• State
  • Locked Locked
  • Replies 12 replies
  • Subscribers 30 subscribers
  • Views 2638 views
  • Users 0 members are here
Support feedback
Options
Options
Related

This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

CC85xx: Some questions about the PCB antenna design

Ibrahim Kamal
Intellectual 390 points
Other Parts Discussed in Thread: CC2590, CC8530

Hello,

We are designing an audio streaming system with the CC8530 and the CC2590.

we deisgned the PCBs to be 4 layers, almost exactly like the modules that come with the cc8530 evaluation kit.

The problem is that we can't get the same range as with the kit, and our antenna is very sensitive. we can't go beyond 10 meters, and at that range, anyone getting close it causes the connection to be lost. Strangely, in the same conditions, the evaluation module is much more robust.

In this post, i would like to expose the differences between our PCB design, and the one of the evaluation kit. Could any experienced user or TI expert tell me if those differences could be causing the poor performance of our RF link?

1- The isolation of the GND plane around the trace going to the pcb antenna in the not the same. it's much bigger on the evaluation kit (black) than on our pcb (blue)

2- On our PCB, the antenna itself is not on the same layer as CC2590 and all other components. As you can see in the image below, under the yellow circle, the antenna signal goes from the bottom to the top layer.

(on the image below, the GND planes are hidden on purpose to make it easier to see the tracks)

3- Finally, we have less GND vias around the CC2590 than on the evaluation board.

We are going to design new PCBs, do you think only those 3 points need to be corrected? can you think of anything else that can maximize our chance of having a robust radio link?

Thank you very much,

  • 0
    Intellectual 390 points

    Also, can anybody point me to a nice tutorial about PCB antenna design for CC2590? 

    I would also like to add to my post above that the RF connection is lost if someone get his hand too close the antenna, let alone the fact of touching the pcb antenna. Strangely enough, the pcb antenna of the evaluation kit is much, much more robust. We can touch the PCB at will, and the connection stays unaffected.

    Do you think there may be abother problem (more than the ones expressed above)? Do we have to do something to be sure we're using maximum Rx sensitivity? 

    Thanks a lot,

  • 0 in reply to Ibrahim Kamal
    Intellectual 390 points

    There is one last difference i noticed between the evauation kit and our PCB:

    We didn't instert this resistor on the differential lines : R241.

    How bad is that! could this also be a reason for low performance and losing connection when one touches the PCB?

    More importantly, what is the value of that resistor? The CC2590 also shows an inductance or a capacitor in its place.. what is the right component to place, and what should be its value?

    Thank you very much,

  • 0 in reply to Ibrahim Kamal
    TI__Expert 7160 points

    Hi Ibrahim,

    All the things you mention (except for the non-existing R241) are probably impacting your range. Could you send me your gerber files and I can give you a full list of recommended actions?

    -Kristoffer

  • 0 in reply to Kristoffer S
    Intellectual 390 points

    Thanks a lot kristoffer, 

    I will provide you with the Gerber once i am back at the office (all i have now is Eagle files, and i don't know how to generate gerbers.. only my collegue does that :) )

    Your input is highly valuable to us, that's a lot!

    Since we are on it, what about R241..? is it totally optional? 

  • 0 in reply to Ibrahim Kamal
    TI__Expert 7160 points

    Hi Ibrahim,

    The notation R_0402 indicates that it is a 0402 reisistor with no value, hence a do-not-mount component. Some CC parts require a cap or an inductor here, but not the CC85xx. I guess it still hangs around from early days when we didn't know whether or not we needed a component here, and a do-not-mount serves as a placeholder where you can solder on a component if you want. Since this placeholder does no harm to the design or the RF performance we never removed it from the design.

    -Kristoffer

  • 0 in reply to Kristoffer S
    Intellectual 390 points

    Thanks for those details, now it's clear!

    Back to the antenna problem, here are the gerber files perpared by my colleague:

    6175.gerber-1.zip

    We'll start redesigning as soon as we get your feedback about the PCB design!

    Thanks a lot,

  • 0 in reply to Ibrahim Kamal
    TI__Expert 7160 points

    Hi Ibrahim,

    Can you please provide the schematic as well?

    Thank you.

    -Kristoffer

  • 0 in reply to Kristoffer S
    Prodigy 10 points

    Hello Kristoffer,

    I'm working with Ibrahim on this project. Here are the schematics (EAGLE):

    7331.ikalogic.zip

    Thank you for your support (and your EHIF library :)).

  • 0 in reply to Vladislav Kosinov
    Intellectual 390 points

    And in case EAGLE files are a problem, here is the PDF version of it :)

    7331.rf_board.pdf

  • 0 in reply to Ibrahim Kamal
    TI__Expert 7160 points

    Hi Ibrahim,

    Here are my comments to your design:

    • It is highly recommended to have a separate GND layer and a separate VDD layer as the 2 middle layers. Let's say you have the RF parts in layer 1. Then layer 2 should be GND and layer 3 should be VDD. See how we have done it in the headset ref erende design: http://www.ti.com/litv/zip/swrr079 
    • The decouple capacitors on CC85xx should be placed as close to the VDD pin as possible. You seem to miss decouple caps on pin 10, 12, 18, 20 and 40. When populating decouple caps make sure you follow the guidelines in the picture below. On pin 37 for example you have the VDD via between the pin and the cap and this is not recommended.
    • Pin 26,27,28 should have one decouple cap of 0.1uF and one of 220pF. You have 2 of 0.1uF.
    • In order to pass regulations you should add 6.8nH inductors on the following CC85xx pins: 11, 14, 15, 16, 17, 36 and 38.
    • To get good grounding avoid thermal relief on ground pads (for example C6)
    • The antenna should be in the same layer as the rest of the RF parts.
    • You should add a lot more GND vias. This is to make sure you have good grounding. See how many we have in the ti reference design. On all the decouple caps place a via close to the GND pad.
    • In the RF match make sure to copy TI's measurements (trace thickness, distance to GND copper pour etc.
    • Which device is U6? It seems to need MCLK, but you have connected BCLK to MCLK? If you choose to connect MCLK from CC85xx make sure this trace also has a 6.8nH inductor.
    • Just a question: Don't you need a CC reset on th programming connector?
    • It is also recommended to add a tuning network in the RF match (between the antenna and the RF match). This is done by (seen from the match) a series zero ohm resistor followed by a do-not-mount shunt component to ground (see picture below). You can then find a combination of L and C components here to match the antenna impedance (if necessary).

    Best regards

    Kristoffer

  • 0 in reply to Kristoffer S
    Intellectual 390 points

    Thanks a million Kristoffer!

    That's really a forum post we'll have to print and pin to the wall :D

    As for the Reset pin, you're right, of course.. for this first prototypes batch, we had to solder some jumper wires to program them... it's a pain, but worth it since it allows us to test the rest of the design. At least now we should be very close to getting it 100 right next time!

    Again, that's a lot!

  • 0 in reply to Ibrahim Kamal
    TI__Expert 7160 points

    Hehe, a picture says more than 1000 words...