Post by thread:Re: [EE] Through Hole pad size?

On May 6, 2012, at 4:58 AM, Electron wrote: > what is the typical/standard size for a circular pad surrounding a hole of X mils, to get maximum reliability? Well, "obviously" the width of the ring of copper around the hole should be at least as wide as the minimum track width of the PCB process being used. So if your have an 8mil design requirement for track width, you'd get padDiameter = holeDiameter + 16mil. Add on tolerance factors for drill position and consider whether some inexperienced human is going to be poking at it with a hot soldering iron, and you frequently get limited by lead spacing and how many tracks (and of what width) you want to fit between the leads. In EAGLE, for a hobbyist design and hand-soldering, I usually increase the "minimum" "RestRing" DRC parameter as much as I can without violating "clearance" DRC parameters. BillW

At 03:08 AM 5/7/2012, you wrote: >On May 6, 2012, at 4:58 AM, Electron wrote: > > > what is the typical/standard size for a circular pad surrounding > a hole of X mils, to get maximum reliability? > >Well, "obviously" the width of the ring of copper around the hole >should be at least as wide as the minimum track width of the PCB >process being used. So if your have an 8mil design requirement for >track width, you'd get padDiameter = holeDiameter + 16mil. Add on >tolerance factors for drill position All this (and the difference between drilled and finished hole sizes) is usually covered by a specification from the board mfr called 'minimum annular ring' or 'minimum ring'. It may vary by layer and by copper thickness. For example (double and multilayer boards) Inner: 0.5oz: 5mil 1oz: 6mil 2oz: 8mil 3oz: 12mil 4oz: 15mil 5oz: 18mil 6oz: 20mil Outer: 1/ 3oz -0.5oz: 4mil 1oz: 5mil 2oz: 7mil 3oz: 10mil 4oz: 16mil 5oz: 18mil 6oz: 20mil To get the minimum pad diameter, take the nominal finished hole size and add twice the minimum annular ring. Sometimes vias are different from pads (a different drilling process may be used). The above is for plated-through holes, where the main concern is that the hole does not completely break through the side of the pad. You may choose to use larger pads for physically stressed parts (switches, encoders, pots, connectors) or heavy parts (transformers, buzzers etc.) to improve reliability. Single-sided boards generally demand much bigger pads than the minimum the process would allow, because the adhesion under the copper is all that's holding the pads on. Usually you would use large pads for heavy components, mechanically stressed components, or components with thick leads. It's not uncommon to use pads as big as 0.25" or larger for some parts. Deciding how big is best is a bit of an art- if in doubt it's best to go bigger and add a jumper or two if necessary. Cheaper materials tend to require bigger pads than good materials for the same strength. Seems like lousy processing can also weaken the adhesion. If in doubt, try to follow consumer designs subjected to similar abuse. When the pad lifts and breaks right where the trace meets it, it can become a nasty intermittent fault that is hard to see. --sp