mA per square mils - Page 1
Forum section: electronics / projects

author: Alex Eisenhut
author_rank: Super Contributor
timestamp: July 04, 2023, 07:02:00 pm
content: When doing simulated DC drop analysis on PCBs, one of the parameters is current density. I guess that's what's called ampacity in wires? But what values are good or bad? It's not something I can get a gut feel for or even what it's supposed to measure.Like of course it means part of the copper will heat more where the density is higher, but what amount am I supposed to aim for?

author: langwadt
author_rank: Super Contributor
timestamp: July 04, 2023, 07:10:04 pm
content: usually done with a calculator and the maximum allowed temperature rise

author: Alex Eisenhut
author_rank: Super Contributor
timestamp: July 04, 2023, 07:25:28 pm
content: Yeah that's what I thought too but the simulation doesn't take into account the solder on pads or the thermal mass of the PCB and the components. At least I don't think so.So would you just look up ampacity charts for wires and start there?

author: wraper
author_rank: Unknown
timestamp: July 04, 2023, 07:42:26 pm
content: Solder on the pads have barely any effect. While it will absorb the heat due to thermal mass, the effect is only temporary. Once it heats up, final temperature will be nearly the same as there is barely any surface area increase compared to bare copper. Think about a copper cube, it can take a lot of heat until it heats up, but once it's hot, it will be a really poor heatsink. Also I'm pretty sure I've seen PCB calculator taking into account copper polygons nearby.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 04, 2023, 10:08:52 pm
content: Practical values are on the order of 10 A/mm^2. Preferably use SI units, and the multiplier is specified. (Technically "square millimeters" is a derived unit, but it's trivially equal to micro square meters; you can read the multiplier as associative with the exponent i.e. milli milli meters squared.) Don't bother with that archaic junk, it only adds to the confusion.How much is acceptable depends on trace width, board conductivity, and nearby material (especially inner plane -- excellent heat spreading), and allowed temperature rise.Trace calculators assume infinite length, or at least several times the lateral spreading distance, so that the trace comes to equilibrium with its own heat flow (there's no heat flowing lengthwise in the middle).For typical copper thickness on PCB, the heat spreading distance is on the order of an inch or so. Proportional to conductivity, so, thicker board = longer distance = more heat dissipation from a given device.When you have high current densities, you're better off keeping the paths short, than trying to spread the current out into an ampacity-rated cross section, only to neck it back down again towards other components. So, MOSFETs in a motor drive: solder bus bars on top and bottom (+V/GND), stack the FETs between them (minimal distance between D/S and bus bars), and use big fat terminals to connect the motors. (Some consideration of loop inductance and turn-off rate or snubbing is also required.) The motor terminals may well prove effective heatsinking for the low side FETs (connected to drain tab), and you can add thermal vias and backside gap pad and all that for improved dissipation. (This is also assuming SMTs, probably DFNs in the 3x3, 5x6, etc. mm packages; THT you can heatsink in the usual way of course.)As for solder, you can calculate the effect. Typical HASL is minuscule (< 0.1mm?), and wave is only a bit more (say 0.2mm, depending on width and geometry). Hand soldering can get arbitrarily blobby, but it's extra labor. It's not much, as solder is like a 10 times poorer conductor than copper.But there are places where solder helps significantly. If you can arrange to fill vias with solder (i.e. you don't need masking/clearance from other nearby pads, and don't have solder thieving issues like for via-in-pad), the thermal and electrical resistance might be about halved. Most times you can just use twice as many vias or whatever, and there are a lot of places where the resulting uneven surface (solder blob on pad) might be unacceptable as well (e.g. makes it harder to apply a thermal pad), but for the remaining cases, it's interesting to have.Again regarding hand soldering, or one-offs or protos, you can fill vias as selectively and blobbily as you like, so there is that. In production, it'd be most practical for wave soldering, with certain paste reflow (paste-in-pad) or CNC processes (e.g. laser + solder wire) also being capable -- the more specialized you get, the more expensive, of course.Tim

author: hbozyq
author_rank: Contributor
timestamp: July 06, 2023, 01:56:06 pm
content: I've heard from somewhere it may tolerance around 5A/mm before it burst into fire for standard 1OZ fr4 PCB.

author: EEEnthusiast
author_rank: Frequent Contributor
timestamp: July 06, 2023, 02:52:41 pm
content: Quote from: hbozyq on July 06, 2023, 01:56:06 pmNo..I have had boards work fine with 15A/mm^2 on outer layers with exposed solder mask. There are thumb rules available from different sources which state the limits from 5A/mm^2 to 15A/mm^2 depending on the board thickness, no of metal layers, the actual layer on which the current flows and so on...Also, a 0.5 oz copper can have better current density than say 2oz copper. It may seem counter intuitive, but given that you make the traces on 0.5oz and 2oz copper with the same cross section , the 0.5oz one will have a larger width and it will dissipate more heat.

author: Siwastaja
author_rank: Super Contributor
timestamp: July 06, 2023, 06:00:32 pm
content: Also a ground plane on a 4-layer (or more) PCB is a HUGE factor, even if it's electrically a different net! This is because the prepreg is so thin, so even FR4 is quite acceptable thermal conductor at 150-200µm thickness. Most online trace width calculators ignore this heatsinking effect.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 06, 2023, 11:27:41 pm
content: Quote from: Siwastaja on July 06, 2023, 06:00:32 pmSpecifically, ignore IPC-2221 which is the older one, and use IPC-2152 which is based on somewhat newer materials and techniques (but still fairly old IIRC?).This is a reasonable one:https://www.smps.us/pcb-calculator.htmlTim

author: EEEnthusiast
author_rank: Frequent Contributor
timestamp: July 07, 2023, 05:19:12 am
content: Quote from: Siwastaja on July 06, 2023, 06:00:32 pmThe PCB Toolkit from Saturn seems to consider this effect to some extent.https://saturnpcb.com/saturn-pcb-toolkit/

author: Dave
author_rank: Super Contributor
timestamp: July 07, 2023, 08:29:11 pm
content: Quote from: EEEnthusiast on July 06, 2023, 02:52:41 pmI'm fairly certain he's talking about 5A per millimeter of trace width, not mm². With copper weight of 1 oz./sqft, that means around140 A/mm².I can see how that could result in immolation.

author: EEEnthusiast
author_rank: Frequent Contributor
timestamp: July 08, 2023, 03:00:11 am
content: Quote from: Dave on July 07, 2023, 08:29:11 pmOh yes. 5A per mm of trace width for 1oz copper is near the flash point. We typically use a thumb rule of 1A per mm (1A per 40 mils) for power supply traces on 1oz Cu