I am designing a board by incorporating a cellular module. Could any one please provide the procedure to add microstrip line or RF trace on the PCB as well as how to controller trace impedance to 50Ohm?
You can use the built-in Track Impedance calculator found under Utilities > Design Calculators to work out the target track width. Just change the dropdown next to Calculate to "Required Track Width".
There are other calculators available such as Saturn PCB Toolkit.
Open Setup Technology and Nets, Net Classes then create a new netclass, called imp50R_cellular or something similar.
Then in your design select the tracks that require impedance control and using Setup Technology Nets change the nets over to the netclass you created.
Then you can set up rules in either the Schematic, that get copied over to the PCB, or directly in the PCB Editor itself, for the required track thickness and creepages that you've calculated.
You can also create construction layers to represent the prepregs between copper layer and enter the thicknesses here to include on a layer stack diagram for the documentation layer.
Finally, you should add a note, and a call out indicating the tracks that require impedance control on the documentation layer, and tell the fabricator the required impedance and tolerance.
There are two approaches to working with this now. One is to specify the materials and thickness yourself. The other is to advise the fabricator and let the fabricator use thier skill and judgment, and more expensive software to attain your target impedance.
This is assuming that you haven't got the High Speed options on your license.