Kaye: We use guard traces in quite a few of our designs, however most are
single or double sided surface mount (no wavesolder).
1. The obvious; can you move the guard traces to the topside of the board?
2. Are the solder bumps really causing a problem not allowing the guard
traces to do their designed job or is it a belief or perception? We have not
seen it to be a problem when an occasional bead or lump of solder is on the
circuit.
3. We usually go with a 10 mil or larger soldermask clearance per side
around the guard traces. If you want it tighter most fabricators should be
able to get by with a 3 mil clearance per side.
4. When laying the out the guard traces in most cases we use a "soft" angle
45 degrees or more. Stay away from very acute or right angles and square
shapes. They have a tendency to trap solder in the wave.
5. For bottom side guard traces we try to run them parallel to the direction
of board travel thru the wave.
6. Exposed guard edge to pad edge clearance is typically 25 mils or larger.
However we usually have mask around the outside periphery of the pad instead
of leaving it completely open.
7. If you are water washing the boards after wavesolder I would look into a
screenable aqueous temporary soldermask. A screen image could be created for
your intricate patterns then applied using a single pass squeegee
application. Similar to how permanent soldermask is applied. We have used
this approach for many years.
8. Selective solder fixtures may also be an alternative.
9. What is the final solderable finish on the board? You may want to
consider OSP vs HASL or Au/Ni.
10. Although you are working as a board designer I would take a close look
at the wavesolder process and see if there can be some improvements to the
process to reduce the "solder beads" . You should not be seeing a lot of
this on the guard traces if the process is set up and running correctly.
Preheat, conveyor speed, flux application/density, wave flow, etc can all
influence this.
Regards
Michael Barmuta
Staff Engineer
Fluke Corp.
Everett WA
425-446-6076
-----Original Message-----
From: Kaye Knotts [mailto:[log in to unmask]]
Sent: Monday, June 03, 2002 7:59 AM
To: [log in to unmask]
Subject: [TN] Solder beads on soldermask relieved traces
We are having a problem that I would like to solicit the help of Technet.
The problem is solder beads after wave process on soldermask relieved bottom
side traces,
which our Manufacturing Department is having to touch-up to remove the
beads.
We have a few printed circuit boards which require soldermask
relieved guard traces on the bottom side of the board. These
guard traces completely encircle the affected net and the only
parameter our engineer's require is that the trace be relieved of LPI
soldermask
a small amount, like a couple of mils. I think that our board vendors
are opening the relief aperture wider than the given guard trace sizes
of approximately 5 mils, 7 mils, and 10 mils to accommodate
their registration tolerances.
We have experimented with different geometries for encircling the
affected net; for instance, rounded, square, and angled corners.
It would appear that square corners and intricate intersections
are culprits for capturing solder beads, but our problem is also with
long (approx. 1-1/2" or greater) straight exposed traces,
both parallel and perpendicular to the wave. We have also
experimented with varying distances from guard to net and find
inconsistencies in that a distance of say 10 mil from exposed
pad to exposed trace is no problem, but in another area of the
board a distance of 35-40 mils will produce a bridge.
Does anyone out there have any experience with exposing guard traces.
Would increasing the aperture size of the guard trace make a difference? If
so, how
much of an increase would be enough. What would be an acceptable
distance to avoid bridging? We have considered using a temporary soldermask
to cover these traces during the wave process, but it becomes costly to
apply to intricate patterns and then remove. Any help or advice on this
matter would be appreciated.
Thank you
Kaye Knotts
Sr. P. C. Board Designer
Keithley Instruments, Inc.
Solon, Ohio
----------------------------------------------------------------------------
----- 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 e-mail to [log in to unmask]: SET Technet NOMAIL To
receive ONE mailing per day of all the posts: send e-mail to
[log in to unmask]: SET Technet Digest Search the archives of previous posts
at: http://listserv.ipc.org/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
----------------------------------------------------------------------------
-----
---------------------------------------------------------------------------------
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 e-mail to [log in to unmask]: SET Technet NOMAIL
To receive ONE mailing per day of all the posts: send e-mail to [log in to unmask]: SET Technet Digest
Search the archives of previous posts at: http://listserv.ipc.org/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
---------------------------------------------------------------------------------
|
