I always use a rule of thumb of 1mm per amp ( I actually lay the board out in inches, but the rule is easier to remember than 40mil/amp) . (This is 2.5A per 100mil ) So on this basis you would be limited to 2A per pin for a 0.100" pitch connector. My rule of thumb gives dT of ~ 5-10C depending on whose tables you use.
If I can't get a thick enough track to fit on the first attempt , then I start looking up the tables / graphs.
My experience indicates that proximity is an important consideration, i.e. proximity to a large island of copper, proximity to a SMD diode, proximity to another current carrying track. Also beware of putting down a serpentine track as a current sense element, it's a lot of heat packed into a small area.
One PCB (for a battery powered motor control) of mine has a 3mm (120mil) track running 3/4" between two big islands of copper. Average current around 3-4amps for maybe 2minutes operation, some returned PCB's showed evidence of heat damage (probably due to a stalled motor condition at ~ 6-8A) . The odd thing is the scorching / discoloration occured only for a short distance at the exact middle of the track, so evidentally a lot of heat is conducted back to the "islands".
I think it comes back to the aspect ratio of the "bridge" joining the "islands" , I think at 5 x width you've reached the "infinite approximation" , my hunch is that for an aspect ratio of 2:1 , you could double the current rating, e.g. with my 1A/mm rule , a bridge 5mm wide and 10mm long could carry 10Amp (rather than 5A for a long track).
A bigger problem with necking of power traces is the inductance and potential EMI issues, particularly on the ground plane. I endeavour to put in some extra bridging on another layer around the neckdown, even if I have to move some components/tracks to get that bridge in. If it's a power trace with a neckdown , then I put MLCC bypass cap to GND on either side of the neckdown.
Another trap for the unwary is the ground pin of USB connectors. Some pcb designs connect only pin4 to the gnd plane with an 8mil width track, so at the first power supply mishap on your test bench, the earth trace blows and lots of volts flow back into your PC on the remaining 3 wires. What you need to do is connect the shell of the connector to the ground plane, as the shield in the USB is good for several amps.
Rules of thumb are good for planning, but with IPC-2152 available you can push the limits with confidence. It is a very accessible document at an affordable price (when compared with many standards). Even if your company won't pay for it - buy it for your own library. Its worth it.
To people designing boards for high-speed signals, they think of power integrity differently, mostly in terms of frequency and impedance. At icrowave frequencies, things are different. You have to deal with impedance matching, signal loss in vias, reflections, balanced differential traces, skin effect, EMI, and so on. You have to deal with PCB material characteristics such as glass weave and the fact that FR4 is running out of gas at today's frequencies.
#MeasurementBlues this is true. The thrust of this series was the "what about DC" aspect. Something exciting to note is the accessibility of new tools, like In Circuit Design, which allow you to accurately model power plane impedances on your PCB layer stackup, and then see the effects of adding real capacitor models for decoupling. Watch this space...