TRF37A73: unexpected oscillation near 5GHz on empty PCB (no input connected)

您好，

已经收到了您的案例，调查需要些时间，感谢您的耐心等待。

Hi there,

From reviewing your PCB layout, i believe that the oscillation could be caused by some resonance happening in the power supply. On the output, you have several open circuited stubs, shown in red. Depending on the exact PCB stackup and lengths, these could look like a lumped element component placed either series or to ground. I suggest following the TI layout guidelines for this part.

he 2.2uH inductor would be ok, but im suspicious on the SRF of it. You need to ensure that the self resonant frequency (SRF) is at least an octave (2x) above your frequency of interest. The one TI uses on the EVM for this device would be a good choice, the 0603HP-R10XJLW from CoilCraft. The SRF is the reason behind the choice for 100 nH over a higher value component.

Additionally, since the inductor we used was an 0603 package, we could land the pad directly on the output trace, eliminating the stub you have here. (shown in blue circle)

The RF Bypass capacitors should be located physically close to the VCC pin and the bias inductor input to limit the power supply picking up the RF.

Here is a lumped element example of the potential parasitics that i see from your board layout. The TI EVM for this part is a good example of how to do RF layout. Lots of unintentional resonators could potentially cause you issues with your board. 

A few more things:

1. The trace widths and spacing to ground should be accurate to a 50 ohm transmission line to limit reflections. You are using Grounded Coplanar Waveguides (GCPW) here. You can look up a calculator online that can give your trace and gap dimensions depending on your stackup. Or if you send your stackup information, I can give you some dimensions.

2. Via stitching should be included on the ground planes surrounding the RF, to contain the fields coming from the traces, and to ensure the correct trace impedance.

3. You should choose your core dielectric material to work good at your frequency of interest. FR4 is good to like 1 to 2 GHz but after that, TI uses Isola 185HR, Isola 370HR, Panasonic Megtron6, Rogers 4350B (in order of usage in low frequency to high frequency) due to their controlled dielectric constants. You can check the datasheets for these materials for more info.

4. TI removes the soldermask above the RF trace, because the soldermask permittivity is not controlled and can cause your trace impedance to be incorrect from calculations.

Let me know if you have any more questions,

Hi

Thank you for your detailed response to my previous question about the TRF37A73 PCB layout. However, it seems that the images you included in your reply did not display correctly on my end.

Would you mind re-uploading the images? This will help me better understand  layout recommendations you mentioned.

感謝您重新上傳圖片，但我這邊仍然無法看到您回覆中的任何圖片。
網站提示我沒有查看圖片的權限。
是否能麻煩您將圖片直接複製貼上到留言處，或者使用不需要特別權限的方法分享圖片呢？
又或者從datasheet能否對照出您上傳的圖片呢
非常感謝您的協助！

Thank you for re-uploading the images. However, I still cannot see any of the pictures in your response.
The website indicates that I do not have the necessary permissions to view the images.

Would it be possible for you to directly copy and paste the images into the reply or use a method that does not require special viewing permissions?

Alternatively, if the images you referenced are available in the datasheet, could you please indicate which section or figure corresponds to the points you were trying to highlight?

Thank you very much for your support!