[SI-LIST] Re: Current Carrying Capacity

Yaping,
While searching in the DESIGNERCOUNCIL archives, I found a reference to
Jenning's report 
    Jennings, C. W., "Electrical Properties of Printed Wiring Boards,"
    Sandia Labs SAND75-0663, May 1976.
being available through the IPC Order Department as IPC-TP-117, $10 for
IPC members and $20 for non-members.

The IPC was the Institute of Interconnecting and Packaging Electronic
Circuits until 1999, when they changed their name to just "IPC".  Their
web site is:
    http://www.ipc.org/

Their Online Store doesn't list IPC-TP-117, but maybe you can get the
IPC's library to copy it for you.

                                        John Barnes
                                        dBi Corporation
                                        http://www.dbicorporation.com/



 Zhou wrote:
> 
> John:
> 
> Thank you for your very useful information.
> 
> Do you know how to get copies of the papers you mentioned ?
> 
> Regards,
> 
> Yaping
> 
> ~~~~~~~~~~~~~~~~~~~~~~~~~~~
> Yaping Zhou
> Package Electrical Design and Analysis
> (512)933-5803  Austin, Texas
> Modeling and Simulation Group
> FMTC, Semiconductor Products Sector (SPS)
> Motorola Inc.
> ~~~~~~~~~~~~~~~~~~~~~~~~~~~
> ----- Original Message -----
> From: "John Barnes" <jrbarnes@xxxxxxxxx>
> To: <si-list@xxxxxxxxxxxxx>; <doug@xxxxxxxxxx>; <akmishra@xxxxxxxx>
> Sent: Tuesday, July 09, 2002 8:22 AM
> Subject: [SI-LIST] Re: Current Carrying Capacity
> 
> AK, Doug,
> If you would like to be on the conservative side, use
>      I = 56*diameter
> where:
>      I in Amps.
>      diameter in inches
> will keep the temperature rise in the via below 10C.
> 
> Are you concerned just with vias, or also with plated-through holes for
> components?  At my previous company we would plate vias solidly into
> power/ground planes, because we didn't need to worry about unsoldering
> them.  But the plated-through holes into power/ground planes would have
> a pad with an 0.006"-wide annular ring, with four 0.015" wide spokes
> coming through an 0.012"-wide thermal-isolation ring.  The idea was to
> keep the power/ground planes from taking away all the heat when we
> manually soldered/unsoldered the component(s).
> 
> The ampacity (current-carry capacity, from National Electrical Code
> article 310) of a via may be limited by:
> *  The cross-sectional area of the barrel.
> *  The cross-sectional area between the barrel and an external (on the
>    top or bottom of the board) pad or power/ground plane.
> *  The cross-sectional area between the barrel and an internal pad or
>    power/ground plane.
> 
> For a plated-through hole we also need to consider:
> *  The cross-sectional area of the spokes into an external power/ground
>    plane.
> *  The cross-sectional area of the spokes into an external power/ground
>    plane.
> 
> To add to the fun, internal copper layers may be scrubbed and lightly
> etched as part of the manufacturing process, so they may be only 74% as
> thick as an external copper layer of the same nominal thickness.  For
> example, one specification I found gives:
> *  Internal 0.5 ounce/ft^2 copper >=      0.00050 inches thick
> *  Internal 1 ounce/ft^2 copper >=        0.00100 inches thick
> *  Internal 2 ounce/ft^2 copper >=        0.00200 inches thick
> *  Internal 3 ounce/ft^2 copper >=        0.00300 inches thick
> *  External 0.5 ounce/ft^2 copper >=      0.00068 inches thick
> *  External 1 ounce/ft^2 copper >=        0.00135 inches thick
> *  External 2 ounce/ft^2 copper >=        0.00270 inches thick
> *  External 3 ounce/ft^2 copper >=        0.00405 inches thick
> 
> I spent over a year researching the ampacity of printed circuit boards,
> from summer 1999 to September 2000.  The vast majority of the published
> data, including MIL-STD-275, IPC-D-275, IPC-2221, and copies thereof is
> derived from
>     Jennings, C. W., "Electrical Properties of Printed Wiring Boards",
>     Sandia Labs SAND75-0663, May 1976.
> 
> Another major source, where the authors actually ran the experiments
> versus just copying someone else's graphs, was
>     Friar, Michael E., and McClurg, Roger H., "Printed Circuits and High
>     Currents," Design News, vol. 23 no. 25, pp. 102-107, December 6,
>     1968.
> 
> The equations that I finally came up with were:
> *  external I = 1500*thickness^0.72*width^0.75*deltaT^0.45
> *  internal I = 7500*thickness^0.72*width^0.75*deltaT^0.45
> where,
> *  I in Amps
> *  Thickness in inches
> *  Width in inches
> *  DeltaT in degrees C
> 
> These are reasonably close to the equations derived in:
> *  McHardy, John, and Gandhi, Mahendra, "Empirical Equation for Sizing
>    Copper PWB Traces," IPCWorks 1997 technical paper SO6-2-1.
> *  Brooks, Douglas, "Temperature Rise in PCB Traces," Proceedings of the
>    PCB Design Conference West, 1998.
> 
> One somewhat surprising result of my study was that the spokes on
> plated-through holes tended to limit the ampacity.  For a 10C
> temperature rise:
> *  Multilayer boards max'ed out at:
>    -  1.08A going into 0.5 ounce/ft^2 copper, for >= 0.024" holes.
>    -  1.77A going into 1 ounce/ft^3 copper, for >= 0.026" holes.
>    -  2.92A going into 2 ounce/ft^2 copper, for >= 0.050" holes.
>    -  Otherwise I = 56*diameter, where I is in Amps and diameter is
>       in inches, is conservative.
> *  Doublesided cards max'ed out at:
>    -  2.67A going into 0.5 ounce/ft^2 copper, for >= 0.044" holes.
>    -  Otherwise I = 56*diameter, where I is in Amps and diameter is
>       in inches, is conservative.
> 
> John Barnes
> dBi Corporation
> http://www.dbicorporation.com/
> 
> Doug Brooks wrote:
> >
> >  At 04:53 PM 7/8/2002 -0400, AK Mishra wrote:
> >
> > I am in search for a formula for calculating "Current Carrying capacity"
> of
> > a Via. All the Books talk about Traces only. Help me out..
> >
> > Thanks!
> > UltraCAD has just posted a new article on this subject on its web page
> > http://www.ultracad.com
> > [1]Title:
> > Current Carrying Capacity of Vias
> > Some Conceptual Observations
> >
> >
> ____________________________________________________________________________
> _
> > [       Å
> ------------------------------------------------------------------
> To unsubscribe from si-list:
> si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
> 
> or to administer your membership from a web page, go to:
> http://www.freelists.org/webpage/si-list
> 
> For help:
> si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
> 
> List archives are viewable at:
> http://www.freelists.org/archives/si-list
> or at our remote archives:
> http://groups.yahoo.com/group/si-list/messages
> Old (prior to June 6, 2001) list archives are viewable at:
>   http://www.qsl.net/wb6tpu
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field

or to administer your membership from a web page, go to:
http://www.freelists.org/webpage/si-list

For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field

List archives are viewable at:     
                http://www.freelists.org/archives/si-list
or at our remote archives:
                http://groups.yahoo.com/group/si-list/messages 
Old (prior to June 6, 2001) list archives are viewable at:
                http://www.qsl.net/wb6tpu

Other related posts: