Trace impedance calculation in Altium for RF

Question

I am routing the RF trace for a Microchip RN2903 LoRa module. The datasheet states the following:

I wanted to use Altium to calculate the width of the trace automatically, so that it had a 50 Ohm impedance. In my layer stack manager, I have the following:

Note that Altium calculates that the trace should be ~100 mil wide, which is significantly higher than what the datasheet suggests (0.75 mm=30 mil). The datasheet is using an FR4, 1 oz copper, 2-layer PCB, with a thickness of 1.55 mm. I am using these same values, except the width of my PCB is 62.992mil=1.6 mm (not significantly thicker).

Any ideas as to why this discrepancy? The only thing that could vary would be the Dielectric Constant of the FR4. I am using Altium's default: 4.8. Maybe this is another value, any ideas as to what it should be?

EDIT: Modified first figure to point to 6mil=0.15mm gap between RF trace and ground plane.

Answer 1

Results from a trace width calculator I use:
Using Er = 4.8 (I normally use 4.2 since we use Isola 370HR)
Gap between trace and upper ground plane = 6 mils, as used in Figure 5.1
Z = 50 ohms
Trace width = 30 mils (36 mils for Er = 4.2) which closely matches with Figure 5.1.

With a gap between trace and upper ground plane = 60 mils, the trace width is 100 mils which is close to Altium's calculator.

You can use an online coplanar waveguide calculator to play around with your design.

Edit:
The following image shows the differences between the coplanar and microstrip transmission lines. Trace width = 30 mils, gap = 6 mils, dielectric thickness = 60 mils. The images were created with ATLC2. The colors represent the materials; green is the ground plane, red is the conductor, and turquoise is the pcb dielectric with an Er of 4.8. You can see how the fields are affected by the ground plane on the surface of the board.