RF trace thickness from RF module pin to SAM connector - 433Mhz antenna

I do not have much knowledge regarding RF PCB design so my queries would be very basic:sad:

I have a 433MHz RF module on PCB, its RFM69W by HOPERF. PCB that I am using is a 1.6mm 4 layer board. PCB stack up is TOP signal layer, ground plane, power plane, Bottom Signal layer.
I plan to have an 50 ohm SMA connector on PCB to connect whip antenna.

Wanted inputs regarding thickness of antenna trace on top layer (routed as microstrip line) which would run from RF module antenna pin to SMA connector. Trace needs to be of 50 ohms impedance.

Trace thickness provided by PCB vendor for 50 ohm microstrip line is 13.067 mils, this is considering ground reference plane on layer 2.
Now, I read few app notes which suggest quite thicker trace widths of about 1mm (but they do not provide details for separation between trace and ground reference plane)

So, what layout should I follow to route this antenna trace? Trace length would be 10mm.

Or should I keep maximum separation between RF trace and ground plane (by having no copper under RF trace on layer 2&3) to reduce signal absorption and have ground plane under RF trace on layer 4? In this case what would be the trace thickness?

Trace width is heavily dependent on the spacing between the plane and the trace, for a 1.6mm spacing (on a standard 2 layer FR4) you end up at ~2.8mm or so.
for a 4 layer stack it highly depends on the thickness of the dielectric between outer layers.

For example 0.2mm spacing, microstrip with Er = 4.6 gives ~0.3mm width for 50 ohms.

Grab a copy of the free 'Saturn PCB Toolkit' and play with the Conductor impedance tab to get a feel for this.

Regards, Dan.

You'll notice that transmission lines of given impedance can be easily scaled in dimensions. If you have already a correct calculation for one substrate height you also know the results for others.

If you are stuck to a thick substrate you might consider coplanar scrips with to ground to reduce the trace width.

Dan,
Yes, for a 4 layer stack, with 8 mils spacing, trace thickness for 50 ohms is 13.067 mils. This is similar to what I got from our PCB vendor stackup drawing. Have attached stackup here.

I am confused after reading a few app notes which suggest that for 50 ohm antenna trace you should have max spacing between trace and ground place, to minimize RF signal absorption by close ground plane.

So I wanted to know weather I should use layer 2 as ground plane or should I have no copper pour (below antenna trace) on layer 2 & 3 and use layer 4 as ground plane.

Talking of "absorption by close ground plane" actually means confusing things. A smaller trace has a higher resistance (assume constant skin depth in a first order), in so far absorption increases. There's a trade-off between losses and PCB size, just your decision.

Could also be talking about dielectric losses, not going to be important for this, but can be an issue when running real power at UHF and up.

I have seen boards burn because of the dielectric losses @ 70cms with a few hundred watts in play, annoying when it happens to your reflection bridge, it is however not going to be any kind of issue with the flea power your little module puts out.

Regards, Dan.