1 of 1 people found this helpful
yes, it should be connected to the ground plane below.
I'm not well practiced with high speed design. Does this 273 mil grounded trace act as a decoupling capacitor to the signal?
Also, the pattern of ground vias in the ground plane was not really clear in the App Note. Here's what I did in Eagle:
Should I put vias at every 30 mils (horizontally and vertically) or just at the borders of the planes, as it looks like in the App Note?
Another question: The width of the signal trace goes from 20 mils on the antenna to 65 mils. Is this necessary, as I will be connecting the signal to the ANT pin of the PSoC 6. On the PSoC 6 devkit, it looks like the traces is kept at 20 mils all the way to the PSoC.
Yet another question: Should I leave the copper of the antenna uncovered or it doesn't matter if it's covered in solder mask?
It is OK to add additional via as long as it does not affect the strength of the PCB.
The width of the trace connecting the Antenna to the ANT pin of PSoC should be determined by the PCB stack-up (whatever gives 50 ohms characteristic impedance for the trace). In the example depicted in the Application note, it is wide because the PCB is a two layer 60 mil PCB.
The 273 mil grounded trace is a short circuited stub to compensate for the parasitic capacitance between the Antenna and the ground (since the Antenna is bent and runs parallel to the ground).
Thank you, that is really helpful.
Indeed, I saw in the app note that the width of the trace (W) goes down when the thickness of the PCB goes down as well.
I measured the thickness of the Pioneer Kit for PSoC 6 and it is also 60 mils, but it's an 8 layer PCB, and there's a ground plane right below the top level (where the antenna is). Does the thickness that defines W is based on the space between the 2 immediate layers (in the Pioneer kit case, TOP + GND1)?
We will have a 6 layer PCB with ~35 mils thickness, and a ground plane directly below the top level (where the antenna is). Do you have a resource to recommend that would help me figure out the width that I need?
I just read in the App Note that if the transmission line is short enough (which it will be), the trace width criterion is not as strict, so I'll go with that.
Nevertheless, if you have a resource about trace impedance to recommend, I'd very much like to read it.