On Sat, 25 Oct 1997 16:05:26 +0800, you wrote:

>Can any of you let me know the 'typical' drill sizes you are using for your PCB designs.
>
>The last time I drilled any boards was about 10 years ago, and I haven't the faintest idea what size the bits were after all these years...
>
>The holes that I'm most interested in are -
>
>        'Standard' DIL IC pins (no socket)
0.8mm
>        Axial components e.g. 1/8 watt resistors
0.8mm
>        0.1" male IDC (Berg) headers
1.0mm
>The application will eventually be on double-sided plated-through fibreglass.
>
>I would also be interested to know the pad sizes you are 'normally' using with these drill sizes for 'easy' hand assembly and soldering...
0.8mm : 65 mil ( you can get a 12.5 mil trace between)
(50 mil for vias)
1.0mm : 75 mil, or larger if space allows, especially on single layer
(for mechanical strength)
>Many thanks
>MC
All the above sizes are for both hand etched/drilled boards (Laser
print/UV) and production runs.
Default minimum trace width 12.5 mil, 20 mil where possible (allows
for more defects). 10 mil is possible with laser/UV handmade PCBs
Trace density at 12.5mm width 40/inch (i.e. 25 mil grid) 

Remember that number of different hole sizes affects board cost, and
you may have to use different components in the future - you can use
0.6mm for some resistors and ICs, but if you change supplier, or
decide to socket you may have a problems. The vast majority of my PCBs
only use 0.8, 1.0, 1.2 (for terminal blocks, big diodes etc.) and 3.5
(mounting), occasionally 1.5 for transformers & SMPS inductors (in
which case I use 1.5 for terminal blocks etc as well to reduce number
of sizes.