g-code.txt

[[cha:g-codes]]
= G Codes

:ini: {basebackend@docbook:'':ini}
:hal: {basebackend@docbook:'':hal}
:ngc: {basebackend@docbook:'':ngc}

== Conventions

Conventions used in this section

In the G code prototypes the hyphen ('-') stands for a real value
and ('<>') denotes an optional item.

If 'L-' is written in a prototype the '-' will often be referred to
as the 'L number', and so on for any other letter.

In the G code prototypes the word 'axes' stands for any axis as defined
in your configuration.

An optional value will be written like this '<L->'.

A real value may be:

* An explicit number, '4'
* An expression, '[2+2]'
* A parameter value, '#88'
* A unary function value, 'acos[0]'

In most cases, if 'axis' words are given
(any or all of 'X Y Z A B C U V W'),
they specify a destination point.

Axis numbers are in the currently active coordinate system,
unless explicitly described as being
in the absolute coordinate system.

Where axis words are optional, any omitted axes will retain their original value.

Any items in the G code prototypes not explicitly described as
optional are required.

The values following letters are often given as explicit numbers.
Unless stated otherwise, the explicit numbers can be real values. For
example, 'G10 L2' could equally well be written 'G[2*5] L[1+1]'. If the
value of parameter 100 were 2, 'G10 L#100' would also mean the same.

If 'L-' is written in a prototype the '-' will often be referred to
as the 'L number', and so on for any other letter.

== G Code Quick Reference Table[[gcode:quick-reference-table]]

(((G Code Table)))

[width="75%", options="header", cols="2^,5<"]
|====================================================================
|Code                               |Description
|<<gcode:g0,G0>>                    |Coordinated Motion at Rapid Rate
|<<gcode:g1,G1>>                    |Coordinated Motion at Feed Rate
|<<gcode:g2-g3,G2 G3>>              |Coordinated Helical Motion at Feed Rate
|<<gcode:g4,G4>>                    |Dwell
|<<gcode:g5,G5>>                    |Cubic Spline
|<<gcode:g5.1,G5.1>>                |Quadratic B-Spline
|<<gcode:g5.2-g5.3,G5.2,G5.3>>      |NURBS, add control point
|<<gcode:g7,G7>>                    |Diameter Mode (lathe)
|<<gcode:g8,G8>>                    |Radius Mode (lathe)
|<<gcode:g10-l1,G10 L1>>            |Set Tool Table Entry
|<<gcode:g10-l10,G10 L10>>          |Set Tool Table, Calculated, Workpiece
|<<gcode:g10-l11,G10 L11>>          |Set Tool Table, Calculated, Fixture
|<<gcode:g10-l2,G10 L2>>            |Coordinate System Origin Setting
|<<gcode:g10-l20,G10 L20>>          |Coordinate System Origin Setting Calculated
|<<gcode:g17-g19.1,G17 - G19.1>>    |Plane Select
|<<gcode:g20-g21,G20 G21>>          |Set Units of Measure
|<<gcode:g28-g28.1,G28 - G28.1>>    |Go to Predefined Position
|<<gcode:g30-g30.1,G30 - G30.1>>    |Go to Predefined Position
|<<gcode:g33,G33>>                  |Spindle Synchronized Motion
|<<gcode:g33.1,G33.1>>              |Rigid Tapping
|<<gcode:g38,G38.2 - G38.5>>        |Probing
|<<gcode:g40,G40>>                  |Cancel Cutter Compensation
|<<gcode:g41-g42,G41 G42>>          |Cutter Compensation
|<<gcode:g41.1-g42.1,G41.1 G42.1>>  |Dynamic Cutter Compensation
|<<gcode:g43,G43>>                  |Use Tool Length Offset from Tool Table
|<<gcode:g43.1,G43.1>>              |Dynamic Tool Length Offset
|<<gcode:g43.2,G43.2>>              |Apply additional Tool Length Offset
|<<gcode:g49,G49>>                  |Cancel Tool Length Offset
|<<gcode:g53,G53>>                  |Move in Machine Coordinates
|<<gcode:g54-g59.3,G54-G59.3>>      |Select Coordinate System (1 - 9)
|<<gcode:g61-g61.1,G61 G61.1>>      |Path Control Mode
|<<gcode:g64,G64>>                  |Path Control Mode with Optional Tolerance
|<<gcode:g73,G73>>                  |Drilling Cycle with Chip Breaking
|<<gcode:g74,G74>>                  |Left-hand Tapping Cycle with Dwell
|<<gcode:g76,G76>>                  |Multi-pass Threading Cycle (Lathe)
|<<gcode:g80,G80>>                  |Cancel Motion Modes
|<<gcode:g81,G81>>                  |Drilling Cycle
|<<gcode:g82,G82>>                  |Drilling Cycle with Dwell
|<<gcode:g83,G83>>                  |Drilling Cycle with Peck
|<<gcode:g84,G84>>                  |Right-hand Tapping Cycle with Dwell
|<<gcode:g85,G85>>                  |Boring Cycle, No Dwell, Feed Out
|<<gcode:g86,G86>>                  |Boring Cycle, Stop, Rapid Out
|<<gcode:g89,G89>>                  |Boring Cycle, Dwell, Feed Out
|<<gcode:g90-g91,G90 G91>>          |Distance Mode
|<<gcode:g90.1-g91.1,G90.1 G91.1>>  |Arc Distance Mode
|<<gcode:g92,G92>>                  |Coordinate System Offset
|<<gcode:g92.1-g92.2,G92.1 G92.2>>  |Cancel G92 Offsets
|<<gcode:g92.3,G92.3>>              |Restore G92 Offsets
|<<gcode:g93-g94-g95,G93 G94 G95>>  |Feed Modes
|<<gcode:g96-g97,G96>>              |Spindle Control Mode
|<<gcode:g98-g99,G98 G99>>          |Canned Cycle Z Retract Mode 
|====================================================================

