5 Replies Latest reply on Jul 13, 2018 10:49 AM by chris_d85_3416111

    CY8CMBR3116 Design rules 4 Layer PCB with shield for proximity sensing

    chris_d85_3416111

      Hi,

       

      I have a 4 Layer PCB with the CY8CMBR3116 chip.

      I do have 2 proximity sensors and 4 buttons

       

      I read the design guide for 4 Layer PCB (3.8.6.2) where it says

      LAYER TOP:     Sensors
      LAYER 2:          Sensor Traces

      LAYER 3:          Hatched GND fill (7mil trace 70 mil spacing)

      LAYER BTM:    Components + hatched GND fill (7mil trace 70 mil spacing)   


      it refers to Figure 3-62   as an example but in fthis figure it looks like

      LAYER TOP:     Sensors + GND
      LAYER 2:          Sensor Traces

      LAYER 3:          Hatched GND

      LAYER BTM:    Components

       

      And i do wan't to use the shield electrode for proximity sensing (3.18.14.1)
      There the deisgn guide only mentions 2 layer PCB where

      LAYER TOP:   Hatch fill with driven shield (7 mil trace 45 mil spacing)

      LAYER BTM:   Hatch fill with driven shield (7 mil trace 70 mil spacing)

       

      So i am unsure what i should do in my 4 layer PCB?

      Currently i do this one:

      LAYER TOP:     Sensors + Hatch fill with driven shield (7 mil trace 45 mil spacing)
      LAYER 2:          Sensor Traces

      LAYER 3:          Hatched GND fill (7mil trace 70 mil spacing)

      LAYER BTM:    Components +Hatch fill with driven shield (7 mil trace 70 mil spacing)

       

      But i am not really sure if i understood the design guide.

      There is also another guide for 4 layer when using shield for liquids which differs ahgain where Layer 2 is filled with hatched shield  and the Layer 3 is solid ground fill.

      I am a little bit unsure whats the best solution...

       

      Any advices?

       

      Thank you!

        • 1. Re: CY8CMBR3116 Design rules 4 Layer PCB with shield for proximity sensing
          rzzh

          Hi Christian,

           

          For proximity application. If you want to get a farthest sensing distance, GND is the less, the better, and if shield is considered, the shield is more far away with GND, the better. HOWEVER, if there is no enough GND on the board, noise would be larger than expected which will reduce SNR seriously. Decide the area of GND, sometimes is do trade off between proximity sensitivity and noise immunity.

          Based on your 4 layer design. I feel the exchange of layer-3 and layer-BTM could be better:

          LAYER TOP:    Sensors + Hatch fill with driven shield (7 mil trace 45 mil spacing)
          LAYER 2:          Sensor Traces

          LAYER 3:          Hatch fill with driven shield (7 mil trace 70 mil spacing)

          LAYER BTM:    Components + Hatched GND fill (7mil trace 70 mil spacing).

          Does someone have other suggestions? It is welcome.

           

          Thanks,

          Ryan

          2 of 2 people found this helpful
          • 2. Re: CY8CMBR3116 Design rules 4 Layer PCB with shield for proximity sensing
            nmit

            Christian,

            What Ryan said is correct. I would add one more point that the signal should also get the ground reference at every point (may be not close enough) so as to prevent ground bounce. You should give a ground not far but not close. Also instead of plane you could run a trace to have tight coupling.

             

            Regards

            Nishant

            2 of 2 people found this helpful
            • 3. Re: CY8CMBR3116 Design rules 4 Layer PCB with shield for proximity sensing
              chris_d85_3416111

              Thank you very much for all your suggestions!

               

              rzzh

              I will fill the BTM Layer with Hatched GND instead of Shield but i have a problem to design Layer 3 as a Shield Layer because it's my main GND Layer.

              I'm not able to route the circuit without having a ground layer except i would route the GND Traces within the Shield Layer (Layer 3)

              Would this be ok to cut the Shield Layer (Layer3) for GND Traces, or should i use the Sensor Traces Layer (Layer 2) for this ?

               

              nmit

              Sorry, I do not understand. Which Signal should get ground reference?

              I have to admit that i never paid any attention on ground bouncing

              I am a bloody amateur

               

              I've attached my pcb as images

              It should be a 4x Touch-Switch with proximity ability (Swipe up / swipe down) for my KNX-Home Automation System.

              I decided to make the switches by myself because i didnt find any which fits my need and which i liked

              (Notice that i have not changed the BTM Layer to be a Hatch GND in this images as suggested, but I'll do this soon)

               

              TOP
              Sensor Pads and Proximity traces+ one LED driver trace and one I²C trace

              SwitchTOP.png+

              LAYER2
              SENSOR SIGNALS + some others like RESET trace and INTERRUPT trace

              SwitchLAYER2.png

              LAYER3

              Currently HASHED GND. Should be SHIELD + GND traces?

              SwitchLAYER3.png

              BOTTOM
              Currently Hashed Shield (Should be Hashed GND), parts and most of the traces

              SwitchBOTTOM.png

              • 4. Re: CY8CMBR3116 Design rules 4 Layer PCB with shield for proximity sensing
                nmit

                You are correct Chris,

                Your design looks good after the changes on the layering you will do. Since you have instant ground references for the PROX I dont see problem of ground bounce in your layout.

                Do make sure that digital lines (LEDS) , I2C or SWD lines do not run parallel to the PROX line as it can add offset to your raw count.

                 

                Regards

                Nishant

                1 of 1 people found this helpful
                • 5. Re: CY8CMBR3116 Design rules 4 Layer PCB with shield for proximity sensing
                  chris_d85_3416111

                  Thank you all very much for your inputs and suggestions!

                  .

                  I have changed my design like following:

                   

                  LAYER TOP:     Sensors + Driven shield  hatch fill (7 mil trace 45 mil spacing)
                  LAYER 2:          Sensor Traces

                  LAYER 3:          Driven shield hatch fill (7mil trace 70 mil spacing) + GND traces

                  LAYER BTM:    Components + VCC + Other traces + GND Hatch fill  (7 mil trace 70 mil spacing)

                   

                   

                  Thanks!

                  1 of 1 people found this helpful