[SI-LIST] Re: Remove ground plane under connector pads?
- From: "Lee " <leeritchey@xxxxxxxxxxxxx>
- To: <scott@xxxxxxxxxxxxx>, <jonathan.lloyd.riley@xxxxxxxxx>
- Date: Mon, 8 Dec 2014 09:41:02 -0800
From tests we have made, removing ground from underneath the mounting pads
of capacitors is not worth doing.
-----Original Message-----
From: Scott McMorrow
Sent: Saturday, December 06, 2014 5:36 PM
To: jonathan.lloyd.riley@xxxxxxxxx
Cc: si-list@xxxxxxxxxxxxx ; Jim Nadolny ; michael.p.brownell@xxxxxxxxx ;
andrew@xxxxxxxxxxxxxxxxxx
Subject: [SI-LIST] Re: Remove ground plane under connector pads?
The answer is. It depends. The ultimate solution is to promise with a 3D EM
tool like HFSS. But a good first approximation for most commercial boards
with thin dielectrics with plane on layer 2 is to create an antipad on
layer 2 that is ate same size as the pad. It will not be optimal, but it
will help.
Scott
On Dec 6, 2014 6:49 PM, "Jonathan Riley" <jonathan.lloyd.riley@xxxxxxxxx>
wrote:
> Hi Andrew
> One problem with connector pads is that they're frequently rather wider
> than the traces that you're using. This results in a lowering of the
> impedance at that point. To maintain a constant impedance for a
> differential signal you can change both the trace width and the
> separation,
> but even so, there are limits and going from a 0.11mm trace to a 0.5mm
> trace (the pad width) is too much for just increasing the separation.
>
> Instead the approach is to increase the distance of the signal from the
> reference plane. We can't make the PCB thicker, but it is possible to cut
> away the copper underneath the pads, thus increasing the distance from the
> connector pad to the plane and so raising the impedance. How useful the
> technique is will also depend on how close the next layer down happens to
> be and just how big the apertures are that you're going to make. Also the
> amount of perforations in the reference plane will affect the assumptions
> made when the advice to do this was given and too many holes too close
> together will sooner or later make those assumptions break down. At that
> point the advice becomes counter productive. The impedance where the holes
> are is higher, but not exactly uncontrolled, rather it is now dependent on
> more factors. The key thing is that you've moved it in the right
> direction.
> It remains a fairly crude approximation though.
>
> There are a number of manufacturers that recommend this practice in their
> application notes for things like PCIe and other differential serial
> interfaces. Some also require this for the AC coupling capacitors that are
> often a feature of differential links.
>
> If the manufacturer tells you to do this, it is best to follow their
> instructions since if there are problems you can say that you followed
> their instructions correctly.
>
> Perhaps others in the group might have data on the actual difference
> between a board with apertures and the same one without them. People with
> 3D solvers will be able to model this and know what the impedance does
> where the apertures are.
>
> Regards
> Jon
>
> On 6 December 2014 at 19:23, Brownell, Michael P <
> michael.p.brownell@xxxxxxxxx> wrote:
>
> > Have you checked with Jim Nadolny at Samtec?
> > Regards,
> >
> > Mike
> >
> >
> > -----Original Message-----
> > From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx]
> > On Behalf Of Jory McKinley
> > Sent: Saturday, December 06, 2014 11:04 AM
> > To: andrew@xxxxxxxxxxxxxxxxxx; si-list@xxxxxxxxxxxxx
> > Subject: [SI-LIST] Re: Remove ground plane under connector pads?
> >
> > Hello Andrew,Removing metal under the SMT pads without regard to return
> > currents will create a local uncontrolled impedance which will most
> likely
> > affect your channel margins through launch discontinuities, potential
> > unwanted coupling and mode conversion. These affects may or may not be
> > problematic depending on your overall channel. If you able design your
> SMT
> > launch to include a return reference which will in most cases be
> somewhere
> > lower (higher) in the board stack-up. Need to do this analysis with a
> > 3D
> > tool.Regards,-Jory Jory McKinley McKinley Consulting
> > e-mail: jory_mckinley@xxxxxxxxx
> > phone: (774)-285-2859
> > From: Andrew Holme <andrew@xxxxxxxxxxxxxxxxxx>
> > To: si-list@xxxxxxxxxxxxx
> > Sent: Saturday, December 6, 2014 9:28 AM
> > Subject: [SI-LIST] Remove ground plane under connector pads?
> >
> > Hi,
> > Is it standard practice to remove copper from the ground plane under
> > high-speed connector SMT pads?
> >
> > I'm designing a board with 100-ohm differential pairs carrying 5.4 Gbps
> > data terminating at a Samtec ERM8 connector. For my stack-up, the
> > differential traces are 0.11 mm wide and 0.17 mm apart. The connector
> pads
> > are 0.5 mm by
> > 2.0 mm. Should I remove an equal area of copper from the ground plane
> > directly under each pad?
> >
> > Thanks,
> > Andrew.
> >
> > ------------------------------------------------------------------
> > 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
> >
> >
> >
> >
> >
> > ------------------------------------------------------------------
> > 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
> >
> >
> > ------------------------------------------------------------------
> > 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
> >
> >
> >
>
>
> ------------------------------------------------------------------
> 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
>
>
>
------------------------------------------------------------------
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
-----
No virus found in this message.
Checked by AVG - www.avg.com
Version: 2015.0.5577 / Virus Database: 4235/8691 - Release Date: 12/06/14
------------------------------------------------------------------
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
Other related posts:
