In my design practice I have always used smaller traces than what the
pad size is. However the biggest thing that you have to remember is....
If you do it on one side of the part do the same thing on the other side
of the part so that when the solder paste reflows the part will not be
pulled off the smaller traced pad. The solder mask in this case acts
like a solder damm and if you have a very wide trace on one side and a
small trace on the other side when reflow occurs the part itself wants
to swim around on its new molten pool. Where ever the majority of the
solder flows is where the part will come to rest. So to keep the part
centered put the same size trace on both sides of the part or balance
the part.
I agree with everything that has been said in this thread....
Everyone has made good points. However in power supply design there has
been occasions that I have had SMT parts with no thermal relief in the
pad at all. Yes, for rework you have to get out a blow torch, but the
design you are doing may dictate such design practices.
To make your engineer happy, just place the same size trace on
both sides of your 0805 and neck down from the via to your QFP for power
traces. For Signal traces you might what to use the argument that more
copper will give him more resistance and actually will cause more
impedance to the rise time on his circuit. This may cause him to
rethink his request. Sometimes if you talk their language you can get
your point across without having to use other drastic measures. ;-)
Joe J. - C.I.D.
-----Original Message-----
From: DesignerCouncil [mailto:[log in to unmask]] On Behalf Of
Allen T. Maddox
Sent: Friday, July 29, 2005 8:48 AM
To: [log in to unmask]
Subject: Re: [DC] Trace width ratio to pad
Good Point. Mostly what I am talking about are QFP with a 20mil pitch
connecting to 0805. The concern is for the fast edge of the device, not
necessarily the clock speed. What bothers me is that technique this is
used across the whole board, PS, analog, and digital sections. Even when
the 0805 are connected to each other, a trace the width of the resistor
pad is used. Sometimes this means that a smaller trace is used on one
side of the resistor or cap than the other side.
Someone had mentioned that an oven profile could be set up to compensate
for this, but to tell you the truth, it's not being done. Mostly because
our facility is old and it takes time that the manufacturing engineer
cannot commit to. We do a lot of small runs, so things need to be made
similar in order to diminish set up times. The board that I'm working on
does not fit into what 80% of what our boards are. This needs special
handling and is causing a headache down the line. I need to find the
compromise so most of my "customers" (i.e. engineering, manufacturing,
board vendor) are somewhat satisfied.
Thanks,
Allen Maddox C.I.D.
Sr. PC Board Designer
GAI-Tronics, Corp
610-796-5854
PO Box 1060
Reading, PA 19607-1060
[log in to unmask]
www.gai-tronics.com
>>> [log in to unmask] 07/28/05 06:14PM >>>
Allen and other responders,
I have read all of the responses to this thread, and excepting a fer
specific issues dealing with a QFP and a Flip Chip, nobody deals with
the real issue, or should I say, "question"?
What is the size of the smt pad, what are youu hooking it to, and are
there any adjoining pads that are closely spaced.
The issue you appear to be specifically referencing, is called a
"thermal relief", and depending specifically on the size of the pad and
just what that pad (either thru hole or smt) is connected to, you may or
may not need to provide a "thermal relief" for the pad in question.
Generally, the "thermal relief" is provided when a pad connects directly
to a large "bus" or a "plane".
The real critera, is just what will be needed in your specific instance,
in terms of manufacturability.
While a few examples of why a trace should be necked down have already
been given in a few of the previous post, I am going to give an example
of where NOT to neck down, for design reasons.
In some work I have done for one engineer, he would design his stackup
such that all of his exterior 50 ohm traces in a 2.4GHz design would be
20 mils wide, exactly the width of his 0402 component pads, such that he
could seamlessly enter and exit any components, such as a coupling
capacitor between stages. In such an instance, you absolutely would NOT
want to neck down for a "thermal relief", no matter what (even at the
risk of the expense of hand soldering if necessary).
So back to where I began, just what size smt pad are you talking about,
what is it connected to, and what are you connecting it to?
JaMi Smith
*******************************************************************
This email and any files transmitted with it are confidential and
intended solely for the use of the individual or entity to whom they are
addressed. If you have received this email in error please notify the
system manager.
This footnote also confirms that this email message has been swept for
the presence of computer viruses.
www.hubbell.com - Hubbell Incorporated
------------------------------------------------------------------------
---------
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
---------------------------------------------------------------------------------
|
