Where is home on a milling machine?

[JAZZCNC]

Ok Standing in front of the mill then X- is Left X+ right Y+ is moving away from you Y- towards Z + is upwards Z-. So the Dir & Step you would set relative so the motors turn in this direction.

Now I think your confusion comes from not under standing the difference Between Machine coordinates and Work Coordinates and how the Home switches relate to these coordinates. Also the Spindle position in relation ship to table.?

Forget Limit Switches now has they just define the machines limits of travel.

Home switches Define the ZERO point in MACHINE coordinates ONLY. This MACHINE ZERO point is Fixed and can only be Changed if you move the Switches.
Now where MACHINE ZERO's(HOME) located is some what user dependent but Personally I would set it so all moves are in the Positive with the exception of the Z axis which is always Negative. So X0 would move the tool to the Extreme Left and Y0 Closest to you, Z0 would be at the top.
Looking from a Top down view this would put the tool in the upper Left corner.
This then Emulates your CAD system to Some degree but forget that for the minute has it Can be confusing with the difference between MACHINE & WORK coordinates.

Now where I think your getting confused is with the Relation ship between MACHINE and WORK coordinates.
WORK coordinates or WORK OFFSET X0 Y0 is anywhere you care to define on the machines table or material, Z0 is often the Top of material. This WORK coordinate is an OFFSET from the MACHINE ZERO and because the MACHINE coordinate is Fixed by the Switches then The Control can always return to the Exact WORK OFFSET by HOMING to the switch then returning to the WORK OFFSET which is stored in memory when you DEFINE the WORK OFFSET X0 Y0 Z0 point on the material.

This is also where it can confuse some folks because While the MACHINE coordinates will always travel in a positive direction IE: Away from L-Corner & Forward, The WORK coordinates can travel in the MINUS direction.???
To help explain think of it like this your cutting 100mm square and In CAD/CAM you defined the X0 Y0 has the Centre of the Square, so you Jog your machine to roughly centre of the Material and Set the WORK Zero Position(Work offset). The material is 110 mm square and the corner is set 50mm from table edges or Machine X & Y ZERO.
Now to cut this Square half the moves will be in the Negative direction BUT if you where to look at the MACHINE coordinates then they will be a POSITIVE number. So position X-50 Y-50 in the WORK coordinate will be X55 Y55 in MACHINE Coordinates the Actual WORK ZERO will be X105 Y105 in MACHINE coordinates.

Now Here's where it can get confudddling for some folks when G-codes like G54 are used which is a WORK OFFSET reference. You can have Multiple WORK OFFSET's each with there Own Zero Position. So imagine you have 2 vices on your machine each with piece of material in it but 2 different jobs so different tool-paths. You have decided the Corner of each Vice will Be WORK Zero.
Now what you can do is define WORK OFFSET's in the Control system, so you'd jog to the corner of each vice and in the Control set the WORK OFFSET for that Vice in WORK OFFSET table. The table consists of Numbers 54 thru to however many WORK OFFSETs the control allows.? Mach3 allows 255.
So you'd set Vice #1=54 #2=55
Now in the G-code file your first part would start with the G-code command G54 this then Sets The WORK OFFSET ZERO to the corner of Vice #1 and cut the part. Then further down and before the Second parts G-code you'd have G55. This then sets WORK OFFSET ZERO to corner of vice #2.

Now in practice most users only ever use G54 OFFSET which is the default OFFSET in most Controls.

Hope this Lot makes sense.!!