[PCB_FORUM] Re: GND Clearance Under SMD Pads
- From: ameehan@xxxxxxxxxxxxxx
- To: icu-pcb-forum@xxxxxxxxxxxxx
- Date: Wed, 13 Oct 2010 09:05:57 -0700 (GMT-07:00)
I asked for more details, and:
1. Yes, it is for impedance matching purposes, as Gerry said
2. It is for coupling capacitors, not decoupling (sorry)
Thanks for all your feedback. I've created a footprint with that clearance and
tested it, and as long as we match layer names (from footprint to .brd), it
works great.
-----Original Message-----
>From: "Schwartz, Jerome" <jschwa01@xxxxxxxxxx>
>Sent: Oct 13, 2010 7:25 AM
>To: icu-pcb-forum@xxxxxxxxxxxxx
>Subject: [PCB_FORUM] Re: GND Clearance Under SMD Pads
>
>I have seen this requirement, in the data sheets, for series caps in an
>Ethernet application.
>I use anti-etch with split planes. Maybe you could build into your
>footprint
>an anti-etch all layer.
>
>Jerry
>
>
>
>-----Original Message-----
>From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
>[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Dave Schaefer
>Sent: Wednesday, October 13, 2010 10:21 AM
>To: icu-pcb-forum@xxxxxxxxxxxxx
>Subject: [PCB_FORUM] Re: GND Clearance Under SMD Pads
>
>Would like to see where the requirement came from, I'm quite certain
>it's untested/unproven. Without a measurement, it seems you would be
>decreasing your decoupling capacitance effectiveness.
>
>Be interesting to get the source of the requirement and cross post to
>the experts over on SI List to get their opinions.
>>
>> From: "Jean Bratton" <jean.bratton@xxxxxxxxxxxxxx>
>> Date: 2010/10/13 Wed AM 06:56:02 CDT
>> To: <icu-pcb-forum@xxxxxxxxxxxxx>
>> Subject: [PCB_FORUM] Re: GND Clearance Under SMD Pads
>>
>> I've seen this request for AC Blocking caps on high speed nets,
>reasons
>> as suggested by Gerry, but not decoupling caps...
>>
>>
>>
>> Jean Bratton
>>
>> Senior PCB Designer
>>
>> Freedom CAD Services, Inc.
>>
>> Phone: 603-864-1349
>> begin_of_the_skype_highlighting 603-864-1349 end_of_the_skype_highlighting
>>
>> Skype: jean.bratton
>>
>> Email: jean.bratton@xxxxxxxxxxxxxx
><mailto:jean.bratton@xxxxxxxxxxxxxx>
>>
>> Visit us at http://www.freedomcad.com <http://www.freedomcad.com>
>>
>>
>>
>>
>>
>> From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
>> [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Randy Dawson
>> Sent: Wednesday, October 13, 2010 4:43 AM
>> To: icu-pcb-forum
>> Subject: [PCB_FORUM] Re: GND Clearance Under SMD Pads
>>
>>
>>
>> Hi Alexis,
>> Unless I am missing something here, you want that decouple cap signal
>to
>> launch immediately to the GND layer...
>>
>> No voids underneath in it either. Question them.
>>
>> Randy
>>
>>
>>
>> ________________________________
>>
>> From: kathy_descoteaux@xxxxxxxxxxx
>> To: icu-pcb-forum@xxxxxxxxxxxxx
>> Subject: [PCB_FORUM] Re: GND Clearance Under SMD Pads
>> Date: Tue, 12 Oct 2010 20:17:36 -0400
>>
>> Hi Alexis..
>>
>> Did you try to add a route keepout on the second layer? It should
>clear
>> out the gnd plane on the second layer if its a dynamic shape. There
>may
>> be an issue when it's placed on a brd with a different layer name for
>> the second layer... a minor update to the footprint and you should be
>> good to go. Just thinking... not sure if it will work.
>>
>> Kathy Descoteaux
>>
>>
>>
>>
>> ________________________________
>>
>> Date: Tue, 12 Oct 2010 20:07:19 -0400
>> From: ameehan@xxxxxxxxxxxxxx
>> To: icu-pcb-forum@xxxxxxxxxxxxx
>> Subject: [PCB_FORUM] GND Clearance Under SMD Pads
>>
>> For a high speed application, we've had a request from engineering to
>> create a special footprint for decouplers (0402, 0201) with a GND
>> clearance under the pads. The clearances will be the same size as the
>> pads, and will just affect the ground plane on layer 2. I'm trying to
>> figure the best way to do this. I thought I could just build a special
>> padstack, but Allegro (using XL 16.3) won't allow me to build an SMD
>> padstack with an anti-pad unless I define a drill, bottom side pad,
>etc.
>> But I'm not seeing a clean way to build this into the footprint symbol
>> either. Any ideas?
>> Thanks.
>> Alexis Meehan
>> Violin Memory Inc.
>> Mtn View, CA
>> ----------------------------------------------------------- To
>> subscribe/unsubscribe: Send a message to
>> icu-pcb-forum-request@xxxxxxxxxxxxx with a subject of subscribe or
>> unsubscribe To view the archives of this list go to
>> //www.freelists.org/archives/icu-pcb-forum/ Problems or
>Questions:
>> Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
>> -----------------------------------------------------------
>>
>>
>>
>
>-----------------------------------------------------------
>To subscribe/unsubscribe:
>Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx
>with a subject of subscribe or unsubscribe
>
>To view the archives of this list go to
>//www.freelists.org/archives/icu-pcb-forum/
>
>Problems or Questions:
>Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
>-----------------------------------------------------------
>-----------------------------------------------------------
>To subscribe/unsubscribe:
>Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx
>with a subject of subscribe or unsubscribe
>
>To view the archives of this list go to
>//www.freelists.org/archives/icu-pcb-forum/
>
>Problems or Questions:
>Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
>-----------------------------------------------------------
-----------------------------------------------------------
To subscribe/unsubscribe:
Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx
with a subject of subscribe or unsubscribe
To view the archives of this list go to
//www.freelists.org/archives/icu-pcb-forum/
Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
-----------------------------------------------------------
Other related posts:
