see: Todd Hubing, "Power Bus Decoupling on Multilayer Printed Circuit Boards",
IEEE Trans. Electromagnetic Compatibility, May 1995.
In a configuration similar to yours, Todd measured about 2nH
(see the paper for details). One difference between his
setup and yours is that I believe Todd was using a four-layer
board, with a substantially larger gap from the top surface
to the ground plane than you are planning. His gap was
probably on the order of 20-30 mils. You are planning 14 mils.
That should cut your inductance to half of his (or about 1 nH).
Other brief notes:
The new 0612 SMT capacitors (with pads on the long sides, as opposed
to the 1206-style with pads at the ends) have a better
aspect ratio, and thus a lower inductance. They do even
better than 0805's. Check with you vendor to see if
they make an 0508 side-mounted style.
Best regards,
Dr. Howard Johnson
>X-From_: [email protected] Mon Nov 25 14:44:43 1996
>Errors-To: [email protected]
>From: "Don Abernathey" <[email protected]>
>Date: Mon, 25 Nov 1996 14:37:21 -0800
>To: [email protected]
>Subject: (Fwd) Re: Help with decoupling cap inductance
>
>Hello!
>
>Here is Larry's input to my inductance problem.
>
>I appreciate the input. :)
>
>
>
>*************************
>Thank you |
> Don Abernathey |
>(503)690-6234 |
>[email protected] |
>*************************
>
>--- Forwarded mail from [email protected] (Larry Smith)
>
>Date: Mon, 25 Nov 1996 14:07:57 -0800
>From: [email protected] (Larry Smith)
>To: [email protected]
>Subject: Re: Help with decoupling cap inductance
>
>Don - I did some finite element (Ansoft) modeling of a structure similar
>to yours, and decided the loop inductance was about .85 nH.
>
>My structure was an 805 size capacitor sitting on solder pads with vias
>to the power and ground planes at the outside edges of the pads:
>
> +-------+ +-------+
> | | | |
> | +--------------+ |
> - | | -
> / | | \
> | O | | O |
> \ | | /
> - | | -
> | +--------------+ |
> | | | |
> +-------+ +-------+
>
>cap: 80x50 mils
>pad: 40x?? mils
>space: 60 mils (therefor, via pitch was 100 mils)
>via pad: 30 mils
>via barrel: 12 mils
>via depth to 1st power plane: 14 mils
>
>I assumed that the capacitor was a perfect conductor because I wanted the
>loop inductance at high frequency. This will make my answer a bit low
>because current really travels through the capacitor body, which is further
>above the PCB power planes. The most important part of the problem is the
>space between the vias (100 mils), via diameter and depth to the power
>planes.
>This determines the loop area that current must go around. I put a 2d
>current
>source in one of the vias to force current around the loop. Ansoft told
>me there was some amount of energy when I forced 1 amp. Energy is 1/2 L*I*I,
>so loop inductance was easily calculated to be .85 nH.
>
>Your vias are a long way apart (215 mils). You have further to go to your
>power planes (probably 20 mils if copper thickness is included). My guess
>is that your loop inductance is closer to 2.61 nH. You might want to go
>negotiate with manufacturing to put those vias in the pads.
>
>regards,
>Larry Smith
>Sun Microelectronics
>
>----- Begin Included Message -----
>
>>From [email protected] Mon Nov 25 10:13:18 1996
>From: "Don Abernathey" <[email protected]>
>Date: Mon, 25 Nov 1996 10:12:49 -0800
>To: [email protected]
>Subject: Help with decoupling cap inductance
>Cc: [email protected]
>Mime-Version: 1.0
>
>Hello!
>
>I don't have access to a 3D field solver and I'm not sure that I trust
>hand calculations.
>
>I need some help determining the inductance contribution of a via, as
>part of the loop formed by an 0805-size MLC capacitor connected
>between power and ground as is commonly done for IC decoupling
>applications.
>
>Here is a common layout for an 0805 SMT decoupling cap:
>
> |<-----------------Total------------------->|
> | | | | | | | |
> |Via|Trace|Solder pad|Space|Solder pad|Trace|Via|
> | | | | | | | |
> VCC GND
>
>Via = 25mil OD pad, 13mil drill, 10mil finished hole
>Trace = 20mil long, 25mil wide
>Solder pad = 50mil square pad
>Space (distance between pads) = 40mil
>Total (center to center) = 215mil
>
>The following is a portion of the layer stackup of a board. The cap
>layout described above be created on the pad layer. The GND via would
>be connected to both layers 2 and 5. The VCC via would be connected to
>layer 6.
>
>1 ----Pad Layer----
> XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX 3mil
>2 ------------------------------------------------------------ GND
> XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX 5mil
>3 --signal---
> XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX 5mil
>4 --signal--
> XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX 5mil
>5 ------------------------------------------------------------ GND
> ZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZZ BC 2mil
>6 ------------------------------------------------------------ VCC
>
>Er = 4.3, GND = 1oz, signals = 1/2oz.
>
>Any input is appreciated.
>
>
>
>*************************
>Thank you |
> Don Abernathey |
>(503)690-6234 |
>[email protected] |
>*************************
>
>
>----- End Included Message -----
>
>
>
>
>---End of forwarded mail from [email protected] (Larry Smith)
>
>
_________________________________________________
Dr. Howard Johnson, Signal Consulting, Inc.
16541 Redmond Way, Suite 264, Redmond, WA 98052
U.S. tel (206) 556 0800 // fax 206 881 6149 // email [email protected]