setting the origin

[JAZZCNC]

but I have found if I’m using a 6mm roughing bit and set it to the outside it tends run down the first line with the centre of the bit on the edge of the material rather than 3mm in per say, but it still completes the piece with the last outside pass at opposite edge at the centre of the bit, just wondering if that is normal?

This is more to do with cutter compensation than the Origin point.? Cutter comp will place the cutter half the cutter dia either to the left or right of the toolpath and often your CAM will deal with this, often it will be called offset.
If your writing code by hand then you'll need to Tell the machine using the G41/42 G-codes which side to apply comp which it then does according to the specified tool IE T1 and the data held for it in the tool table of the control.

The origin is often thought of has just the 0,0,0 or start point of the part being cut. But this really is only the Origin of the WORK coordinate which is located at some point in relation to the Machine coordinate Origin.
Where to place this Work Origin on the bed is totally up to you. The 0,0,0 WORK coordinate is the start point and will never change in relation to the part unless you change it's location in CAD or by writing new G-code.
Where you place it on the bed is entirely upto you and so long has theres enough room for the complete part it doesn't matter because you set the 0,0,0 in WORK coordinates by zeroing the DRO's. The WORK coordinate then has an offset from the MACHINE coordinate Origin which you can not change unless you move the HOME switches. This is how you can get back into position if something goes tits up because the control knows the WORK coordinate 0,0,0 offset point in relation to MACHINE coordinate FIXED Origin.

Micheal mentioned G55/6/7 etc work offsets.? These are just programmable WORK offsets that are a set amount from the MACHINE coordinate origin. These OFFSETS are set in the control. So say your table is 4ft sqr you can effectively divide the table into segments each with it's own 0,0,0 work coordinate.
So say we break it into 4 segments then X0Y0 in MACHINE coords will be first offset, often the Default G54.
X24Y0 will be next offset G55.
X0Y24 will be 3rd offset called G56,
X24Y24 will be 4th G57.
Now Lets say we want to cut a different part in each segment then we would just select G54 for 1st part and the 0,0,0 WORK coordinate starts there at 0,0,0 in MACHINE coords.
Then we select G55 for our next part and the WORK 0,0,0 point shifts to X24Y0 in MACHINE coords and so on for each WORK OFFSET.
So to cut 4 individual parts at the same time each with there own 0,0,0 point we just combine the code in one file with a G54,55,56,57 before the code relating to each part and the control automaticly offsets to that point and uses it has WORK coordinate origin.

Hope this helps and doesn't confuse.??