G00-G99
These codes are not completely standardized
- G00 - Rapid traverse positioning.
- G01 - Linear tool motion at a specified feed rate.
- G02 - Circular tool motion in a clockwise direction.
- G03 - Circular tool motion in a counterclockwise direction.
- G04 - A temporary dwell, or delay in tool motion.
- G05 - A permanent hold, or stopping of tool motion. It is canceled
by the machine operator.
- G08 - Smooth acceleration up to the specified feed rate while other
machine functions are occuring (before the tool contacts the workpiece).
- G09 - An exact stop of one tool motion before the machine goes on to
the next. (Nonmodal.)
- G17 - Selection of the X-Y plane (on machining centers).
- G18 - Selection of the X-Z plane (on machining centers).
- G19 - Selection of the Y-Z plane (on machining centers).
- G20 - Inch data input (on foreign-made machines).
- G21 - Metric data input (on foreign-made machines).
- G22 - Activation of the stored axis travel limits, which are used to
establish a safety boundary.
- G23 - Deactivation of the stored axis travel limits.
- G27 - Return to the machine home position via a programmed intermediate
point (a point somewhere between the current location of the tool and the
machine home position). The machine's control will automatically calculate
the distance to home position once the tool has reached this intermediate
location.
- G28 - Return to the machine home position via a programmed intermediate
point (a point somewhere between the current location of the tool and the
machine home position). The machine's control will automatically cualculate
the distance to home position once the tool has reached this intermediate
location.
- G29 - Return to the workpiece or fixture from the machine home positon
via the intermediate point that was programmmed in the block containing
G28. Any new or old point on the workpiece of fixture can be programmed,
but the tool will first travel to the intermediate point before going there.
- G32, G33 - Thread cutting with a constant lead. If multiple-pass single-point
threading is done, this command will synchronize the start of each pass
at exactly the same point every time so as to avoid the chance of double-threading
the workpiece.
- G34 - Thread cutting with an increasing lead.
- G35 - Thread cutting with a decreasing lead.
- G40 - Cancellation of any previously programmed tool radius compensation
(better known as cutter radius compensation, or CRC).
- G41 - Application of cutter radius compensation to the left of the
workpiece with respect to the direction of tool travel. This feature allows
the finished surface of the workpiece to be the programmed cutter path,
and the tool will automatically be offset to the left of this path by a
distance equal to its radius. On a machining center, G41 is used in climb
milling.
- G42 - Application of cutter radius compensation to the right of the
workpiece with respect to the direction of tool travel. On a machining
center, G42 is used in conventional milling.
- G43 - Activation of tool length compensation in the same direction
of the offset value (as it is stored in the control's memory). If the dimension
stored in the offset register has a negative value, the tool length compensation
will be applied in the negative axis direction. If the dimension stored
in the offset register has a positive value, the tool length compensation
will be applied in the positive axis direction.
- G44 - Activation of tool length compensation in the opposite direction
of the offset value (as it is stored in the control's memory). If the dimension
stored in the offset register has a negative value the tool length compensation
will be applied in the positive axis direction. If the dimension stored
in the offset register has a positive value the tool length compensation
will be applied in the negative axis direction.
- G50 - Establishment of the zero point (absolute zero) in reference
to the current tool positon. This command is commonly used on foreigh-made
CNC lathes in place of G92.
- G53 - Indication that all positioning data is that block is in reference
to the machine home positon. It caused the control to temporarily ignore
the floating zero position. (Used in absolute programming.)
- G54, G55, G56, G57 - Indication that all positioning data is in reference
to the floating zero position on a particular fixture in a machining operation.
For example, G54 would cause all dimensions to refer to the floating zero
on the first fixture, G55 would cause all dimensions to refer to the floating
zero on the second fixture, and so on. (Used in absolute programming)
- G59 - Repositioning of the floating zero. The new location is programmed
incrementally from the current zero positon.
- G60 - An exact stop of one tool motion before the machine goes on to
the next. (Modal)
- G63 - Cancellation of feed-rate override. Used on tapping and threading
operations (in inch-per-minute programmming) where the programmed feed
rate must be maintained in relation to the spindle speed.
- G64 - Cancellation of G60. Allows a slight overlap of the different
tool motions so that a smooth blending of contoured surfaces will result.
When G60 is used, a dwell mark will be left by the tool at the intersection
of motions.
- G70 - Inch data input (on American-made machines).
- G70 - Canned cycle for finish turning on a lathe (foreign-made).
- G71 - Metric data input (on American-made machines).
- G71 - Canned cycle for multiple-pass turning on a lathe (foreign-made).
- G72 - Canned cycle for multiple-pass facing on a lathe (foreign-made).
- G73 - Canned cycle for multiple-pass pattern repeat on a lathe (foreign-made).
- G74 - Canned cycle for pecking in the Z axis on a lathe (foreign-made).
- G75 - Canned cycle for pecking in the X axis on a lathe (foreign-made).
- G76 - Canned cycle for multiple-pass single-point threading on a lathe
(foreign-made).
- G80 - Cancellation of canned cycles on a machining center.
- G81 - Canned cycle for basic drilling on a machining center. Causes
automatic feed in, and rapid out.
- G82 - Canned cycle for drilling with a dwell on a machining center.
Causes automatic feed in, dwell at the bottom, and rapid out.
- G83 - Canned cycle for peck drilling on a machining center. Causes
feed in in multiple pecks and rapid out.
- G84 - Canned cycle for basic tapping on a machining center. Causes
automatic feed in, reversal of spindle rotation, and feed out.
- G85 - Canned cycle for basic boring on a machining center. Causes automatic
feed in and feed out.
- G86 - Canned cycle for alternate boring on a machining center. Causes
automatic feed in, stopping of spindle rotation, and rapid out.
- G87 - Canned cycle for alternate boring on a machining center. Causes
automatic feed in and stopping of spindle rotation. The machine operator
then manually retracts the tool from the hole.
- G88 - Canned cycle for alternate boring on a machining center. Causes
automatic feed in, dwell at the bottom, and stopping of spindle rotation.
The machine operator then manually retracts the tool from the hole.
- G89 - Canned cycle for alternate boring on a machining center. Causes
automatic feed in, dwell at the bottom, and feed out.
- G90 - Absolute positioning. All positioning data will be in reference
to the current zero point (also called the absolute zero). (Modal)
- G90 - Canned cycle for single-pass turing on a lathe (foreign-made).
- G91 - Incremental positioning. All positioning date will be in reference
to the current tool location. (Modal)
- G92 - Establishes the zero point (absolute zero) in reference to the
current tool position.
- G92 - Canned cycle for single-pass threading on lathe (foreign-made).
- G94 - Inch-per-minute programming. The programmed feed rate will be
in inches per minute. G
- 95 - Inch-per-revolution programming. The programmed feed rate will
be in inches per revolution of the spindle.
- G96 - Constant-surface-speed programming. As the diameter turned on
a lathe becomes smaller, the spindle speed will increase to maintain the
programmed surface speed. Inversely, as the diameter turned on a lathe
becomes larger, the spindle speed will decrease.
- G97 - Revolutions-per-minute programming. The spindle speed will be
maintained at the same RPM , no matter what diameter is being turned on
the lathe.
- G98 - Inch-per-minute programming. The programmed feed rate will be
in inches per minute (on foreign-made machines).
- G99 - Indication that all positioning data in that block is in reference
to the machine home position. It causes the control to temporarily ignore
the floating zero position (G92). This command is similar to G53. (Used
on some American-made machines.)
- G99 - Inch-per-revolution programming. The programmed feed rate will
be in inches per revolution of the spindle (on foreign-made machines).