From a fabricator viewpoint, there are one or two things to bear in mind.
Firstly the accuracy of print registration will at best be +/-50um (+/-
2mil) if your fab house uses automatic registration, secondly, the minimum
'web' width that will remain through subsequent processing is about 85um
(2.5 mil) AT THE BOARD SOLDERMASK INTERFACE - this is important because
most masks will be undercut during developing, and may require an artwork
width of 6mils to achieve the web. Add these two factors together, and this
means the only chance of getting a web between pads is if the gap between
pads is 10mils minimum. If your QFP is on a 20 mil pitch (actually 19.6
mil), the pad width will have to be designed at 8 mil (there is an etch
tolerance and you need to understand that the top of the pad and bottom of
the pad will be different widths - which do you specify?). Now most
designers with a 12mil gap will want to run a 4/4 track and gap in there -
now you have soldermask covering the track and the soldermask height is
over the track and therefore the soldermask MUST BE HIGHER than the pad you
wish to solder to. This will create a problem with solder pasting, so the
answer is don't run tracks between these pads if you want to have high
assembly yields.
Dougal Stewart
email [log in to unmask]
telephone +44 1896 822204
mobile +44 7984 629667
-----Original Message-----
From:   Furrow, Robert Gordon (Bob) [SMTP:[log in to unmask]]
Sent:   28 November 2001 13:27
To:     [log in to unmask]
Subject:        Re: [TN] Solder Resist and QFP's

Mike,

I think that a good board shop should be able to avoid contaminating the
pad
surface with resist. The larger concern I would have is if in any areas the
solder resist height is above the surface of the pad, your stencil will not
gasket properly and you can actually increase the number of shorts.

Thanks,
Robert Furrow
Printed Wiring Board Engineer
Strategic Supply Global Account Manager
Supply Chain Networks
Lucent Technologies
978-960-3224    [log in to unmask]

-----Original Message-----
From: Michael Bell [mailto:[log in to unmask]]
Sent: Tuesday, November 27, 2001 5:15 PM
To: [log in to unmask]
Subject: [TN] Solder Resist and QFP's


Hi all,

What are peoples thoughts on solder resist between fine pitch micro pads???
I have recently heard two differing theories regarding this matter, one is
that solder resist between the pads on some very fine pitch QFP's will
reduce the risk of solder shorts. The other theory was that with solder
resist between these pads you could risk getting the resist onto the pads
and reducing the soldering surface???  What is the general consensus on
this
matter???  Which approach to others take on this matter?

Cheers

Mike

 << File: ATT00000.htm >>

---------------------------------------------------------------------------------
Technet 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 Technet
To temporarily halt delivery of Technet send the following message: SET Technet NOMAIL
Search previous postings at: www.ipc.org > On-Line Resources & Databases > E-mail Archives
Please visit IPC web site (http://www.ipc.org/html/forum.htm) for additional
information, or contact Keach Sasamori at [log in to unmask] or 847-509-9700 ext.5315
---------------------------------------------------------------------------------