Congratulations on the CID+ Jack!
Just a thought... The air is typically the final destination for the excess
thermal energy...at least if you are talking about terrestrial earth bound
systems... so being in direct contact with the air is the best of all
worlds. (there are exceptions of course like with space vehicles where all
heat must be radiated away as Infrared energy into the black body of space,
no air available out there... )
As you add other thermal resistances to the thermal model, they slow the
flow of heat to the air... kind of like adding a resistor in an electrical
circuit slows the electrical current in the circuit, so potting the trace
would add an additional thermal resistance greater than air to pass the heat
thru on its way to the ambient air... the thing it is trying to equalize
with.
Air thermal conductivity is the constant against which all other materials
are measured... most materials used for thermal conductivity have a better
thermal transfer characteristic than air does. The white silicon grease that
gets used as a thermal transfer material is really only there to remove the
presence of 'very small air pockets' between thermal conductors because air
can act as a barrier to thermal transfer between the better thermal
conductors of the metal transistor tab and its heatsink for example. As a
side note regarding the white grease... More grease is not better... it's
actually not generally a good thermal conductor but it does work well if it
is kept thin enough to remove the air pockets and allow metal to metal
contact where the surfaces mate well.
So as I would expect, the potting of the circuit is more like adding an
additional resister to the thermal path to the final destination for the
heat trying to reach equilibrium with the ambient air in the circuit... and
it sounds like at 1.1 that it is about as bad as air between two metal
plates... its going to resist the thermal transfer of heat energy almost as
bad as air would...
Thermal analysis is not as intuitive as I wish it was... There is a good
book out there that explains a lot of this stuff... Cooling techniques for
Electronic Equipment by Steinberg.
Best regards,
Bill Brooks, CID+
Datron World Communications, Inc.
3030 Enterprise Court
Vista, CA 92081
(760)597-1500
-----Original Message-----
From: Jack Olson [mailto:[log in to unmask]]
Sent: Wednesday, May 30, 2007 2:11 PM
To: [log in to unmask]
Subject: Re: [DC] Current vs. Temperature (IPC vs. PCBTEMP)
That is a very interesting insight, thanks for sharing it.
sorry for the delayed response, but I got swamped trying to finish stuff
before taking off for a few days to do the CID+ test (I passed! yeah!)
In fact, when I was there, someone told me to just add up all of the
currents and solve for that. For example, if I'm trying to get four 5amp
traces through the same area, just solve for 20amps. The 20amp
result IS higher than the sum of four individual traces. For example,
the calculator says .070 for 5, but .543 for 20 (1ozExternal20rise)
so I am feeling better about that, and its easy to figure
(maybe TOO easy? hmmm?)
Anyway, now I'm really gonna show my ignorance with this next
question.... I see that air has a thermal conductivity of 1, and potting
compound has a higher conductivity, I think around 1.1? Even though
my mind is telling me that the potted external trace seems more like
an INTERNAL trace now, does this really mean I can push more
current through the same trace width if it is potted?
Jack (aka "the new guy")
On 5/12/07, Haldor Husby <[log in to unmask]> wrote:
> 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
----------------------------------------------------------------------------
-----
---------------------------------------------------------------------------------
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
---------------------------------------------------------------------------------
|