[[gcode:g0]]
== G0 Rapid Move
(((G0 Rapid Move)))

-------------------
G0 axes
-------------------

For rapid motion, program 'G0 axes', where all the axis words are optional.
The 'G0' is optional if the current motion mode is 'G0'. This will produce
coordinated motion to the destination point at the maximum rapid rate
(or slower). 'G0' is typically used as a positioning move.

=== Rapid Velocity Rate

The MAX_VELOCITY setting in the ini file [TRAJ] section defines the maximum
rapid traverse rate. The maximum rapid traverse rate can be higher than the
individual axes MAX_VELOCITY setting during a coordinated move. The maximum
rapid traverse rate can be slower than the MAX_VELOCITY setting in the [TRAJ]
section if an axis MAX_VELOCITY or trajectory constraints limit it.


.G0 Example
----
G90 (set absolute distance mode)
G0 X1 Y-2.3 (Rapid linear move from current location to X1 Y-2.3)
M2 (end program)
----
* See <<gcode:g90-g91,G90>> & <<mcode:m2-m30,M2>> sections for more information.

If cutter compensation is active, the motion will differ from
the above; see the <<sec:cutter-compensation,Cutter Compensation>> Section.

If 'G53' is programmed on the same line, the motion will also differ;
see the <<gcode:g53,G53>> Section for more information.

The path of a G0 rapid motion can be rounded at direction changes and depends
on the <<sec:trajectory-control,trajectory control>> settings and maximum
acceleration of the axes.

It is an error if:

* An axis letter is without a real value.
* An axis letter is used that is not configured

[[gcode:g1]](((G1 Linear Move)))

== G1 Linear Move

-------------------
G1 axes
-------------------

For linear (straight line) motion at programed <<sec:set-feed-rate,feed rate>>
(for cutting or not), program 'G1 'axes'', where all the axis words are
optional. The 'G1' is optional if the current motion mode is 'G1'. This will
produce coordinated motion to the destination point at the current feed
rate (or slower).

.G1 Example
----
G90 (set absolute distance mode)
G1 X1.2 Y-3 F10 (linear move at a feed rate of 10 from current position to X1.2 Y-3)
Z-2.3 (linear move at same feed rate from current position to Z-2.3)
Z1 F25 (linear move at a feed rate of 25 from current position to Z1)
M2 (end program)
----
* See <<gcode:g90-g91,G90>> & <<sec:set-feed-rate,F>> & <<mcode:m2-m30,M2>> sections
for more information.

If cutter compensation is active, the motion will differ from
the above; see the <<sec:cutter-compensation,Cutter Compensation>> Section.

