From: Jeff Cain ([email protected])
Date: Thu Oct 21 1999 - 17:24:30 PDT
At one time I actually showed this using an FDTD scheme. The actual "effective" dielectric constant
approaches an asymptote as you add more and more vias. Using the same dielectric constants, 4 and 16,
the "effective" dieletric constant approaches 7.2. So doing the square root stuff leads to an increase of
the velocity by a factor of 0.34, which is indeed very close to Larry's solution.
Not only did the above result come as a pleasant surprise, when we added striplines the propogation
delay did not change. That is to say whether we via-ed the two planes together or not, didn't change the
velocity of the waves on that line.
Larry Smith wrote:
> > From: "Ingraham, Andrew" <[email protected]>
> >
> > An interesting question is what happens if you have a power/ground sandwich
> > around a high-Er material and another around a low-Er material, with the two
> > sets of planes stitched together regularly, which is what I think Tom
> > Woodward was asking. Can that let your noise source get access to more
> > "points" on the high-Er sandwich?
> >
> > Andy
>
> Andy - You bring up an interesting question that I considered some time
> ago. Suppose we have the stackup below with two parallel power planes
> referenced to a center ground plane. The relative permitivity of one
> dielectric is 4 and the other is 16:
>
> ======================== Vdd plane ======================
>
> eR=4 Vel = 0.5 * light
>
> ======================== Gnd plane ======================
>
> eR=16 Vel = 0.25 * light
>
> ======================== Vdd plane ======================
>
> If we started a plane wave on the edge of the PCB by stimulating each
> Vdd plane wrt the Gnd plane, a disturbance would propagate on the top
> layer wrt Gnd at half the speed of light (velocity is proportional to
> 1/sqrt(eR) ) and at 1/4 the speed of light on the bottom plane. At the
> frequencies that we are concerned about in signal integrity, skin
> effect will keep the current on the top surface of the ground plane
> away from the bottom surface of the ground plane, and the top and
> bottom disturbances just move down the PCB without interfering with
> each other, one twice as fast as the other. The velocity is 1/sqrt(LC)
> where L is the inductance per inch and C is the capacitance per inch
> (easily calculated). If the dielectric thicknesses are the same, the
> capacitance of the bottom plane is 4x the capacitance of the top
> plane.
>
> Now suppose we stitch vias from the top Vdd plane to the bottom Vdd
> plane at regular intervals along the way. Neglecting the inductance of
> the vias, the top and bottom plane must be at the same potential wrt
> the Gnd plane. The wavefront on the top and bottom plane must now move
> at the same velocity, or at least re-adjust themselves at every via
> along the way.
>
> A good way to look at the stitched-together power planes is capacitors
> in parallel and inductors in parallel. It turns out that the
> inductance per inch of the connected power planes is half of the two
> independent power planes. The capacitance per inch is C + 4C = 5C,
> where C is the capacitance per inch of the top power plane and L is the
> inductance per inch of either power plane. So the velocity of the
> combined planes is 1/sqrt(0.5L*5C) = 1/sqrt(LC) * 1/sqrt(2.5). It ends
> up being 0.316 times the speed of light, which is somewhere between the
> velocity of each individual dielectric.
>
> In a real PCB, an ASIC or uP that draws power from the power plane is
> likely to located in the center of the board. In this case, a radial
> disturbance will emanate out from the noise source at a velocity that
> is consistent with the combined dielectrics.
>
> Hans Mellberg brought up the possibility of these same power planes
> providing return current for signal traces. This is certainly possible
> and commonly done. If there are signal traces adjacent to the Vdd
> planes (top and bottom in the above stackup), signals on those traces
> propagate at the velocity of light reduced by 1/sqrt(eR) where eR is
> the relative permitivity of whatever dielectric is between the trace
> and the Vdd plane. Once again, with copper power planes of normal
> thickness (1 or 1/2 oz copper), skin effect prevents any coupling
> between power plane currents and signal return currents at the
> frequencies that we are concerned about in signal integrity (greater
> than 10 MHz).
>
> regards,
> Larry Smith
> Sun Microsystems
>
> **** To unsubscribe from si-list: send e-mail to [email protected]. In the BODY of message put: UNSUBSCRIBE si-list, for more help, put HELP. si-list archives are accessible at http://www.qsl.net/wb6tpu/si-list ****
-- Jeff Cain Technical Leader Cisco Systems 170 W Tasman SJ-G1 Santa Clara, CA 95134 408-527-7754 408-526-6899**** To unsubscribe from si-list: send e-mail to [email protected]. In the BODY of message put: UNSUBSCRIBE si-list, for more help, put HELP. si-list archives are accessible at http://www.qsl.net/wb6tpu/si-list ****
This archive was generated by hypermail 2b29 : Tue Feb 29 2000 - 11:39:17 PST