• State
  • Locked Locked
  • Replies 2 replies
  • Subscribers 16 subscribers
  • Views 699 views
  • Users 0 members are here
Support feedback
Options
Options
Similar topics

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.

CC8520: Assistance with PCB layout based on the EM

Andrew Welker
Intellectual 320 points
Part Number: CC8520

Hello,

I am going through the painful process of rebuilding the PCB layout in Altium for the CC85XX-CC2390EM, due to the lack of compatible design files from Ti. I have a few questions about the PCB layout as I wish to make some small changes to the design and add DAC or ADC sections as required. 

I judge the via size on the EM to be 10mil/20mil. Is this correct?

The plane pours seem to have a clearance of 12mil. Is this correct?

I am planning on removing the PCB trace antenna and using a right-angle SMA connector with the same footprint and location as the one on the EM. Because I am removing the trace antenna, is it good practice to also remove C114 and the rotated position/pad for R1 to close the top layer ground plane pour in this area, or should I leave a gap as on the EM?

When the EM module is plugged into the design kit main board, the module overhangs the main PCB. Is this for antenna performance reasons and is the overhang necessary if I am not going to have a trace antenna?

Is there a technical reason for the chaotic positioning of the stitching vias on the EM, or can a grid layout be used? If a grid can be used, what spacing would be recommended?

Finally, if I am going to have an ADC or DAC and power supplies on the same PCB, is it good practice to split the ground plane pours on all layers and join with the RF planes at a single point (star ground), or should I pour and stitch the planes over the entire PCB?

I have limited experience with RF PCB layouts, so I am trying to duplicate the EM as closely as possible. I would appreciate any answers to the above or any suggestions you might have.

Thank you,

AWCC85XX_CC2590EM_Layout.pdf

  • 0
    TI__Guru** 106705 points
    Hi Andrew,

    The vias are either 0.2 or 0.3 mm. It is not critical, so use whatever work for you.

    The readme file says 8 mil copper width / 8 mil clearance.

    If you will only use SMA connector you might aswell remove C114 and R1 aswell.

    The overhang is primarily to get clearance around the PCB antenna, yes.

    I would recommend chaotic stitching to avoid the risk of getting into resonance issues. The distance between the vias should be less than 1.25 cm (wavelength / 10).

    I would recommend having one common ground plane for the entire PCB.

    Regards,
    Fredrik
  • 0 in reply to Fredrik K
    Intellectual 320 points

    Thank you for your suggestions Fredrik!

    So, if I remove C114 and the rotated position for R1 the top layer ground plane will now be closed at the top of the PCB. Is this OK from an RF standpoint, or should the gap in the plane be maintained?

    AW