List of figures

Lathe Tool Orientations
Tool Positions 1, 2, 3 & 4

List of tables

Lathe Format Tool Table

1 Lathe Specifics

This chapter attempts to bring together all the lathe specific information and is currently under construction.

1.1 Lathe Mode

When you set up a lathe using Lathe Mode you need to use a Lathe Tool Table so AXIS will display your tool properly. See the INI File section of the Integrators Manual for info on setting up AXIS for Lathe Mode. Use the "DIA" column for the tool tip diameter.

1.2 Tool Table

The "Tool Table" is a text file that contains information about each tool. The file is located in the same directory as your configuration and is called "tool.tbl". The tools might be in a tool changer or just changed manually. The file can be edited with a text editor or be updated using G10 L1.

T1	P1	D0.125000	Z+0.511000	Q7	I-30	J30	;Facing Tool
T2	P2	D0.062500	Z+0.100000	Q1	I165	J105	;Back Cutting Tool
T99999	P99999	...	...	...	...	...	;You have a big tool changer

Table: Lathe Format Tool Table

In general new tool table line format is:

T - integer tool number
P - integer pocket number
D - abs float tool diameter
X..W - float tool length offset on specified axis
I - float front angle (lathe tools)
J - float back angle (lathe tools)
Q - int tool orientation (lathe)
; - begin of comment

There is tool for converting to new tool tables in src/emc/usr_intf/toolconvert.tcl

Usage: ./toolconvert filename (original file is saved as filename.orig) tooledit.tcl support net table format if needed.

The following figure shows the lathe tool orientations with the center line angle of each orientation and info on FRONTANGLE and BACKANGLE.

Figure: Lathe Tool Orientations

In AXIS the following figures show what Tool Positions look like from the above tool table.

Figure: Tool Positions 1, 2, 3 & 4

Figure:

1.3 Tool Touch Off

When running in lathe mode in AXIS you can set the X and Z in the tool table using the Touch Off window.

A typical session might be:

Home each axis.
Set the current tool with "TnM6" where "n" is the tool number.
Select the X axis in the Manual Control window.
Move the X to a known position or take a test cut and measure the diameter.
Select Touch Off and pick Tool Table then enter the position or the diameter.
Repeat for Z.

Note: if your in Radius Mode you will enter the radius not the diameter.

1.4 Threading

Threading with a lathe requires feedback from the spindle to EMC. Typically an encoder is used to provide the feedback. See the Integrators Manual for more information on spindle feedback.

The G76 threading cycle is used for both internal and external threads for more information see G76[->] in the G Code section.

1.5 Constant Surface Speed

CSS or Constant Surface Speed (G96) uses the machine X origin modified by the tool X offset to compute the spindle speed in RPM. CSS will track changes in tool offsets. The X machine origin should be when the reference tool ( the one with zero offset) is at the center of rotation.

Table of Contents