Searching \ for '[EE] Through Hole pad size?' in subject line. ()
Make payments with PayPal - it's fast, free and secure! Help us get a faster server
FAQ page: www.piclist.com/techref/index.htm?key=through+hole+pad
Search entire site for: 'Through Hole pad size?'.

Exact match. Not showing close matches.
PICList Thread
'[EE] Through Hole pad size?'
2012\05\06@075811 by Electron

flavicon
face

Hello,
what is the typical/standard size for a circular pad surrounding a hole of X mils, to get maximum reliability?

It doesn't make sense to make it too large though, so I'm asking if there's some widely accepted pad size formula (e.g. pad diameter = hole diameter + 16 mils).

Thanks,
Mario

2012\05\07@030824 by William \Chops\ Westfield

face picon face

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

2012\05\07@074139 by Spehro Pefhany

picon face
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

More... (looser matching)
- Last day of these posts
- In 2012 , 2013 only
- Today
- New search...