The datasheet for this part states the input and output are internally matched to 50 ohms.
However what exactly does this mean? For example the output, would I still need a 50 ohm microstrip to connect the output to a SMA connector? Could this instead be done using lumped components and a normal sized trace as the microstrip would be around 120mil?
Matched RF traces means that they have a certain impedance at the relevant frequencies. What does this mean? Basically, the lines have to have a certain geometry (width, thickness, height of board) that provides a certain impedance. Why is this done? Because when you have impedance matched, the power transfer is at its maximum. You don't want to "send" power out and have it return since this is wasteful and in some cases damaging.
user17441 started talking about return loss without defining it.Because the word loss is mentioned part of the term, many people get confused about what it means. You want return loss to be as high as possible (as many dB as possible). Why? You want to send all the power and none needs to return (ideally), therefore, it all has to get "lost" in the antenna. Nothing needs to return (or as little as possible).
However, return loss is a paremeter you measure after you do the design. WHen you have good matching and good grounding, you have good protection.
As a whole, the best approach you can take is to clone the PCB layout of whatever component you're using and use the manufacturer's recommendation. This means placing components the same way, using the same thickness PCB, using the same amount of copper on the board, etc. This is unless you have a different requirement, but using the manufacturer's design will basically get you to the finish line quicker than doing it yourself unless you have experience with RF design.
Usually in PCBs, the microstrip line approach is preferred - basically a track on top and ground plane on the bottom, because it's easy to create and use (other methods are much more difficult. So basically you'd be expected to create microstrip lines with 50 ohm impedance to ensure proper power transfer. A few good references for learning:
Microwave Transistor Amplifiers: Analysis and Design Forget about the fact that the name makes it seem as if it's only about amplifiers. Matching and matching network design is covered at the start of the book and it's very good (with plenty of exercises).
Microwave Engineering by Pozar is another classic text
When you get to creating your own transmission lines (50 ohm line is one example), you can use this free tool:
I've used it to create real boards and it's quite good and flexible.
One alternative is to use coplanar waveguide instead of microstrip.
According to the Microwaves101 coplanar waveguide calculator, if your board shop can do 4 mil feature spacing, you can make a 50 Ohm CPW using a 30 mil trace width:
Notice there is no groundplane beneath the trace on the back side of the board for this type of waveguide. If you have a groundplane on the back side you'll need to recalcualte the dimensions for "grounded coplanar waveguide" or "copper-backed coplanar waveguide".
If your minimum spacing is 6 mil, the trace width needs to increase to about 45 mil, but that's still much smaller than the 120 mil you say you need for microstrip.
