FR4 thermal solution

[Oznog]

Well, I took some interest in this unusual FR4 a guy on eBay has:
http://cgi.ebay.com/10-shts-Copper-...Electronic_Components?_trksid=p3286.m20.l1116

Now there are 2 remarkable things here that might make useful thermal boards. The FR4 is only 0.018" thick instead of the more common 0.062". With this thinner board, even thought the thermal conductivity of FR4 is only 0.25W/mK, this works out to 2.835 C/W per sq in of conduction through the thin FR4 IF the heat is evenly distributed across the top and bottom.

Well he board is 4oz, which is 4x the normal copper thickness. This is important because normal 1oz copper has a significant lateral resistance which means the heat does not spread far. With 4oz, I get that heat conducts down a 1mm wide trace with a resistance of 17.5 C/W per mm.

How good of a heat spreader is that? Well, depends on your package, actually the perimeter of the thermal pad is most important. Unfortunately without finite point analysis software this is difficult to solve for with anything other than rough estimates. Luxeon Rebel's tiny pad has 11.1mm of perimeter area. The area immediately around the pad has to conduct through an 11.1mm ring around the pad but that ring's width gets much wider as we go further out, providing more copper conduction per mm of increased distance. At 1/2" radius the added resistance per mm is 0.219C/W because the circle's circumference is 80mm wide.

Maybe someone with software could work this out, but it seems like this board *could* make a custom thermal board with reasonably low resistance at home and work with solderable pad devices. Flatness may be an issue. 0.018" FR4 is paper-thin. I expect you'll be able to bend the board by hand and it'll stay there because the copper is providing all its stiffness not the FR4 and copper deforms. That causes major trouble mating with a heatsink. Also etching deep-copper boards is its own difficulty. CNC pcb engraving, also very difficult because the FR4 is so thin any engraving into the FR4 could cut right through it.

 

[snarfer]

It seems like you wouldn't be able to really get all the benefit from the thin board unless you could plate your own vias.

Actually you can get boards made with 0.5mm FR-4 and 2 oz. copper for negligible extra charge. So it doesn't really seem worth it just for the extra copper, especially without thruhole plating.

 

[Oznog]

What supplier are you suggesting? I looked into it and thicker copper and thinner board, and plating options, definitely added up.

I did a bunch of analysis of thermal via design in other threads. The benefit's there, significantly better than MCPCB actually.

I agree that factory-made thermal via design with some options added will be better board. And for mounting a single emitter, something in a "standard" configuration, there's no reason to do this at all because there are premade MCPCB/thermal via board that could do this job for $1 anyways. But, a lot of people have reason (or at least an inexplicable desire) to DIY it. A large one-off board with multiple emitters maybe.

 

[dat2zip]

You can get the Rebel Flower board at the Shoppe which is only 0.2mm thick and has vias under the power pad and a copper plane on the bottomside. The thin PCB in my opinion is far better than any MCPCB.

The flower can be cut to make a tri Rebel configuration or individual ones can be cut out with a pair of garage scissors. I wouldn't use the house scissors especially if they are used by others in the family.

There is also a 10mm diameter single thin PCB.

Do a search at the shoppe for thin pcb on the shoppe and you find all the FR4 thin PCBs.

Wayne

 

[Oznog]

Hmm... the Flower looks interesting but looks to me like it's weak on like 3 important points.

One, mounting a thin board is very very difficult. It's not just about getting pressure on it but applying it evenly because any warpage will separate the device from the sink and result in failure. I guess you could thermal epoxy it while clamped then solder the LEDs, maybe that was the idea? That's problematic because once it's heatsunk it's really difficult to reflow LEDs, and also epoxy coming through the PTHs will ruin the solderability. Actually... I'm looking at the pic and it REALLY looks like it's already been solder-tinned (not chemically given a bright tin plating). That's an absolute no-no if it's on the bottom and I don't see how it wouldn't be on the bottom too. Solder makes it impossible to mate well with a flat surface and that can have very negative impacts on thermal resistance.

