Verification for schematic for custom Board

[Moghees]

Hi,

We are design custom Board using nRF52840 SOC.

1. We are operating it in Normal mode, using internal DCDC converter
2. We have used configuration 5 from reference design
3. From reference design we have removed NFC pins connection and USB connection because we do not need it in our design
4. We will be programing our custom board using nRF52840 DK
5. We have attach led using load switch at P0.15
6. We have attach buzzer using load switch at P0.16
7. We have attach button at P0.24
8. We have taken antenna schematic from nRF52840DK hardware files and remove external connector. Have we done it correctly?
9. Have we connected reset button correctly?

I am attaching the Schematic design for our board can you verify it if it is correct or we are missing something, If it is unclear in picture I can also attach schematic file

Thanks in advance

Regards,

Moghees Bin Zahid

[Martin Sivertsen]

Hi Moghees,

Thanks for the detailed information.

When not using USB you can ground VBUS as seen in circuit configuration no. 6:

We have taken antenna schematic from nRF52840DK hardware files and remove external connector. Have we done it correctly?

Yes, but whether or not you only need antenna matching component C23 depends on what type of antenna you are planning on using. If you are copying the antenna layout from the nRF52840 DK, then one antenna matching component will probably work fine, otherwise we'd recommend a pi-network of antenna matching components for greater versatility in tuning the antenna.

The reset button is connected correctly.

What's just as critical is the PCB layout, so feel free to share that when you have it done and we can take a look at it.
If you follow the reference layout exactly you shouldn't have any issues.

Best regards,

Martin S.

[Moghees]

Thanks for the reply Martin. Firstly I want to appreciate the documentation of Nordic.  

Martin Sivertsen said:

Yes, but whether or not you only need antenna matching component C23 depends on what type of antenna you are planning on using. If you are copying the antenna layout from the nRF52840 DK, then one antenna matching component will probably work fine, otherwise we'd recommend a pi-network of antenna matching components for greater versatility in tuning the antenna.

I will be using same Antenna used in nRF52840DK. I want to ask can I copy antenna for nRF52840DK PCB layout and placed it on my PCB layout? If yes then in place of connector that is connected for external antenna of DK I should just extend antenna layout?

I have few others questions:
1. Can I remove net names and wires that I am not using in our design?

2. It is first time I am designing PCB using nRF52840 SoC. Can you recommend me document that I can follow?

3. Can I use reference layout PCB layout and extend it for our PCB?


Regards,
Moghees Bin Zahid

[Martin Sivertsen]

HI Moghees,

Moghees said:

I will be using same Antenna used in nRF52840DK. I want to ask can I copy antenna for nRF52840DK PCB layout and placed it on my PCB layout?

 Yes you can.

Moghees said:

If yes then in place of connector that is connected for external antenna of DK I should just extend antenna layout?

 Yes, you can just remove the MM8130 connector with switch and use an unbroken transmission line from the radio matching network to the antenna matching network (capacitor C23 in your case)

Moghees said:

Can I remove net names and wires that I am not using in our design?

 Yes.

Moghees said:

It is first time I am designing PCB using nRF52840 SoC. Can you recommend me document that I can follow?

Here is some documentation for the reference circuitry of the nRF52840 itself, and here you can download reference layout for the nRF52840 itself, and here is the hardware files for the nRF52840 Development Kit which you can use as reference. You can also search for documentation and reference here on DevZone, there are a lot of cases with tips and guides to creating a custom PCB with an nRF52840.

Moghees said:

Can I use reference layout PCB layout and extend it for our PCB?

 Yes you can.

Best regards,

Martin S.

[Moghees]

Thanks for the reply. I am not closing this discussion because after completing PCB designing I will share my design here. So that you can review it

[Martin Sivertsen]

Hi Moghees, 

That sounds good.

Best regards,

Martin S.

[Moghees]

I have attach Antenna with nRF52840 reference design can you verify it? or you need hardware files to verify it?

Regards,

Moghees Bin Zahid

[Martin Sivertsen]

Hi Moghees,

You should also place capacitor C23 (from the schematic) on the antenna feed point. Look at the nRF52840 Development Kit hardware files to see how it is placed.

Best regards,

Martin S.

[Moghees]

Thanks for the reply. Can you verify latest connection given in below diagram

[Moghees]

I have completed PCB design. I have shared with you schematics and PCB file through private message. Can you kindly verify it

Regards,
Moghees Bin Zahid

[Martin Sivertsen]

Hi Moghees,

That looks good.

Best regards,

Martin S.

[Martin Sivertsen]

Hi Moghees, 

I'll take a look at it now. 

Apologies for the late reply.

Best regards,

Martin S.

[Martin Sivertsen]

Hi Moghees,

I looked at Final.zip and here are my comments for the layout:

1. Remove C22 and add via fencing/shielding on both sides of the RF transmission line as so:

2. Remove all of the unused traces connected to the GPIO's of the nRF52840 that don't connect to anything (they will turn into antennas and pick up noise)

3. I see you use two GPIO's on inner layer 2, but you have lots of available GPIO's on the top layer, so I'd rather use those. That way you can avoid using any of the GPIO's on the inner layer of pads on the nRF52840 and don't need the via in pad which you can also remove (marked in green). Via in pad adds cost when manufacturing the PCB, so if you don't need it I'd remove it.

4. If you do what I mention in comment 3., you can also remove inner layer 1 and 2 of the PCB, as they are not needed for routing or ground or power. This also cuts cost when manufacturing the PCB.

5. Add a matrix of vias in the center pad of the nRF52840 (see reference layout).

6. I highly recommend adding relief connect around the ground pads of the components, at least the ones that are attached to the antenna and RF trace as it makes it a bit easier to solder components on and off by hand (which will have to be done when tuning the radio and antenna matching components).

7. Add ground vias directly next to all ground pads and everywhere else where there is empty space

8. I see many traces on the board that meander when they don't need to, for example the trace going to C24, just rout them straight with 45 degree angles and don't make them longer than you need to. Use the available GPIO's on the top layer as much as possible. (I see now that the trace going to C24 is VDD_nRF, but my point still stands)

9. Place decoupling capacitors closer to their respective IC's (voltage regulator and load switches), and have the trace go through the pad of the capacitor before it connects to the IC. Look at the datasheets for the components and see if they have a recommended layout.

10. Clean up the silk screen component designators. Make them the same size and place them so they don't overlap any other elements, and are placed next to the component they belong to

Best regards,

Martin S.