Hi Jack -
I can't tell you how to derate the IPC curves for two parallell traces, but
depending on your application you may be able to get at this from a
different angle. We all use these curves in the general case, that is on any
application and on any board. The way the curves were developed and are
being used assumes that the heat is transferred to the ambient directly
through air or through the FR4 to air (I trust one or more of the forums 504
members will correct me if I am wrong). But boards today are different from
when the curves were developed, and you can actively use the copper and
components to take heat away, especially on higher power boards like yours.
You can consider the thermal resitance from your trace to some known ambient
instead of reading the curves. 

If your application allows a very thin dielectric between the traces and the
reference (call it GND) plane you presumably have on the adjacent layer, you
may take the heat out through it. Assume you use this configuration to carry
your 5 amps of current:

Trace width:            2.5mm (100 mil) 
Copper wight:           1oz 
Dielectric thickness:   100 um (4 mil) 

In this case the thermal resistance betweeen a square of the trace and the
GND plane is 70K/W or so, but you only dissipate 12.5mW of power, so the
temperture rise relative to the GND plane is less than 1degC. The real
thermal resitance is higher because the real trace is a series of squares in
a row, but overall thermal resistance between a 25mm (1") length of trace
and the GND plane is about 17deg, and since the dissipation in this case is
125mW, the temperature gradient between the hottest spot on the trace and
the plane is just over 2degC. In the first approximation this conduction
path is only influenced by an adjacent trace to the extent that it is able
to inrease the temperature of the GND plane locally, and you have many ways
to manipulate that. Besides, your overall thermal design needs to keep the
temperature of the heat conducting planes well below Tg. Even if you derate
the thermal resistance by a factor 10, you are still OK.

There is a nice little calculator to play around with different topologies here:

http://www.frigprim.com/online/pad_ground.html

There may be other ways to lead the heat away too, for example along the
trace itself to the load which in most cases have a very low thermal
resistance. It works better on boards where the traces are even wider, and
only if they are very short, but it might be relevant to you even so. Once
your trace temperature exceeds 80degC you may also benefit from radiation.
It is harder to calculate that effect, but you can think of it as a small
safety valve, and you can stimulate the effect by using blue soldermask and
painting the inside of your chassis black. 

None of this assumes transfer of heat from the trace to air or to the
dielectric, so if you can assure the thermal design by considering the
thermal resitance, you don't need to use any curves. It takes a bit of
calculations, but you get far with pretty rough ones, and all you need is
already on your desk. You don't need to buy or learn any thermal simulation
software. 

I have been thinking along these lines in planning a design with some tricky
thermal challenges, but a board to measure on is still far off. It would be
great if anyone has made experiences to validate or refute what I have written. 

-------------------------------------------------
Haldor Husby, Senior Development Engineer
Data Respons Norge AS
Kongsberg Næringspark
P.O. Box 1022
NO-3601 Kongsberg, Norway 
Tel: +47 32 29 94 00 Fax: +47 32 29 94 40
Dir: +47 32 29 94 18 Mob: +47 48 04 83 68 
[log in to unmask]
www.datarespons.no

---------------------------------------------------------------------------------
DesignerCouncil 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 DesignerCouncil.
To temporarily stop/(restart) delivery of DesignerCouncil send: SET DesignerCouncil NOMAIL/(MAIL)
Search previous postings at: www.ipc.org > On-Line Resources & Databases > E-mail Archives
Please visit IPC web site http://www.ipc.org/contentpage.asp?Pageid=4.3.16 for additional information, or contact Keach Sasamori at [log in to unmask] or 847-615-7100 ext.2815
---------------------------------------------------------------------------------