Let's take a quick look at what is happening under the covers or if you didn't have a button on the screen to measure a tool length and place it into a tool table.
G-Code for CNC expects to have a co-ordinate system defined. When we refer to machine co-ordinates we're really referring to the G53 co-ordinate system.
Normally by default we use the G54 co-ordinate system which has a series of X,Y,Z values that move that 0,0,0 from the top left corner to somewhere inside the work envelope. That's why if you have 3 fixtures set up with work clamped in each you can set the 0,0,0 for each fixture in say G54, G55, and G56. Now run the same G-Code to machine stuff.
But let's rewind here for a moment. We're still trying to find out how long a tool is and what happens under the covers. To make sure one of these other co-ordinate systems isn't changing our 0,0,0 position we need to execute a:
G49
which cancels any tool length offset from the last tool change. Our reference point is now the bottom of the quill again.
Time to move the table or (or the Quill) to the tool setter location. As there may be offsets in play we'll expressly tell the system to use machine co-ordinates rather than just a simple new position command by preceding each line with the non-sticky G53
; Ensure we're in G90 / absolute mode
G90
; First go up & then move to change position to clear tool setter for long tools just off from home switch.
G53 G0 Z-0.2
G53 X0.500 Y1.000
; and to make sure also cancel the existing tool offset
G49
; And change tool command
M6
Now we've put a new TTS tool into the holder, tightened down the draw bar and we need to measure this tool so let's move over to a point above the tool setter.
G53 X1.00 Y1.000
G53 Z-1.00
Next installment. The actual probing of the tool setter.
