Valerie,
Thanks very much for your explanation. Based on your explanation in light
of our design intent and scope, we are in good shape with current drawing
callouts.
As I replied to Bill Brooks' earlier comment on this thread:
"Our rigid boards are 2, 4 and 6 layer boards where Dk, Tg, and other arcana
are not important enough to warrant any material beyond IPC 4101/21 "normal"
FR-4. We allow the fabricator to choose the prepreg. The standard 2-layer
core is mostly 0.059 inch these days. We're fortunate we can be flexible,
so there's no reason to pay more for what you don't really need, right?"
I appreciate that you validated that I didn't miss anything when going
through those specs; what I was looking for is more or less urban legend :)
Thanks,
Gary
-----Original Message-----
From: DesignerCouncil [mailto:[log in to unmask]] On Behalf Of Valerie
St.Cyr
Sent: Wednesday, March 09, 2005 12:36 PM
To: [log in to unmask]
Subject: Re: [DC] Finished thickness tolerance
Gary,
IPC-4101carries tolerances by Class for laminates; laminates in this case
could be a double-sided thick board or could be the thin cores used to
construct multilayers. IPC does not tolerance the finished thickness of a
multilayer composite of many thin cores and prepregs.
The tolerance of the multilayer is not the sum of the tolerance of the
thin cores and prepregs, otherwise it would always be very large; the
"bet" is that not all the individual elements run to the top of the
tolerance or all the individual parts run to the bottom on their
tolerance, but rather some might be high and some might be low, so the
accumulated tolerance in practice is less than the sum of the individual
tolerances due to some cancelling.
Typical tolerance for a finished multilayer is +/-10%; +/-7%, for
instance, would be considered "tight"; the tolerances you listed would be
considered good tolerances for high yield relative to overall thickness in
a volume running mode.
The other contributor to the tolerance for multilayers is that frequently
the exact thickness of any prepreg section will vary somewhat from the
design nominal effectively "using up" some of it's tolerance. This is
because a single ply fill will press out to one thickness while a two or
three ply (sheets) of the same prepreg fill will press out to something
other than 2 or 3 times the single ply. Also the amount of retained copper
on the facing layers and the thickness of the foil will have a strong
influence on the nominal fill thickness after pressing - and it is likely
to vary somewhat from the design nominal. Those little shifts in thickness
are accounted for in the total tolerance.
Based on the above, boards with fewer elements (cores and sheets of
prepreg) will vary less from nominal, if the nominal is derived from the
empirical build thickness, than boards with many elements. You might be
able to get a tighter tolerance by working with your suppliers. In
general, +/-10%, for the most part, works out for the majority of builds.
Some special builds can be gotten tighter but you need to get close to the
real choices that the fabricator will use for the cores and prepregs, and
even then one board with the same elements as another board will press to
a different nominal depending on the retained copper features on the
foils.
If anyone know more about this, if there is a better guide, I also would
like to know.
Regards,
Valerie
"Brooks,Bill" <[log in to unmask]>
Sent by: DesignerCouncil <[log in to unmask]>
03/09/2005 12:03 PM
Please respond to "(Designers Council Forum)"; Please respond to
"Brooks,Bill"
To: [log in to unmask]
cc:
Subject: Re: [DC] Finished thickness tolerance
Hi Gary,
You'd be surprised how often this sort of question pops up.
The 'standard' thickness for PCB's here in the US I believe was derived
from
the single and double sided board days back in the 1960's era... Material
was offered clad with copper in various thicknesses and in 1/32 inch
increments. It is still the 'defacto' standard. That's why you see so many
people specifying .031 (.03125) .063 (.0625) .094 (.09375) .125 thickness
materials. In fact the industry has become so flexible now that we could
specify just about any thickness we need in .002 in. increments because
that's the standard thickness of the prepreg material used to build up the
final thickness of any multilayer board. I think they still sell the
single
and double side clad materials though... If you check with your chosen
board
manufacturer I'm sure they can tell you what materials they normally stock
and use and will give you a broad range of options for finished board
thickness... even if you are designing in metric. :)
Best regards,
Bill Brooks - KG6VVP
PCB Design Engineer , C.I.D.+, C.I.I.
Tel: (760)597-1500 Ext 3772 Fax: (760)597-1510
e-mail:[log in to unmask]
http://www.dtwc.com
http://pcbwizards.com
-----Original Message-----
From: Gary M. Koven [mailto:[log in to unmask]]
Sent: Wednesday, March 09, 2005 8:05 AM
To: [log in to unmask]
Subject: [DC] Finished thickness tolerance
We design Class 2 boards and have been specifying on drawing finished
thickness 0.031 in +/- 0.004 in or 0.062 in +/- 0.008 in.
I'm looking for the finished thickness tolerance tables by class. I could
not find these details of what I need in IPC-2221, 2222, 6011, or 6012,
just
vague general references. Are these in IPC-4101?
If anyone can verify or correct what we have been specifying and reference
whatever updated standard to use, I'd appreciate it.
TIA and Best Regards,
======================
Gary M. Koven
Engineering Services Manager
Dynazign, Inc.
806 Tyvola Road, Suite 100
Charlotte, NC 28217
P: 704.405.1234 x210
F: 704.405.1402
http://www.dynazign.com/
----------------------------------------------------------------------------
-----
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
---------------------------------------------------------------------------------
|
