Lathe Tool Table

If you are going to use more than one tool in a part with a CNC lathe, you'll need an accurate tool table.

The tool table tells the controller software where the cutting edge is in space. This is necessary as the G Code tells the controller to move, for example from Z0 to Z10 but doesn't contain any information about where the cutting edge is relative to the lathe. For instance, if you are using a left cutting tool and a right cutting tool, the Z position of the cutting edge will be different (Z offset). Or tools might protrude different distances from the tool post (X offset).

Decide on a system for numbering your tools. Label your tools with these numbers (whiteout correction fluid works well for this).

In LinuxCNC the tool table can be edited manually - either by text file, or more easily via the tool table editor, found in the file menu. You'll need to do some manual entry to set up tool angles for tool display in the preview.

The easy way to set X and Z offsets is using touchoff.

1. Home your lathe
2. Pick a tool you want to act as your reference tool. You may want this to be the tool that sticks out the most from the toolpost in case you make a mistake with a tool change at some point.
3. In MDI enter T1 M6 (change tool to 1)
4. Move Z to a known location (that you will be able to reference other tools off)
5. In the manual tab click 'Touch Off', leave the input as 0, Set the drop down to G54 and click ok.
6. Again click 'Touch Off', leave the input as 0, click on the drop down and change it to 'Tool Table'
7. Setting X is easiest done by taking a cut then measuring the diameter (without moving the X axis after the cut)
8. Click 'Touch Off' and enter the diameter in the input field (if you are in radius mode you'll need to enter half the measured diameter). Set the drop down to G54 and click ok.
9. Again click 'Touch Off' and enter the diameter in the input field (if you are in radius mode you'll need to enter half the measured diameter). Set the drop down to 'Tool Table' and click ok.
10. The above steps set up your first (reference tool) as 0,0
11. Select your next tool, mount it on the toolpost and enter T2 M6 in MDI
12. Move the tool so the cutting edge is at the same Z point in space and 'Touch off' Z with tool table selected in the drop down.
13. Make a profile cut, move the tool out of the way in Z (without moving X axis) and then measure the diameter
14. Touch off X and enter this diameter with tool table selected.
15. You should now see an X and Z value in the tool table for tool 2 (you may need to reload tool table).
16. Repeat for further tools.

When changing tools you need to call G43 to load the offsets from the tool table. Thus the command to change tools is 'Tn M6 G43'

When changing back and forth from different tools you should see the tool preview move appropriately. For example, if tool 2 is 10mm shorter than tool 1, in the preview you should see the tool move 10mm out from the part display.

Warning: If you've used 'Touch Off' and selected 'Tool Table' in the drop down, the next time you 'Touch off' the drop down will default to 'Tool Table', this can lead to accidently changing your tool table instead of changing the world coordinate system (e.g. G54)

See the following for more info:

LinuxCNC Tool Compensation

John Thorton's Guide