Reducing Copper Trance Resistances, ideas?

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.

Found what we used at GenRad...

...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

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

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

Best regards,

--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.

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

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

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

Cheers

Klaus

Nice idea :-)

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

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

• 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.

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

Thanks :-)

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

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

Cheers, James Arthur

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.

ry

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

ry

up

is

uting the 3 phases, maximizing the trace thickness

We have a total of about 40mohm trace resistance accross the entire PCB, wi th about 25A rms currents, which translates to approx. 20W loss. Some addit ional resistance is due to connectors, but that is out of my hands

I am running about 20mm wide trace on 3 layers. Each layer has 25A current from a phase.

It is a combination of 70u on outer layers (to allow for fine pitch devices ) and 105u on inner layers (total of 4 layers). So a mix of 2 and 3 Oz.

I think the jumpers may be a good idea. Need to find something cheap for th at. On the other side, increasing to 6 layers avoids the use of leaded asse mbly, which can be the same price as the cost of 2 extra layer

Regards

Klaus