Tool & Work Offsets

A program says X0 Y0 Z0. Two things decide where that actually is: where the part is clamped and how far the tool sticks out. Both live on the OFFSET screen, one on each tab.

Get either wrong and the program is still correct; the machine cuts in the wrong place.

The two tabs

Tab	Holds	Set it
WORK	where the part datum is, per work coordinate system	every time you clamp a new part
TOOL	how long each tool is and how wide it cuts	when a tool is fitted or reground

Setting part zero

Pick the WCS row, G54 through G59, and the axis column. The star marks the one the program is currently using. Then one of four ways:

Key	Does	Use it when
INPUT	writes what you typed into the cell	you already know the offset
+INPUT	adds what you typed to what is there	you are nudging a datum that is nearly right
SET	makes the current position read what you typed (blank means zero)	you have touched off on the surface
HALF	halves the Work reading, putting zero midway	you have touched both sides and want the centre

Touching off with an edge finder or a slip is SET: bring the tool onto the surface, type the thickness you went through, or nothing at all for zero, and press SET. For a plain zero where the tool stands, ZERO X ZERO Y ZERO Z on the MANUAL screen do the same without leaving the jog keys.

+INPUT is the one to reach for after a trial cut: type 0.05, press +INPUT, and the datum moves by five hundredths without you working out what the new absolute value should be.

SET is the one you will use most. Touch the tool on the top of the part, type nothing, press SET: Z now reads zero there. Touch a side and type the tool radius instead, and X reads zero at the part edge.

The tool table

Tool 2 above shows both columns in use: measured at 100.0000, corrected by 0.0050, so the control cuts with 100.0050. The star says it is the tool in the spindle.

Each tool row carries four numbers:

Column	Means	Unit
L.Geom	tool length as measured	mm
L.Wear	correction on top of it, without touching the measurement	mm
R.Geom	tool radius as measured	mm
R.Wear	correction on top of it	mm

Geometry and wear are separate on purpose, and the reason is not really wear.

Geometry is what was measured, by the tool setter, a presetter, or by hand. Wear is what you decided after looking at the part. The measured length is not the length that makes the part come out right: spindle growth over a shift, tool deflection, setter calibration and the material springing back all sit in the gap between them. That gap is what wear holds.

Which is why re-measuring a tool does not wipe your correction. The measuring cycle refreshes the geometry and leaves the wear alone. Otherwise every automatic measurement would quietly undo the judgement that made the last part correct.

What the control uses is always geometry + wear.

A star on the row number is the tool in the spindle. 02* means tool 2 is loaded, the same marking the WORK tab uses for the active offset.

Tool length compensation: G43, G44, H

H selects the tool row, and it is the tool number: H3 uses the row for tool 3.

Code	Effect
G43 H_	apply the length, positive
G44 H_	apply the length, negative
G49 or H0	cancel

The H must match the tool that is actually in the spindle. Nothing checks it: calling H3 with tool 5 loaded runs the whole program at the wrong length, and the first plunge is as deep as the difference between the two tools. The star on the tool table row tells you what is loaded.

Compensation is modal, and it is cancelled by a reset along with the rest of the modal state.

D selects the radius the same way, for cutter compensation.

A macro reads and writes tool length at #5081 onwards, and writes work offsets with G10. See Custom Macros.

What this does not do

• An edit does not reach the cut you are watching. The control reads offsets as it prepares each block, and it has already prepared a run of blocks ahead of the tool. A change lands somewhere further on, not on the pass in front of you. To correct a size, let the pass finish, edit, and run it again.
• Wear is not a substitute for measuring. If a part is out by a millimetre, the tool length is wrong, not worn.

Where to go next

• Probing: letting the machine measure the datum instead of touching off by hand.
• Custom Macros: the rest of the offset and tool variables.