Circuit board insulation and high voltage

I am having a problem with leakage currents through a circuit board.

A product I am working on has a dc-dc converter that converts 12V from a battery to 350Vdc. The two power buses are mostly isolated, where the only connection between them is a differential amplifier with a

1MOhm input impedance. The input impedance of the amplifier centers the high volt output relative to the battery ground. So relative to battery ground the high volt supply is +/- 175V.

I recently added a safety circuit to detect leakage currents between the high volt lines and battery ground. This looks at the voltages on the high volt bus relative to battery ground, and if they are not centered, there is a leakage current. This way the system can detect a fault.

This worked great through development, but now in production I am seeing a 3-5% fallout due to this fault. The boards that pass are dead nuts on. There is no discernible leakage current to the limits of my measurement equipment. The boards that fail show an obvious leakage current, the impedance of the defect is within 100kOhm to a couple MOhm. This only happens with high voltage, a regular DVM shows an open circuit. This appears to be due to a defect within the circuit board itself. When I look at it with a scope I can see the voltages moving around, maybe due to partial discharges. On a couple of the boards I have watched the fault clear itself, and have not been able to get it to reappear.

I am looking for high voltage specifications for PCBs. The design follows the IPC-2221A guide lines for creepage and clearance. Are there other material specs i should be calling out?

Does anybody have an idea of what the failure mechanism is? If a board shows a fault that clears itself, presumably burning out whatever contamination is causing the fault, is it more likely to fail in the future? Are there processing issues that could cause a large leakage current? I have seen a board go through a lead free soldering process and come out charred, but I am pretty sure that is not what is going on here.

Thanks,

Ethan

Reply to
Ethan
Loading thread data ...

Water. What process are you using to solder and clean the assemblies?

Also, you should bake them at 60C for an hour at least, if not 70C, after they have been thoroughly cleaned. A few seconds in a vacuum chamber will also release hidden water molecule entrapments.

After that, a good coating of conformal media might be a consideration.

The other thing is that all components on the HV side should be kept clean from human contact during assembly and all other handling. That is everything from finger oils to "coffee breath". Such residues cause leakage in real HV circuits, perhaps they do also in your medium voltage application. Any capacitor bank you place across the output also should be elevated from the PCB such that you do not provide the path where trapped VOCs etc. can set-up said leakage paths.

Reply to
Archimedes' Lever

es?

n.

so

The solder process is a regular leaded solder, for now we are only selling in the US, so it is not RoHS compliant. It is a surface mount reflow process then a wave solder process for the through hole components. The solder uses a water soluble flux, then the board goes through a normal wash and drying process. It seems the drying process is not drying enough.

There are some fairly big capacitors on the board. I am wondering about their ability to capture moisture. It looks possible.

The assembly is eventually potted. I want to make sure everything is clean and dry before potting captures whatever contaminents.

What I need right now is a way to solidly confirm that this is a problem with moisture.

Thanks,

Ethan

I am going to try leaving the next batch of board in the oven at 65C overnight, to see if that helps. I also need to try to find a board that fails consistently, and see if your vacuum chamber suggestion works, if so that would be good confirmation of water, or some other volatile on the board.

Reply to
Ethan

...

The main problem I have had is where flux gets trapped under a component and can then cause leakage when it absorbs moisture.

I was using voltages up to 150V with 10Meg 1206 resistors and the circuit was sensitive to about 10nA of leakage (equivalent to a leakage resistance of ~10G Ohm).

One approach that seemed to work in this scenario was to relieve the solder mask under the resistor and put a grounded trace between the two pads.

Removing the solder mask gave a few mil of clearance for the water wash to get in and clean the area while the grounded trace diverted any leakage currents.

The level of leakage you are getting seems extremely high. Are you sure that the active circuitry is not causing a problem - what defines the 1 meg input resistance of the amplifier?

kevin

Reply to
kevin93

Do you have the option of redesigning the PCB? For very high voltages, you sometimes see PCB's with slots (air gaps) in them to absolutely guarantee there's no leakage from surface contamination.

Most PCB's these days are FR4 material with some kind of UL flame retardant spec. Your board manufacturer (or layout engineer) will have loads of advice about materials - maybe you're using a cheap material. Perhaps just changing to a thicker PCB will fix it.

How do you know it's not your leakage monitoring circuit? Oh yes - it is measurable at high voltage. Maybe the leakage monitoring circuit has a component that needs a higher voltage rating... 350V AC rather than DC...?

