Express PCB pads - crap

[Simon]

I've just been looking at the pad sizes in expressPCB and measuring up the real parts, it looks like all the holes are like 150% the real max diameter of the pin on the parts. Now what's the point in that ? it will result in awful soldering jobs infact the couple of boards I have done i thought surely it should not be this bad to solder ? well thats why, I'm now redoing all my parts with smaller than the pin holes to ensure i have enough "soldering land, if anyone wants the foot prints let me know and I'll email them over

[mikeselectricstuff]

A general guide for normal hole sizing for thru-hole boards :

DIPs and wire-ended parts :0.8mm
Square-post headers, TO-220 legs : 1.0mm

For DIPs, you can go down to about 0.6mm, but in practice the only time you need to go below 0.8 is if you really need a smaller pad size due to track density, otherwise stick to 0.8. 

Hole size is less of an issue on through-plated PCBs ast the solder will fill the hole pretty much whatever size it is.

You don't went the holes to be anything like a tight fit as it gets much harder to insert components, and also to unsolder them - unsoldering a tight-fitting lead in a plated hole without damaging the plating is pretty much impossible.

[Simon]

my thoughts are that regardless of actual hole diameter in the board the hole in the copper pad should be small so as to ensure that when drilled there definitely is copper around it

[JohnS_AZ]

Holes 150% of the lead thickness doesn't sound out of line. Consider that the IPC standards presume the board will be assembled with automated equipment (where a little slop is a good thing) and then wave soldered.

[Simon]

yea i suppose with wave soldering it won't be an issue but the last board i did was a right pain in the but because i did holes to suit leads and did not have very much to solder too, infact the vibration broke a track

[mikeselectricstuff]

my thoughts are that regardless of actual hole diameter in the board the hole in the copper pad should be small so as to ensure that when drilled there definitely is copper around it

Yes - here there is a difference between homemade PCBs and those intended for production - the former need holes in the artwork for centering when hand-drilling, and these need to be smaller than drill size. However if you then send the same PCB for production the hole sizes need to be right, but no pad holes are needed as PCB houses have accurate drills that don't need centre marks. PCB software typically doesn't put pad holes in gerber output anyway.

The way I handle this is do design the board with correct drill sizes, but when laser printing, I change all hole sizes to 20mil (and remember NOT to save the modified version afterwards!).
A useful facility, which may or may not exist in some PCB packages, would be to be able to specify a fixed hole size for printouts.