One of the first steps of layouting a board should always be to think through where you will have high frequency signals and high currents. You then place the components to what makes sense from this. In cases where you have the combination of high currents and high frequency content you will need to take some extra extra care. A trace will always have some resistance, inductance and stray capacitance which scales linearly to distances. With the current design you will have a lot of current switched at high frequency going through long traces with a huge loop area.Not only will this make the circuit radiate a lot of energy, it will also severely impact the performance and ripple of the boost converter, and since you are feeding a low noise amplifier you’d want the powersupply as clean as possible, even though it might have decent PSRR. Read up on how a boost converter works, understand where the currents are going and place the component accordingly.
Here is an example of a good design, all high current components are connected through short low impedance paths (i.e filled zones, not thin traces)
In general, it’s good to keep power carrying paths as wide as possible and use zones where you can to avoid common mode noise.
There is a tone of information out there on both general guidelines of pcb routing as well as guidelines for boost converters. Dave from EEvblog on youtube is one example of a great source of information, he has done a couple of videos on pcb layout and routing.
One final word about thermal relief which you mentioned previously, normally this refers to cutouts in for example a ground plane around a pad, so that if you reflow a board the solder paste will melt at about the same speed on all pads, preventing tombstoning of small parts. As your parts grow bigger this will become less and less of a problem as their mass will fight against the surface tension of the molted solder. If you are not reflowing parts it is less of a concern, although some thermal relief will make it easier to solder, especially if your soldering iron has limited thermal capability.
I’m guessing that you were referring thermal relief to spacing the components to that they get enough cooling. The only parts that will have a lot of power dissipation and therefore heat will be the LDO and the boost controller. You haven‘t specified the current draw on the 6V line, but I’m guessing it will be in the range of tens of mA, so not very significant. If you want to be sure you could always increase the thermal pad on the ld1117 to get more cooling.
Edit: I forgot your question about voltage and trace width. The width is decided by current carrying requirements, voltage is irrelevant