layer stack for 20Amperes DC current

[flote21]

Hi guys!!

I need to design a PCB board with a very particular feature. It has to supply a bridge of FANs and the current consumption is going to be around 20Amp. I am going to do the routing with Altium Designer and my question is how thick should the board to support 20Amp and if it is better to route the power lines with track or it is better to use a big polygon?

Thanks in advance!

 

[andre_luis]

Just opening the PCB solder allow to reduce the calculated width of copper track required for that routing.

 

[FvM]

Saturn PCB Toolkit calculates temperature rise for different trace widths and plating thickness based on IPC rules. You get e.g. about 10 mm (400 mils) wide trace or polygon for 35 µm (1 oz) plating and 40 K rise. Standard 20K would require 15 mm. If size matters, you may want to switch to 70 µm (2 oz) plating.

 

[marce]

Just opening the PCB solder allow to reduce the calculated width of copper track required for that routing.

No this is bad and outdated advice, calculate the copper required properly and do the job properly... Many boards are not wave soldered, you cannot guarantee how much solder is going to be deposited and solder has far less current carrying capacity than copper!
For 20A a 2oz (70micron) copper foil is recommended...

 

[andre_luis]

No this is bad and outdated advice

In fact, I have to agree that could be considered outdated due to distinct processes currently adopted by different PCB manufacturers, but I was curious to know if there is some drawback on doing that. Whichever the finishing or its thickness, certainly the final conductivity will be somewhat greater than just the original copper, or not ?

 

[marce]

The solder is far less conductive than the copper also controlling the amount of solder on the track is hard to do so I would look for any other alternative, even in t'old days I would never do this as I always considered it a bit dodgy, today with all the rules and regulations and the fact that if anything goes wrong you can be sued or worse I always work out the capacity for copper only and only ever use a 10deg C rise above ambient...

 

[NIKHILRAJ]

if you can not use wide trace with enough copper thickness , then why cant you go for PCB bus bars ?

 

[ArticCynda]

First of all, select 2 oz (70µm) copper thickness for the board, then decide what the maximum allowed voltage drop over the traces is, and finally calculate the trace width accordingly. Pulling back the solder mask from the trace will allow it to dissipate heat easier and, if you're wave soldering, will make for a nice solder layer along the entire length of the trace to increase conductivity.

 

[marce]

4 or 6 ounce copper would be better for the high current layers, both available these days with no problems.

 

[FvM]

4 or 6 ounce copper would be better for the high current layers, both available these days with no problems

Available yes, but only suitable for designs that get along without fine pitch components.

 

[marce]

Done mixed 2 and 4 ounce on the same layer (selective plating), or have 2 oz outer layers and heavier layers inside for current, again done that as well as 1oz outers and 2 and 4oz inners....