I recently got the attached PCB fabricated. My vias on top of the GND pads are not filled and plated. The following happened when I assemble it:
1. About 50% of the PCBs have a bluetooth signal and 50% of the PCBs do not have a bluetooth signal.
What are some possible reasons for this?
Is it related to me not filling and plating the vias on top the GND pads with conductive filling?
2. I have an ADXL362 accelerometer on the bottom of the PCB. On one of the PCBs when I soldered the accelerometer, the bluetooth signal went away and when I desoldered the accelerometer, the bluetooth signal reappeared. The program I was running was the SoC empty example. This happened 3 times repeatedly and the 4th time even after I removed the accelerometer, the bluetooth signal did not reappear. After the 4th time, I looked at the energy profile of the PCB when it was running the SoC empty example and saw a stable line (no peaks at all completely flat) at around 3.2 mA. I placed my phone with the blue gecko app running very close to the PCB. When I was getting the signal, it was between -30dbm to -35dbm each time after I removed the accelerometer until the signal completely disappeared.
A few more notes on my PCB, when comparing the gerber files for it to that of the BRD4302A I noticed that my PCB seems to have a soldermask over all the vias while the BRD4302A doesn't. I also noticed that the soldermask over the BGM121 pads is a lot bigger in my PCB than in the BRD4302.
Another note, my PCB seems to work even when I don't have a 0 ohm resistor connecting the RF_out pin to the ANT pin. I didn't realize this at the very beginning but before I started to solder the accelerometer on, I noticed it and I made a solder bridge between the two pads because I did not have a 0 ohm resistor with me. Do you think this had an effect on anything?
I have the following questions regarding this:
What do you think a possible explanation for this is?
Why is the energy profile a stable line?
Why does the signal disappear and reappear when I soldered/desoldered the accelerometer?
If I plate and fill the GND via-in-pads I have under the BGM121 module, will it solve my issues?
Should I plate and fill all the vias other than the via-in-pads under the BGM121 module (which will be plated and filling with conductive epoxy) with non-conductive epoxy?
On my custom BGM121 board, mine differs from yours:
1. Ground plane/pours go to the edge of the PCB (ie. upper on right).
2. Pin 54 is connected to GND on the top layer also.
3. RF pins are connected directly (rather than through 0 ohm/solder bridge)
4. GND stitching to the right of pad 56
5. Trace between pads 55 and 56 is normal (narrower).
As the documentation says, "Verify the GND connections for the antenna pads for top layer".
I don't use any via-in-pads; just put the vias close to the GND pins. (I have eight GND vias underneath, and none in pads)
Why is the energy profile a stable line?
Could be that something is preventing the MCU to boot normally. For example, it may be stuck at the HFXO startup if there is some issue with the high frequency clock. Do you have any means to verify that your application is able to boot into your main application? Maybe wiggle some free GPIO to verify this?
Getting the "Bluetooth signal" out of a BGM module should be not that critical in terms of PCB layout etc, I have seen prototypes of PCB modules that are literally hanging from wires without any main board at all. Those were PCB modules though, not SIP modules like the BGM121.
Flat line in the energy profiler is a strong indicator that the radio is not active at all, which could mean that your application is stuck somewhere in the init code. Any RF activity is easily spotted from the current profile.
The issues you describe are expected due to the non filled / plated vias and the oversized soldermask openings that you have articulated here in this post and in separate subsequent posts that you have made. You could check with your assembly CM (contract manufacturer) to see if they will x-ray the units which do not have the BLE signal i order to look for shorts or voids. If either are observed, the CM is the best resource to advise you for any other potential design updates such as stencil opening dimension or thicknesses, footprint dimensions and temperature profile due to they know best their own assembly equipment and re-flow process requirements.
Regarding the operation of the antenna without a zero ohm component installed (chip component or solder bridge), this is also expected due to the open circuit represents about 20 to 30 dB of attenuation. Given the remote radio can receive a signal at ~ -95 ish dBm, it is expected that a radio, such as a cell phone, which is placed nearby will still communicate properly with your module. Basically the open circuit reduces the effective range of your module but does not stop your radio from functioning.
Hope this helps,