Synth-DIY Yahoo! Groups Archives

Thread

What pad size?

2005-12-30 by alan00463

I am about to layout my first homemade PCB,
using Eagle 4.16 Light. My circuit will
include:

small transistors - 2N3904 and 2N3906
quarter-watt resistors
half watt resistors
small diodes
large diode
small LEDs
N.O. pushbutton switches

What size pads should I make for these components?
I read on the web that the ** minimum ** pad should
include a 5 mil annulus (ring) around the component
leads. But I don't know what the diameter of the
leads are for these components. So let me ask you
what size pads have you found to work well for these
through-hole parts?

Alan

Re: [Homebrew_PCBs] What pad size?

2005-12-31 by JanRwl@AOL.COM

In a message dated 12/30/2005 10:33:49 P.M. Central Standard Time,
alan00463@... writes:

pad should
include a 5 mil annulus (ring) around the component
leads. But I don't know what the diameter of the
leads are for these components.

This ring-width would be OK perhaps for VERY compact lead-spacing where the
board has ALL plated-through-holes ("PTH").
5 mil is only about twice the width of a thinner human hair! The hole must
be drilled 5 mil LARGER for PTH, as the plating and solder-coating fills in
the holes about that amount. For home-brew, NON-PTH, go for 0.08" or more, or
at least 0.065 for IC's.

[Non-text portions of this message have been removed]

Re: [Homebrew_PCBs] What pad size?

2005-12-31 by Mike Young

----- Original Message -----
From: "alan00463" <alan00463@...>
To: <Homebrew_PCBs@yahoogroups.com>
Sent: Friday, December 30, 2005 3:50 PM
Subject: [Homebrew_PCBs] What pad size?

>I am about to layout my first homemade PCB,
> using Eagle 4.16 Light. My circuit will
> include:
>
> small transistors - 2N3904 and 2N3906
> quarter-watt resistors
> half watt resistors
> small diodes
> large diode
> small LEDs
> N.O. pushbutton switches
>
> What size pads should I make for these components?
> I read on the web that the ** minimum ** pad should
> include a 5 mil annulus (ring) around the component
> leads. But I don't know what the diameter of the
> leads are for these components. So let me ask you
> what size pads have you found to work well for these
> through-hole parts?

The library package definitions will already define hole sizes. For example,
the transistors already "know" that the TO92 holes should 32 mil. Be
generous with pad restring since you're drilling manually. Allow yourself at
least half the drill radius. My default rule set has 70%, I think, and a
large enough max size to accommodate.

Set your drill sizes with Options|Set|Drill. Just click OK to accept the
sizes. Run drill-legend.ulp to create and populate a drill legend layer.

Pulsar www.pulsar.gs sells a white film that sticks to the toner, to
simulate white silkscreen. Transfer the silkscreen toner to the etched
board, and then laminate the white transfer sheet.

Re: [Homebrew_PCBs] What pad size?

2005-12-31 by Stefan Trethan

There is only one valid answer to that question: plated through holes or
not?
If you have the PCBs made with plated holes the 5 mil might be enough,
since the "barrel" inside the hole rivets the two sides together.

If you make your boards yourself, or don't have pth you need MUCH larger
pads.
Remember, not only is it for electrical connection but more importantly as
a mechanical mounting for the component.

What i have found to work well:
For 100mil spaced DIL ICs i use oblong pads of 1.6mm x 4mm.
This allows for a trace between pads (4x2 fits well if there is no trace
needed in between). Run all traces in in the direction of the pads, if you
connect to a corner pin too. If you run in from the side the trace will
terminate exactly where the hole is. If the hole is a bit off center you
can drill off the trace and not notice. I had such a fault keeping me
searching for hours, so ALWAYS run the trace into one of the ends of the
pad.

Use the same oblong pads for headers, but offset to one side on dual-row
headers so they don't short in the middle, and make the pads wider since
the pins of headers are drilled larger.

For resistors absolute minimum is 2mm round, preferrably more. The larger
the component the larger the pad. Most transistors get 4x2mm or 4x1.6mm
too. Remember to give caps larger pads as well, they are often the highest
parts and thus most stressed.

So, you see, i make the pads as large as i can often having to use oblong
shapes because the spacing will not tolerate large enough round pads. i
have lifted enough pads in the early days to have learnt that lesson.

If a component is not pressed against the top of the PCB to prevent
pushing forces on the pad it must be huge, avoid that. Use spacers and
such if you put like LEDs in a elevated position.

ST

On Fri, 30 Dec 2005 22:50:19 +0100, alan00463 <alan00463@...> wrote:

> I am about to layout my first homemade PCB,
>
> using Eagle 4.16 Light. My circuit will
>
> include:
>
>
> small transistors - 2N3904 and 2N3906
>
> quarter-watt resistors
>
> half watt resistors
>
> small diodes
>
> large diode
>
> small LEDs
>
> N.O. pushbutton switches
>
>
> What size pads should I make for these components?
>
> I read on the web that the ** minimum ** pad should
>
> include a 5 mil annulus (ring) around the component
>
> leads. But I don't know what the diameter of the
>
> leads are for these components. So let me ask you
>
> what size pads have you found to work well for these
>
> through-hole parts?
>
>
> Alan
>
>

Re: What pad size?

