7 Replies Latest reply on Aug 2, 2017 10:13 PM by BoonT_56

    Issue with a new PCB for the BCM20737S module




      We already produced 2 PCBs with the BCM20736S. They work properly, without any issue.

      We wanted to launch a production, and we modified the layout. We just wanted to improve the layout in respect of the recommendations given in the technical manual. We manufactured 10 prototypes that -unfortunately- do not work at all. The current consumption of the board is quite high (200mA instead of 10mA for the previous version) and we are not able to program the internal EEPROM (UART). Moreover, the BCM20737S is getting hot quickly.

      More information :

      • If we remove the SiP, the board does not present the issue anymore (at least for the current consumption). Only the SiP is hot, and the problem seems to be there.
      • I realized that there is a small golden arrow on the bottom side of the SiP (a pin 1 marker). This metallic area seems to be connected to ground. Unfortunately, we have a via to Vcc at the exact same position... It could be the source of our problems but the solder mask covers the via and I guess that it should be a sufficent protection.
      • I see also several wires in relief on the bottom side of the SiP, themselves protected by a dark solder mask. I was wondering whether some high frequency signals are going thru these wires. In this case, it could be possible that I introduced some important capacitors between these wires and my ground plane (or some of my signals). Could it be the cause of my issues ? Is it recommended not to have anything metallic on the top layer of the PCB, under the SiP ? I didn't find such recommendation in the technical manual but it would make sense...

      Thanks for your help/suggestions.



        • 1. Re: Issue with a new PCB for the BCM20737S module

          The peak current consumption of the module is no more than 35mA. If you are measuring about 200mA and the module is hot, it "appears to suggest a short circuit" somewhere be it in your carrier board or module. There shouldn't be any "wires in relief" anywhere too. If you believe that the module is a probable cause, please contact your supplier immediately to initiate a FA.

          1 of 1 people found this helpful
          • 2. Re: Issue with a new PCB for the BCM20737S module

            Thanks for your answer.

            For the 'wires in relief', I meant that the bottom side of the SiP looks like a PCB, and a few traces are visible on the surface. Do you know if there is any clock / RF signals on these traces ?

            We tried to isolate the problem by connecting the SiP we removed with only two wires (Vbat and Gnd). The high consumption is still present while everything is normal if we apply the same connection to a new device (same batch/manufacturing code). In conclusion, it seems that we destroyed the modules.

            We didn't provide any information to our subcontractor (the same who already soldered the first two series of working prototypes). Do you think that the problem could be a manufaturing process with these new boards ?

            Again, thank you for your help.


            • 3. Re: Issue with a new PCB for the BCM20737S module

              I'm not inclined to point the finger to the module as it is a very mature product and has been in service for three years. However I cannot rule out issues due to manufacturing defects, that's why I urge you to seek a recourse from your module supplier.


              From what you had described above, it appeared that the failure (due to excessive current consumption) occurred only when you de-soldered the module from your PCB. There was a risk that you may have damaged something during de-soldering and caused a local short circuit. On the other hand, if you simply apply power to Vbat and return via GND on a new module, and the issue did not surface, then this is an affirmation that the module is fine.


              Pin 1, 44, and 43 are GPIOs and Pin 2 is GND. The "small golden arrow" is just to point to Pin 1, it is not electrically connected to anything. Ask a steady HW engineer to take a closer look for anomalies on these pin locations in juxtaposition with your PCB board.


              I will refrain from commenting on your PCB board as I have not seen nor review them.

              • 4. Re: Issue with a new PCB for the BCM20737S module

                My comments may be limited in scope obviously because I haven't got the benefit of seeing your boards physically. They are purely based on what you have described...

                • 5. Re: Issue with a new PCB for the BCM20737S module

                  I double-checked on new devices and I confirm that the small arrow (pin 1 marker) is really connected to GND, without any doubt... However, I believe that the problem is somewhere else, because the solder mask looks strong enough to avoid a shortcut with my VBat

                  The SiP we de-soldered was destroyed (getting hot) BEFORE de-soldering (not after). I just wanted to check whether the consumption was 'high' out of the board, and it is the case. The conclusion of this would be that the SiP has been destroyed, either by the manufacturing process or by the powering up on the board.


                  I made a few new trials:


                  I took a new board (never powered) and I tried to increase slowly the voltage from 0. The consumption stays normal (almost less than 5mA) between 0 and 1.8V. I have 10mA for 2.1V, 20 mA for 2.2V, 30 mA for 2.3V, and I stopped  there. If I make the same test on a 'already destroyed board', I see the same behaviour.


                  I de-soldered the SiP of my very last board (again never powered) and I made the same test (increasing slowly the voltage) on the SiP (out of the board) =>> no consumption. The conclusion would be that the SiP looks good as long as it has not been powered on this board... My first feeling was that the manufacturing created the problem, but it seems not to be the case and I am quite confused.


                  Last information : we also manufactured another board with the exact same schematic, but with the SoC (instead of the SiP). The rest of the schematic is identical.  We were not very confident with this board (because we didn't have a perfect understanding of what is on the SiP) but it works fine, with a normal consumption.  We didn't plan it, but the board with the SoC could be our solution if we don't understand how to fix the other based on the SiP.



                  • 6. Re: Issue with a new PCB for the BCM20737S module

                    After analysing our different results, our conclusion would be that the problem could be caused by this 'arrow marker' connected to GND. I thought that the solder mask should be a good insulation, but one of my colleague who has a better knowledge of the manufacturing process tells me that it is not the case (at least not the purpose of a solder mask that could be very thin...). Not very lucky to have the VBat via just at this position...

                    1 of 1 people found this helpful
                    • 7. Re: Issue with a new PCB for the BCM20737S module

                      I confirmed with the module manufacturer that the "small golden arrow" is indeed grounded. My bad as I thought it was on the silkscreen layer. Glad that you have found out the root cause.

                      1 of 1 people found this helpful