pcb wire

[fifahaywire]

i'm using eagle to make my pcb. i'm doing a bridge rectifier (input 240Vac),
a few questions..

-do i need a fuse at the input? but measuring the input current it doesn't go up much.
-what's the proper width for the wire traces? is 0.4mm fine?
-for the input..can i use this connectors? View attachment 63588 or should i use something else?

thanks!

 

[kubeek]

The questions you ask don't make me too confident that you should be playing with mains.
You MUST! use fuse especially if you're building something on your own. Also you should use GFCI to protect you from electrocution.

The width of the traces depends on the current you're using - i.e. the load and the bulk capacitor size.
The much more important factor is the DISTANCE between the traces. You should have at least 5mm between a mains wire and anything else. This also means that the connector needs to have 5.08mm pitch and not the more common 2.54, so you should not use the terminal blocks you posted, unless you take out every other pin.

 

[panic mode]

mains? it's 240VAC, what's the worst that can happen? ZZZZZAPPP!!!

joke aside, kubeek is absolutely right...

cross section of conductor and to some degree it's shape (ability to radiate heat) determine it's ampacity.
standard copper clad boards have 1oz of copper per square ft (but you can get 0.5, 1, 2, 3, 4 oz/ft^2). in metric, i think it works to some 35um of thickness (too lazy to look it up or calculate).
anyway, IF the thickness IS known, all it is left is width of the trace. there are charts, tables and programs that can do the calculation for you. it is good if they follow some standard like IPC2221 for example. Recent version of KiCad sports such calculator tells me that at 5A and copper thickness of 35uA and 10degC temperature raise, trace width of outer trace is 2.77mm.
inner traces have worse cooling and therefore required width here is greater (7.2mm).

if the traces are not coated, you can increase thickness by soldering some wire to it (or just use solder itself) to increase cross section.

as kubeek mentioned, you should look for PCB terminals with 0.200" or 5.08mm pitch (or greater).
voltage ratings require clearance between traces. if the board is not coated, additional clearance is required etc.
for your application if board is cleaned and uncoated traces can be as close as 1.25mm if board is used at elevation up to 3000m
above that clearance requirements increase a lot (~ tenfold...) so coating is again better option.

using present info trace width of 2.77mm and clearance of 1.25mm we get minimum pitch of 4.02mm, therefore 5.08mm terminals (0.2") would do here.
if we wanted 10A, then we get 7.2mm trace width for outer layers and 18.7mm for inner. obviously this is too much for selected terminals in this case boards with thicker copper would be needed.

 

[fifahaywire]

mains? it's 240VAC, what's the worst that can happen? ZZZZZAPPP!!!

joke aside, kubeek is absolutely right...

cross section of conductor and to some degree it's shape (ability to radiate heat) determine it's ampacity.
standard copper clad boards have 1oz of copper per square ft (but you can get 0.5, 1, 2, 3, 4 oz/ft^2). in metric, i think it works to some 35um of thickness (too lazy to look it up or calculate).
anyway, IF the thickness IS known, all it is left is width of the trace. there are charts, tables and programs that can do the calculation for you. it is good if they follow some standard like IPC2221 for example. Recent version of KiCad sports such calculator tells me that at 5A and copper thickness of 35uA and 10degC temperature raise, trace width of outer trace is 2.77mm.
inner traces have worse cooling and therefore required width here is greater (7.2mm).

if the traces are not coated, you can increase thickness by soldering some wire to it (or just use solder itself) to increase cross section.

as kubeek mentioned, you should look for PCB terminals with 0.200" or 5.08mm pitch (or greater).
voltage ratings require clearance between traces. if the board is not coated, additional clearance is required etc.
for your application if board is cleaned and uncoated traces can be as close as 1.25mm if board is used at elevation up to 3000m
above that clearance requirements increase a lot (~ tenfold...) so coating is again better option.

using present info trace width of 2.77mm and clearance of 1.25mm we get minimum pitch of 4.02mm, therefore 5.08mm terminals (0.2") would do here.
if we wanted 10A, then we get 7.2mm trace width for outer layers and 18.7mm for inner. obviously this is too much for selected terminals in this case boards with thicker copper would be needed.

yes, but im working with a low ac voltage first just to see how it'll turn out. im using a testboard.

as for the connector. i measure and true enough the one i have is 5.08mm. i took the picture in google because i didn't have the connector with me.