Second, that large PTH size shouldn't really be under the pad. On larger vias the solder can flow to the underside which prevents post-reflow placement of the board. But also a problem is it's compromising the critical copper area directly under the pad.

Third... I mean, more copper is helpful. It would have been easier to leave more thermal trace. Why etch it away?? That and thermal vias further out should be effective unless they used thin copper like normal 1oz stuff (that would generally be a bad choice).

The lack of masking is kind of a problem because you can't accurately place the devices, they can flow wherever they feel like it if you're not careful and hand-tweaking several into position at once is very difficult. Which isn't necessarily a problem as long as optics aren't involved which require them to be in a very specific location.

Hard to say without a board to look at closer. For the price I'd kinda expect something a bit nicer.

 

[snarfer]

I just priced it on PCBcart.com and it was $50 tooling plus a few bucks per board depending on how many you ordered. That was for 0.5mm FR-4 with 2oz. copper. I think that is only about $10 more for the tooling than the regular FR-4. It would be considerably more for 4 oz. copper though.

I usually order from ourpcb.com though. They are even cheaper, but don't have an online quote system. On my last order they filled tons of tiny PTH with epoxy and routed curved edges to the boards at no extra charge.

I like to have the thermal vias filled with epoxy. I have this idea that it will prevent solder leaking through during reflow and also might make it less likely to lift a pad. But then again not much solder leaks through a 0.35mm hole anyway.

 

[Oznog]

What combination of options did you use to get $58 tooling? I couldn't get that when playing around.
Pay attention to minimum hole size. There's some calculations required, IIRC the 0.5mm via was best. Larger and it's less helpful because its area goes up with square of radius but the thermal conduction along is circumference is linear. AND they increase the lateral thermal resistance to vias further away by removal of surface copper. On the other hand, smaller vias become less productive because the mfg will not allow you to space smaller diameter vias much closer so the vias/sq in doesn't go as much as the circumference goes down.

2oz is sort of "marginal", but a good board is still possible. I think HASL is going to be something we don't want. OSP is also a question. See AFAIK OSP is a like a lacquered flux. For the solderable pads that's no problem. For the heatsink side, it probably IS a problem because that layer won't be displaced by solder. Not unless you have a way to strip it before applying thermal grease.

Right as the holes get very small the likelihood of solder bleeding through is reduced.

The thermal epoxy backfill is nice but calculations show only marginal benefit. I'm actually slightly concerned about burning that when reflowing although it should probably be ok.

 

[snarfer]

Maybe you're running into the extra charge for really small boards? I just priced it again - 70 um copper, 0.5mm FR-4, 50mm x 50mm boards, 20 pieces, and got $55 tooling cost with $3.34 per board, but that went down to $1.74 per board on 50 boards. I'm sure ourpcb.com is cheaper though. I put in a similar order a month ago there, but with regular 1.6mm FR-4 and it was only $0.54 per board and similar tooling cost.

I read an article a while back about advantages of filling vias with epoxy and they did thermal calculations and came up with the interesting conclusion that the advantage cooling-wise of conductive epoxy was far outweighed by some other negatives, forgot what they were. The recommendation was to fill with non-conductive epoxy and put vias right in the middle of the pads. I have now reflowed 20 or so boards made that way and had absolutely no problems.

I had boards made with a number of areas filled with 0.3 and 0.4mm PTH and center-center distance of 0.8mm. The board manufacturer had no problem with that, and there was no extra charge. Some of the areas were directly underneath cooling pads for power mosfets in no-lead type packages, and there was no problem whatsoever with reflow. I guess I could have used even more holes even closer together, but as this was for a power converter, not an LED mounting application, it was already more than adequate.

For surface coating Immersion Silver would certainly seem like the way to go, and is same price as HASL.

I had another idea actually, but really it doesn't fit with my current project so I haven't pursued it. Probably cost like $1000 to do, but maybe you could do it at home with manufacturer samples. Flex PCB can be ordered with 4 oz. copper conductor, and 1 mil (or even 0.5 mil!) Kapton dialectric. I have seen a site where someone was DIY etching flex using a wax type printer and sample material Dupont sent him for free. Oh here it is. And the material is Dupont Pyralux, try Pyralux AP, LF, or FR for 4 oz. copper.

