Reducing Copper Trance Resistances, ideas?

First, make sure you are treating the real problem. The power wasted in

power divided by the thermal mass, minus the cooling (which is proportional to the temperature difference between the hot parts and the coolant). The temperature itself is the result of the temperature increase over time.

Since your problem is too high temperatures, there are several ways to combat it - and the best choice is application dependent.

  1. Reduce the current. Assuming the output power is fixed, you can do this by increasing the voltage.

  1. Reduce the resistance. You can do this with shorter tracks, thicker tracks, wider tracks, or more tracks (including inner layers if you are careful about cooling). Or you can add bus bars, external wires, etc. Removing the solder mask and adding solder helps a bit, but the resistivity of solder is much higher than that of copper.

  2. Increase the thermal mass. This will help if you have a short duty cycle for the active period, when you won't have enough time to reach high temperatures. Soldering over the tracks is an easy way to increase the thermal mass.

  1. Increase cooling. Fans, heat pipes, heat sinks, etc. are all good, if circumstances allow. You should probably also aim to spread the heat around the pcb - have plenty of vias (without thermal reliefs) from the internal tracks to external tracks or polygons. Good ground planes help to spread heat. And try to get strong thermal connections between the pcb and mounting frames.

  2. Reduce the time that the high power is running.

You might also find it practical to simply accept that the power board is going to get hot, and keep it physically separate from the control board (which is likely to have more sensitive components). That also lets you use thicker copper on the power board and fine dimensions on the control parts.

Reply to
David Brown
Loading thread data ...

Depending on the production environment/scale you can solder big fat copper wires to them (or silver if you really have scratch and want the last little bit of conductivity.) You could even use strip stock bent-up on edge to get more surface area for cooling and/or skin effect. This does require at least one truly skilled worker.

Alternatively, delete the traces and put in a jumper [I come from the crude but effective school of thought, and have done this on a (low-volume) production board.] If you for some reason HAVE to keep this as a "in-board" solution, a very wide internal power layer or layers might be another approach (ie, dedicate a whole layer to moving this current around, or two if the geometry demands that, just like an internal power plane.)

--
Cats, coffee, chocolate...vices to live by 
Please don't feed the trolls. Killfile and ignore them so they will go away.
Reply to
Ecnerwal

You could do it in segments, or some appealing lozenge tiled pattern.

I wonder if there might be pick-and-place copper strips that you could solder on top of traces.

--
John Larkin         Highland Technology, Inc 

jlarkin att highlandtechnology dott com 
 Click to see the full signature
Reply to
John Larkin

Found what we used at GenRad...

...Jim Thompson

--
| James E.Thompson                                 |    mens     | 
| Analog Innovations                               |     et      | 
 Click to see the full signature
Reply to
Jim Thompson

That's a good product idea.

I like the bare-jumper technique.

.----. .-----. .----. .----. .-----. .----. .----. .-----. .----.

My handy copper-trace spreadsheet says 3x16AWG is as good as 1" x 4oz (25mm x 140um).

Cheers, James

Reply to
dagmargoodboat

I've seen some through-hole (vertical) bus bars (can't remember where exactly). They could be custom made (either horizontal flat or vertical with pins) using a chemical etching (subtractive) process.

Lots of PCB makers are touting really thick copper- more than

6oz/ft^2- up to 120 or even 200oz, which would be several mm thick!

Of course special design rules apply to the xtreme pcbs (and special xtreme pricing, no doubt).

Best regards,

--Spehro Pefhany

Reply to
Spehro Pefhany

IPC rules (IPC-2152 and older) assume the same performances for inner and outer layers. Dissipation by heat radiation is negligible, and the prepreg material is so thin that generating the heat at the PCB surface or 10 mils beyond doesn't really make any difference.

Plus, if you parallel identical traces using more layers, the hottest track will have a slightly higher resistance than the others, therefore the process should be also self-balancing. If you have enough PCB space you can also connect the tracks not just at the beginning and the end, but also in the middle with a lot of vias. This will spread the current and the heat even better.

