Review schematic and PCB layout

[Irfan Memon]

Hi,

We are the Manufacture of LED lighting.we want to developing nRF52840 Module for one of our projects.

Please Review the schematic and PCB Layout.

Documents are confidential please care.

Regards,

Irfan20210516_nRF52840_V1-0 Gerber.rarMeshtek_nRF52840.pdf

[Kaja]

Hi,

Due to public holidays in Norway, there is some delay with the review. We will come back to you as soon as possible.

I apologies for any inconvenience caused.

Best regards,

Kaja

[Kaja]

Here is the review:

1. Remove L4, DCCH should be floating when you use normal voltage mode.
2. VBUS should be grounded when USB is not in use, DECUSB, D+ and D- can be left floating. 
3. Correct the deviasjons form the reference design for IC1:
*
4. The RF path should be directly copied from the reference design, placement of the components, traces, cut out area in the ground, the green line should be a 50 Ohm transmission line (a coplanar waveguide).
5. The DCDC components should be grounded via the VSS pin, B7, the center pad and the local ground plane on the top layer. 
6. On PCBs with more than two layers, put a keep-out area on the inner layers directly below the antenna matching circuitry (components between device pin ANT and the antenna) to reduce the stray capacitances that influence RF performance.
7. I can't open any of the drill files in my gerber viewer.. could you upload a new drill files? or a picture of the top layer with vias. 



Best regards,
Kaja

[Irfan Memon]

Hi,

Thanks for the suggestions,

Here the PCB file as you need.

I have some queries as above,

5)which are the DC-DC components ?we have done as you mention please check twice.see the layout file

6)Put a keep out area-means gnd and vcc layer both or only gnd should not pass under this section

7) we have attached pcb file here please check

Regards,

IrfanPCB FILE.rar

[Kaja]

5) L3, L5, C12 and C10
6) Means nothing, not ground no routing:

7) Wow, many vias! Small ground islands should be grounded with more then one via. 4*4 vias in the center pad should be enough. Vias along the RF path is good, and vias close to the grounding pads of the components are good. 

Best regards,
Kaja