2005-12-31 by bob_ledoux

Don't press the limits when making your first board. As experience
builds you will learn just how fine your construction techniques can go.

I've seen commerically prepared boards, intended for amateur
construction, with extremely small through hole pads. This invites
builders with limited experience, and big soldering irons, to lift traces.

When making simple through hole boards my basic rule is to make
everything big. I like .080 diameter pads, they provide enough
clearance to avoid contact between two .100 spaced pins. This gives
plenty of soldering surface and reduces chances of lifting the pad
with heat. For simple boards like this I also like traces .050 wide.
These are very forgiving of excess etching. Why etch away more
copper than you need to?

Leave the hole in the pad center so the drill can center on the etched
out hole.

If you pass traces between .100 spaced pins the pads need to be
reduced. I reduce the pad size, make it rectangular, and generally
use about a .015 wide trace between the pins.

The whole design concept changes when making surface mount boards.
Much less surface area, and less soldering heat, is required when you
don't pass a wire through the board.

--- In Homebrew_PCBs@yahoogroups.com, "alan00463" <alan00463@y...> wrote:
>
> I am about to layout my first homemade PCB,
> using Eagle 4.16 Light. My circuit will
> include:
>
> small transistors - 2N3904 and 2N3906
> quarter-watt resistors
> half watt resistors
> small diodes
> large diode
> small LEDs
> N.O. pushbutton switches
>
> What size pads should I make for these components?
> I read on the web that the ** minimum ** pad should
> include a 5 mil annulus (ring) around the component
> leads. But I don't know what the diameter of the
> leads are for these components. So let me ask you
> what size pads have you found to work well for these
> through-hole parts?
>
> Alan
>

Re: [Homebrew_PCBs] Re: What pad size?

2005-12-31 by Stefan Trethan

On Sat, 31 Dec 2005 15:26:33 +0100, bob_ledoux <bobledoux@...>
wrote:

>
>
> The whole design concept changes when making surface mount boards.
>
> Much less surface area, and less soldering heat, is required when you
>
> don't pass a wire through the board.

And, usually, the forces on the pads are much smaller. A 1206 resistor
doesn't pull much, even of you apply a insane amount of G's.
OTOH i don't quite trust SMD connectors and stuff, i still make those
throughhole. They might just come off if abused.
Pads usually only lift during repair/rework anyway if the thing is
designed properly never during normal use.

When i repaired a mobile phone not long ago i found a 8 pin SMD IC ripped
off the PCB and stuck to a piece of foam applied to the back cover.
Apparently the glue holding on the foam had soaked through, and stuck the
SMD to the back cover better than the pads to the board.
Was only a comparator used for detecting the presence of a headset and
instead of hunting down the right traces and wiring it in again i just
hardwired the phone for no headset.

ST

Re: What pad size?

2005-12-31 by alan00463

Thank you, Bob, Mike, Jan, and Stefan for the info. on pad sizes.
I've taken notes that I will refer to when I make the artwork.

Of course, I know we were talking about ***minimum*** pad and trace
sizes. I will certainly enlarge their widths if ample board "real
estate" exists.

Alan

Re: What pad size?

2006-01-03 by aleph_and_torasu

> Use spacers and
> such if you put like LEDs in a elevated position.
>
> ST

Where's a good place to get those? My LEDs look like wobbly spider legs.

Re: [Homebrew_PCBs] Re: What pad size?

2006-01-03 by David Griffith

On Tue, 3 Jan 2006, aleph_and_torasu wrote:

> > Use spacers and
> > such if you put like LEDs in a elevated position.
>
> Where's a good place to get those? My LEDs look like wobbly spider legs.

Mouser has standoffs in many different sizes.

Try a pair of popsicle sticks clipped or glued together, especially for
several LEDS in a row. Stacked fragments of perfboard also work well.

--
David Griffith
dgriffi@...

A: Because it fouls the order in which people normally read text.
Q: Why is top-posting such a bad thing?
A: Top-posting.
Q: What is the most annoying thing in e-mail?

Re: [Homebrew_PCBs] Re: What pad size?

2006-01-03 by Wayne Topa

aleph_and_torasu(robline@...) is reported to have said:

> > Use spacers and
> > such if you put like LEDs in a elevated position.
> >
> > ST
>
> Where's a good place to get those? My LEDs look like wobbly spider legs.

Maybe <http://www.allelectronicd.com>

search for part # HLED-3 or HLED-4 (5mm Led) or HLED-5 (3mm)

Other then that, I don't know.

Wayne