Important is, that all the components of osclliator are located as close as ever possible to the micro, as suggested above. This minimizes the loop area formed by the oscillator currents through the burden caps and crystal, minimizes the voltage drops along ground connections between burden caps and ground pin of micro and minimizes the charge injection into surrounding signal traces via stray capacitance. In order to keep the latter minimal, it's important to fully embed the oscillator traces into a solid ground plane. This will heaviliy minimize the stray capacitance to other signal traces, allowing you to route other signals in rather close distance to the osclliator section. For optimum results the use of a solid ground plane under the oscillator signal traces is obligatory!

Imagine you would not have a double sided board with solid ground plane embeding the oscillator traces but a single sided board and you would like to achieve as minimal stray capacitance to surrounding signal traces as when using the solid ground plane. Then you would need to keep all other signals at least 5cm away from oscillator section!

If the burden caps are that close to the ground pin of micro, then it's allowed to connect the ground pins of burden caps to ground pin of micro via the common ground plane, as shown above. But if only a single sided board is used, then the copper traces connecting the ground pins of burden caps and ground pin of micro must not be part of common ground routing of board! Give them an own copper trace.

You are right: What you see above is the top layer, assuming, that all other signals are also routed in the top layer. The solid ground plane is in the bottom layer then. Whether you have the solid ground plane on top or on bottom of your board doesn't really matter. But you should have the oscillator traces embeded into a solid ground plane, at least a local one, call it ground fill if you want, and you should have a solid ground plane under the osclliator traces.

What I said above is only half the truth. Not mentioned so far is, that there's also a ground return current from the burden caps to the supply voltage decoupling cap of micro, which often sits near the Vcc pin of micro. So, also this connection must possess as small inductivity as possible, which can only offer the solid ground plane. But even when benefiting from it, it's a huge difference whether you have a TQFP, a PLCC or even a DIL40 package! With a DIL40 package you will always have huge ground noise, which cannot be pushed under a certain, rather unsane value, even not with a multilayer board! If you need really little ground noise, maybe because you want to design a mixed analog/digital application, then only the choose of a very small package for the micro will help!

DIL40 package is a thing from the stone age. Today, I do only use micros in TQFP-packages.


Do not use a splitted ground plane here. It would only result in an increase of impedance and finally result in a loss of efficiency and increase of stray capacitance. Connect both ground planes, means the local ground plane or ground fill on top, which embeds all the oscillator currents and ties the crystal enclosure to ground, and the solid ground plane on bottom together by as many vias as possible, evenly distributed over the whole board. Use about 10 vias directly at the oscillator section, to give you a number. As you surely have noticed it, all these extra vias are missing in the example above!!

Kai