--
Fletto i muscoli e sono nel vuoto.
Reply to
dalai lamah

Yes, and the cost is not allowed to increase much. Not more than we would pay for going to a siz layer board

Regards

Klaus

Reply to
risskovboligrenovering

All good suggestions, but for our PCB we cannot change any of that except f or helping the existing tracks to cope better, thus reduce the resistance

Regards

Klaus

Reply to
risskovboligrenovering

We are using 30mm wide traces in average, duplicated in 4 layers for routing the 3 phases, maximizing the trace thickness

Cheers

Klaus

Reply to
risskovboligrenovering

Nice idea :-)

Reply to
risskovboligrenovering

that's why I suggested the smd shunts/jumpers from Harwin, they come in rolls and are made for pick-n-place, but they are a bit small if you need +200mm

We occasionally get special solder-on shielding cans made, there is a bit of NRE because they need to make tools for the bending. But I think a flat shape would be much cheaper since they are made by etching similar to PCBs

If guess those who make stencils could do the same, though I think they mostly use stainless steel

So strips made in the shape of the traces reflowed on top of the traces?

-Lasse

Reply to
Lasse Langwadt Christensen

That is a hugely wide trace. How little power loss are you trying to achieve? I assume your problem is that this is a parasitic loss rather than the temperature rise of the PCB? Using an online calculator I find that the temperature rise of a single surface layer of 3 oz copper

the resistance is just 1 mohm the voltage drop is 27 mW and the power dissipated is 678 mW. Which of these is a problem?

It is not clear to me if you are saying that each of the three phases is carried on 30 mm wide traces on all four layers or that you have four layers to route the three phases up to a single 30 mm wide trace for each. If you combine four layers of traces, all 30 mm wide for a single phase, that would cut the voltage drop and power by a factor of four.

If you are running four layers of copper for each phase, I can't imagine much more you can do in the PCB. I think you need to either add jumper wires or the bus bar stiffeners some are pointing you to. If you can find space to add runs of 14 gauge wire, each two jumpers will have the same resistance as one of your 30 mm wide traces approx. So 8 jumpers of 14 gauge wire will give you about half the resistance you currently have.

Is this a volume production item where wire jumpers are not such a good idea?

BTW, in reviewing your posts you start off saying you have increased the copper thickness from 70 to 105 um, but you later say you are limited to

2 oz copper thickness which is 70 um. Which is it?
--

Rick
Reply to
rickman

  • Poor excuse. Mask out all fine pitch stuff and areas were you do not want extra thickness. Then plate up as desired. However, busbars or custom copper heatpipe with fins are better choices.
Reply to
Robert Baer

  • Back Of Envelope. Only consumed materials: paper and pencil; computer is grey mater between ears.
Reply to
Robert Baer

Thanks :-)

Reply to
Klaus Kragelund

Yes. I have an option, to mount the microcontroller on a seperate PCB (fine pitch), and solder that directly onto the PCB with thick layer stackup (crude pitch)

Regards

Klaus

Reply to
Klaus Kragelund

It's not an excuse, it's a PCB etching limitation. They can't make skinny, skinny traces super-tall.

Cheers, James Arthur

Reply to
dagmargoodboat

Custom copper busbars probably the most cost-effecte solution; they stick up off the board and allow airflow cooling. There are hundreds of companies that will stamp out the pattern(s) you would need, meaning a lot of competition and decent pricing. Look at: Seems that the "popular" name for what you want is "circuit board stiffener": Also: And: Another:

Make a design where the length and "pins" covers all you need and trim later for actual use(s). Makes for ordering and stocking of one ("universal") item and possible reduction of overall costs.

Reply to
Robert Baer

r

ry

e

up

is

uting the 3 phases, maximizing the trace thickness

I get similar results. I calculate that a single 70um x 30mm x 200mm trace (2 oz.) has a resistance of 1.8 milliohms, and dissipates 1.1W @ 25A d.c.

Cheers, James Arthur

Reply to
dagmargoodboat

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.