1 2 Previous Next 21 Replies Latest reply on May 7, 2014 5:00 PM by dmiya

    BCM20732 layout options


      I noted the suggested layout on the datasheet the problem is that I need the module to sit on a PCB that is 10mm wide, but can be as long as 25mm. Is there a general guideline for a non-square layout?





        • 1. Re: BCM20732 layout options

          Hello Joel,

            We get a lot of questions about the GND & Keepout areas shown in the TRM.  First keep in mind that this is the 'recommended' layout for maximum RF performance to get maximum range, ~150ft / 50m.  This is not to say that this is the ONLY layout that will work just what is recommended for maximum antenna efficiency.  If you are willing to compromise a bit on range then there are other scenarios that will work.  Taking a look at the parameters that are recommended for the PCB layout lets consider what should be a good option to explore.

          So if you align side A at the edge of your PCB you have 6.5 + S + H = 12.1mm  So we are 2.1mm over your 10mm requirement.  Something that would be worth exploring is to reduce S & H by 1.05mm thus squeezing in your 10mm width PCB.  If you have the capability you may want to experiment with some different options.  One other item to keep in mind is that the L shaped GND plane does not have to be on the top layer.  This could also be on the 2nd layer possibly.  This would be useful if you need to place components in this area.  In conclusion I have not necessarily implemented this but again if you are willing to compromise on Maximum range there are other options that can work for the GND/Keepout areas.




          • 2. Re: BCM20732 layout options

            Note also that the L-shaped ground plane is required for the embedded PCB antenna.


            It's also my understanding that the simulated antenna efficiency will be around 10% when side A is not located at the board edge. With that said, the datasheet does not specify minimum dimensions for the Keep-out area along side A; I know from working with other customers that the minimum is 5 mm.Lastly, the Keep-Out area is a void in the copper on all layers.


            We can also provide the .brd/PCB file if needed.

            • 3. Re: BCM20732 layout options

              Thanks for the quick response. I am willing so sacrifice the maximum range. I need and really only want <5M range (direct line of sight so this will be longer for multipath and also the device is handled so may be obscured by the hand).


              Also one further question I have is whether or not the whole pink area is a keep-out area, or just on side A? Also if I have traces coming out of the chip (as is expected to talk to peripherals for general purpose IO and ADC), what is the preferred path? underneath the chip on the bottom layer, or on top with the ground plane on the bottom layer?  Is it possible to get a reference layout for connection to the module and suggestions for bypass capacitors for the module? Also, Is there a description of what the test pin does (not complete in the module datasheet)? If I want to have programming pins to reprogram on the board is that possible and is there a note or guidance on that?





              • 4. Re: BCM20732 layout options

                For the programming question I think it is best to post this as a separate topic.


                Hello Joel,

                  The Keepout area is to be void of copper.  For your case of having such a short range you can follow the guidelines below for routing signal traces.  As Mike indicated I can send you a *.brd file and *.dsn file shows the PCB layout of a PCB with the SiP on it.  If you want this you can send me a message and I can shoot it to you. 

                For the Test Pin I would just leave this unconnected or put a jumper as a means to pull this high if you want to put the 20732 into a TEST MODE.  To the best of my knowledge there is not an automated/pre-programmed 'Test Mode'.  This is more for manufacturing/test to be able to put the module into a Test Mode that you would define based on reading this pin. 


                1. The L-shape GND plane is required for integrated antenna and please must keep the L-shape GND plane continuous, do not cut off the GND shape due to routings.
                2. The L-shape GND plane is required (Green color area) to enhance the performance of the integrated antenna. If the L-shape GND plane is arranged on top layer of PCB, It’s not recommended to place components in this area. If components need to be mounted in this area, the L shape GND plane should be arranged in bottom layers and avoid a GND plane on top layer. (This is to ensure the L-shape GND plane for antenna is continuous.)
                3. It is fine to bring signal traces out of module from Side B (between Pin#16 and Pin#19), Side C (between Pin#27 and Pin#31) and Side D (between Pin#37 and Pin#42) with overlapped routings to minimize the area metal traces occupied in the keep-out area.

                  Please do not bring signal trace from Side A.




                • 5. Re: BCM20732 layout options

                  THanks for the answers,  Please send me the design file you have, if you have a gerber that would be good or dxf as I probably don't have the same pcb design package as you.





                  • 6. Re: BCM20732 layout options

                    Hi Frank,


                    What is the recommended pad pattern under the SIP itself? As close to a solid plane as possible, as little copper as possible, or a specific pattern (like the L-shaped ground)?


                    Excluding the VBAT on pin 3 and the I/O on pin 1, side A is all GND; what's the recommended way to get a solid ground there without encroaching on the keepout area?

                    • 7. Re: BCM20732 layout options

                      Can you make the chip disappear in the picture you posted so I can see how power and gnd is delt with under the module.



                      • 8. Re: BCM20732 layout options

                        I will work with the local Broadcom support team and see if we can get the module PCB files over to you (Gerbers and Allegro). Unfortunately, we cannot post these directly to the forum.

                        • 9. Re: BCM20732 layout options

                          Could I also get those geber files? I'd greatly appreciate it.

                          • 10. Re: BCM20732 layout options

                            MichaelF_56 "the datasheet does not specify minimum dimensions for the Keep-out area along side A; I know from working with other customers that the minimum is 5 mm"


                            Did you really mean 5mm keepout area on side A? That would make side A keepout area thicker than the rest.

                            • 11. Re: BCM20732 layout options



                              Is there a DXF file for the BCM20732S? I saw on data sheet all dimensions for the module but it's still missing some data like the position of central pads from the edges.




                              • 12. Re: BCM20732 layout options

                                Hello Rtenedini,

                                Here is a sample set of Gerbers for the BCM20732S:


                                Sample BCM20732S PCB Layout


                                This is an inital BLOG Post, but it should get you started

                                Hope this helps



                                • 13. Re: BCM20732 layout options

                                  Good morning, Frank,


                                  Thanks a lot for clarifying the layout.

                                  Could you please send me the gerber files (*.brd file and *.dsn)?

                                  Thanks again, have a great weekend.


                                  • 14. Re: BCM20732 layout options

                                    Hello Myron,

                                      The PCB files are at the following link.  The *.dsn file is not currently there but should be posted shortly.


                                    Sample BCM20732S PCB Layout





                                    1 2 Previous Next