If 'G53' is programmed on the same line, the motion will also differ;
see the <<gcode:g53,G53>> Section for more information.

It is an error if:

* No feed rate has been set.
* An axis letter is without a real value.
* An axis letter is used that is not configured

[[gcode:g2-g3]]
== G2, G3 Arc Move
(((G2, G3 Arc Move)))

----
G2 or G3 axes offsets (center format)
G2 or G3 axes R- (radius format)
G2 or G3 offsets|R- <P-> (full circles)
----

A circular or helical arc is specified using either 'G2' (clockwise
arc) or 'G3' (counterclockwise arc) at the current 
<<sec:set-feed-rate,feed rate>>. The direction (CW, CCW) is as viewed from the
positive end of the axis about which the circular motion occurs.

The axis of the circle or helix must be parallel to the
X, Y, or Z axis of the machine coordinate system.
The axis (or, equivalently, the plane perpendicular to the axis)
is selected with 'G17' (Z-axis, XY-plane),
'G18' (Y-axis, XZ-plane), or 'G19' (X-axis, YZ-plane).
Planes '17.1', '18.1', and '19.1' are not currently supported.
If the arc is circular,
it lies in a plane parallel to the selected plane.

To program a helix, include the axis word perpendicular to the arc
plane: for example, if in the 'G17' plane, include a 'Z' word. This
will cause the 'Z' axis to move to the programmed value during the
circular 'XY' motion. 

To program an arc that gives more than one full turn, use the 'P' word
specifying the number of full turns plus the programmed arc. The 'P' word
must be an integer. If 'P' is unspecified, the behavior is as if 'P1' was
given: that is, only one full or partial turn will result. For example, if a
180 degree arc is programmed with a P2, the resulting motion will be 1 1/2
rotations. For each P increment above 1 an extra full circle is added to the
programmed arc. Multi turn helical arcs are supported and give motion useful
for milling holes or threads.

If a line of code makes an arc and includes rotary axis motion,
the rotary axes turn at a constant rate so that the rotary
motion starts and finishes when the XYZ motion starts and finishes.
Lines of this sort are hardly ever programmed.

If cutter compensation is active, the motion will differ from
the above; see the <<sec:cutter-compensation,Cutter Compensation>> Section.

The arc center is absolute or relative as set by <<gcode:g90.1-g91.1,G90.1
or G91.1>> respectively.

Two formats are allowed for specifying an arc:
Center Format and Radius Format.

It is an error if:

* No feed rate has been set.
* The P word is not an integer.

=== Center Format Arcs

Center format arcs are more accurate than radius format arcs and are
the preferred format to use.

The end point of the arc along with the offset to the center of the
arc from the current location are used to program arcs that are less
than a full circle. It is OK if the end point of the arc is the same
as the current location.

The offset to the center of the arc from the current location and
optionally the number of turns are used to program full circles.

When programming arcs an error due to rounding can result from using a
precision of less than 4 decimal places (0.0000) for inch and less than
3 decimal places (0.000) for millimeters.

.Incremental Arc Distance Mode
Arc center offsets are a relative distance from the start location of the arc.
Incremental Arc Distance Mode is default.

One or more axis words and one or more offsets must be programmed for an
arc that is less than 360 degrees.

No axis words and one or more offsets must be programmed for full circles.
The 'P' word defaults to 1 and is optional.

For more information on 'Incremental Arc Distance Mode see the
<<gcode:g90.1-g91.1,G91.1>> section.

.Absolute Arc Distance Mode
Arc center offsets are the absolute distance from the current 0 position of the axis.

One or more axis words and 'both' offsets must be programmed for arcs
less than 360 degrees.

No axis words and both offsets must be programmed for full circles.
The 'P' word defaults to 1 and is optional.

For more information on 'Absolute Arc Distance Mode see the
<<gcode:g90.1-g91.1,G90.1>> section.

.XY-plane (G17)
----
G2 or G3 <X- Y- Z- I- J- P->
----
* 'Z' - helix
* 'I' - X offset
* 'J' - Y offset
* 'P' - number of turns

.XZ-plane (G18)
----
G2 or G3 <X- Z- Y- I- K- P->
----
* 'Y' - helix
* 'I' - X offset
* 'K' - Z offset
* 'P' - number of turns

.YZ-plane (G19)
----
G2 or G3 <Y- Z- X- J- K- P->
----
* 'X' - helix
* 'J' - Y offset
* 'K' - Z offset
* 'P' - number of turns

It is an error if:

* No feed rate is set with the <<sec:set-feed-rate,F>> word.

