCB design of the
output-connector region, with its 1.1kV potential,
the same attention.)

I wonder if we can count on about 0.1" of PCB
insulation to maintain a low-leakage (over 500M)
over time. Perhaps we should spray or coat this
region of the PCB with a conformal-coating sealant,
after a careful cleaning.

We have made 160 of these rather complex amplifiers,
and now we're seeking advice for a robust, but we
hope not too painful, solution to this problem.

Can you saw a slit in the board to remove the chance of carbon
tracking? That is done a lot in the HV circuits on TVs and video
monitors.


--
Service to my country? Been there, Done that, and I've got my DD214 to
prove it.
Member of DAV #85.

Michael A. Terrell
Central Florida

 

[J.Stockton]

After experiencing a PCB high-voltage meltdown, I am
driven to ask for advice from experienced folks here
on s.e.d. s/n 19 of my new +/-1100-volt amplifier
suffered a severe insulation breakdown between two
BNC output-connector-mounting holes and pads, spaced
only 0.10-inch apart. A carbon path is now clearly
visible on the bottom of the PCB. The HV breakdown
is so severe that after being exposed to 500V, 3mA
pumped into the output can't raise the voltage more
than 100 volts (implying a 33k short).

It's possible the carbon pathway first began forming
in an uncleaned solder-flux region between the two
pads. The carbonization eats well into the interior
of the PCB, obscuring evidence of the initial path.

The guilty pc-mounting BNC connector (not my choice,
BTW), with its two holes and pads, is not being used.
The high-voltage hole is needed for an output wire.
The guilty ground hole 0.1" next to it was also used,
but the ground connection can be made elsewhere.

My solution for now is to completely drill out the
dangerous ground hole, leaving only surface conduction
to a ground plane 0.1" away. (The rest of the board
has healthy clearances for the up to 2.5kV voltages
seen, but sadly I didn't give the PCB design of the
output-connector region, with its 1.1kV potential,
the same attention.)

I wonder if we can count on about 0.1" of PCB
insulation to maintain a low-leakage (over 500M)
over time. Perhaps we should spray or coat this
region of the PCB with a conformal-coating sealant,
after a careful cleaning.

We have made 160 of these rather complex amplifiers,
and now we're seeking advice for a robust, but we
hope not too painful, solution to this problem.

Win
You didn't say what the pcb material was so I am going to assume FR4. If you
clean the boards thoroughly and then bake them out to remove any water that
was absorbed, they will be pretty high resistance. Then conformally coat
with a silicon based coating and bake out. This should eliminate the
problem. Cutting the slit in the board like Michael recommended is also a
good idea. I have had problems with leakeage in FR4 boards and it gets much
worse with increasing temperature. The conformal coating seems to help.
Good luck
Jim Stockton

 

[Eeyore]

After experiencing a PCB high-voltage meltdown, I am
driven to ask for advice from experienced folks here
on s.e.d. s/n 19 of my new +/-1100-volt amplifier
suffered a severe insulation breakdown between two
BNC output-connector-mounting holes and pads, spaced
only 0.10-inch apart.

IEC 60065 says 4.73mm for 2200V btw.

Graham

 

[Eeyore]

but sadly I didn't give the PCB design of the
output-connector region, with its 1.1kV potential,
the same attention.)

Is it single ended or differential ?

~ 2.5mm is supposed to be OK for 1kV ( but it is the *minimum* ).

Graham

 

[Homer J Simpson]

After experiencing a PCB high-voltage meltdown, I am
driven to ask for advice from experienced folks here
on s.e.d. s/n 19 of my new +/-1100-volt amplifier
suffered a severe insulation breakdown between two
BNC output-connector-mounting holes and pads, spaced
only 0.10-inch apart. A carbon path is now clearly
visible on the bottom of the PCB. The HV breakdown
is so severe that after being exposed to 500V, 3mA
pumped into the output can't raise the voltage more
than 100 volts (implying a 33k short).

