Re: Thermal Relief Design

Jeff Seeger ([email protected])
Mon, 16 Jun 1997 19:38:25 -0400

[email protected] wrote: (edited for brevity)
> Each pin can carry up to 15A and there are up to
> five 2 oz. planes in the stackup that connect to the hole.
> My dilemma is heat vs. dc resistance. I need to use a thermal relief on
> all 5 planes that will allow me to heat the hole enough for solder to flow.
> a problem with IR drop.

[email protected] wrote: (edited for brevity)
: were concerned with the same problem that you are facing now and
: to use multiple pins on the connector but limited the number of
: planes to TWO 2 oz planes. Please note that the thermal relief area
: of contact to the pin should be taken into account in calculating
: total current carrying capacity.

Over the last year we've seen an increase in this problem.
It seems the connector manufacturers are improving the contact
systems but have forgotten the solder attach problem. What's
good for current carrying is bad for heat retention. I'll assume
that the problem you seek to obviate is heat retention for wave

The only standard I've seen on thermal relief design is from the
IPC-D-275, which states,

"Total cumulative copper web for all layers in any plated-through
hole {which is intended for solder-attach} should not exceed 4.06mm
(0.160") for 1 oz/sqft Cu or 2.03mm (0.080") for 2 oz/sqft Cu."

Unfortunately the same standard points to a current rating of 3
amps with that geometry at a 10oC rise over ambient temperature
(minimum charted) on an inner layer, or twice that on an outer

Far better to plan on the use of either press-fit connector
systems or non-wave soldering techniques such as hand solder or
intrusive reflow. However, each of these have caveats:

Intrusive reflow techniques heat the entire thermal mass to allow
solder flow, so relief geometry is not required, but this method
is not in widespread use (to my eye). The hole geometries for a
connection this size do not lend themselves to stencil-printing
sufficient solder paste, but solder "washers" are being introduced
that would allow deposition of sufficient solder volume, albeit
with alot of effort to put the rings in place.

Depending on your product volume, acceptance/performance criteria,
and resource availability, simply planning for hand solder may be
the correct approach. Another option we have seen used is to go
with larger than IPC sizes and assume touch-up after inspection.
With a doubling of the max geometry, and using outer layers, you
can reach ~12 amps at minimal DC drop (heat rise) and distribute
to your multiple planes with a field of vias. Speaking entirely
anecdotally, the associated touch-up was not show-stopping, but
some acceptance criteria mandate zero touchup.

And, of course, even if you move to press-fit you may find that
some PWB manufacturers still require relieved connections to ensure
an epoxy-to-epoxy bond.

I'd be most happy to hear of a more robust thermal relief guide-
line! The IPC standard set does tend to seek 100th percentile
acceptability on issues like this.

Good luck, and regards to all,

      Jeff Seeger                             Applied CAD Knowledge Inc
      Chief Technical Officer                      Tyngsboro, MA  01879
      jseeger "at" appliedcad "dot" com                    508 649 9800