Filter capacitance in PCB layout trace

Hi,

I'm laying out a DC/DC converter in a PCB layout software. In the input filter where the high current will go through, I have an array of capacitors laid on a large pad (to decrease trace resistance). This might be a dumb question... but will having the large pad affect the capacitor filter array and how much the signal is filtered?
Just to try to illustrate what I'm trying to ask, I've inserted a picture. Since I1 is going right at the surface of the capacitor, it will be filtered. But since I have such a large pad, will there be current (I2) going through the top and won't be filtered through the capacitor? Or since capacitors filter out voltage changes, does having a large pad just won't affect it?

Thanks!

Hi peatear,
At the frequencies of a DC/DC converter, your whole pad is a single node, i.e. both red dots are short circuited, unless you don't have enough copper, so the larger the better. In particular, on your drawing, the current is going from the "in" node into the capacitors, and from the capacitors to "out". Very little will go directly from in to out, and it will take the path of least impedance = resistance + inductance, i.e. i1.

JP

For an exact analysis, all involved circuit impedances must be considered.

I presume that a lumped circuit analysis is appropriate (dimensions < 1/10 wavelength). You can decompose the copper pour into a 2-D ladder of partial inductances. In so far it's correct to say there's a path around the bypass capacitors. But to adjust the view, the inductance values must be considered, too. The capcacitors' series and ground connection inductances will considerably larger than that of the copper pour. And the source impedance will be probably even larger.

Generally, a reasonably designed low-pass filter is comprised of a series filter element (usually an inductor) and a parallel capacitor. If the sum of series and source impedance isn't high enough, the capacitor can't work. The same for a large capacitor series inductance or bad ground connection.

The best way to lay out surface mount capacitors for maximum filter effect is to run the signal directly through the pad for each capacitor. Thus the line should narrow down to the pad height at each capacitor (unless that trace width is too narrow for the current going through it). That will minimize the bypassing of the high frequency noise around the pad and capacitor. And the bottom (ground) side of the capacitor should go directly to a ground (flooded) plane thermal relief pad on the same side of the PCB as the capacitor.