Without seeing a photo of the section it's a tad hard to make concrete
suggestions, but I would cut away the bad bits and try to use ceramic
insulators/standoffs for repair.

 

[Jon Elson]

After experiencing a PCB high-voltage meltdown, I am
driven to ask for advice from experienced folks here
on s.e.d. s/n 19 of my new +/-1100-volt amplifier
suffered a severe insulation breakdown between two
BNC output-connector-mounting holes and pads, spaced
only 0.10-inch apart.

You're running 1100 V on a BNC? You can get away with this
sometimes, but you are really pushing things. If the connector
solder pins are .1" apart, my only surprise is that SN 1-18 didn't
suffer the same fate.

A carbon path is now clearly
visible on the bottom of the PCB. The HV breakdown
is so severe that after being exposed to 500V, 3mA
pumped into the output can't raise the voltage more
than 100 volts (implying a 33k short).

It's possible the carbon pathway first began forming
in an uncleaned solder-flux region between the two
pads. The carbonization eats well into the interior
of the PCB, obscuring evidence of the initial path.

You didn't even CLEAN the flux off of an 1100 V small-clearance
circuit? It is possible the PCB itself had enough conductivity due
to contamination in it, to break down eventually. But, leave
flux on the board and you really invite trouble. And, once it
starts, there may be no way to repair it without a Dremel tool.

The guilty pc-mounting BNC connector (not my choice,
BTW), with its two holes and pads, is not being used.
The high-voltage hole is needed for an output wire.
The guilty ground hole 0.1" next to it was also used,
but the ground connection can be made elsewhere.

My solution for now is to completely drill out the
dangerous ground hole, leaving only surface conduction
to a ground plane 0.1" away. (The rest of the board
has healthy clearances for the up to 2.5kV voltages
seen, but sadly I didn't give the PCB design of the
output-connector region, with its 1.1kV potential,
the same attention.)

I wonder if we can count on about 0.1" of PCB
insulation to maintain a low-leakage (over 500M)
over time. Perhaps we should spray or coat this
region of the PCB with a conformal-coating sealant,
after a careful cleaning.

Yes, I think that would be advisable. Look at the sweep transistors
on computer monitors and such. They often make slots in the PCB
between the drain or collector trace and the other transistor leads.
The slot is a heck of a lot better insulator than even a clean PCB.
If you still have 1 KV across .1" of board, then the coating sounds
like a must. If you can remove the grounded area, then maybe just
that and a thorough cleaning will be sufficient.

I've seen PCB fires in the last vacuum tube gear made with PC
boards with plate supplies in the 400 V range. These were in
commercial audio gear. On the other hand, I guess PC board materials
are probably a lot better today.

We have made 160 of these rather complex amplifiers,
and now we're seeking advice for a robust, but we
hope not too painful, solution to this problem.

I have made small production runs of several photomultiplier tube
bases (voltage dividers) in the past, and some of these run 1000 to
1800 V or so. I've never had a fire or breakdown in them. We use
SHV connectors for the bias supply to avoid this sort of disaster
when going over 1 KV. (We also used the .156" Molex connectors
and skipped a pin between gnd and HV. This worked quite well,
even in VACUUM!)

Jon

 

[Ancient_Hacker]

I suppose in a perfect world, with a clean, washed board, low humidity,
no dust, low frequencies, and perfect DC balance you can run 10kv per
inch. But if it gets muggy, and a little dust gets attracted, or
there's some flux and a DC offset, things can get ugly. But you
already know that.

The grinding wheel sounds like a good solution. Air is a cheap and
relatively good insulator.

 

[Winfield Hill]

Jon Elson wrote...

You didn't even CLEAN the flux off of an 1100 V
small-clearance circuit?

Jon, Jon, Jon, we're talking about students here!
You don't think I'm going to build 160 amplifiers,
with over 150 parts each, myself, do you?