* No offsets are programmed.

* When the arc is projected on the selected plane, the distance from
  the current point to the center differs from the distance from the end
  point to the center by more than (.05 inch/.5 mm) 
  OR ((.0005 inch/.005mm) AND .1% of radius).

Deciphering the Error message 'Radius to end of arc differs from radius to start:'

* 'start' - the current position
* 'center' - the center position as calculated using the i, j, or k words
* 'end' - the programmed end point
* 'r1' - radius from the start position to the center
* 'r2' - radius from the end position to the center

=== Center Format Examples

Calculating arcs by hand can be difficult at times. One option is to
draw the arc with a cad program to get the coordinates and offsets.
Keep in mind the tolerance mentioned above, you may have to change the
precision of your cad program to get the desired results. Another
option is to calculate the coordinates and offset using formulas. As
you can see in the following figures a triangle can be formed from the
current position the end position and the arc center.

In the following figure you can see the start position is X0 Y0, the
end position is X1 Y1. The arc center position is at X1 Y0. This gives
us an offset from the start position of 1 in the X axis and 0 in the Y
axis. In this case only an I offset is needed.

.G2 Example Line
[source,{ngc}]
----
G0 X0 Y0
G2 X1 Y1 I1 F10 (clockwise arc in the XY plane)
----

.G2 Example

image::images/g2.png[align="center", alt="G2 Example"]

In the next example we see the difference between the offsets for Y if
we are doing a G2 or a G3 move. For the G2 move the start position is
X0 Y0, for the G3 move it is X0 Y1. The arc center is at X1 Y0.5 for
both moves. The G2 move the J offset is 0.5 and the G3 move the J
offset is -0.5.

.G2-G3 Example Line
[source,{ngc}]
----
G0 X0 Y0
G2 X0 Y1 I1 J0.5 F25 (clockwise arc in the XY plane)
G3 X0 Y0 I1 J-0.5 F25 (counterclockwise arc in the XY plane)
----

.G2-G3 Example

image::images/g2-3.png[align="center", alt="G2-G3 Example"]

In the next example we show how the arc can make a helix in the Z axis
by adding the Z word.

.G2 Example Helix
[source,{ngc}]
----
G0 X0 Y0 Z0
G17 G2 X10 Y16 I3 J4 Z-1 (helix arc with Z added)
----

In the next example we show how to make more than one turn using the P word.

.P word Example
----
G0 X0 Y0 Z0
G2 X0 Y1 Z-1 I1 J0.5 P2 F25
----

In the center format, the radius of the arc is not specified, but it
may be found easily as the distance from the center of the circle to
either the current point or the end point of the arc.

=== Radius Format Arcs

----
G2 or G3 axes R- <P->
----
* 'R' - radius from current position

It is not good practice to program radius format arcs that are nearly
full circles or nearly semicircles because a small change in the
location of the end point will produce a much larger change in the
location of the center of the circle (and, hence, the middle of the
arc). The magnification effect is large enough that rounding error in a
number can produce out-of-tolerance cuts. For instance, a 1%
displacement of the endpoint of a 180 degree arc produced a 7%
displacement of the point 90 degrees along the arc. Nearly full circles
are even worse. Other size arcs (in the range tiny to 165 degrees or
195 to 345 degrees) are OK.

In the radius format, the coordinates of the end point of the arc in
the selected plane are specified along with the radius of the arc.
Program 'G2' 'axes' 'R-' (or use 'G3' instead of 'G2' ). R is the
radius. The axis words are all optional except that at
least one of the two words for the axes in the selected plane must be
used. The R number is the radius. A positive radius indicates that the
arc turns through less than 180 degrees, while a negative radius
indicates a turn of more than 180 degrees. If the arc is helical, the
value of the end point of the arc on the coordinate axis parallel to
the axis of the helix is also specified.

It is an error if:

* both of the axis words for the axes of the selected plane are omitted
* the end point of the arc is the same as the current point.

