Contradicting ideas about differential signal route, confining fields vs Increasing impedance
keep pair intra-distance as close as possible for field cancellation.


No! You need to adhere to a defined distance to get a defined wave impedance. What you describe is a coupled microstrip line.


  Fill surround of pair with GND plane and have via near to it to confine the fields, prevent incoming interference and making it.


... in a defined distance to get a defined impedance.

In fact, you don't need a surrounding GND plane on the same layer – practically all field will be between the two differential conductors; what would be good would be a plane below!


  The source have 200 ohm differential impedance and the load is 1k differential.


So, that's a high-impedance load and not really a low-impedance source. I'd recommend having two matching networks: one at the source to match the source to the transmission line impedance, and one at the sink. 

You could then use an arbitrary transmission line impedance, e.g. the microwave-typical 50 Ω or the 75 Ω. In theory, 200 Ω should work (and would save you the source matching), too, but it might be hard to build using your PCB materials – it depends, can't tell without knowing with what you're working.


  And these are contradicting each other can you explain why?


They are not contradicting. A perfect transmission line does not radiate, so your "as close as possible" simply isn't right – yes, close, but not "as close as possible". 

Use a specific calculator to calculate the right dimensions for a coupled microstrip line on a PCB substrate of your PCB's thickness, with your PCB's \$\varepsilon\$, and on the frequency you work on.