Design of 50 ohms RF trace for 2.4GHz...Double layer FR-4 PCB
Your calculations check out for the given values, but keep in mind that the dielectric constant of FR-4 is not tightly controlled, and may vary between 4.35 and 4.7 between manufacturers [1]. Since your trace length is very short, this variation will not have a big effect (you can try the values in the calculator). For more demanding applications, special high-frequency PCB materials (for example: Rogers RO4000 [2]) are available, however they are much more expensive to produce.

It can be beneficial to disable the thermals around the GND-pin holes of the RF connector. By having a solid ground connection, you reduce the parasitic inductance in the return current path, which will improve your signal integrity. 

If you use a coplanar waveguide, the copper pours below and on the sides of the conductor must be strongly referenced to each other. This means putting vias to 'stitch' the top and bottom planes together, along both sides of the conductor, to surround it with the ground connection. This is discussed in [3].

The recommended stitching distance between vias should be at most λ/4, with λ/10 as an optimum. For 2.4GHz this results in a via distance of maximum 3.12cm, with 1.25cm recommended. So, for longer trace lengths and higher frequencies stitching becomes more important than in this case with a very short trace length. 

[1] https://en.wikipedia.org/wiki/FR-4 see: dielectric constant permittivity

[2] https://www.rogerscorp.com/documents/726/acs/RO4000-LaminatesData-sheet.pdf

[3] Choose the size of via for shielding and stitching