.G2 Example Line
[source,{ngc}]
----
G17 G2 X10 Y15 R20 Z5 (radius format with arc)
----

The above example makes a clockwise (as viewed from the positive Z-axis)
circular or helical arc whose axis is parallel to the Z-axis, ending
where X=10, Y=15, and Z=5, with a radius of 20. If the starting value
of Z is 5, this is an arc of a circle parallel to the XY-plane;
otherwise it is a helical arc.

[[gcode:g4]]
== G4 Dwell
(((G4 Dwell)))

----
G4 P-
----
* 'P' - seconds to dwell (floating point)

The P number is the time in seconds that all axes will remain unmoving.
The P number is a floating point number so fractions of a second may be used.
G4 does not affect spindle, coolant and any I/O.

.G4 Example Line
----
G4 P0.5 (wait for 0.5 seconds before proceeding)
----

It is an error if:

* the P number is negative or not specified.

[[gcode:g5]]
== G5 Cubic Spline
(((G5 Cubic spline)))

----
G5 X- Y- <I- J-> P- Q-
----
* 'I' - X incremental offset from start point to first control point
* 'J' - Y incremental offset from start point to first control point
* 'P' - X incremental offset from end point to second control point
* 'Q' - Y incremental offset from end point to second control point

G5 creates a cubic B-spline in the XY plane with the X and Y axes only.
P and Q must both be specified for every G5 command.

For the first G5 command in a series of G5 commands, I and J must both
be specified.  For subsequent G5 commands, either both I and J must be
specified, or neither.  If I and J are unspecified, the starting
direction of this cubic will automatically match the ending direction of
the previous cubic (as if I and J are the negation of the previous P and
Q).

For example, to program a curvy N shape:

.G5 Sample initial cubic spline
----
G90 G17
G0 X0 Y0
G5 I0 J3 P0 Q-3 X1 Y1
----

A second curvy N that attaches smoothly to this one can now be made
without specifying I and J:

.G5 Sample subsequent cubic spline
----
G5 P0 Q-3 X2 Y2
----

It is an error if:

* P and Q are not both specified
* Just one of I or J are specified
* I or J are unspecified in the first of a series of G5 commands
* An axis other than X or Y is specified
* The active plane is not G17

[[gcode:g5.1]]
== G5.1 Quadratic Spline
(((G5.1 Quadratic spline)))

----
G5.1 X- Y- I- J-
----
* 'I' - X incremental offset from start point to control point
* 'J' - Y incremental offset from start point to control point

G5.1 creates a quadratic B-spline in the XY plane with the X and Y axis
only.  Not specifying I or J gives zero offset for the unspecified axis,
so one or both must be given.

For example, to program a parabola, through the origin, from X-2 Y4 to X2 Y4:

.G5.1 Sample quadratic spline
----
G90 G17
G0 X-2 Y4
G5.1 X2 I2 J-8
----

It is an error if:

* both I and J offset are unspecified or zero
* An axis other than X or Y is specified
* The active plane is not G17

[[gcode:g5.2-g5.3]]
== G5.2 G5.3 NURBS Block
(((G5.2 G5.3 NURBS Block)))

----
G5.2 <P-> <X- Y-> <L->
X- Y- <P->
...
G5.3
----

Warning: G5.2, G5.3 is experimental and not fully tested.

G5.2 is for opening the data block defining a NURBS and G5.3 for
closing the data block. In the lines between these two codes the curve
control points are defined with both their related 'weights' (P) and
the parameter (L) which determines the order of the curve.

The current coordinate, before the first G5.2 command, is always taken
as the first NURBS control point.  To set the weight for this first
control point, first program G5.2 P- without giving any X Y.

The default weight if P is unspecified is 1.  The default order if L is
unspecified is 3.

.G5.2 Example
[source,{ngc}]
----
G0 X0 Y0 (rapid move)
F10 (set feed rate)
G5.2 P1 L3
     X0 Y1 P1
     X2 Y2 P1
     X2 Y0 P1
     X0 Y0 P2
G5.3
; The rapid moves show the same path without the NURBS Block
G0 X0 Y1
   X2 Y2
   X2 Y0
   X0 Y0
M2
----

.Sample NURBS Output

image:images/nurbs01.png[align="center", alt="Sample NURBS Output"]

More information on NURBS can be found here:

http://wiki.linuxcnc.org/cgi-bin/wiki.pl?NURBS[http://wiki.linuxcnc.org/cgi-bin/wiki.pl?NURBS]

[[gcode:g7]]
== G7 Lathe Diameter Mode
(((G7 Lathe Diameter Mode)))

----
G7
----

Program G7 to enter the diameter mode for axis X on a lathe. When in
the diameter mode the X axis moves on a lathe will be 1/2 the distance
to the center of the lathe. For example X1 would move the cutter to
0.500” from the center of the lathe thus giving a 1” diameter part.

