Dave;
Another thing to keep in mind is that when you look closely, these guidelines are meant for through hole "mounting pads", that is, component holes. The intent is to insure that there is sufficient annular ring to form a reliable solder joint. This need is non existent for a via, therefore the guidelines do not apply 100%. For a via, the only real requirement is that the hole not break out excessively, as Phil points out. If, by design, you can provide annular ring of .2mm, you are doing well for a small via. (.4mm dia over max finished hole dia) The guidelines we usually use revolve more around the aspect ratio. Although many shops are breaking new thresholds in the aspect ration arena, I 'tend' to try and keep the aspect ratio no greater than 8:1.
Denis Lefebvre, C.I.D.
Senior PCB Designer
408-542-3832
Finisar Corporation
1308 Moffett Park Drive
Sunnyvale, CA 94086
www.finisar.com
-----Original Message-----
From: DUTTON Phil [mailto:[log in to unmask]]
Sent: Wednesday, July 24, 2002 11:24 PM
To: [log in to unmask]
Subject: Re: [DC] IPC 2221
Hello Dave,
There is a formula and set of tables in IPC-2221 (the 2220 series replaced
275, which in-turn replaced Mil-275).
Land size, minimum = a+2b+c
a= maximum diameter of finished hole
b= minimum annular ring requirements
c= fabrication allowance
There are 3 levels of defined manufacturability A,B & C, with A being the
easiest to manufacture.
At the A level you would need a land diameter 0.5mm bigger than your maximum
finished hole diameter.
At the B level you will need 0.35mm in diameter.
At C this reduces to 0.3mm
This is a minimum, but your supplier seems to be asking for twice this.
55110 is no longer current, Mil-prf-31032 replaces it.
Missregistration (hole to land?)depends on the performance class of your
boards.
Generally acceptance referring IPC-600 class 2 allows for the hole to break
out of the pad by no more than 90 degrees of it's circumference as long as
it does not occur at the track entry to the pad.
Class 3 does not allow any breakout.
I hope this helps.
regards,
Phil Dutton C.I.D.
Tenix Defence.
-----Original Message-----
From: Dave Sharples [mailto:[log in to unmask]]
Sent: Thursday, 25 July 2002 13:34
To: [log in to unmask]
Subject: [DC] IPC 2221
Hi,
I do not have quick access to ICP 275 and IPC 2221.
I am told by my PCB supplier that the distance from hole edge to pad edge
should not be less than 0.5 mm in IPC 275 and 0.6 mm in IPC 2221 for the
design of through hole vias.
If this is so how do you fanout fine pitch BGA components or even 35 mil
pads on 50 mil pitch.
Is there a tolerance on missregistration in the Mil 55110 spec.
Your help will be most appreciated.
Regards,
Dave Sharples
www.pcbdesign.co.za
+ 27 (0) 72 397 5824
----------------------------------------------------------------------------
-----
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 set a vacation stop for delivery of DesignerCouncil send: SET
DesignerCouncil 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
----------------------------------------------------------------------------
-----
---------------------------------------------------------------------------------
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 set a vacation stop for delivery of DesignerCouncil send: SET DesignerCouncil 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
---------------------------------------------------------------------------------
---------------------------------------------------------------------------------
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 set a vacation stop for delivery of DesignerCouncil send: SET DesignerCouncil 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
---------------------------------------------------------------------------------
|