 

[PeteS]

Winfield Hill wrote:




Is it single ended or differential ?

~ 2.5mm is supposed to be OK for 1kV ( but it is the *minimum* ).

Graham

I would be a little concerned at 0.1 inch at over 1kV. Is there any way
of cutting back the ground plane at that zone, Win?

As I recall, the breakdown of air at 20% RH is ~10kV/inch. ( I fully
expect contrary responses

At that, it makes 0.1" good up to 1kV in free air. So a coating might
well help. FR4 is much better - about 50kV per inch or more, so a
conformally coated board (with suitable breakdown characteristics of the
conformal coat) might very well solve the issue.

Apart from that, good advice from many - I had 'holes in boards' from
insufficiently cleaned units that were then conformally coated (sealing
in the contaminants). As others, I would suggest thorough cleaning and a
silicone based conformal coat to prevent other issues (apart from the
distance issue above).


Cheers

PeteS

 

[Martine Riddle]

After experiencing a PCB high-voltage meltdown, I am
driven to ask for advice from experienced folks here
on s.e.d. s/n 19 of my new +/-1100-volt amplifier
suffered a severe insulation breakdown between two
BNC output-connector-mounting holes and pads, spaced
only 0.10-inch apart. A carbon path is now clearly
visible on the bottom of the PCB. The HV breakdown
is so severe that after being exposed to 500V, 3mA
pumped into the output can't raise the voltage more
than 100 volts (implying a 33k short).

It's possible the carbon pathway first began forming
in an uncleaned solder-flux region between the two
pads. The carbonization eats well into the interior
of the PCB, obscuring evidence of the initial path.

The guilty pc-mounting BNC connector (not my choice,
BTW), with its two holes and pads, is not being used.
The high-voltage hole is needed for an output wire.
The guilty ground hole 0.1" next to it was also used,
but the ground connection can be made elsewhere.

My solution for now is to completely drill out the
dangerous ground hole, leaving only surface conduction
to a ground plane 0.1" away. (The rest of the board
has healthy clearances for the up to 2.5kV voltages
seen, but sadly I didn't give the PCB design of the
output-connector region, with its 1.1kV potential,
the same attention.)

I wonder if we can count on about 0.1" of PCB
insulation to maintain a low-leakage (over 500M)
over time. Perhaps we should spray or coat this
region of the PCB with a conformal-coating sealant,
after a careful cleaning.

We have made 160 of these rather complex amplifiers,
and now we're seeking advice for a robust, but we
hope not too painful, solution to this problem.

I thought BNC was only good for ~600v. I've seen PL259's used beyond that.

Cheers

 

[Winfield Hill]

Martine Riddle wrote...

I thought BNC was only good for ~600v.

Yes. Although I can think of cases where 1, 1.5
or even 2kV uses have worked for years on end.
But then there's the spectacular failure at 1kV,
or less. So, yes, 600 volts sounds about right.

I've seen PL259's used beyond that.

Indeed, with substantial modifications, all the
way to 15kV. I've found there are two issues,
1) basic coax-cable dielectric HV withstanding
capabilities, which are dependent on pinholes
and the like, and 2) issues having to do with
the outer woven-shield connector termination of
the coax, creating small, high, local electric
fields that can disastrously break down at 1/3
to 1/10 of the coax dielectric-breakdown limit.

Well-designed high-voltage connectors deal with
the shield termination in an innocuous fashion.

 

[Eeyore]

I thought BNC was only good for ~600v. I've seen PL259's used beyond that.

Sounds far more suitable to me.

Graham

 

[Robert Latest]

On 18 Oct 2006 14:28:53 -0700,

Jon, Jon, Jon, we're talking about students here!
You don't think I'm going to build 160 amplifiers,
with over 150 parts each, myself, do you?

What do you need 160 for these beasts for?

