[HomeCNC]

Let me help you with #4.

In order to fully use the fixture offsets you should have the home switches installed.
Mach 2 is following the G-code standard to the tee. a lot of other controllers don't.

Let me first talk about how the fixture offsets work in Mach 2. Fixture offsets is a way of assigning multiple coordinate systems anywhere that your tool can reach (the 3D space of your machine). Mach 2 can hold 6 or more (can't remember how many) of these 0,0,0 coordinate positions. For each position there is a corresponding G-code to access it. The first one is the machines 0,0,0 position most of the time called the HOME position. In G-code it's G53. All of the other 0,0,0 positions you set will be referenced from this machine home position.

You can play with this feature even if you don't have your home/limit switches installed. Move the machine to the far edges of movement and set the dro's to zero. I think this is the same thing as referencing the axis. Now move the machine with the jog keys to a new position. Take note of the DRO's new readout, these new number will need to be entered in the fixture 1 offset's table. Move to another spot and enter the numbers into the #2 fixture offset table. Make sure you push the save button after entering the data.

Now go to the MDI interface. The G-code to access the first offset is G54. The second offset is G55. If you enter G54 into the MDI you should see the DRO change it's values to reflect the new 0,0,0 location. Enter G1 X0 Y0 Z0 F10. The machine should go to your first offset. Next try the second offset G55.

To use the tool length offset you just need to have your tool lengths measured and entered into the tool table. Mach 2 uses the G-code "G43 H#" The # is the tool number. You can also play with this command in the MDI. Type G43 H1. If you have a length entered into the tool table for tool #1 you should see the Z DRO change to reflect this.

To do a proper tool change your code should have the following:

T1 M6 The M6 is the command to make the tool change. (Configure > Logic)
G43 H1 Set the tool length offset. Issue this before any Z movement.