1) I've got a 30mm dia circular PCB. Should I place the BGM121 at the edge of the board (as indicated in datasheet (page 47) and the BGM121/123 Hardware Design Guidelines video: https://youtu.be/5DCn7AzIyig?t=211), or should I place it more in the center so that I can increase the width of the ground plane to be as close as possible to the 44mm (as prescribed on page 49 of the datasheet and here https://youtu.be/5DCn7AzIyig?t=313)? Which constraint is more important (edge or width)?
2) I have a feeling that the answer for the above question is WIDTH, which would mean placing the chip toward the center of the board so as to maximize the ground plane. If this is true, we will need to place some components on the side other side of the antenna. The datasheet (page 85) shows a 1.00mm keepout area to the left of the antenna-ground-loop-trace... can we place components to the left of this, or should there be a larger keepout area?
3) The datasheet for the BGM121 indicates that the board trace/pour that attaches to the internal antenna (P53), should be 0.7mm wide. However, the 4302A gerber layout has the width of this section being 0.625mm. Does this width matter? Which width should we go with?
Thanks for clarifying,
1. The most important constraints are the edge and width of the GND plane. So, the SiP module can move towards to the center from the board edge while keeping copper clearance between the board edge and SiP module, GND plane and thus the wider GND plane reference can be ensured for the module as well.
2. No. That area requires clearance in terms of copper pour or components. The clearance area should at least be around 20 mm (reactive near-field region) to have no basically no effects in performance.
So, for small circular PCBs it is a kind of trade-off in terms of performance vs. component density restrictions. If the PCB size is comparable with a coin cell battery, i.e. the antenna area is being affected by the coin cell itself, then try to move the module closer to the board edge to minimize the effects of coin cell battery. See some KBA references under the links below - note that the antenna impedance can be re-tuned by adjusting the antenna clearance area dimension.
3. Thanks for highlighting that discrepancy in our documentation, will initiate to fix it. However, the performance is basically the same with using any of those widths mentioned. I'd recommend to go with the datasheet layout recommendations, including the thermal strap connections to those big GND pads to avoid any possible soldering yield issues.
Zoltan, thank you for clarifying.
1 & 2) So, to summarize, for a smaller circular board, it sounds like the best case scenario would be to place the BGM121 in the center of the circle, with a keepout area to the left of the antenna (i.e. the left section has no copper pour (e.g. ground plane), no traces , and no components - just raw FR4 fiberglass board). However, if we have a coin cell on the other side of the board, then we should move the chip over so the coin cell is not directly overlapping the antenna trace/area.
3) I also noticed that some of the PCB layout images in the datasheet show thermal isolation around the antenna ground pads, but the PCB Layout Guideline video (https://youtu.be/5DCn7AzIyig?t=287) explicitly states NOT to use thermal isolation. The 4302A gerber files also have NO isolation, so I'm assuming the video / 4302A board is correct?
4) For the land pads, I noticed you created a recommended land pad file (https://www.silabs.com/content/usergenerated/asi/cloud/attachments/siliconlabs/en/community/wireless/bluetooth/forum/jcr:content/content/primary/qna/bgm12x_footprint-8uiu/here_is_apreliminary-h4ez/Recommended%20PCB%20land%20pattern%20preliminary.jpg). Should I use that one or the one in the datasheet? (Yours has some larger pads for the ground pads (0.7mm instead of 0.6mm), and shortens the corner pads from .5mm to .45mm).
Thanks for your help. I saw some posts of people having yield issues and wanted to ensure we got the land pad / layout right.