Hitesh,
I have to agree with Alex: worse case. In addition to the variations in the X
Y alignment, there is also the variation in Z, prepreg thickness after press.
Do you care about routing density?
Aubrey
Sent from my iPhone
On May 11, 2017, at 2:10 AM, Alexander Ippich
<alexander.ippich@xxxxxxxxxxxxxxx> wrote:
Hitesh,
you are talking about the worst case scenario with a broadside coupled
stripline with laminates between signal and reference and prepreg between
the pair.
In manufacturing, the signal and reference layer will be aligned (with the
obvious tolerances) to each other for a laminate. One side of the laminate
(for the sake of discussion, say it's the upper side) will have the
fiducials for the post-etch punch.
So for the upper laminate, there will be a misalignment between the trace
and the fiducicals on top already. Then you add tolerances in the process
of punching the alignment holes for the laminates.
For the lower laminate, the fiducials for PEP would be on the same side as
the traces, so not additional tolerance beside the ones from the punching
process itself
Then you continue into lay-up, where you but the laminates on top of each
other with prepreg in between. Alingment between the cores in the stackup
will be by means of alignment pins, using the holes created by the
post-etch-punch. Yes, there are pinless lamination processes as well, but
most shops will use pins.
Because of the mechanical process, the holes will be not perfect.
Sometimes, operators push them too hard over the pins and things like
that. End result: laminates will be shifted against each other.
Bottom line, the upper and lower trace in your differential pair may see
significant misalignment, easily in excess of 0.004". So I would recommend
to either use broad-side coupled pairs with the traces on the same
laminate or edge-side-coupled.
Best regards,
alex
--------------------------------------------------------------------------
--------------------------------------------------------------
Alexander Ippich
Senior Signal Integrity Engineer
OEM Marketing Europe
e-mail: alexander.ippich@xxxxxxxxxxxxxxx
web: www.isola-group.com
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx]
On Behalf Of Hithesh
Sent: Thursday, May 11, 2017 8:51 AM
To: SI-List
Subject: [SI-LIST] PCB Manufacturing tolerance vs impedance
For the case of broadside coupled striplines with prepreg as dielectric
layer between them, what is the typical tolerance.
Ideally, the offset (in x direction) will be zero for stripline on either
side of prepreg. So the traces will be on top of each other.
How much tolerance should I expect from PCB manufacturing typically?
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
List archives are viewable at:
//www.freelists.org/archives/si-list
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
--
Any quotation or order confirmation provided with this communication is
subject to Isola’s standard terms and conditions of sale which can be found
here http://www.isola-group.com/about-us/terms-conditions/ ;
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
List archives are viewable at:
//www.freelists.org/archives/si-list
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
