TECHNET Archives

January 1998

TechNet@IPC.ORG

Options: Use Monospaced Font
Show Text Part by Default
Show All Mail Headers

Message: [<< First] [< Prev] [Next >] [Last >>]
Topic: [<< First] [< Prev] [Next >] [Last >>]
Author: [<< First] [< Prev] [Next >] [Last >>]

Print Reply
Subject:
From:
Jerry Cupples <[log in to unmask]>
Reply To:
TechNet Mail Forum.
Date:
Wed, 14 Jan 1998 17:42:46 -0600
Content-Type:
text/plain
Parts/Attachments:
text/plain (79 lines)
Interesting....

Ken Patel asked:

Is there any problem spelling out "ALL GROUND/POWER PLANE CONNECTIONS SHOULD
HAVE THERMAL RELIEF " on my fab drawings.

Please provide me pros and cons before I make a call.
Your help is greatly appreciated.

Raymond Klein replied:

>Ken,
>
>I usually take the other approach and specify thermal relief ONLY ON PIN
>THROUGH PARTS. (No thermal relief is needed on press fit parts). Vias to
>power and ground planes do not usually need thermal relief and it makes for
>a much more continuous plane which give better electrical characteristics
>and are easier for the PWB designer to route (vias can be closer together).
>I've also had dense designs which would have had large gaps in the power
>and ground planes if I'd used thermal relief on the hundreds of vias that
>connected to these planes.
>
>Problems with lack of thermal reliefs may occur if a very short and wide
>(>.025 in) trace is used to connect a SMT part to a via to a gnd/pwr plane.
>
>Ray Klein

At Interphase, our boards are typically fairly dense 6 layer designs with
SMT parts on both sides. 98% of all active parts are SMT packages, which
have ground or power connection to internal layers by way of 0.010" PTH's.
These holes have a cartwheel pattern thermal relief with four spokes.

The thermal relief pads are shown on the Gerber files as "flashed"
patterns. When examining the internal plane film layers, the thermal relief
pads are scattered in the hundreds. The dominant majority of these
connections go up through the hole, and then to an 0.030" external pad,
connecting with a 0.010" width trace to an SMT rectangular pad which is
0.015" or 0.010" wide.

My guess is that this design approach is a hangover from the requirements
of the wave solder process days when it was necessary to get good wetting
up the hole and to the topside pads.

I'm not sure that there is any reason to do this on modern designs as I
describe, and tend to believe Ken's approach would work, but since this is
NOT what we do, can't say that there wouldn't be thermal variation in
reflow on the power leads of a QFP, for instance.

The electrical impedance of the power connection would likely be better
(lower inductance) if the plated hole connects to the plane around the
entire circumference.

If there are others who use the "no thermal relief" internal connections
extensively, I'd sure like to hear how it has affected (if it has) the
profile and delta T, and whether it has caused any coincidental issues.



regards,


Jerry Cupples
Interphase Corporation
Dallas, TX USA
http://www.iphase.com/

##############################################################
TechNet Mail List provided as a free service by IPC using LISTSERV 1.8c
##############################################################
To subscribe/unsubscribe, send a message to [log in to unmask] with following text in the body:
To subscribe:   SUBSCRIBE TECHNET <your full name>
To unsubscribe:   SIGNOFF TECHNET
##############################################################
Please visit IPC web site (http://www.ipc.org/html/forum.htm) for additional information.
For the technical support contact Dmitriy Sklyar at [log in to unmask] or 847-509-9700 ext.311
##############################################################


ATOM RSS1 RSS2