Review PCB design for nrf52840 for Matter or Thread use

[Sarvesh_dhar]

Hi, I am new to PCB design, so I want suggestions for my designed PCB. Please review it once and provide feedback upon that. I am making this PCB to use this with Thread and matter-related products. I have used EasyEda to design the PCB and used the reference designs provided by Nordic. 

 nRF52840 PCB & Antenna Design 

 General PCB design guidelines for nRF52 series 

[Jared]

Hi,

1. On the SWD header you want to route out VCC not 3V3, so that it follows whatever voltage VCC is at. 
2. You need a full Pi-network to tune your antenna. Only C15 is not enough. 
3. DEC4_DEC6 node is connected to the wrong node. It should be over capacitors of the DC/DC components.
4. You need decoupling on pin A22.
5. Pullup on Reset pin is not necessary.
6. What is the internal capacitance of your HFXO and LFXO crystals?

For the PCB you need to follow the reference design much more closely. Where is your GND layer?

regards

Jared 

[Sarvesh_dhar]

Hi, Thanks for the response, I have updated the design with the Gnd. I will update here after changing the other points you have mentioned . Would you please look into this once and find any improvements

 

[Jared]

Hi,

1. The first capacitor in the matching network should only be grounded to the centerpad, it should not be connected to the rest of the GND layer directly.
2. It seems that there is a stump, in the matching network, you should remove this.
3. You need a full matching network the chip antenna.
4. You need 4x4 vias in the centerpad.
5. Much more vias in general to stich the GND layer together. 
6. The transmission line does not look like 50 ohm. 

regards

Jared

[Sarvesh_dhar]

Hi Jared, Thanks for the reply,

Sorry, but I am not well in understanding the terms that you have used to describe my issue. would please clear bit more in simple.

1- It should be grounded with centerpad - what does this mean, it is a two-layer PCB?

2- What does stump mean. ?

5- Much more vias in general to stick the GND layer together - mean Top and Bottom layers? , and I need to give more vias to connect the ground of the Top and Bottom layers of the copper area?

6- The transmission line does not look like 50 ohm.  How do you guess that, although I have tried to tune it as I have attached the screenshot, is that incorrect?

[Jared]

Hi,

Sarvesh_dhar said:

1- It should be grounded with centerpad - what does this mean, it is a two-layer PCB?

The centerpad, meaning the die ground pad itself needs to be connected to the GND layer by using vias,

Sarvesh_dhar said:

2- What does stump mean. ?

A stump, in this sense is an extension of a wire/transmission line that isn't connected to anything. In the antenna path it's important to avoid stump, because it will move the impedance of the line. I marked the stump with a circle, you should remove it.

Sarvesh_dhar said:

5- Much more vias in general to stick the GND layer together - mean Top and Bottom layers? , and I need to give more vias to connect the ground of the Top and Bottom layers of the copper area?

Yes, in general, the more vias the better as you will make sure that all of GND on your board is on the same potential. 

Sarvesh_dhar said:

6- The transmission line does not look like 50 ohm.  How do you guess that, although I have tried to tune it as I have attached the screenshot, is that incorrect?

It's a guess ,I have not measured it. But if you have based the dimensions on by calculating it to be 50 ohm then it's ok.

regards

Jared 

[Sarvesh_dhar]

Thanks Jared , your inputs are very valuable and helpful , let me do the changes , I will let you know after that . 

[Sarvesh_dhar]

Gerber_PCB_nrf52840_2024-04-13.zip

Hi, I have implemented the points that you have suggest , would you  please review it once 

[Jared]

Hi,

1. What is this:

2. The matching components for the radio needs to be placed much more closer to the radio.

3. It seems that you changed the ANT path, can you share the schematic for the new revision as well?

4. Did you place the matching network for the chip antenna? You need a full PI. They should be placed very close to the antenna. 

5. What is the trace width that you're using?

regards

Jared 

[Sarvesh_dhar]

Jared said:

The matching components for the radio needs to be placed much more closer to the radio.

How close are you saying they should be?

Jared said:

It seems that you changed the ANT path, can you share the schematic for the new revision as well?

No, I have not changed the ANT path, I have added a connector also via Resistor to use the external antenna or onboard antenna options

Jared said:

What is the trace width that you're using?

All the traces are 0.051 mm in width, and ANT traces is 2.92 mm

Jared said:

Did you place the matching network for the chip antenna? You need a full PI. They should be placed very close to the antenna. 

Yes, there is an RC filter for that as well.

[Jared]

Hi,

You need at full Pi network for the tuning the chip antenna, C15 and R3 alone are not enough.

Regarding the trace width, we recommend 8 mils = 0.2032 mm

Can you share the datasheet of the antenna?

Regarding decoupling capacitors, they should be placed as close as possible to the pin that they are decoupling. For example on your design you have placed C5, which is the decoupling for VDD AD14 on the other side of the IC, and then routed the signal on the bottom layer. 

Also, you should avoid routing anything under the DC/DC components and tracks. It should be solid ground under.

regards

Jared 

[Sarvesh_dhar]

Hi Jared,

I appreciate your efforts and patience. Thank you for helping me till now. 

Jared said:

Regarding the trace width, we recommend 8 mils = 0.2032 mm

But if I set all the lines coming out for the CHIP to this width the causes the DRC error. so can I fan out the pins from the IC, then after that all the connections it will make with 0.2032 mm width?

Here is the datasheet for Antenna  - Part no - 2450AT18A100E

www.johansontechnology.com/.../2450AT18A100.pdf

[Jared]

Hi,

I think that you get DRC error because you have set the track clearance too high. 

The datasheet for the antenna specifies that antenna should be placed at the corner of the board, and that minimum a T network is required for tuning:

regards

Jared