Antenna datasheet

[okw]

I am having a hard time understanding a few things in a datasheet (1206 bluetooth chip antenna).
Page 4 in the datasheet says terminal 2 is NC (just for mounting I guess).
But on "evaluation board and matching circuits" (page 5), it seems this NC terminal is actually connected to ground?
What's more confusing is that INPUT has half of the terminal area also connected to ground.
When making a footprint/land pattern for this part, should I make a replica of the 5x6mm shown in the attached picture (with ground on the 2.25x0.74mm top left "leg" and all of the right 1.8x1.25mm area) and RF feed line, just the 0.62x0.74mm lower left?
And the top image says PI-matching on the feed line, but the image below shows an L-network.

All this is very confusing to me, so any help would be appreciated.

[RFDx]

I am having a hard time understanding a few things in a datasheet (1206 bluetooth chip antenna).
Page 4 in the datasheet says terminal 2 is NC (just for mounting I guess).
But on "evaluation board and matching circuits" (page 5), it seems this NC terminal is actually connected to ground?

Technically GND is 1.25mm away.
 

What's more confusing is that INPUT has half of the terminal area also connected to ground.

Same situation, GND is 2.25mm away. The short "wires" that go to the input pad and to ground are small inductors and are part of the antenna.

When making a footprint/land pattern for this part, should I make a replica of the 5x6mm shown in the attached picture (with ground on the 2.25x0.74mm top left "leg" and all of the right 1.8x1.25mm area) and RF feed line, just the 0.62x0.74mm lower left?

You would be well advised to stick to the layout and dimensions provided in the datasheet. As the layout shows, there is more to it than just the BT antenna.

And the top image says PI-matching on the feed line, but the image below shows an L-network.

Always make room for a PI-network on the board. Place only the components you need.

[okw]

Then I understand even less. All the orange area is GND, right? And to place the 1206 chip, it has to go over the to mini legs on left, and big on right? As seen in the lower part of the image. I tried to replicate this in the footprint I made.

[tszaboo]

You really have to copy the recommended layout down to the micrometer. The funny part about RF is, that everything on that layout is GND when you are measuring it with a multimeter. Every single pad will be connected to GND. About the matching circuit, have some place for some 0402 or 0201 (if you dare) and maybe 0603 if you really must.
Have place for a PI network as RFDx said. And have a VNA ready to use, the standard values never work. You cannot tell the difference between a working antenna circuit, and one which is 99 % worse if you just look at it.

[RFDx]

All the orange area is GND, right?

The orange area on top is first and foremost copper. You have to also look at the copper layer on the bottom (grey colour) to find out what part of the orange area can be considered as RF-GND. The vias around the clearance area (yellow area) should give you a hint. The yellow area is free of copper. Same on the bottom, no copper in the designated 5x6mm clearance area. This means that the two thin traces connected to the feedpoint of the chip antenna have no counterpart GND layer on the bottom of the PCB and have to be viewed as inductors/radiators.

Unfortunately the datasheet is incomplete because a very important fact, the bottom copper layer (grey colour), is missing in the second picture that shows the whole board. For comparison take a look at the following datasheet of another (dual band) chip antenna from the same manufacturer that has a similar layout. 

https://www.mouser.de/datasheet/2/1052/02042021_Quectel_Antenna_YC0011AA_Datasheet_V1_1-2001055.pdf

If still in doubt maybe switch to another chip antenna with similar gain and bandwidth that doesn't need such an elaborate distributed network:

https://www.mouser.de/ProductDetail/Pulse-Electronics/ANT3216LL00R2400A?qs=VAB4DzKv5wVywAIgVVebaA%3D%3D