FEDEVEL
Platform forum

Sniper2 , 05-21-2024, 06:20 PM

So there is this trace net that will need to carry 70A max and i was wandering what is a safe minimum ( also related to the last video i saw).
the 5mil trace was ok aqt 1A so extra interpolating it is 8.9mm lets say 10mm bare minimum.

Saturn PCB designer mentions with 10mm that i will drop .45W over 30mm length + there is also the conductor current metric in the bottom right that is 19A but i am not sure what is supposed to be /mean ? is that the IPC 2152 current rating?
also what is better to use IPC2221 or that 2152?

Realisticaly ill use /go as wide as i can but i am not sure what is an acceptable minimum .
NOTE: 70A is max+ safetymargin and it is worst case scenario too for continuous load maybe a few hours max then way less even that not sure how realistic is. But i got to math out worst case of all stuff.
Can anyone give me a bit of real world ok situations + sizes ?

QDrives , 05-22-2024, 09:20 PM

Current carrying capabilities depend on many factors:
- Inner or outer layer
- Trace width
- Trace thickness
- Allowed temperature rise
- Frequency of signal (skin depth)
- Cooling capabilities
- Plane presence (also a cooling or heatsink capability)
- Ambient temperature
- Dielectric used
IPC 2152 is the more accurate one.
PCB toolkit, 20mm wide, outer layer, 105um (70um+18um), plane present (2oz & 0.1mm distance), DC, FR4, 22°C ambient gets 58°C warmer for ~70A.

Sniper2 , 05-23-2024, 05:48 PM

ok now it raises the question how i for 10mm as fine whit 1oz cu

Sniper2 , 05-23-2024, 05:48 PM

i am doing something very wrong

Mini , 05-23-2024, 06:56 PM

Can you share screenshot? I'm getting around 40A with 1 oz copper on outer layers and with 2 oz around 60A when temperature rising 58 degrees over ambient

Mini , 05-23-2024, 06:56 PM

Screenshot of PCB toolkit i mean

Mini , 05-23-2024, 06:58 PM

I don't know your options, but if possible I would add copper plates over tracks if possible or add some heatsink or at least cover with some solder. These methods improve current capability a lot. Not really sure how to calculate, I personally just order prototype and test.

Sniper2 , 05-23-2024, 06:59 PM

well it is geting it as close as i can

Sniper2 , 05-23-2024, 06:59 PM

i want to remove mask then solder 10-6 AWG wire over pour if needed

Sniper2 , 05-23-2024, 06:59 PM

first time dealing with this high of a current

Sniper2 , 05-23-2024, 07:00 PM

then again it is worse ever possible

Mini , 05-23-2024, 07:02 PM

Just do as wide tracks/polygons as possible. Order prototype and test.

Sniper2 , 05-23-2024, 07:04 PM

That is the plan anyway

QDrives , 05-23-2024, 10:10 PM

Do note that "2 oz" is about 35um base with 18um plating.
But more importantly, do you use the IPC-2221 mode (outdated)? (Tools / program options).

QDrives , 05-23-2024, 10:25 PM

"or at least cover with some solder. These methods improve current capability a lot." -- actually this one (cover with solder) does not do a "lot", it does help a bit. However, the amout of improvement is relatively lower the thicker copper you use.
Either Robert made a video about it or Dave Jones. I guess it was a 'simple' board and would have had 35um (1 oz) copper.

Mini , 05-24-2024, 12:24 PM

Yes obviously covering with solder can't help too much, maybe should of been more specific. You obviously can't add a lot of solder either. But it does help a little. I meant mainly adding extra copper bars over the traces or adding heatsink. I personally added big copper bars over the traces and it helped obviously a lot. I have also seen people using soldering wick over the traces.

Mini , 05-24-2024, 12:31 PM

I chose no plating that's where our difference came. Thanks. 1 oz is still only 52A. 2 oz is very expensive. And temperature rise by 58 degrees is a lot in my opinion. OP seems to want 1 oz as well. So must add something over the traces/planes to give extra headroom.