[[gcode:g8]]
== G8 Lathe Radius Mode
(((G8 Lathe Radius Mode)))

----
G8
----

Program G8 to enter the radius mode for axis X on a lathe. When in
Radius mode the X axis moves on a lathe will be the distance from the
center. Thus a cut at X1 would result in a part that is 2" in diameter.
G8 is default at power up.

[[gcode:g10-l1]]
== G10 L1 Set Tool Table
(((G10 L1 Tool Table)))

----
G10 L1 P- axes <R- I- J- Q->
----
* 'P' - tool number
* 'R' - radius of tool
* 'I' - front angle (lathe)
* 'J' - back angle (lathe)
* 'Q' - orientation (lathe)

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.

.G10 L1 Example Line
----
G10 L1 P1 Z1.5 (set tool 1 Z offset from the machine origin to 1.5)
G10 L1 P2 R0.015 Q3 (lathe example setting tool 2 radius to 0.015 and orientation to 3)
----

It is 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

For more information on cutter orientation used by the 'Q' word,
see the <<lathe-tool-orientation,Lathe Tool Orientation>> diagram.

[[gcode:g10-l2]]
== G10 L2 Set Coordinate System
(((G10 L2 Coordinate System)))

----
G10 L2 P- <axes R->
----
* 'P' - coordinate system (0-9)
* 'R' - rotation about the Z axis

G10 L2 offsets the origin of the axes in the coordinate system specified to
the value of the axis word. The offset is from the machine origin established
during homing. The offset value will replace any current offsets in effect for
the coordinate system specified. Axis words not used will not be changed.

Program P0 to P9 to specify which coordinate system to change.

.Coordinate System

[width="50%", options="header", cols="^,^,^"]
|========================================
|P Value |Coordinate System |G code
|0 |Active |n/a
|1 |1 |G54
|2 |2 |G55
|3 |3 |G56
|4 |4 |G57
|5 |5 |G58
|6 |6 |G59
|7 |7 |G59.1
|8 |8 |G59.2
|9 |9 |G59.3
|========================================


Optionally program R to indicate the rotation of the XY axis around the Z axis.
The direction of rotation is CCW as viewed from the positive end of the Z axis.

All axis words are optional.

Being in incremental distance mode (<<gcode:g90-g91,'G91'>>) has no effect on 'G10 L2'.

Important Concepts:

* G10 L2 Pn does not change from the current coordinate system to the one specified by P,
  you have to use G54-59.3 to select a coordinate system.
* When a rotation is in effect jogging an axis will only move that axis
  in a positive or negative direction and not along the rotated axis.
* If a 'G52' local offset or 'G92' origin offset was in effect before
  'G10 L2', it will continue to be in effect afterwards.
* When programming a coordinate system with R, any 'G52' or 'G92' will
  be applied *after* the rotation.
* 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 is currently active, the new coordinates take effect immediately.

It is an error if:

* The P number does not evaluate to an integer in the range 0 to 9.
* An axis is programmed that is not defined in the configuration.

.G10 L2 Example Line
[source,{ngc}]
----
G10 L2 P1 X3.5 Y17.2
----

In the above example the origin of the first coordinate system
(the one selected by 'G54') is set to be X=3.5 and Y=17.2. 
Because only X and Y are specified, the origin point is only moved in X and Y;
the other coordinates are not changed.

.G10 L2 Example Line
[source,{ngc}]
----
G10 L2 P1 X0 Y0 Z0 (clear offsets for X,Y & Z axes in coordinate system 1)
----

The above example sets the XYZ coordinates of the coordinate system 1 to the machine origin.

The coordinate system is described in the <<cha:coordinate-system,Coordinate System>> Section.

