Jack,
Good boiler-plate answers.
I agree, however in some cases reflow oven speed and temperature profile
are not always ideal due to manufacturing needs. The faster you put the
board through the oven the better from a manufacturing throughput
standpoint. This sometimes causes thermal shadows on the boards
particularly on 0402 components close to larger parts. A large trace or
multiple traces MAY pull heat from the small 0402 pad. This has been my
experience with IR ovens in a high volume environment. If the problem can
be contributed to something else let me know.
As far as solder paste flowing along an exposed trace, this problem can
be solved by increasing the solder stencil opening to match the solder
mask size and not the pad size (please note that I was/am specifically
referring to 0402 components). This would not work on small pitch parts.
As far as 8 Amps are concerned, I don't think you need to worry about it
on a trace routed to an 0402 component. It will never see it.
Like you said "Don't take everything you hear on faith". Some people just
like to hear themselves talk.
Scott
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
__________________________________
Scott Buscomb, Senior CAD Designer
[log in to unmask]
voice 770 338-6170
MTCC/Panasonic, Pager Development
1225 Northbrook Pkwy, Ste 2-358
Suwanee, GA USA 30024
__________________________________
|
