Is there any reasonable justification for not using via hole to route RF signals?
I am a little bit confused regarding the use of via hole.
My supervisor discourage me in using via holes to route a RF signal, but I didn't find in scientific litterature a justification. Moreover, nowadays there are several commercial electromagnetic solver which can help me to predict the behaviour of via-hole and minimizing the unwanted effects.
Why should not I use the via-hole?
Is there application notes or study cases where someone else has designed a RF board using via-hole?
Make me undestand, I pray you
Thanks & Best regards
Antonio
Antonio, routing RF signals through vias is fine if you can keep the line impedance. If you want to pass from one side of a ground to another, you need to control the via/cutout ratio.
https://www.polarinstruments.com/support/si/AP8178.html
The via itself has some series inductance, now you need to control the shunt capacitance to make a "good" via transition that matches your line impedance.
Sometimes the line with signal + ground is both passed through via holes. Example: I recently designed a chip -> module -> PCB transition with >50GHz bandwidth. The placement of signal and ground vias then controls the line impedance in "vertical" direction.
For more specific references: what is your application for routing RF through vias? Why do you want/need to do that?
When routing RF, you need to be careful with where your ground and where your signal is. Your signal and ground path should always be continous to prevent any parasitic or PIM products from occuring. It depends on your stackup of PCB board and the type of Tline method that you use(microstrip, Coplanar etc) What are you planning to do?
your supervisor is a smart person!
If we are talking about 500 MHz, go for it. If we are talking above 5 GHz....things get interesting quickly. You need to transfer the RF current on the microstrip line from one side to the other of the board....but equally important you need to transfer the GROUND currents from one ground plane to another. Usually you need a ring of grounding vias to do that, and as the frequency goes up, that gets harder and harder to do correctly.
BTW, i have never seen it done above 18 Ghz.
I'm designing a RF trasmitter. However, the via issue is at 500 MHz frequency, a very low frequency to bring to light this problem (in my opinion).
Anyway, my question is very general. I want to understand why I should not use the vias to route RF signals.
I think it is very complicated to use them, but we have the support of electromagnetic simulators. Of course, if the company wants the reduce the costs and the time-to-market, it will prefer a simpler approach. I know that, but in our case we forced to use them because of size constraints.
Help me to understand.
xBiff44: Why do you say that it is harder to realize a ring of grounding vias? Why is difficult at high frequencies?
Best regards to everyone.
Antonio
In RF due to high frequency and wavelength of signal, it is important where is your reference point is. The signal that you are tracing also has a ground path, meaning when you carry a current through via to another layer, you also need to carry the corresponding ground as well. So, when you carry the signal through a via to another layer, how do you carry the ground? Imagine the current buckling through the via and passing to another level; but when doing so, you need to provide a path for ground as well; thats why it becomes trickier as frequency goes up.
These issues are more important as the frequency goes up to Gh'z levels; not so much at 500 MHz. At 5Mhz your wavelength is 60cm. so at every 15cm, the phase of your signal changes by 90 degrees. Imagine it being a simple sinewave, so in 15cm you are going from 1-->0. For this, you need to be careful with how you route the signal.
I would advise Pozar's Microwave Engineering book to read about this topic and to understand the physical phenomenon behind it.
Ask your supervisor what he was thinking. I don't agree that this rule applies in such a general way. You just need to do the vias right for signal and ground, as I explained above.
GHz signals across vias between multiple layers is widely used in high speed digital backplanes or in every DDR4 memory board (> 2GHz on the data lines).
General speaking, the Vias will create discontinuities on the Transmission Line even they are well dimensioned, therefore Vias are avoided due to this discontinuity resulting to changing Characteristic Impedance.( and surely loss ) But under few hundred MHz, they are not potential problem.For instance, Vias are necessary to tie the GND connections of a transistor,matching circuit etc.
So there is no general rule for them.