Ken,
There are manufacturability reasons for both dimensions. It is not
uncommon for small caps and resistors to pull to the center of one of their
respective pads. This can result in an open if the component pulls far
enough away from the opposing pad; and often results in tombstoning if the
pull gets just enough torque to lift the lead away from the solder on the
opposing pad. Moving the two pads closer together is the safest and easiest
way to prevent tombstoning. This is because when one side of the cap or
resistor is pulled towards a pad due to different wetting speeds, the
opposite end of the component will still remain squarely on the opposing
pad, allowing the small amount of surface tension on the slower wetting
termination to resist the torque of surface tension on the pulled side. To
prevent tombstoning, the centerline of the pads should match the centerline
of the component termination.
It is also not uncommon for solder paste to get squeezed underneath a
component when it is placed on the board. When this happens, it often
occurs that the squeezed solderpaste does not coalesce into the molten
solder comprising the joint. Instead, the squeezed solderpaste emerges from
underneath as a free-floating solder ball, sometimes called a squeeze-ball.
One common method of preventing this is to use a home plate design on the
solder-paste stencil. The home plate design is intended to reduce the
amount of solder-paste that can get squeezed underneath the component. An
alternate method of reducing the amount of solder paste underneath the
component is to move the two pads farther apart so the ends of the component
just touch the solder paste.
As you can see, the reason behind the two different dimensions depends on
the point of view a person is coming from. My personal point of view is to
put the pads close together, and put the solder-paste stencil openings
farther apart (the stencil guys hate me), solving both problems.
Another reason behind pad farther apart is for wave soldering as you
implied. With wave soldering, it is often assumed the component will be
glued first; thus preventing it from pulling to one side on another. Having
the pad reach under the component serves no purpose, so the pads can be
farther apart, allowing a larger surface to catch solder from the wave.
I hope this helps
Thanks
Ryan Grant
Advanced Technology Engineer
MCMS
(208) 898-1145
[log in to unmask]
> -----Original Message-----
> From: Ken Patel [SMTP:[log in to unmask]]
> Sent: Friday, November 17, 2000 1:03 PM
> To: [log in to unmask]
> Subject: [TN] Designer/Assembler: Need help on 0603 spacing problem.
>
> Designer/Assembler,
> I was surprised to see 35 mil spacing between pads of 0603. Looking the
> IPC-SM-782 that number is 24 mils. Why such as difference? Does any user
> aware of requiring 35 mils spacing for 603 cap using any standard foot
> print
> library? What is the spacing being used for reflow and wave for 0603 caps.
> Can Assembly house shall catch this kind of problem across the board
> during
> prototype? And how difficult is that job or is it almost impossible, I
> mean
> using any program as later on design engineer said that they never
> complained before and why now!
> I still have to contact my layout house yet on his foot print selection.
> re,
> ken patel
>
> --------------------------------------------------------------------------
> -------
> Technet Mail List provided as a free service by IPC using LISTSERV 1.8d
> To unsubscribe, send a message to [log in to unmask] with following text in
> the BODY (NOT the subject field): SIGNOFF Technet
> Search previous postings at: www.ipc.org > On-Line Resources & Databases >
> E-mail Archives
> Please visit IPC web site (http://www.ipc.org/html/forum.htm) for
> additional
> information, or contact Keach Sasamori at [log in to unmask] or 847-509-9700
> ext.5315
> --------------------------------------------------------------------------
> -------
---------------------------------------------------------------------------------
Technet Mail List provided as a free service by IPC using LISTSERV 1.8d
To unsubscribe, send a message to [log in to unmask] with following text in
the BODY (NOT the subject field): SIGNOFF Technet
Search previous postings at: www.ipc.org > On-Line Resources & Databases > E-mail Archives
Please visit IPC web site (http://www.ipc.org/html/forum.htm) for additional
information, or contact Keach Sasamori at [log in to unmask] or 847-509-9700 ext.5315
---------------------------------------------------------------------------------
|
