Re: Power/ground connections/bypassing on ICs

Don Abernathey (
Mon, 28 Apr 1997 14:45:47 -0700

Power and ground connections seem to be dictated by layout concerns
and soldering concerns. E.g. a BGA and an SOIC use different pad to
via connection techniques, the BGA using a short (xxxmil) trace to via
or sometimes pad-in-via, and the SOIC using a pin-escape (short, fat

Assuming for a moment that pad-in-via yields the lowest inductance
connection, I can tell you that I have never seen pad-in-via done on
an SOIC footprint. Why? Because it is harder to solder. I believe that
short-trace-to-via (dog bone) and pad-in-via are done in BGAs
primarily because they are the most cost-effective (mainstream) method
of high-density soldering, with dog bones seemingly more popular than

These are correct tradeoffs since the mainstream applications for our
technology are cost driven. Volume, mainstream manufacturing technology
is more important than engineering performance. Design
it once but build a zillion. It could be that a few less DPM (solder
joints) is worth more than a few extra millivolts of noise margin.

I have used long, thin microstrip traces (pad layers) and a couple
0805 SMT caps to make an analog filter for an ethernet chip. But to
tell the truth it was a shot in the dark. I knew the value of the
inductances and capacitances and SPICE told me the behavior of the
network over frequency, but I had no clue what the interaction with
the ethernet chip would be. But this was also a fairly safe design
since the Bit Error Rate of ethernet is something that few folks would
notice unless it is grossly bad.

I have also had IC vendors write app-notes dictating the use of
ferrite beads and split planes without providing one shred of evidence
that it was necessary, but only the words "good analog design
practice"- yeah right. No design target.

I believe in low-impedance connections for bypassing, high-impedance
for filtering and split planes when I want to make sure that I know
where currents are flowing. About the only thing that is accomplished
by mixing filtering with the bypassing is to slow the edge rate -
great if that is what you want to do.

Thank you |
Don Abernathey |
(503)690-6234 | |

On Apr 28, 11:40am, Andy Ingraham wrote:
> 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 of excerpt from Andy Ingraham