• State Resolved
  • Locked Locked
  • Replies 9 replies
  • Subscribers 19 subscribers
  • Views 2865 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.

cc2540 PCB design help (second try)

natanel
Intellectual 590 points

Other Parts Discussed in Thread: CC2541, CC2540

Hi

this should be bee board [url]http://www.seeedstudio.com/wiki/Bluetooth_Bee[/url] with TI cc2540/cc2541 bluetooth low energy MCU [url]http://www.ti.com/product/cc2540&DCMP=LowPowerRFICs+Other&HQS=Other+OT+cc2540[/url]

I am posting second board (first board http://e2e.ti.com/support/low_power_rf/f/155/p/208830/741982.aspx) after comments of  and  (thanks you help alot)

I have few questions

in generaly which issues you can inspect in this design?

 remarks

1) "to many cutouts"

I am new to this what are exactly the cutout (black square without ground?), this is two layers board any way to reduce this cutouts 

2) " Copy the reference design for the balun"

did it, is it look ok?

3) "You need to make your ground plane a ground plane, that is you cannot have traces in the ground plane"

 I can not see away to do it in two layers board, is it mean it will not work/ drastic limit the receive/ transmit ?

do you have any idea how to solve it (increase board size+ground in specific direction, add some passive competences, other)


 remarks

1) "VDD trace on the bottom layer going underneath the RF traces"

moved it

2) " The antenna is too close to the ground plane"

it is now like the reference, W2 = 0.5mm, L6=4.9mm, D4=0.4mm, L1=3.94, is it look ok?

3) "I would change to 0.3mm vias"

change it to 0.3mm, is there enough vias or need more?

4) "The decoupling capacitors should preferably be even closer to the power pins"

did my best, is it ok? which need to move closer?


thanks

Natanel

  • 0
    Guru 22270 points

    Hello Natanel,

    Great work on the board! I can't comment on the correctness of the layout, but it looks like this is for the CC2541.

    If it is a general breakout board I would include P0_0, P0_1 and P0_6. Also, you might as well provide pins for DGND_USB and DVDD_USB, allowing you to get the most out of you design now and in the future.

  • 0
    TI__Guru** 106705 points

    Hi Natanel,

    This looks much better than the first revision and will most likely work very well.

    L301 can be omitted, it is not required.

    Regarding TA12012 comments I would say that for a 2-layer design it is impossiple not to have any routing on the ground plane layer. However, you have now done a much better job on making the ground plane as big and continuous as possible by routing the VDD trace in a U-shape instead of cutting the ground plane in half as in the previous version of the design. The balun design looks good.

    As for my comments, it seems like you have solved all the issues I pointed out.

    /Fredrik

  • 0
    Guru 22270 points

    Hello Natanel,

    I could be looking at you board incorrectly, but at coordinates (19, 5) on the blue schematic, it looks like those pads are for another crystal (32.768kHz).  The traces go through R11 and R1 which appear to be connected to P1_1 and P1_0.  For the CC25xx, it should be connected to P2_3 and P2_4.

    You should be able to fit pads for a USB mini connector by removing the three visa at (13, 4) and moving the traces over.

    The work you have done is very good! Let us know how it performs.

  • 0 in reply to Greenja
    TI__Guru** 106705 points

    Based on the pins used and the series resistors I would guess that these are pads for LEDs.

    It is anyway a good catch that there is no 32 kHz crystal, however this is only required if you plan to use power modes.

    /Fredrik

  • 0 in reply to Fredrik K
    Intellectual 590 points

    Hi

    the P1_1 and P1_0 are used for led indication the same as bluebee board

    P2_4 and P2_3 are for allowing also to connect 32 kHz crystal

    P2_2 and P2_1 are for allowing debug  DC and DD

    P2_0 is for ADC T allowing  (which I don't really understand what is it "T")

    P0_2 to P0_5 for USART_0 RTS,CTS,RX,TX

    UDP and UDN cc2540 also for SCL SDA cc2541, need to think how I can add mini usb or be able to get also DGND and DVDD usb

    P1_4 to p1_7 are for SPI_1 MI,MO,C,SS (copy paste error the first MI in the board should be clock)

    P1_3 , P1_2 just was able to spread them also

    P0_7  to enable an ADC A7

    I need to check and see if I can add those usb GND and DVDD

    probably remove button 3.3v add GND and push the SPI right one place, but then it will not be like bluebee board (confused)

    I tried it will look like this so it can be used by Arduino, but I do not see there usb GND and DVDD (how they used it?)

  • 0 in reply to natanel
    Guru 22270 points

    1. You would have to put the 32kHz on the board with traces that can be cut  if you want to use the pins as regular outputs.

    2. The T is for trigger that allows you to start an ADC conversion from a external input on that pin.  The info is in the CC253x/CC254x guide. http://www.ti.com/lit/ug/swru191c/swru191c.pdf

    3. The USB ground can be tied directly to ground and the USB Vdd can be tied to 3.3V.  You would then have to add a LDO regulator that would allow the board to be directly powered from the PC USB.  It would be the VBus.  You can look at the USB Dongle schematic as an example.  There you will notice that P1_0 is used to enable the USB. http://www.ti.com/tool/cc2540usb-rd

    4. For the USB mini, you would not have the pads going to the bottom header, so the pin configuration would still match the the Arduino.

    You definitely want to add the missing P0 pins because they can be used for the timer (PWM) as well as ADC.  There are some in used header pins you could use for these.  You could also have just a through hole pad in a convenient location.

  • 0 in reply to Greenja
    Intellectual 590 points

    Hi greenja

    1) 32KHz is it must?? does with out it the BLE is not low energy? any way I don't find a place to put it on board

    2) if 32KHz is connected to the pins P2_4 and P2_3 from external board, is it to far to be used?

    3) adding USB  include many components (count 14 in the usb mini doungle schematics) I can not see how to add them, if I will follow to bluebee design it should be external board connected to this one

    4) was able to add all P0 pins except P0_1, this si the best I can do


    thanks all for the help

  • 0 in reply to natanel
    Guru 22270 points

    1. The 32kHz is not required for BLE. You could go with the through hole one, it should fit.  As Fredrik stated, it is only required for the different power modes.

    2. I'm not sure of the maximum distance but, I would imaginge that is would have to be as close to the chip as possible due to capacitance. 

    3. The USB only requires the resistors.  The other components are only required if you want the board to be powered by the USB.  Otherwise, it can remain self powered when USB Vdd is tied directly to 3.3V

    4. You will want to add the P0 pins that are used in the BLE Stack examples.  This will help when you start developing and testing BLE applications.  You can pick which board you want to design off of by looking at the Keyfob schematic. These can be found in the CC2540 technical data section

  • 0
    TI__Mastermind 36415 points

    Natanel, 

    Your new PCB looks very good, I only found one small item i would like to recommend. Everything looks good except the ground return on the lower right hand corner of the device, I would recommend to add one more ground via to tie top and bottom together as shown below.

    Regards
    /TA