Yes you should account for capacitor+layout+leads but I would have to
agree with what Howard Johnson wrote in Electronic Design, April 14,
1997, p167, that is digital circuit decoupling will work above
resonance too, as long as the impedance is below a certain magnitude.
(be sure your font for the pictures are fixed length, i.e. courier)
C R L
Rough Plot Of Real World Capacitor: ---||---/\/\/\----OOO----
| \ /
| \ /
| \ /
Z |----\ ----/------ Z say = 1 ohm
| \ /
| \-/
|---------------------
frequency
I do agree that putting vias in parallel will decrease the inductance,
put in a lot but they cost and they take up routing channels so you will
be in a fight with the layout folks. We are always in the trade-off
business.
So that's my two cents.
Keep up the discussions...
John
>----------
>From: [email protected][SMTP:[email protected]]
>Sent: Monday, April 28, 1997 10:56 AM
>To: [email protected]
>Cc: [email protected]
>Subject: Re: Power/ground connections/bypassing on ICs
>
>
>Andy,
>
>One question and a lot of different answers, here's mine:
>
>Decoupling for me is to stop the noise from an IC before it spreads all
>over the board. You need a *good* groung plane for this and the right
>bypass capacitor with a low-inductance layout. Bringing ground from
>the plane is not what I would do, you possibly have a slight ground shift
>depending on the consumption and additional inductance.
>
>
>Try it like this:
>
>
> +----------+
> ###| |###
> vias | |
> x x ###| |###
> ===== | |
> x=###=x ###| GND |###
> capacitor | | | |
> =###===###| VCC |###
> x=====x | |
> x x ###| |###
> +----------+
> I.C.
>
>
>Putting several vias in parallel decreases inductance and thus increases
>the resonance frequency.
>
>Decoupling only works below the self-resonance of capacitor+layout+IC leads.
>
>A different approach to this subject you can find in the article of Prof.
>Christian Dirks in the german magazine "Elektronik" 23/1996.
>
>Regards,
>Michael
>
>
>----- Begin Included Message -----
>
>From [email protected] Mon Apr 28 18:10:57 1997
>Date: Mon, 28 Apr 97 11:40:12 -0400
>From: [email protected] (Andy Ingraham)
>To: [email protected]
>Cc: [email protected]
>Subject: Power/ground connections/bypassing on ICs
>
>I am tempted to open, once again, the discussion about how to connect
>power and ground pins to ICs on a multi-layer PCB, and how best to
>bypass them.
>
>I have held the firm belief that IC power and ground pins should
>always be tied right to their planes as soon as possible, with the
>shortest trace lengths. Then bypass capacitors can be added near
>those pins.
>
>Some have suggested the alternative of bringing power and ground from
>the planes, first to the bypass capacitor, and then to the IC pins,
>something like this:
>
> +----------+
> ###| |###
> | |
> ###| |###
> vias | |
> X=====###========###| |###
> | | | |
> X=====###========###| |###
> bypass | |
> capacitor ###| |###
> +----------+
> I.C.
>
>I feel this is dangerous because of the added inductance. The
>power/ground planes are your best high frequency bypass capacitor
>(although a small one), so I'd think you want to get your IC pins
>brought to them as quickly as possible, without wasting etch going to
>a discrete capacitor which may not be very effective anyway if it's
>above self resonance. Also the power and ground pin inductance is
>effectively in series with all output drivers when they switch. So
>I avoid this technique.
>
>But I recently had a short discussion with an engineer who promoted
>the latter, and insisted it was better in mixed-signal environments.
>Most of my work has been straight digital lately, though I do find
>myself surrounded by a smattering of mixed-signal components for such
>things as ethernet.
>
>The presumed justification is that these mixed-signal devices benefit
>from the additional small filtering provided by the trace inductance.
>
>By the way, the IC under discussion had all digital inputs and
>outputs, but some internal clock re-timing, and no vendor
>recommendations regarding power filtering.
>
>Does it make sense to do this? Do I want to adopt a strategy of using
>the first method for straight digital devices, and the second method
>for mixed-signal devices that don't use filtered power?
>
>Is it wise to do this with both power and ground leads? Or should
>ground pins always route directly to the ground plane, with longer
>traces in only the power leads? (Assuming no PECL, of course.)
>
>Thanks for advice.
>Regards,
>Andy Ingraham
>
>
>----- End Included Message -----
>
>