Hi David,
I just have a few comments regarding your question...
To question one ... the answer is yes. The calculation for Minimum annular
ring is a+2b+c where:
a= Maximum Diameter of the finished hole (hopefully large enough to allow
the pin to fit correctly)
b= Minimum annular ring requirement (see IPC 2221 9.1.2 class levels of
boards affect the requirements)
c= standard fabrication allowance ( supplied by the manufacturer of the PCB
and different from manufacturer to manufacturer, classified by 3 classes of
performance specs based on PCB usage and application see IPC 2221 table 9-1)
(ref IPC-2221 9.1.1 Land Requirements)
Minimum annular ring requirements depend upon the design objective. In this
case, it sounds like you have a supported hole application with a component
pin installed and soldered in it near or at the edge of a fiberglass/epoxy
PCB, used in a standard Class 1 or 'general electronics' category with level
A or 'general design complexity' performance requirements (with my
assumptions included)..
First question would be how much pad is required to get a good solder fillet
around the pin? That's subjective based on the following.
Second question is how strong does it need to be? The longer the pin is, the
more likely it will be stressed, the more strength of the mechanical
attachment to the board needs to be, the larger the pad may need to be
unless swaging or staking is employed. Only you can determine the strength
of the joint requirement and after doing that, go back to question 1.
There are potentially many other questions I could ask but let's assume the
complexity requirements of your design are not too complex.
Much depends on the geometry of the board and pin and the way in which the
pin is expected to be used and the ways the pin/board assembly can be
'abused'. Reliability and survivability depend on your choices.
Personally, I prefer not to design against the minimums. For High
reliability I usually de-rate my calculations by 50% or in essence, I make
them twice as strong as they may appear to need at nominal. I don't always
need High reliability in all the designs I do. So your judgment is essential
in determining the level of reliability you need for this application.
How close can a pad be to the edge of the board? Actually, a Pad can be as
close as you want. Some pads are split by the edge of the board creating an
edge plating effect or castellation effect by having a plated through hole
on the board edge and by trimming through the hole, bisecting it.
Again, it depends on the design requirements. Understand that there are
undesirable consequences for choosing to put a pad too close to the edge of
a board... shorting to mounting hardware, interference with mechanical
assemblies, burrs and sharp edges on the edge of the board will have to be
dealt with... etc.. etc.. I do not think there is a pat answer for your
question, especially since all the parameters of the design are not known in
your description. But you have no restriction on the use of your design
ability and imagination when dealing with a design... just check with your
PCB manufacturer and find out how much it is going to cost you to make it
and find out if that will affect your bottom line. Specs are not created to
stop creativity or imagination. They serve as a guide to the enlightened to
control costs, and improve manufacturability and set standards for
acceptability in manufacturing quality. And for that task, the IPC specs
perform admirably!
Bill Brooks, CID
"The person who says it cannot be done should not interrupt the person doing
it."
--Chinese Proverb
-----Original Message-----
From: David Harman [mailto:[log in to unmask]]
Sent: Tuesday, July 22, 2003 5:39 PM
To: [log in to unmask]
Subject: [TN] Design Question
Hello technet.
I have a question on PCB design. We are redesigning our board and a
question came up that I am unable to verify. We are looking at having a
plated through-hole near the end of the board. This plated through hole
will be used to place a post through and soldered into place for
electrical contact.
The question that I have is as follows,
? Is there a requirement indicating that an annular ring is to be a
certain diameter larger than the actual through hole? And how far from
the edge of board should an annular ring be placed?
Thanks for your help.
---------------------------------------------------
Technet Mail List provided as a free service by IPC using LISTSERV 1.8e
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 or (re-start) delivery of Technet send e-mail to
[log in to unmask]: SET Technet NOMAIL or (MAIL)
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 1.8e
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 or (re-start) delivery of Technet send e-mail to [log in to unmask]: SET Technet NOMAIL or (MAIL)
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
-----------------------------------------------------
|
