I want to know If I put the ground plane on the bottom as you have shown and on the top layer I put the Vcc plane will that be a better Idea or not.

Hallo Prahlad,

no, this would not be a better solution. Ground plane makes much more, than only providing low inductivity of ground connections!! One additional benefit is, that ground plane is shielding the many signals from each other. If you have a multilayer board you get a distance of about 100µm between the individual layers. So, if two tracks running next to another are farer away from each other than their distance to ground plane, then both tracks are very effectively shielded against each other. Means, stray capacitance between them decreases very much and finally reaches a level which can be ten times smaller, as if there were no ground plane to them.
If you have only a double sided PCB, then both layers have a distance of about 1.6mm. Then, this shielding of underlaying ground plane does not work so good. In this case it's of benefit also to have a bit ground plane between the traces.

Another effect of ground plane is to drastically decrease loops formed by signal and Vcc lines and their according ground return currents. Here the additional ground plane on component side additionally minimizes the resultant loop area, because with only double sided PCB, distance to solid ground plane is much higher than with multilayer board. To achieve this both ground planes must be connected to another at many places, either at pins of chips (through hole parts) or by many vias.

Additional ground plane on component side has another task. With double sided PCB it's not easy always to provide real solid ground plane, if extended bus structures has to be routed. As result, the solid ground plane becomes more and more interrupted. Then, like Michael mentioned, this additional ground plane on component side can drastically help to regain the benefits of solid ground plane.

Make no mistake, in my last reply I stated, that low inductivity ground connections are needed. But also for Vcc connections inductivity must be low, even if it's less demanding than for ground connections. Inductivity of Vcc tracks can be heavily decreased, if power supply decoupling capacitors are used with EACH chip, so that distance of undecoupled Vcc tracks is no longer than about 5cm, or so. Many people always think of resonance frequency of decoupling capacitors and believe, that this resonance frequency must be very high in order to provide effective decoupling even at very high frequencies above 100MHz, where 74HCMOS chips produce a lot of noise. And finally the toy arround with 100pF capacitors. They totally forget, that there's always a certain distance between terminals of decoupling capaitors and power supply terminals of digital chips. It's the inductivity of these copper tracks which counts. And it's the solid ground plane running from ground pin of decoupling capacitor to ground pin of digital chip, which is the ONLY way to minimize this effective inductivity!!!

At ultra high frequencies, between 100MHz to 1GHz, decoupling capacitor in combination with its ground plane connection to ground pin of digital chip only looks like pur einductiviy, in the equivalent circuit model. No storage capabilities, only inductivity. And the only benefit of this decoupling capacitor is, that it heaviliy minimizes source impedance of Vcc connection to power supply unit. Assume a narrow copper track of 5mm width and 20cm lenght is running from your digital chip to power supply unit. Then this gives an inductivity of about 200nH as a rule of thumb. But if you connect a decoupling capacitor next to your digital chip, the chip won't see this very high inductivity, it would see the parallel circuit of 200nH and about 5nH...20nH. Where the latter is the inductivity of local decoupling arrangement, means decoupling capacitor with its ground plane connection to ground pin of digital chip.

From this above you can see, what counts: Use double sided PCB. Try to route one layer as as solid ground plane as possible. Use free area on other layer and fill it with ground plane. Use wide enough Vcc tracks, about 2mm...5mm, depends on current consumption of individual chips. Decouple each digital chip, so that undecoupled Vcc tracks will have a distance of no longer then 5cm, or so.

Again, I do not want to tell you that double sided PCB is better than a proper multilayer design. But if costs play a role, this double sided PCB with solid ground plane can be the only option. Then it's nice to know, how the optimum can be taken by simple design rules.
One major advantage of multilayer board is, that the distance between individual layers is much smaller than with traditional double sided PCBs. This gives more shielding, less inductivity and smaller loops...

Kai