This documentation is no longer maintained. For documentation of the current version of emc2, please see

Table of Contents

List of figures

List of tables

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.

1.2 Tool Files

Lathe Tool Files differ from mill tool files by the addition of FRONTANGLE, BACKANGLE and ORIENT. The following table show the lathe format for a tool table. Use the "DIA" column for the tool tip diameter.

1 1 0.000 0.000 0.10 105.0 165.0 1 60 deg
2 2 0.000 0.000 0.05 22.5 67.5 2 45 deg
3 3 0.000 0.000 0.10 277.5 352.5 3 75 deg
4 4 0.000 0.000 0.10 255.0 195.0 4 60 deg
5 5 0.000 0.000 0.10 202.5 157.5 5 45 deg
6 6 0.000 0.000 0.10 90 45 6 45 deg
7 7 0.000 0.000 0.10 -22.5 22.5 7 45 deg
8 8 0.000 0.000 0.10 247.5 292.5 8 45 deg
9 9 0.000 0.000 0.10 0 0 9
Table: Lathe Tool File

The Tool Table can be set using G10 L1 with the exception of FRONTANGLE ,BACKANGLE and COMMENT which must be set manually at this time.

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: Tool Position 2

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:

  1. Home each axis.
  2. Set the current tool with "TnM6" where "n" is the tool number.
  3. Select the X axis in the Manual Control window.
  4. Move the X to a known position or take a test cut and measure the diameter.
  5. Select Touch Off and pick Tool Table then enter the position or the diameter.
  6. 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.