Chris,
To simplify the formula, consider this:
The total of the web size is equal to 60% of the pad size.  Each web segment
is equal to the total divided by the number of segments.  Therefore:

For a .060" pad, the total web size would be .036", (.060 X .6 = .036).  For
a four-segment web, each segment would be .009" (.036 / 4 = .009).  For a
three-segment web, each would be .012" (.036/ 3 = .012), etc.

In addition, if your pad size is larger than the calculated minimum pad size
(minimum pad size = max finished hole size + (2 * annular ring) + fab
allowance) you need to decrease the web size by a like percentage.  I.E.
Calculated minimum pad size = .060" but you decide to use a .075" instead.
In this case, your actual pad size is 25% larger than the calculated
minimum.  So, you would need to decrease the total web size by the same 25%
from .036" to .027".  The reason for this makes sense, once you consider the
purpose of a thermal relief - to prevent too much copper area (in planes and
copper pours) for a given hole size from sinking the heat necessary to cause
the solder to flow completely to the top surface of the PCB during wave
soldering.  It also facilitates de-soldering of parts, without destroying
the external pads.

Additionally, again, :-), the total web size for all layers should never
exceed .160" for 1 oz copper or .080" for 2 oz copper.  (Notice the
decreased size for the heavier copper?  Same rules apply as for increased
pad size.)

I hope this has helped.  Feel free to contact me if you need additional
information.

Ray Humphrey
DynaCad Design Services

----- Original Message -----
From: Chris Robertson <[log in to unmask]>
To: <[log in to unmask]>
Cc: <[log in to unmask]>
Sent: Friday, September 17, 1999 12:02 PM
Subject: I hope


> Regarding thermals, I was trained to make the ID of the thermal the
> same as an internal pad/land + 10Mil + 10%
> The OD and the web at 25% of the ID (pad/land)
>
> Researching this several years ago I found that this was above and beyond
> most specs.
> I'm now looking at the IPC spec and it dosen't make a hell of a lot of
> sense.
> I'm sure there are others out there that don't quite understand.
> Could someone clarify?
>
> If there are any bugs, suggestions, etc. there is a "format"
> that would help tech support identify our problems.
>
> Software;    Accel PCB
> Version;    V15
> Date;
> Subject;
> Description;
> Reason; (If necessary)
>
> I'm assured that this will help Tech support process out emails.
>
>
> Chris Robertson
> PCB Designer
> Lockheed - Martin Services, Inc.
> [log in to unmask]
> Ph/Fax (256) 722-2626
> ICQ# 13541566
>
> This has been cross posted. Please ignore irrelevant information
>
>
>