I am finishing up routing a 4 layer DC-DC converter PCB. My concern right now is whether or not it is safe to have a ground plane directly under a Bluetooth module on my PCB. Since this is a switching converter, my concern is that the ground plane may become noisy, and will interfere with the antenna (or possible the entire Bluetooth module) and will prevent the module from receiving proper signals. I am not very experienced in RF, so my knowledge is pretty limited, but I just wanted to get a second opinion. The Bluetooth module I'm using is the HM-11, and the frequency of my buck-boost converter is set to 750 kHz, in case that info is needed.
The manufacturer of the Bluetooth module will typically specify a keep-out area around the antenna area of the module, which usually will extend at least 1/4" in all directions.
In some cases, even without a ground plane, the presence of G10 or etched PWB material under the antenna section can be sufficient to detune the antenna and affect its performance. In all cases, it is best to refer to the documentation for the Bluetooth module you are using.
The module you are referring to uses a TI cc2451 chip. Looking at the extensive documentation on this chip on the TI web site, I found Application Note AN043 which describes different antenna designs. When referring to the type of antenna used in your module, they state that " It is also recommended to use the same thickness and type of PCB material as used in the reference design. [...] To compensate for a thicker/thinner PCB the antenna could be made slightly shorter/longer."
So simply placing the module over an un-etched PWB will be largely similar to increasing the thickness of the PWB, which will affect the antenna's performance. It is possible that the module's antenna was designed to be placed over unetched PWB but without knowing for sure, you are betting either way.
Good practice is to keep an area at least 1/4" or 1/2" around in all directions free from metal. You most likely will not suffer severe degradation. A ground plane under the antenna is certainly a bad idea.
The ground plane is safe under the module. I assume you are placing it on the top layer. Keep it the same as the module's ground plane, do not route anything under the antenna, on any layer, where the module's solder mask is missing.
The biggest influence on your reliability will be decoupling Vcc - do you have the usual caps on Vcc, with a via right to the ground plane?
Also, make sure the ground plane is continuous and not interrupted by signal routes, especially where DC-DC converter will have high current across L1/U6/C13/C10.
If you have a ground plane under the corner of the module, you can stitch the two together with vias - just to be conservative.
Overall, the risk is low to get interference, as you properly decoupled Vccand used short traces on the module's control inputs.