Just curious.
robert

 

[Robert Baer]

After experiencing a PCB high-voltage meltdown, I am
driven to ask for advice from experienced folks here
on s.e.d. s/n 19 of my new +/-1100-volt amplifier
suffered a severe insulation breakdown between two
BNC output-connector-mounting holes and pads, spaced
only 0.10-inch apart. A carbon path is now clearly
visible on the bottom of the PCB. The HV breakdown
is so severe that after being exposed to 500V, 3mA
pumped into the output can't raise the voltage more
than 100 volts (implying a 33k short).

It's possible the carbon pathway first began forming
in an uncleaned solder-flux region between the two
pads. The carbonization eats well into the interior
of the PCB, obscuring evidence of the initial path.

The guilty pc-mounting BNC connector (not my choice,
BTW), with its two holes and pads, is not being used.
The high-voltage hole is needed for an output wire.
The guilty ground hole 0.1" next to it was also used,
but the ground connection can be made elsewhere.

My solution for now is to completely drill out the
dangerous ground hole, leaving only surface conduction
to a ground plane 0.1" away. (The rest of the board
has healthy clearances for the up to 2.5kV voltages
seen, but sadly I didn't give the PCB design of the
output-connector region, with its 1.1kV potential,
the same attention.)

I wonder if we can count on about 0.1" of PCB
insulation to maintain a low-leakage (over 500M)
over time. Perhaps we should spray or coat this
region of the PCB with a conformal-coating sealant,
after a careful cleaning.

We have made 160 of these rather complex amplifiers,
and now we're seeking advice for a robust, but we
hope not too painful, solution to this problem.

*If* the board was cleaned, 25 mils is sufficent to hold off 1250V up
to 210C; soldermask is the coating.
At 2600V and 20C, surface arcing over the sodermask will occur;
cannot say where the voltage "breakdown" is.
Helps to severely limit the current (20uA seems to not create
carbonized paths in time periods less than 10 seconds).
Granted, there are no intermediate layers of copper "in the way" and
that the board material we use is not FRxx.
Perhaps so-called "no-clean" solder was used, which obviously leaves
crap behind.
TINSTAAFL.

 

[Michael A. Terrell]

Martine Riddle wrote...

Yes. Although I can think of cases where 1, 1.5
or even 2kV uses have worked for years on end.
But then there's the spectacular failure at 1kV,
or less. So, yes, 600 volts sounds about right.


Indeed, with substantial modifications, all the
way to 15kV. I've found there are two issues,
1) basic coax-cable dielectric HV withstanding
capabilities, which are dependent on pinholes
and the like, and 2) issues having to do with
the outer woven-shield connector termination of
the coax, creating small, high, local electric
fields that can disastrously break down at 1/3
to 1/10 of the coax dielectric-breakdown limit.

Well-designed high-voltage connectors deal with
the shield termination in an innocuous fashion.

I thought the HN connector was designed for high voltage coaxial
connections? I remember using them in a early '50s RCA TV transmitter.


--
Service to my country? Been there, Done that, and I've got my DD214 to
prove it.
Member of DAV #85.

Michael A. Terrell
Central Florida

 

[Winfield Hill]

Robert Latest wrote...

Winfield Hill wrote


What do you need 160 for these beasts for?
Just curious.

Anti-proton trapping experiments at CERN; the
HV amplifiers drive the trapping electrodes,
and apparently there are a lot of them!

 

[[email protected]]

Manufacturers and suppliers readily publish data on FR4 dielectric
strength, usually around 400-500V per mil. But this is only valid for
80 or 100 seconds. I haven't seen a datasheet contain any practical
information on operational breakdown performance.

Does anyone have more accurate guidelines for the operational voltage
range of FR4 if you want to, for example, avoid any possibility of a
failure within 10 years of continuous operation? In electrical printed
circuit boards, the breakdown voltage means something only to those few
that are worried about transient spikes. I've always wondered why they
dont publish specs that would be useful to the other 95% It would be
nice to stick to the UL guidelines, but 500V sot-23 transistor pad
spacings make a mockery of those. There must be a study out there some
where.