[[gcode:g10-l10]]
== G10 L10 Set Tool Table
(((G10 L10 Set Tool Table)))

----
G10 L10 P- axes <R- I- J- Q->
----
* 'P' - tool number
* 'R' - radius of tool
* 'I' - front angle (lathe)
* 'J' - back angle (lathe)
* 'Q' - orientation (lathe)

G10 L10 changes the tool table entry for tool P so that if the
tool offset is reloaded, with the machine in its current position
and with the current G5x and G52/G92 offsets active, the current coordinates
for the given axes will become the given values. The axes that are
not specified in the G10 L10 command will not be changed. This could be
useful with a probe move as described in the <<gcode:g38,G38>> section.

.G10 L10 Example
----
T1 M6 G43 (load tool 1 and tool length offsets)
G10 L10 P1 Z1.5 (set the current position for Z to be 1.5)
G43 (reload the tool length offsets from the changed tool table)
M2 (end program)
----
* See <<sec:select-tool,T>> & <<mcode:m6,M6>>, and
  <<gcode:g43,G43>>/<<gcode:g43.1,G43.1>> sections for more information.

It is 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

[[gcode:g10-l11]]
== G10 L11 Set Tool Table
(((G10 L11 Set Tool Table)))

----
G10 L11 P- axes <R- I- J- Q->
----
* 'P' - tool number
* 'R' - radius of tool
* 'I' - front angle (lathe)
* 'J' - back angle (lathe)
* 'Q' - orientation (lathe)

G10 L11 is just like G10 L10 except that instead of setting the entry
according to the current offsets, it is set so that the current
coordinates would become the given value if the new tool offset
is reloaded and the machine is placed in the G59.3 coordinate
system without any G52/G92 offset active.

This allows the user to set the G59.3 coordinate system according to a
fixed point on the machine, and then use that fixture to measure tools
without regard to other currently-active offsets.

// .G10 L11 Example FIX ME!
// ----
// G10 L11 P1
// ----

It is 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

[[gcode:g10-l20]]
== G10 L20 Set Coordinate System
(((G10 L20 Set Coordinate System)))

----
G10 L20 P- axes
----
* 'P' - coordinate system (0-9)

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.

.G10 L20 Example Line
----
G10 L20 P1 X1.5 (set the X axis current location in coordinate system 1 to 1.5)
----

It is an error if:

* The P number does not evaluate to an integer in the range 0 to 9.
* An axis is programmed that is not defined in the configuration.

[[gcode:g17-g19.1]]
== G17 - G19.1 Plane Select
(((G17 - G19.1 Plane Select)))

These codes set the current plane as follows:

* 'G17' - XY (default)
* 'G18' - ZX
* 'G19' - YZ
* 'G17.1' - UV
* 'G18.1' - WU
* 'G19.1' - VW

The UV, WU and VW planes do not support arcs.

It is a good idea to include a plane selection in the preamble
of each G code file.

The effects of having a plane selected are discussed in Section
<<gcode:g2-g3,G2 G3 Arcs>> and Section <<gcode:g80-g89,G81 G89>>

[[gcode:g20-g21]]
== G20, G21 Units
(((G20 Units)))

* 'G20' - to use inches for length units.
* 'G21' - to use millimeters for length units.

It is a good idea to include units in the preamble
of each G code file.

[[gcode:g28-g28.1]]
== G28, G28.1 Go/Set Predefined Position
(((G28 Go/Set Predefined Position)))

[WARNING]
Only use G28 when your machine is homed to a repeatable position and the
desired G28 position has been stored with G28.1.

G28 uses the values stored in <<sub:numbered-parameters,parameters>> 
5161-5169 as the X Y Z A B C U V W final point to move to. The parameter
values are 'absolute' machine coordinates in the native machine 'units' as 
specified in the ini file. All axes defined in the ini file will be moved when
a G28 is issued. If no positions are stored with G28.1 then all axes will go to
the <<sec.machine-corrdinate-system,machine origin>>.

* 'G28' - makes a <<gcode:g0,rapid move>> from the current
  position to the 'absolute' position of the values in parameters 5161-5166.

* 'G28 axes' - makes a rapid move to the position specified by
  'axes' including any offsets, then will make a rapid move to the 'absolute'
  position of the values in parameters 5161-5166 for all 'axes' specified. Any
  'axis' not specified will not move.

* 'G28.1' - stores the current 'absolute' position into parameters 5161-5166.

