• State Resolved
  • Locked Locked
  • Replies 18 replies
  • Subscribers 40 subscribers
  • Views 1841 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.

Schematic review of MSP430+CC3000

Swarika Jain
Intellectual 555 points

Hi,

Somebody please review my schematics before I give it for manufacturing.

I have attached the design file here.

Thanking in advance,

Swarika Jain

  • 0
    Expert 2685 points

    Is this design optimized for cost? What is the cost of the GPS module that you are using? Also why did you decide to keep all the 0 Ohm resistors and the non-existent inductor in the CC3000 part of the design?

  • 0 in reply to Ivor Sargoytchev
    Intellectual 555 points

    Hi Ivor,

    Thanks for such a quick reply. I really appreciate it.

    Well, the design is in accordance with the schematic given on the product page of CC3000. So, we kept the 0 ohm resistors and the non existent inductor because it was given in the CC3000 schematic.

    We will remove them. What else would you suggest?

    Also,

    we would like to make our design cost effective. The GPS module we have used costs us $12 - $13 approx.

    We wanted to use the CC4000 GPS module by TI but it is not available as a standalone module, we can only buy the CC4000 as a development board. So, we decided not to use it.

    Any other GPS module that you would like to suggest?

    Thnaks a lot.

    Regards,

    Swarika Jain

  • 0 in reply to Swarika Jain
    Expert 2685 points

    Well, for the GPS you cold probably find one for $10, but you are already pretty close to that. Also I wold look into loosing the crystal, most 5th Series MSP430s have a built in DCO that will do just fine, as long you don't go over 8MHz on the SPI bus.


    The biggest and most important portion of the design these days is the software that you write. However the actual board layout is important as well, especially the RF part of the CC3000.

  • 0 in reply to Ivor Sargoytchev
    Intellectual 555 points

    Hi Ivor,

    Could you please elaborate on the RF part of the CC3000 ?

    Do you think our design will give good RF performance?

    Regards,

    Swarika Jain

  • 0 in reply to Swarika Jain
    Expert 2685 points

    The RF performance depends 100% on your PCB design. The RF part is the trace between the CC3000 and its antenna and the two caps plus the one inductor that are connected to this trace. This is not a simple trace, it is actually a waveguide built into the PCB. Without it the RF performance will be so bad that you will not be able to connect to an AP unless it is sitting right next to your device.

    All the distances of this waveguide are precisely calculated and need to be matched in your PCB design. Luckily TI provides two different boards that you can use as a reference - the CC3000EM and the CC3000BOOST. The first is a 4-layer board and the second is a 2-layer board. So, what you can do is copy the RF part of the design from the board that matches the number of layers of your board. But you need to be precise down to 1 mil, otherwise you will not be able to get the same RF performance as one of these boards. Also you need to make sure you use exactly the same parts for the antenna, the inductor and the two caps.

    Of course you can avoid all this by integrating one of these boards into your design, but that would double your cost. Another option is to learn about RF PCB design and come up with your own waveguide layout, but this is also expensive in terms of time.

  • 0 in reply to Ivor Sargoytchev
    Intellectual 555 points

    Hi Ivor,

    Thanks for the information.

    Could you also please review our board layout design. We need to send it for manufacturing.

    Regards,

    Swarika Jain

  • 0 in reply to Swarika Jain
    Expert 2685 points

    Very nice idea for two board compact design! And your bottom board with the MCU looks good.

    However your top board with the CC3000 is not done correctly. It looks like you haven't followed most of the PCB guidelines in the datasheet. Your waveguide will not work without the copper pour and the via stitching. Also because of the lack of copper pour under the CC3000 this thing will radiate in all directions. Also the heat sinking will be very poor and the CC3000 might get hot. This design might work if the AP is very close, but otherwise it won't.

    But even if you make all these corrections, I am not sure if you don't need to adjust some of the RF circuit values. You need a RF PCB engineer to advise you on this, and I am not one. This is why in my design I copied the RF part from the CC3000BOOST board.

    Note that the CC3000 footprint is wrong in the datasheet and in your design as well. Please see this post:

    http://e2e.ti.com/support/wireless_connectivity/f/851/t/293285.aspx

    One more thing - before making lots of these you need to make a couple of prototypes to see if your GPS will get good reception with the CC3000 right under it.

  • 0 in reply to Ivor Sargoytchev
    Intellectual 555 points

    Hi Ivor,

    We have made a few changes.

    Please review the design and advise

    Thank you.

