• State Resolved
  • Locked Locked
  • Replies 3 replies
  • Subscribers 30 subscribers
  • Views 1071 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.

TIDEP-01012: Antenna and feed line impedance matching

Timur Suanov
Intellectual 290 points
Part Number: TIDEP-01012

Hello, TI experts!

Antenna feed line trace width in reference design TIDEP-01012 is about 0.213 mm (8.5 mil) while design value (50 Ohm target impedance) is about 0.267 mm (10.5 mil). I have estimate impedance for actual stackup and trace width (0.213 mm, soldermask is opened) using PCB CAD, and calculated value is about 60 Ohm. 

Have you measure or simulate (using SHFrequency CAD) antenna feed line impedance someway? Is the actual line width provides antenna and feed line impedance matching in needed frequency range?

Thanks,

Timur

  • 0
    TI__Genius 17910 points

    Hi Timur, 

    I will check into this and get back to you. Might take a few days.

    Thank you,

    -Randy

  • 0 in reply to Randy Rosales
    TI__Genius 17910 points

    Hi Timur,

    How are you evaluating the impedance of this GCPW transmission line? I have looked at this both in HFSS full field sim and in wCalc (closed form approximation wcalc.sourceforge.net/coplanar.html).

    The HFSS sim was used to determine the final dimensions in the design. In HFSS I see around 47ohm @ 77GHz and 48ohm @ 20GHz. The same GCPW is used for fan-out of both the RF TX/RX and the LO SYNCIN/SYNCOUT fan-out.

    In HFSS, one issue that I ran into initially during simulation was placing the waveport too far away from the GCPW ground vias near the edge of the board cutout. I used a 1 inch x 1 inch RO3003 + L1 and L2 copper layer cutout with the same properties and GCPW line and via dimensions as the Cascade EVM design.Looking at 20 GHz performance things looked good, but my initial RF sim (adaptive frequency sim centered at 78.5GHz) was showing a much higher impedance at around ~60ohm. The S11 for the wave-port also looked funny (bad match for perfectly matched port). Looking into the E-fields of the copper and substrate revealed standing waves that were developing from the boundary of the port.

    I ended up modifying the geometry to include an additional set of GND vias intersecting with my waveport boundary and re-ran the sim. In this case the values were in the expected range.

    Please let me know if that helps.

    Thank you,
    -Randy

  • 0 in reply to Randy Rosales
    Intellectual 290 points

    Hi Randy!

    Thanks very much for your quick and detailed response! It is more than sufficient.

    As for my estimation of trace impedance, - it is incorrect due to improper PCB CAD I have used, GCPW was treated as a microstrip.

    Thank you,
    Timur