.G28 Example Line
----
G28 Z2.5 (rapid to Z2.5 then to Z location specified in #5163)
----

It is an error if :

* Cutter Compensation is turned on

[[gcode:g30-g30.1]]
== G30, G30.1 Go/Set Predefined Position
(((G30 Go/Set Predefined Position)))

[WARNING]
Only use G30 when your machine is homed to a repeatable position and the
desired G30 position has been stored with G30.1.

G30 functions the same as G28 but uses the values stored in
<<sub:numbered-parameters,parameters>> 5181-5189 as the X Y Z A B C U V W
final point to move to. The parameter values are 'absolute' machine
coordinates in the native machine 'units' as specified in the ini file.
All axes defined in the ini file will be moved when a G30 is issued.  If no
positions are stored with G30.1 then all axes will go to the
<<sec.machine-corrdinate-system,machine origin>>.

[NOTE]
G30 parameters will be used to move the tool when a M6 is programmed
if TOOL_CHANGE_AT_G30=1 is in the [EMCIO] section of the ini file.

* 'G30' - makes a <<gcode:g0,rapid move>> from the current
  position to the 'absolute' position of the values in parameters 5181-5186.

* 'G30 axes' - makes a rapid move to the position specified
  by 'axes' including any offsets, then will make a rapid move to the
  'absolute' position of the values in parameters 5181-5186 for all 'axes'
  specified. Any 'axis' not specified will not move.

* 'G30.1' - stores the current absolute position into parameters 5181-5186.

.G30 Example Line
----
G30 Z2.5 (rapid to Z2.5 then to the Z location specified in #5i83)
----

It is an error if :

* Cutter Compensation is turned on

[[gcode:g33]]
== G33 Spindle Synchronized Motion
(((G33 Spindle Synchronized Motion)))

----
G33 X- Y- Z- K- $-
----
* 'K' - distance per revolution

For spindle-synchronized motion in one direction, code 'G33 X- Y- Z- K-'
where K gives the distance moved in XYZ for each revolution of the spindle.
For instance, if starting at 'Z=0', 'G33 Z-1 K.0625' produces
a 1 inch motion in Z over 16 revolutions of the spindle.
This command might be part of a program to produce a 16TPI thread.
Another example in metric, 'G33 Z-15 K1.5' produces
a movement of 15mm while the spindle rotates 10 times for a thread of 1.5mm.

The (optional) $ argument sets which spindle the motion is synchronised
to (default is zero). For example G33 Z10 K1 $1 will move the spindle in
synchrony with the spindle.N.revs HAL pin value. 

Spindle-synchronized motion waits for the spindle index and spindle at speed
pins, so multiple passes line up. 'G33' moves end at the programmed endpoint.
G33 could be used to cut tapered threads or a fusee.

All the axis words are optional, except that at least one must be used.

[NOTE]
K follows the drive line described by 'X- Y- Z-'. K is not parallel to
the Z axis if X or Y endpoints are used for example when cutting tapered
threads.

.Technical Info[[gcode:g33-tech-info]]
At the beginning of each G33 pass, LinuxCNC uses the spindle speed and the
machine acceleration limits to calculate how long it will take Z to
accelerate after the index pulse, and determines how many degrees the
spindle will rotate during that time. It then adds that angle to the
index position and computes the Z position using the corrected spindle
angle. That means that Z will reach the correct position just as it
finishes accelerating to the proper speed, and can immediately begin
cutting a good thread.

.HAL Connections
The pin 'spindle.N.at-speed' must be set or driven true for the motion to
start. Additionally spindle.N.revs must increase by 1 for each revolution
of the spindle and the spindle.N.index-enable pin must be connected to
an encoder (or resolver) counter which resets index-enable once per rev.

See the Integrators Manual for more information on spindle synchronized motion.

.G33 Example
----
G90 (absolute distance mode)
G0 X1 Z0.1 (rapid to position)
S100 M3 (start spindle turning)
G33 Z-2 K0.125 (move Z axis to -2 at a rate to equal 0.125 per revolution)
G0 X1.25 (rapid move tool away from work)
Z0.1 (rapid move to starting Z position)
M2 (end program)
----
* See <<gcode:g90-g91,G90>> & <<gcode:g0,G0>> & <<mcode:m2-m30,M2>> sections for more information.