Lathe tool table

I'm assuming you don't have an automatic tool changer?

G43 is for tool length compensation and G41/42 is for tool diameter compensation. In the case of a lathe your tool diameter would be equal to the tip diameter of your insert.

www.linuxcnc.org/docview/html//lathe_lathe-user.html

John

Basically, yes. Though EMC2 needs to know which tool is loaded.
M6 T1 G43 is something I type automatically now (you can skip the H if you want the offset of the current tool, rather than a different tool)

The way I work (and there are other ways) is to have a zero-length in the table for tool 1. I then touch-off with tool 1 into the G54 coordinate system (I have not yet ever used a different one) and touch off other tools selecting "Tool Table" in the dialog box. That way the tool table is a table of X and Z lengths _relative_ to tool 1.

(Being clever, tool 1 could even be a touch-probe)

In practice the way I work (as I mainly work semi-manually) is to machine my first part oversize then measure the diameter to touch-off the X.

I do something similar to Andy but different not because my way is better but because it works for me and I can remember how to do it from day to day... sometimes. So pick a way that works best for you...

First I change to G55 so I know there is no offsets in effect and then for each new tool in my turret I touch off the tool table Z offset off of my spindle face (any fixed point will do) by moving away from the face of the spindle until a dowel (always the same size) can just roll between the tool and the spindle face. That has set the Z offset for every tool on the turret to the same place.

For X I take a test cut and measure that and enter that in the tool table offset being careful to be in diameter mode if I enter a diameter measurement. For more tools I'll paint the test cut with a permanent marker then move then next tool up to the test part with the spindle turning (slow) until I touch the ink then touch off the X tool table offset to the magic number I measured during the test cut. This sets the X offset for each tool. I usually use aluminum for setting up as it is a bit more forgiving.

Now I change back to G54 which is where I do all my work on my lathe.

Now all the tools have an offset relative to each other so to speak. So if I load a tool with T3 M6 G43 every tool will go to the same X Z position when I enter a move command.

Now the only thing left is a work offset for the material in the spindle. I take any tool (within reason) and making sure I have the Z axis selected in the Manual Control tab i touch off the Z face of the material in the G54 Coordinate System and enter a value that makes sense for the job. For example I might put in 0.020 if I want to take a 20 thou face cut and then have Z0 be nice and clean. Now all the tools will be set to the material in X and Z if you did it correctly.

Tools like parting tools and threading tools and right hand inserts take some special measure to get the Z tool table offset but that is another story...

The things that will foul you up the most are being in G54 with an offset in effect, not selecting the correct axis for the touch off, being in radius mode and entering in a diameter. I'm sure I've discovered more ways to foul it up but can't remember them atm.

John

For some reason unknown to me I do...

T3 M6
G43

and yes I do a T3 M6 in the MDI window to make the turret change tools then when that is done I do a G43 then proceed to touch off as needed.

Also make sure you set the insert tip diameter for turning type of tools in your tool table.

John