--
Nemo
Reply to
Nemo

It is not a problem with the voltage monitoring circuit. I have tested the circuit and it is working correctly. The voltage rating of the components have plenty of margin, The input resistance to the diff amp is built from four resistors in series, each is rated for 200V. The creepage distances on the board were maintained at 2.5mm, which is the IPC-2221A recommendation.

The IPC guidelines for voltage creepage and clearance in my experience are pretty reasonable. They are conservative enough that everything works reliably, but not as conservative as something like UL "inherently safe". I use the UL specs in places where someone could get a shock, and the IPC specs if all I need to do is make the equipment work reliably, and it is not a safety issue.

I have become convinced that my problem is due to moisture contamination. Baking out the boards at 65C overnight fixes the problem. This is not the best solution, adding a 12 hour step to the production flow is not exactly lean manufacturing. Also, if there is moisture trapped under a component, it is likely to have not been cleaned adequitly and leaves some ionic contamination even after it has dried out. So moisture due to high humidity or something would allow a leakage current again. Earlier someone suggested raising the large capacitors off the board a little bit to allow the wash to get under them, and then to allow them to dry out seems to be the way to take care of the problem.

Ethan

Reply to
Ethan

It IS the best solution, but 12 hours is more than a bit of overkill. When you are talking about HV design, baking out of assemblies is a required step and should be factored into a cost analysis. That IS as lean as it gets.

The voltage across your multiplier, assuming there is one, would determine whether or not the multiplier section of the device should be potted. Also human contact circumstance, as you indicated., but that cannot be avoided at the output lead or port of an HV supply case. Only as it relates to the guts, and that should not be having human proximity anyway.

A few things that will insure a long lived circuit in WallyWallWhackr's HV circuit realm are:

Hard anodized cases. Hard anodized Aluminum yields a non-conductive surface, reducing any coronal attraction that a case might normally cause.

Use of an insulative partition. Using 'Nomex' insulator paper (transformer paper) or a suitable polymer plastic sheet, or Kapton tape layering is needed in the HV section of a design typically for any un-potted HV device, and has benefits when properly positioned in potted cases as well. Potting only the HV end is 'doable' and allows for a bit more serviceability on the control/drive section.

Leave any multiplier area free of any solder mask (yes, bare board). Solder mask adheres to potting very poorly. It adheres to bare FR4 or G10 much better, IF the board is clean and any primer step followed.

Use slots between nodes that are separated by high potential differences. Have the PCB maker use his 0.035 mill to cut slots, just like those used when arraying boards out on a palette setup. Between the nodes of the HV caps, and diodes. I can post a picture in abse (alt.binaries.schematics.electronic) if you want to see a good multiplier design, if you get that group. The slots allow potting to flow into them and that makes partitions between the nodes that are nearly impossible to breach.

Clean the boards VERY well both before and after the assembly / solder process. Keep fingers OFF of HV components and the PCB. ALL of the PCB. circuit boards are hygroscopic. They grab water like a sponge, and finger oils as well. If your process is aqueous, the oils cause a problem in the HV area. Even 'coffee breath' causes a problem without a subsequent cleaning step. Aqueous usually gets air knifed fairly dry, but a good two hour bake should evaporate any and all remaining water. A few seconds in a vacuum doesn't hurt either for pulling water out of trapped pockets (another reason to use no mask)

If your process uses solvents instead of water, you should consider a hot alcohol bath and rinse before you bake the assembly out, and a vacuum should be looked into as the board will want to suck up water right away. For integration into the case, you should either be careful of the humidity level in the room or do a quick bake again while in the case. All bakes are at your temp of 65C.

I would not go the 12 hour bake though as that shortens your EL cap life a bit, and the water evaporates even at less than boil temps, so the job gets done pretty quickly.

If you are not potting, then a conformal coat will seal in a well baked board so it no longer sucks water like Bill Gates sucks corporate cash coffers.

WallyWallWhackr

Bakings? We don' need no stinking bakings! :-)

Reply to
StickThatInYourPipeAndSmokeIt

Elevating parts is good (shoot for less than 2mm). It usually violates IPC-610, but in the HV realm, we do all kinds of things not done elsewhere (solder blob nodes, for example). What you get is a clean wash and low VOCs. A good conformal coat, particularly a vacuum aided conformal coat session will seal it up real good too.

Try Dolph's for sealing things up to industry specs. That coating application will also end up adding stanchion to the elevated parts.

Reply to
StickThatInYourPipeAndSmokeIt

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.