The flex PCB manufacturers can etch not only the copper, but also the Kapton. And they can layer it as needed. So you could make a board with copper circuitry in the middle and etched Kapton on both sides. In other words, do away with the vias entirely and just bond the heatsink to one side of the copper layer, and the LED thermal pads to the other side of the copper layer. I'm sure there are lots of other details to work out, but it does seem like the ultimate solution. Actually I thought about making entire assemblies, power converter, wires, the whole thing, with flex.

Furthermore, Kapton has a relatively low thermal resistance, especially if it's only 1 mil thick, so for the DIY solution you could just etch it yourself, then reflow, and stick the LED assembly onto the heatsink with the adhesive built into the Pyralux. I didn't do the calculations, but it does seem like it would work a whole lot better than the thin FR-4 without thermal vias.

 

[Oznog]

Well, thermally conductive epoxy has no real liability other than cost as long as it's properly applied and doesn't have any residue on either face.

The thing is it has very little advantage on small holes. Some, but quite minor. As a hole gets smaller, the ratio of its cross section area- which determined the conductivity of the epoxy fill- to the circumferential area- which determined the conductivity of the PTH wall- decreases. The tiniest vias are almost completely closed in with copper.

The epoxy's supposed to allow you to put the via under the pad with no risk of solder wicking to the backside. True but again I don't think that's even a problem with 0.35mm vias.

Immersion silver sounds great, I agree!

Yeah I talked with Gold Phoenix PCB awhile back, he said the via proximity limitation is a problem where the dust from the drilling gets stuck in the holes created in earlier drilling. I guess at some point you undermine the board's strength too.

Remember, this flexible stuff is going to be a problem to mount. If proper thermal via design already has the board resistance down extremely low, what's the point? If the board is flexible and fails to screw down flat then you could take on many C/W in additional resistance. Thus it's not only more expensive and difficult to obtain but a worse solution.

 

[dat2zip]

Hmm... the Flower looks interesting but looks to me like it's weak on like 3 important points.

One, mounting a thin board is very very difficult. It's not just about getting pressure on it but applying it evenly because any warpage will separate the device from the sink and result in failure. I guess you could thermal epoxy it while clamped then solder the LEDs, maybe that was the idea? That's problematic because once it's heatsunk it's really difficult to reflow LEDs, and also epoxy coming through the PTHs will ruin the solderability. Actually... I'm looking at the pic and it REALLY looks like it's already been solder-tinned (not chemically given a bright tin plating). That's an absolute no-no if it's on the bottom and I don't see how it wouldn't be on the bottom too. Solder makes it impossible to mate well with a flat surface and that can have very negative impacts on thermal resistance.

Second, that large PTH size shouldn't really be under the pad. On larger vias the solder can flow to the underside which prevents post-reflow placement of the board. But also a problem is it's compromising the critical copper area directly under the pad.

Third... I mean, more copper is helpful. It would have been easier to leave more thermal trace. Why etch it away?? That and thermal vias further out should be effective unless they used thin copper like normal 1oz stuff (that would generally be a bad choice).

The lack of masking is kind of a problem because you can't accurately place the devices, they can flow wherever they feel like it if you're not careful and hand-tweaking several into position at once is very difficult. Which isn't necessarily a problem as long as optics aren't involved which require them to be in a very specific location.

Hard to say without a board to look at closer. For the price I'd kinda expect something a bit nicer.

The important factor is getting the heat to the bottom. The vias are all that are needed. There is no need for top side copper if the thermal resistance to the bottom is good.

As for reflow. The LEDs snap into place. I haven't had any issues.

I agree getting the board flat. I cut an acrylic template that sits on top that gives me a flat surface that makes clamping easier.

The price is based on small volume runs. Considering if you only buy one it's a good deal as it would be hard to find a PCB shop that will make a single one for that price.

Wayne