Jack,

Regarding number 3 below, we still see evidence of heat-sinking due
to copper density in surface mount boards.  However, this effect has
been greatly reduced since the introduction of forced-convection reflow
ovens.  (5 years ago, when infrared ovens were prevalent, this was a
serious problem.)  At present, this effect is usually limited to very small
chip components (e.g. 0402 and 0603 chips).

Here's an example:  Let's suppose you have an IC with several adjacent
leads/lines that need to be terminated.  So you place a row of capacitors
parallel to the leads on the IC.  You bring traces from the leads to one
side
of the capacitors.  On the other side of the capacitors you have two
choices:
you can drop individual vias to your closest plane for each capacitor or you
could drop a single via to the plane and bus all of the capacitors to that
via.

If you choose to bus the capacitor pads together, you will see this heat
sink
effect.  The pads that are bussed together create a small heat sink and the
pads that are connected to the IC will begin to reflow first.  The surface
tension
of the solder during reflow exceeds the amount of force required to
tombstone
0402 or 0603 chips.

Again, the effects of heat-sinking due to copper are greatly reduced when
using forced convection ovens.  But these effects can still be seen when
using
0402 and 0603 chips.  Imagine what fun we'll have with 0201 chips...

Brad
Circle M



 ----------
>From: owner-designercouncil
>To: DesignerCouncil
>Subject: Re: [DESIGNERCOUNCIL] Connections from land patterns

>> JoAnn Amerson wrote:
>> > I was told that it is best to limit the number of tracks leading
>> > to/from a pad to one.  Two at the most and three is highly
>> > discouraged.  Can anyone verify this for me?  Are there any specs
>> > that apply?  I asked a fellow designer and he'd never heard it
>> > before either.
>>
>> Well, I thought you would get some good answers so I wasn't gonna
>> jump on this one, but so far you have recieved some confusing and
>> conflicting messages and I kinda feel sorry for you...
>>
>> I'm no expert (just a lowly layout guy) but the way I see it:
>>
>> I agree that you should TRY to limit to one connection per pad for
>> SMT connections, but its not so important for through hole.
>> There are several reasons, and I'm not sure which would be most
>> important, but consider:
>>
>> 1) There is a limited amount of solder paste squeegeed (sp?) onto
>> each pad. As the solder melts, it will tend to "bleed out" onto
>> the trace that is attached to it. The more connections you have,
>> the less volume of solder fillet is connecting the lead to the
>> pad. You want all the paste to stay between the pad and the lead,
>> the more the better in the case of SMT, because besides being an
>> electrcal connection, its all that is holding the part on the
>> board in most cases (a mechanical connection). The soldermask
>> itself will help, naturally, but don't give that limited amount of
>> solder too many places to go, ok?
>>
>> 2) Imagine what the solder is going to do when it melts. It has a
>> "surface tension" like a drop of water. If there are NO traces on
>> the pad you will see a beautiful perfectly formed solder fillet,
>> you can see this if you look at the pins of a component that is
>> not connected (many ICs have unconnected pins). Pins that have one
>> trace coming out the end are nice too, especially if the trace is
>> slightly smaller than the pad width, the fillet is symmetrical. I
>> have been told that symetrical fillets are preferred for:
>>
>>  a) mechanical strength
>>  b) will tend to "center" the component on the pad
>>
>> Now imagine one trace coming out one side of a pad, and another
>> trace connecting at an angle into an opposite corner of the same
>> pad. Common sense seems to suggest that the solder fillet that
>> results will not be "ideal", right?
>>
>> 3) Whoever said it is thermal related, I would like to see some
>> data for this. From my (limited) understanding, a reflow oven
>> heats up the entire board and all the components to a temperature
>> hot enough that any solder anywhere will flow. Therefore, there is
>> no real "heatsinking" going on, right? Its ALL hot. But i still
>> agree that three traces to an SMT is BAD, I just agree on the
>> reason. (Please correct me if I'm wrong)
>>
>> 4) You also must consider the current in some cases. If you need 8
>> amps, and you know how much copper you need to carry 8 amps, too
>> bad if its hard to solder, you NEED the copper. But on the other
>> hand, we have done boards with 4 ground planes, and some pins have
>> to connect to ALL of them (through-hole pins). In this case you
>> DON'T use thermal wagon wheels with 25 mil spokes, you can barely
>> hand solder it, and I would bet you would damage the board
>> material integrity in the process. You be surprised how much
>> current four 8mil spokes can handle... just a thought.
>>
>> I can't remember the other strange answers you got, so I'm done.
>> Don't take everything you hear on faith, TEST or ASK.
>> Good Luck,
>>                                                              Jack