Congratulations on your + certification!!!
Denis Lefebvre, CID+
Sr. PCB Designer
Finisar Corporation
(408)542-3832
-----Original Message-----
From: DesignerCouncil [mailto:[log in to unmask]] On Behalf Of Jack Olson
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
---------------------------------------------------------------------------------
|
