At 10:15 PM 5/12/02 -0500, you wrote:
>Hello everyone,
>
>When creating a pad, how do you know what diameter to make the pad, given
>you know the drill size?

There are a few factors at work:

1)      You want to make the pad as small as possible, so more conductors
         can go between pads (make it easier to route)

2)      You want to make it as big as possible for mechanical strength

3)      It had better not be too big, or it might be hard to solder

4)      You don't want the PCB maker's hole centering inaccuracy to cause the
         hole to break through the side of the pad (they have a minimum spec,
         the annular ring, which you will typically do a DRC on).

5)      Pads for single-sided boards should be bigger than those for 2 or
         more layer boards due to 2). If the part is heavy, or subject to
         stress from users (eg. terminal blocks) it should be large enough to
         safely withstand the force. You may have to physicaly restrain the
         part if the pads cannot be made large enough or the part is very
         heavy or subject to much force of other kinds.

6)      You should also consider that the drill size you call out may (or
         may not) be nominally equal to the final hole size.

For example, if you are designing a board where one conductor will go between
0.1" pitch pads, and the hole is to be 0.032 and the trace and space width
0.015", then the pads should be 0.1 - 0.045 = 0.055" diameter and the annular
ring is 0.0125".

If you are not sure, one way is to emulate a professionally designed board
that you feel is well made.

Best regards,

Spehro Pefhany --"it's the network..."            "The Journey is the reward"
speff@interlog.com             Info for manufacturers: http://www.trexon.com
Embedded software/hardware/analog  Info for designers:  http://www.speff.com
9/11 United we Stand

--
http://www.piclist.com hint: PICList Posts must start with ONE topic:
[PIC]:,[SX]:,[AVR]: ->uP ONLY! [EE]:,[OT]: ->Other [BUY]:,[AD]: ->Ads