There is a related thread at:
http://groups.google.com/group/sci....nk=st&q=breakdown+fr4&rnum=1#a7d1c2bacacbb04b


A useful trick to decrease the likelyhood of breakdown and arcing is to
bond a layer of copper clad Kapton to the bottom side of the PCB,
ofcourse this only works for SMD only boards. The Kapton film is copper
on one side and 0.1mil teflon on the other (Kapton FN). The teflon
makes an excellent thermoplastic adhesive above 280degC and sticks to a
PCB nicely. The copper side is grounded which puts a perfect ground
plane 2mil below the PCB. If the PCB is thin, this causes the electric
field to be directed downward, and due to the dielectric properties,
concentrate in the Kapton, thus avoiding breakdown of the FR4. With the
addition of some thermal vias, and an aluminium plate, you can also
make an excellent heat-spreader or heat-sink attachment, in this case
forget the copper layer, use two sided kapton FN and bond direct to the
metal backing.

You can also lay the components directly on kapton, but you only get
traces on one side. A better option is microwave type, copper clad
teflon, which is relatively low-cost and can be processed like 2 layer
FR4, except you wont get plated through vias unless you deal with a
specialty manufacturer.

/Andrew

 

[joseph2k]

Manufacturers and suppliers readily publish data on FR4 dielectric
strength, usually around 400-500V per mil. But this is only valid for
80 or 100 seconds. I haven't seen a datasheet contain any practical
information on operational breakdown performance.

Does anyone have more accurate guidelines for the operational voltage
range of FR4 if you want to, for example, avoid any possibility of a
failure within 10 years of continuous operation? In electrical printed
circuit boards, the breakdown voltage means something only to those few
that are worried about transient spikes. I've always wondered why they
dont publish specs that would be useful to the other 95% It would be
nice to stick to the UL guidelines, but 500V sot-23 transistor pad
spacings make a mockery of those. There must be a study out there some
where.

There is a related thread at:
http://groups.google.com/group/sci....nk=st&q=breakdown+fr4&rnum=1#a7d1c2bacacbb04b


A useful trick to decrease the likelyhood of breakdown and arcing is to
bond a layer of copper clad Kapton to the bottom side of the PCB,
ofcourse this only works for SMD only boards. The Kapton film is copper
on one side and 0.1mil teflon on the other (Kapton FN).

Nothing of the sort. Kapton(tm) has no chemical relation to Teflon(tm).

Kapton® Polyimide Film



DuPont™ Kapton® is a leader in the high performance films industry, offering
over 40 years of diverse products, global technical support and customer
service. DuPont has set a high standard in the polyimide film markets with
its durability and performance in extreme temperature environments.
Kapton® has a unique combination of electrical, thermal, chemical and
mechanical properties and retains these properties over a wide range of
industrial environments and applications.


From miniaturized electronic components to Mars rover heaters, from high
speed locomotive motors to airbag seat sensors, DuPont™ Kapton® polyimide
films make innovative design solutions possible.

The teflon
makes an excellent thermoplastic adhesive above 280degC and sticks to a
PCB nicely. The copper side is grounded which puts a perfect ground
plane 2mil below the PCB. If the PCB is thin, this causes the electric
field to be directed downward, and due to the dielectric properties,
concentrate in the Kapton, thus avoiding breakdown of the FR4. With the
addition of some thermal vias, and an aluminium plate, you can also
make an excellent heat-spreader or heat-sink attachment, in this case
forget the copper layer, use two sided kapton FN and bond direct to the
metal backing.

You can also lay the components directly on kapton, but you only get
traces on one side. A better option is microwave type, copper clad
teflon, which is relatively low-cost and can be processed like 2 layer
FR4, except you wont get plated through vias unless you deal with a
specialty manufacturer.

/Andrew

Other than that your post ain't tooo bad.