Sniper2 , 05-24-2024, 01:48 PM

Yea

Sniper2 , 05-24-2024, 01:48 PM

Also I have 4l at least

Sniper2 , 05-24-2024, 01:48 PM

Might dedicate 2 maybe 3 for this large current

QDrives , 05-24-2024, 09:13 PM

How many units do you want to produce?
If it is only a few, then the measures you mention can be done. However, not for mass production.
Yes, I know 58°C temperature rise is a lot. However, not many boards can have traces wider than 20mm too.
@Mini I do not see how you get 52A with 1oz?
And 2oz is not very expensive (for the outer layer). It is a standard 35um and plating. Thicker copper (>= 105um, 3oz) or >= 70um (2oz) for the inner layers is more expensive.

Sniper2 , 05-24-2024, 09:27 PM

not sure atm 2-5 prototypes to develop and test

Sniper2 , 05-24-2024, 09:27 PM

i can expand later if needed

Sniper2 , 05-24-2024, 09:28 PM

thing is that those areas will be sort of small and there will be some cooling due to the rest of the board

Mini , 05-25-2024, 12:56 PM

I used all your options and just chose 35 um as base copper weight.

QDrives , 05-25-2024, 01:35 PM

Smoke will tell you if it is to thin.

Mini , 05-25-2024, 02:51 PM

That's always true I guess. I personally design with a lot of overhead... And in the end best is to try out yourself.

Mini , 05-25-2024, 03:10 PM

Was just looking JLCPCB and it should be 35 um base copper weight + 18 um for plating thickness... which means 53 um not 70 um. But I guess they are very cheap as well.

Sniper2 , 05-25-2024, 05:18 PM

2oz and more are boing to be a pain when dealing with the SMD parts

Sniper2 , 05-25-2024, 05:18 PM

main aim is to keep is at 1oz and use 2-3 layers for this

Sniper2 , 05-25-2024, 05:19 PM

i would rather make the pcb wider

Mini , 05-25-2024, 09:20 PM

I did exactly same, mainly because if you don't have room constraints there is no reason to pay extra.

Sniper2 , 05-25-2024, 09:27 PM

ha same

QDrives , 05-26-2024, 08:14 PM

A 35um (1oz) outer layer copper board is made from 18um base copper + plating (minimum 18um).
For 70um, the base copper is 35um (theoretical) and plating. Yes, you get something like 55um...60um in reality.

Mini , 05-27-2024, 11:41 AM

If that's true then it sucks even more. I wrote to JLCPCB as well to confirm that. Is plating thickness same on 1 oz and 2 oz (18 um)? 18 um is kind of low btw, but i guess they are cheap as well because of that.

Mini , 05-27-2024, 02:38 PM

I got the answer from JLCPCB.

Mini , 05-27-2024, 02:38 PM

Mini , 05-27-2024, 02:39 PM

It seems to be 35 um + 18 um so 53 um in total. For 2 oz i assume 70 um + 18 um, but can ask to confirm that.

Mini , 05-27-2024, 02:39 PM

Anyway for 2 oz price difference is quite big depending on board size.

QDrives , 05-27-2024, 02:47 PM

That makes doing controlled stack-up a lot more difficult (do note this is not controlled impedance).

Mini , 05-27-2024, 02:51 PM

Do you mean for us to design with controlled impedance or for them to produce PCB-s? Can you explain a bit what you mean by that?

Sniper2 , 05-27-2024, 04:00 PM

how if u know how it works u can math it out

QDrives , 05-27-2024, 08:41 PM

With controlled impedance the board fabricator changes things to get the correct impedance of traces. With controlled stack-up, the designer specifies the stack-up in detail and assumes the fabricator produces it that way. The last is a little cheaper as the fabricator does not need to 'correct' things.
However, if the copper is thicker than specified (53um and not 35um) the impedance calculation is not correct.

Besides in the answer from JLCPCB - 18um is the IPC minimum for plating within the vias. On average it is closer to 25um on top of the traces. Base copper would be more like 30um. This leaves you with about 55um.

Mini , 05-27-2024, 09:15 PM

I have usually chosen impedance control on JLCPCB and put their numbers in. I could simply rise outer layers thickness from 35 um to 53 um, but not sure is it good if they give under parameters outer layer thickness as 1 oz. So indeed I guess calculation are a bit off?

Mini , 05-27-2024, 09:20 PM

I just checked and it is kind of hard to choose 53 um when only options are 35 um and 70 um under JLCPCB impedance calculator. Although in Altium I can choose any copper thickness I want.

Sniper2 , 05-28-2024, 04:13 AM

U can also chose in kicad

Sniper2 , 05-28-2024, 04:13 AM

Devboard in 4L 1oz but is like half the current I would need but also has half the fets placed