RF via for high power
Following my design constraints i need to route rf signal from top side pcb to bottom through via. Main problem is that i talking about 50W RF signal. Do anybody have experience/ recommendations for such kind of pcb via?
Thanks
For Impedance considerations check discussion here:
http://www.edn.com/design/components...impedance-vias
For power considerations find out skin depth at your frequency and calculate required crosssection to optimize losses.
... another way around actually:
First determine size of your via from power considerations, then make sure it is matched. You can do all that in EM modeler ... if you got one.
But if i determine size via for such power it can be very big (electrically too) and causes to losses and mismatch
For high DC currents what we usually do we put some smaller vias instead one. It's interesting if it possibly for rf too.
via cannot be 50ohm so missmatch loss is unavoidable of you decided to have via.
http://www.edn.com/design/components...impedance-vias
the via suggested by AndreyG looks interesting. take note that this is not conventional via with hole in the middle and ground at the side. they are talking about having signal in the middle. its a novel via but i dont know about implementation cost and difficulty..
it's obvious that via cause to mismatches. i am curious about idea of using two or three conventional vias
Use more than 1 via. I've use this technique with power levels up to 15 watts, although it will also work at higher powers. If you HAVE to flip to the other side, vias are your most reasonable option.
you can try simulating your idea and see if it makes any difference. my worry is 50W is too high any kind of via.
I fear you are right... usually i use vias only for small signal and trying to place/route high power parts without need for vias. But in my current project it can't be done... unfortunately
And... AndreyG thanks, very interesting
What is your frequency? I suggest to use SIW (substrate integrated waveguide). If you do not need DC on this line, SIW is pretty easy to make. You can make first microstrip to SIW transition on one plane on the board, and the SIW to line transition on the other side of the board. I think it is good solution if your frequency at least greater than 5GHz.
Before looking at vias please describe us what kind of traces you use for propagating 50W power over your PCB. (And as already asked - what is your frequency of operation?).
Back to traces - they are not the regular 2 mm wide 1/2 oz copper lines correct? I would imagine something heavier would be required for pumping 50W power.
My expectation is: implementation of via will be consistent with traces used.
Guys, everything much simplier that you think. I usually use short microstrip line 65 mil wide and 2oz thickness . frequency is 100-512MHz
According to my math a 0.5 mm (20 mil) via has already a circumference equal to the trace width. So what are you asking at all?
I believe however that the trace width may be insufficient at 0.5 GHz. Did you calculate?
Skin depth at 0.5 GHz is 3 μm. About 100 mW losses per inch at 50 W/50 ohm (Irms 1 A). Should be no problem.
I used such microstrip to route high power in previous projects that were without vias at higher power part.
It's ok for 500MHz - for simple reason - it's already works.
Considering that skin depth is only 3 μm, there should be no problem to use vias with 20 mils (0,5 mm) drill for this traces.