PCB tinning to increase current in tracks

[Romain]

Hi all

I'm looking for the good practices to do PCB tinning to increase the current handling capability of traces on a power supply board.
Dave made a video on it but he doesn't really talk about the "how-to".


My questions are:
- is there any table of the tinning width/thickness and the increased current handling?
- should the soldermask windows be aligned or perpendicular to the solder wave direction?
- is there a min/max/ideal width, should it cover the track completely or leave some soldermask on the edges?
- what about tinning ground planes to increase thermal?

For example:


I posted in the video thread a few days ago, but it dates back to 2012...
See for reference: https://www.eevblog.com/forum/blog/eevblog-317-pcb-tinning-myth-busting/msg1161755/#msg1161755

Thanks!

[MagicSmoker]

I haven't watched the video, but I suspect one of the points made is that solder - even silver solder - has about 6x to 9x higher resistivity than copper, so any improvement in total ampacity of a trace from HASL/tinning will be minimal.

If you really need higher ampacity for a given trace width then choose thicker copper plating for the board (e.g. - 2oz/0.07mm or 4oz/0.14mm). Same if you need better thermal conductivity.

[Mattylad]

I have seen thicker wire (2.5mm+) soldered on top of wide exposed tracks in order to allow a greater current to be passed.
A lot depends upon what current you are wanting to pass along it, if your trace cannot go wider then it has to go thicker, so use 2-3oz+ copper.

Discussing this soldering tracks, a more knowledgeable engineer than me would always be muttering about the skin effect.

[Monkeh]

I haven't watched the video, but I suspect one of the points made is that solder - even silver solder - has about 6x to 9x higher resistivity than copper, so any improvement in total ampacity of a trace from HASL/tinning will be minimal.

You say that.. 35µ copper, 3mm wide, 50mm length, ~8mohm. Now, let's tack a 2mm wide, .5mm thick layer of tin on top of that: ~6mohm. Now we're looking at under 4mohm resistance: Half the loss.

Doesn't seem like a lot, but consider this is often applied to things which handle 30A+.

[Romain]

Exactly, considering this is "free" (as opposed to increasing the copper thickness) then any gain is worth it! 

My primary need is for thermal.
Should I just open the whole ground plane soldermask, or make strips (or any other pattern) to benefit the most from the solder wave?

[Romain]

Continuing m research, I found Mike's video, and the same question by tom66:
https://www.eevblog.com/forum/chat/tinning-traces-for-more-current/25/

Should I do diagonal strips in the ground planes as a trade-off?
Has the wave soldering technique become some well thought-through that any shape should work nowadays?
What about simply opening the whole plane?

Tks

[DerekG]

My primary need is for thermal.
Should I just open the whole ground plane soldermask

That's what I do on the solder (bottom) side to dissipate more heat & increase the current carrying capabilities of the tracks.

Just remember that for compliance & certification reasons, you should design the width of the tracks to take the current you need & any opening of the soldermask just increases the safety margin.

Below are 2 pics - one of the bottom side that shows the opening of the solder mask & one of the top side of the same board that shows the opening of the solder paste stencil to increase thermal cooling for the two high current (expensive) mosfets (Fairchild FDB075N15A).

In addition, there are approx 120 x 0.35mm holes in the mosfet pads to push current & heat to the bottom side of the board. These holes are plated "fully closed" & these boards are 2oz copper.

The solder paste stencil is 0.2mm thick to set down a bit more solder under the mosfet pads.

Also, there are multiple dual row pads surrounding the mosfets. These allow the for the installation of dual row header pins which act as "heat fingerlings" to substantially improve the heat transfer into the surrounding air. This is done as an economical alternative to conventional heatsinks in our low profile enclosure.

These dual mosfets push around 2.5KW at 150V DC without any fan forced cooling. The full sized boards measure 130mm x 100mm. All designed in Diptrace ver 3 (I moved over from Altium 2 years ago .......... just because I like DipTrace).

PS: The V-grooved panels & solder stencils are made by PCBWAY. As they say in Australia "I'm a very happy Vegemite".

[Romain]

Hi Derek, great piece of info you've posted there, thank you!

Does the board go through reflow and wave soldering? Do you have pictures of an assembled board?
I'd like to see how the solder behaves when dragged over a large surface.

There is this video where Dave talks about solder shadowing.


So basically, I need as much solder as possible from the wave solder passing along the board surface. A guess would be to make the soldermask window strips perpendicular to the solder wave direction to maximise this effect.

[DerekG]

Does the board go through reflow and wave soldering?

Yes, both. The reflow is done in a vapour phase oven (so not infrared) as we get a more consistent result.

Do you have pictures of an assembled board?

Not of that new prototype, but we will in several weeks time when all the parts have arrived.

I'd like to see how the solder behaves when dragged over a large surface.

It is not all bad news though. Below is the previous board which is similar, just not as "polished" in design or layout.

This model is designed for 1.5KW to be pushed through the mosfets. The through holes in the heatsink are 0.9mm & you can see the top layer is pretty neat but the solder on the bottom side is not so neat due to the "sucking" effect the through holes cause.

So basically, I need as much solder as possible from the wave solder passing along the board surface. A guess would be to make the soldermask window strips perpendicular to the solder wave direction to maximise this effect.

Dimpling the solder's surface will actually aid heat dissipation into the air, however raw current carrying capabilities relies on the track's "thickness" being consistent from one end to the other.

[Romain]

Great pictures thanks!
The "solder drag" effect is easy to see, the wave starts at the top of the board, and as it progresses it pulls the solder and only leaves a few microns on the surface except at the bottom where we can see the solder lump.

Just as you, I'm improving the design of my board and use every trick
Dissipation isn't such a problem in my case because the board is mounted vertically. However having a better heat-spreading over the big ground plane is essential.

[DerekG]

Great pictures thanks!

Your welcome.

The "solder drag" effect is easy to see, the wave starts at the top of the board, and as it progresses it pulls the solder and only leaves a few microns on the surface except at the bottom where we can see the solder lump.

Quite right. The boards direction of travel over the wave solderer was chosen to maximise the solder deposited on the thick track at the bottom of the board.

Just as you, I'm improving the design of my board and use every trick

Yes, it is an process of evolution. Our original design criteria was for 1.5KW, but our end customer quickly had requests for 2.25KW then 2.4KW ........ hence the upgrades.

Dissipation isn't such a problem in my case because the board is mounted vertically.

Our board is also mounted vertically. The "heatsink fingerlings" actually aid cooling considerably on the vertical board. The legs also pull much more heat (& much more current) to the bottom side of the board.

[Romain]

Quick update, I decided not to add extra solder on this board.
Instead, I really nailed the component placement and ground plane stitching. Thanks for your reply.

Sent from my ASUS_Z00AD using Tapatalk