Antenna not working

[Walkar2902]

Hello,

I am working on nRF52382 IC. I am accessing GPIO also. But still i don't get the access of antenna. I have make the circuit as per the development board of nRF52.

Could any one help me to solve this issue?

Here, i am attaching the layout files. please check that also.

TOP layout.pdf BOTTOM layout.pdf

[Andreas]

Hi,

 

Sorry for saying this, but your layout is not good enough. Please replicate the reference layout, either the downloadable HW files on the product page or the section inside the silk screen rectangle on the DK.

 

Specific improvements:

• Place components closer to the IC and as per the layout above.
• Ground:
  • Ground pour, not trace ground.
  • Multiple vias in the center pad of the IC.
  • Solid ground underneath the RF part, if not possible use a 4 layer board and use an internal layer as solid ground.
  • Via close to all ground pads of components.
• Do not route the power rail though the center pad.
• The RF section needs straightening out and if you have a coaxial connector in there it is not connected right.
  
• The antenna is way too small and crammed in too close to ground and traces. Due to the battery underneath though a PCB antenna will likely not be very successful, you should either use an on-ground SMD antenna or make the PCB slightly larger.

 

Best regards,

Andreas

[Walkar2902]

Thank you for the suggestion. But we have the space limitation which is 27mm diameter. I will do whatever you say me about the ground trace and power rail. We are not using Coaxial  connector but you are right the connector connection is wrong. This note is consider. Can we place the all components under 26mm diameter? Including antenna?

[Andreas]

Hi,

 

The antenna needs the space it needs due to physics. You will just have to tuck everything away and see how much space you end up with for your antenna. One alternative is to use a SMD antenna instead, they generally require less space.

 

Best regards,

Andreas

[Walkar2902]

Thank you so much. I will do this thing & again verify the layout from you.

[Walkar2902]

We need to design antenna on pcb, pcb specification are

Copper thickness: 0.035mm(35 micron), We can adjust to 17.5 micron or 70 micron

Material: FR4

Thickness of PCB:1.6mm

Please guide me to design antenna. Please let me know the tack width and length of antenna.

If you have any other solution then also please let me know.

[Andreas]

Hi,

 

See this whitepaper: https://infocenter.nordicsemi.com/pdf/nwp_008.pdf?cp=14_19

 

If you make a meander antenna (like the one in your previous design) or another fairly complex shape you should replicate all sizes and dimensions like in the original design. You can e.g. look at nRF52840 Dongle HW files.

The Copper thickness and PCB specs are fine.

 

Best regards,

Andreas

[Walkar2902]

Hello sir,

We make the changes and make the  new layout design. could you please verify this layout? Please let me know if there is any changes.

TOP_1-3.pdfBOTTOM_1-3.pdf

Please check above document for layout.

Thanks.

[Andreas]

Hi,

 

This definitely looks better. I still recommend some changes though:

• Red: add/improve ground pour to improve the grounding of these components.
• Green: do not ground the cap on the ANT pin to the ground pour, instead route it into the center pad through pin 31 (VSS_PA). This is by design and optimal for spurious rejection.
• Yellow: You can omit the two caps on P0.25 and P0.26 by shorting the pads to the center pad, this is a similarly effective workaround to errata 138 which the capacitors are added to solve.
• Blue: Add a pi network for matching the antenna to  50 ohm.

 

Best regards,

Andreas