Am I likely to experience problems with this?
most of which suggest of course filling as much of the board, both sides, as possible with ground copper.
No putting a ground plane everywhere will just help the interference get into the ground plane.Keep the ground plane away from interference, do not put it under devices likely to cause it.
Star grounding would look somewhat impressive with so many grounds :-)
I have seen that it works better to keep power and motor control switching more to there self. And run signal line to them far less noise pick up. And as said don't loop the gnd or the VDD line.
1. just lay out the pcb with the normal microcontroller cktry on one side and the h-bridge cktry on the other side, and only connect them together at a single ground point. Some people will use an inductor [choke] or ferrite to make the connection.
2. once this is in place, simply run the h-bridge control signals from the microcontroller across to the h-bridge. Always good to put series-Rs in these lines to help protect the uC from motor noise feeding back from the h-bridge.
3. locate the main terminals for motor power on the h-bridge side of the board, so the motor currents never cross to the other side, and never flow through the single point ground connection of item #1. Add bypass [0.1 uF] and reservoir [100 uf or more] caps right at the same terminals.
4. it's best to use 2 separate external power supplies, one for the logic part and another for the motors. If you can't do this, then the next best thing to do is connect a single supply to the motor side, and jumper "1" wire over externally to supply logic power. This way, the motor currents are always confined to the h-bridge side, and not flowing between the 2 sides. Don't make an external ground connection between the 2 sides, as then you will have a ground loop.
5. if you have analog cktry on the pcb, confine it to a separate area from the digital logic cktry, and also on the opposite side of the pcb from the h-bridge cktry.
]Can you you arrange it so that insted of all components being one layer of the board and allk the rest the other layer, have one group be one end of the board and the other group be the other end?Then any traces & vias needed to make the routing work can be with the similar signal levels, and the high voltage/high current traces & vias can be seperated away, not overlapping the more sensitive lower voltage/current parts.
Yeah, I meant to mention earlier and forgot, as Bob says, there is no rule that says it's necessary to keep the power/ground and signal traces on opposite sides of the board.
Are my 220 and 1uF caps across the bridges power pins not the 'main' caps however? The diagram on th page you linked certainly imply that?