SET COORDINATE SYSTEM (G10 L20)

SET COORDINATE SYSTEM (G10 L20)

G10 L20 is similar to G10 L2, except that instead of setting the offset/entry to the given value, it is set to a calculated value that makes the current coordinates become the given value.

Program: G10 L20 P~ X~ Y~ Z~ A~

  • P~ is the number of coordinate system to use (G54 = 1, G59.3 = 9)
  • X~ is the X-axis coordinate
  • Y~ is the Y-axis coordinate
  • Z~ is the Z-axis coordinate
  • A~ is the A-axis coordinate

TROUBLESHOOTING

It’s an error if:

  • The P number does not evaluate to an integer in the range 0 to 9
  • An axis other than X or Z is programmed

SET COORDINATE SYSTEM (G10 L11)

SET COORDINATE SYSTEM (G10 L11)

G10 L11 is just like G10 L10, except that instead of setting the entry according to the current offsets, it’s set so that the current coordinates would become the given value if the new tool offset is reloaded and the mill is placed in the G59.3 coordinate system without any G92 offset active. This allows you to set the G59.3 coordinate system according to a fixed point on the mill, and then use that fixture to measure tools without regard to other currently active offsets.

Program: G10 L11 P~ X~ Z~ R~ I~ J~ Q~

  • P~ is the tool number
  • R~ is the radius of tool

TROUBLESHOOTING

It’s an error if:

  • Cutter Compensation is on
  • The P number is unspecified
  • The P number is not a valid tool number from the tool table
  • The P number is 0

SET TOOL TABLE (G10 L10)

SET TOOL TABLE (G10 L10)

To change the tool table entry for tool P so that if the tool offset is reloaded with the mill in its current position and with the current G5x and G92 offsets active, program: G10 L10 P- Z~ R~ I~ J~ Q~

  • P~ is the tool number
  • R~ is the radius of tool

The current coordinates for the given axes become the given values. The axes that are not specified in the G10 L10 command are not changed. This could be useful with a probe move (G38).

TROUBLESHOOTING

It’s an error if:

  • Cutter Compensation is on
  • The P number is unspecified
  • The P number is not a valid tool number from the tool table
  • The P number is 0

SET TOOL TABLE (G10 L2)

SET TOOL TABLE (G10 L2)

To define the origin of a work offset coordinate system, program: G10 L2 P~

  • P~ is the number of coordinate system to use (G54 = 1, G59.3 = 9)

The G10 L2 P~ command doesn’t change from the current coordinate system to the one specified by P. Use G54 through G59.3 to select a coordinate system. The coordinate system whose origin is set by a G10 command may be active or inactive at the time the G10 is executed. If it’s currently active, the new coordinates take effect immediately.

EXAMPLE – If a G92 origin offset was in effect before G10 L2, it continues to be in effect after.

TROUBLESHOOTING

It’s an error if:

  • The P number does not evaluate to an integer in the range 0 to 9
  • An axis other than X or Z is programmed

SET COORDINATE SYSTEM (G10 L1)

SET COORDINATE SYSTEM (G10 L1)

To define an entry in the tool table, program: G10 L1 P~ X~ Y~ R~ I~ J~ Q~

  • P~ is the tool number
  • R~ is the radius of tool

G10 L1 sets the tool table for the P tool number to the values of the words. A valid G10 L1 rewrites and reloads the tool table.

EXAMPLE – G10 L1 P2 R0.015 Q3 (setting tool 2 radius to 0.015 and orientation to 3).

TROUBLESHOOTING

It’s an error if:

  • Cutter Compensation is on
  • The P number is unspecified
  • The P number is not a valid tool number from the tool table
  • The P number is 0