Burn In Board design inputs

[glicos]

This is my first time designing a burn in board and need an expert advice from the community. Board will be subjected to the following:

• 1,000V reverse breakdown voltage for diode
• @ 125 degrees Centigrade

• Is FR4 material enough for this application or have to use Polyimide material for much higher temperature range and dielectric strength?
• What the best finish material, ENIG or HASL?

Any more inputs will be highly appreciated. Here's the initial layout:

TOP:


BOTTOM:


PERSPECTIVE:


Thanks for any input or suggestion...

[Rerouter]

for a start the pcb does not tell me much about how it tests it,

but i can already tell your connector is not laid out ideally, for 1000 volts, you want a full dummy pin between voltage carrying pins, while the breakdown of dry air is about 3KV per mm, its much safer to work it out at 1KV per mm to cover humid air,  and the breakdown of fr4 (clean) is generally 10x this so if you focus mainly on airs breakdown you should be covered,

fr4 on its own can constantly handle 125C, but it will discolor quickly,

equally you may want to avoid lead free solder, and go generoulsy on flux when mounting these things, as a dry joint could give you a premeture failure at those temps,

[glicos]

for a start the pcb does not tell me much about how it tests it,

but i can already tell your connector is not laid out ideally, for 1000 volts, you want a full dummy pin between voltage carrying pins, while the breakdown of dry air is about 3KV per mm, its much safer to work it out at 1KV per mm to cover humid air,  and the breakdown of fr4 (clean) is generally 10x this so if you focus mainly on airs breakdown you should be covered,

fr4 on its own can constantly handle 125C, but it will discolor quickly,

equally you may want to avoid lead free solder, and go generoulsy on flux when mounting these things, as a dry joint could give you a premeture failure at those temps,

Thanks for the inputs Rerouter. Actually, layout is the same as the original, but customer wants to remove the even numbered pins because of its closeness with its adjacent pins, causing premature discoloration of the pcb probably cause by the high voltage inputs.

[Rerouter]

sorry about that, my eyes saw the white as a space and the green as a trace for unknown reasons,  still you seem to void that seperation on some of the traces, why was each done seperatly rather than a mirror?

e.g. third from the left on the top image (apart from the upper via) has wider clearences than the rest,

also after reading over a few things, it appears in general soldermask is moderatly leaky for high voltages, while some colours are better than others it comes down to which one your maker uses,

and that it is generally the fr4 that discolours and not the mask,

http://www.pcbstandards.com/forums/showthread.php?p=12415

[free_electron]

First of all: FR4 is a classsification for flammability. There are hundreds of different substrates that are classieifed as FR4 with various operating temperatures.

Saying you will use an Fr4 material is like saying you will use a resistor... Without specifying wattage,  tolerance and standoff voltage or ohms value. Useless.

For burn-in boards we typically use a high temp FR4 material up to 138 degrees C (nelco 4000 series or idola 400 family.) Above that we switch to a different material typically a polyimide based substrate.

You essentially need a material with a high Tg..

As for layout : remove the unwanted pads on the connector to increas the creepage and fill that empty space with soldermask. For the soldermask you also need a high temperture mask. Typically a dry-film mask will work better than a liquid soldermask for such things.

You need to talk to your board house for these things as they may have other materials. Every boardhouse has different stuff and while they can order non-standard, you will pay for that. Ask them for a what they typically stock and go with that. I may have easy access to Nelco but that doesn't mean your boardhouse does. It may be easier for them to get Rogers or Isola or some other substrate maker's material. Depends on where you are in the world.

As for what is best in terms of surface finish : that is dictated by the edge connector. You will need hard gold plating there if you want any kind of durability and extend the longevity of the connector in the oven itself. You will need to chamfer the board and provide the plating short outside the chamfer. Again, you will need to talk to the board house. Enig and hard gold are not really compatible processes. Hard gold requires electroplated nickel and electroplated gold, while enig is electroless nickel. Depending on how the boardfab is setup there may be extra costs as they need to do selective plating and masking.

For this kind of low tech board i would go with HASL and do a selective edge plated hard gold connector.

Now, on to your sockets .. I assume you have a kind of zif socket to plug the DUT in. You may want to add stiffeners to the pcb structure as this board is going to flex .. So provide screw holes for the stiffner slats....