Hi Lee Lot of presentation and simulation prove this is a useful tech for most of high speed application. Regards. Tesla At 2014-12-09 01:57:28, "Scott McMorrow" <scott@xxxxxxxxxxxxx> wrote: >It depends on the stackup thickness between L1 and Ground. > >Scott McMorrow >Teraspeed® Consulting - A Division of Samtec >16 Stormy Brook Rd >Falmouth, ME 04105 >(401) 284-1827 Business >http://www.teraspeed.com > >On Mon, Dec 8, 2014 at 12:41 PM, Lee <leeritchey@xxxxxxxxxxxxx> wrote: > >> 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 > > ------------------------------------------------------------------ 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