    Regards,

    Swarika Jain

  • 0 in reply to Swarika Jain
    Expert 2685 points

    It is not really possible to see anything from this image. Can you post larger images (at least 3x) with the layers separated?

  • 0 in reply to Ivor Sargoytchev
    Intellectual 555 points

    Hi Ivor,

    Sorry for the inconvenience.

    Here are the better images.

    Thank you.

    Regards,

    Swarika Jain

  • 0 in reply to Swarika Jain
    Expert 2685 points

    Your waveguide is still incorrect. Here are the issues:

    1. The via stitches should be connected to the ground plane on both sides of the board. Also you don't want the copper pour sea-sawing around them.
    2. I cannot measure any distances from the image, but I can tell that the gap between your RF trace and the copper pour is way more than 5 mil.
    3. The RF trace from the CC3000 to C9 should be perfectly straight. Instead yours has a bend in the middle and then it curves towards C9.
    4. The footprint of the CC3000 is still incorrect -  I mentioned this in my previous post.
    5. The hole under your GPS should not extend to the CC3000 layer - this is not a big deal.

    But most importantly you must make sure the RF trace is exactly 20 mil wide and the gap is exactly 5 mil. Also make sure the gap is completely uniform. You can use the free "gerbv" Gerber Viewer to measure it.

    If your manufacturer cannot meet these specifications, you can use a free program called TXLINE 2003 to calculate a different trace width and gap width. You should use the "CPW Ground" model. You want to make the impedance as close as possible to 50 Ohms:

    Also the TI specified board height (H) and copper thickness (T) are not standard in some parts of the world. You should also use this program to see how the board that your manufacturer can make changes the impedance of the waveguide.

  • 0 in reply to Ivor Sargoytchev
    Intellectual 555 points

    Hi Ivor,

    Thanks a lot for such a detailed explanation.

    We will make the advised changes.

    Regards,

    Swarika Jain

  • 0 in reply to Swarika Jain
    Intellectual 555 points

    Hi Ivor,

    We have made the mentioned changes.

    We will really appreciate it if you could please review it once more.

    We have checked the footprint too.

    Please advise if any other change has to be done.

    Thank You.

    Regards,

    Swarika Jain

  • 0 in reply to Swarika Jain
    Expert 2685 points

    Hi Swarika,

    At this point I cannot tell if there is a problem with the image or your layout, but the vertical trace doesn't look right. Please post the Gerber of the CC3000 layer instead.

    Your CC3000 footprint is still incorrect - don't look at the datasheet because it is incorrect there as well. Look at this post instead as I have already mentioned this previously:

    http://e2e.ti.com/support/wireless_connectivity/f/851/t/293285.aspx

  • 0 in reply to Ivor Sargoytchev
    Intellectual 555 points

    Hi Ivor,

    We now realized what was wrong in our footprint. We have now finally corrected it.

    I am inserting gerber files. Please have a look and advise.

    0640.Design.rar

     

    Thank You.

    Regards,

    Swarika Jain

  • 0 in reply to Swarika Jain
    Expert 2685 points

    The RF trace looks good. There are some very minor miss-alignments, but they should not affect the waveguide characteristics. There is one major issue though that I never noticed before - looks like you forgot to connect Pin 5 to Pin 7 of the CC3000.

    Also I have a question - are you using a 0402 inductor or larger. I wanted to go with 0603 in my design, but I never found one that matches the parameters of the 0402 that TI recommends, so I was forced to use 0402, which is very small for my taste. If you are using a larger inductor, can you send me the link to its datasheet?

  • 0 in reply to Ivor Sargoytchev
    Intellectual 555 points

    Hi Ivor,

    We will be using a 0603 inductor.

    Datasheet of a 2.2nH 0603 inductor is inserted here. It can be ordered from Mouser. The manufacturing part no. is: B82496C3229A

    1452.b82496c-40686.pdf

    We have now connected together pin5 and pin7 of CC3000.

    We had earlier connected both to the ground. Thanks for identifying this mistake too.

    Please suggest if there are any other changes required.

    Thanks a lot.

    Regards,

    Swarika Jain

  • 0 in reply to Swarika Jain
    Expert 2685 points

    Yes, I looked at these inductors as well. All the 2.2nH 0603 inductors have a max DC resistance of 350 mOhm, compared to the 160 mOhm of the 0402 inductors. No one was able to tell me if this difference matters, so I decided to go with the 0402 inductor in order to perfectly match TI's specs.

    Everything else looks good. Please let me know how is the reception once you manufacture it. I am playing with a couple of different deign myself, but nothing this compact yet.