I normally use (127mm, 127mm) as some reference location on the PCB. It can be a corner, but it can also be the center of a mouning hole, pin1 of some important connector, or even just a fiducial and then draw the PCB around it. The goal is to have a common reference for both metric and that other grid. Then I place all THT connectors on a 2.54mm grid. I do this for matrix board compatibily and it makes it easier to make modifications if needed. Outline of the PCB and mounting holes are preferably placed on a whole mm grid, and I also lend towards even values. Unless of course it has to fit in some pre-existing cabinet with mandated hole pattern.
Then make sure this is selected:
Pcbnew / Preferences / Preferences / PCB Editor / Editing Options / Magnetic pads / Snap to Pads: When creating tracks This lets you easily start and end a track on a pad that is not on a grid point.
That was easy, now comes the most difficult part.
And the answer is …
It is just not relevant in most components which have an imperial grid. On top of that, your tracks do not stay where you put them, because the interactive router pushes them around a bit every time you are routing another track. The important part is that you set up your design rules properly, so clearances are adequate.
Do you have any rational reason why such tracks should be right in the middle between pads?
There are a lot of metric components these days on a 0.5mm or even 0.4mm or smaller grid. If you want to route tracks between that, tough luck.
Some time ago I routed a TQFP-48 with a 0.5mm pitch between the pins, and it was rotated 45 degree for easier breakout on the pins on a 2 layer PCB. That was a bit annoying, because KiCad wants to break-out tracks horizontally and vertically and with a 0.5mm pitch I’m not sure if there will be any soldermask left between the pads, and even parts of the tracks near the pads may become exposed copper when the PCB is made in some random chinese cheap fab, and therefore any extra clearance reduces the risk of solder bridges and therefore improves solderability.
With such coarse components with a 1.27mm pitch there is plenty of room for solder mask between the pads, and when your tracks are covered by solder mask it really does not matter at all whether your track is exactly in the middle between two pads or not.
As I wrote before, I tend to put mounting holes and PCB outline on a whole mm grid, and those non-metric components on a 2.54mm grid, but all else is moot. If you insist on wanting the tracks smack in the middle between the pads, then one way to do so is to use a non-metric grid that fits the routing around that connector and use a metric grid for other parts of the PCB. KiCad even has shortcut keys defined to switch between pre-defined grids quickly. Another way is to first measure the distance between two of the connector pads, and then set up the design rules so that the current track width plus two clearances is just slightly smaller then the room available. (“Slightly smaller” to leave some room for rounding errors, even a few micrometers is enough. KiCad works internally with 32bit integers on a nanometer grid (So max PCB from around +2meter to -2meter)).