[HomeCNC]

Here is the way I use tool offsets with Mach 2 on my jobs. (I also use fixture offsets in combination with it)

In order to fully use tool offsets you need to use fixed collets to hold your tools. The mills are clamped into the holder by some means like a set screw. This keeps the tool at the same place when the collet seats in the spindle.

First you need to record the length of all your tools. My example will be with my CNC router and my Porter Cable router with my fixed tooling. I move the Z axis (with no tool) down until I just touch the spindle on the table. If you can't go that far down with no tool then use some spacer blocks under the spindle to raise the surface up. when you just touch this surface you need to zero the axis manualy. Raise the Z axis and place your first tool in the spindle. Move back down until you just touch and read the axis readout for Z. This is the length of that tool. Enter this length in the tool offset database in Mach 2. Do this with all your tools.

To begin the job I home the machine so my X=0, Y=0, & Z=0 at the far end of my table. I move the tool to the corner of my part and note the X, & Y readout. I enter this data in the fixture offset #1 for X and Y. Now I remove any tools and lower the Z axis to touch the spindle on the material top. I record this number in the fixture offset for Z distance.

In order to use the fixture offset and tool offset in Gcode I need to make sure that I have the proper code for them in the file. A G54 will use fixture offset #1 and a G43 T# will use the offset for that tool #.

You should see the DRO change when you activate the offsets. If you instruct the tool to move to 0,0,0 you should be at the corner of your material and just touching the top of the material with the tool in the spindle.