G Codes

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:

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.

For rapid linear (straight line) 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 linear motion to the destination point at the current maximum traverse rate (or slower if the machine will not go that fast). It is expected that cutting will not take place when a G0 command is executing.

If cutter compensation is active, the motion will differ from the above; see the Cutter Compensation Section.

If G53 is programmed on the same line, the motion will also differ; see the G53 Section for more information.

It is an error if:

For linear (straight line) motion at programed 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 linear motion to the destination point at the current feed rate (or slower if the machine will not go that fast).

If cutter compensation is active, the motion will differ from the above; see the Cutter Compensation Section.

If G53 is programmed on the same line, the motion will also differ; see the G53 Section for more information.

It is an error if:

A circular or helical arc is specified using either G2 (clockwise arc) or G3 (counterclockwise arc). 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 a P word specifying the number of full or partial turns of arc. If P is unspecified, the behavior is as if P1 was given: that is, only one full or partial turn will result, giving an arc less than or equal to one full circle. For example, if an arc is programmed with P2, the resulting motion will be more than one full circle and up to two full circles (depending on the programmed endpoint.) 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 Cutter Compensation Section.

The arc center is absolute or relative as set by G90.1 or G91.1 respectively.

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

It is an error if:

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.

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 G91.1 section.

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 G90.1 section.

It is an error if:

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

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.

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.

The above example line will make 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=16, and Z=9, with its center offset in the X direction by 3 units from the current X location and offset in the Y direction by 4 units from the current Y location. If the current location has X=7, Y=7 at the outset, the center will be at X=10, Y=11. If the starting value of Z is 9, this is a circular arc; otherwise it is a helical arc. The radius of this arc would be 5.

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.

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:

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.

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.

It is an error if:

G5.1 creates a quadratic B-spline in the XY plane with the X and Y axis only. The offsets are I for X axis and J for Y axis.

It is an error if:

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 their parameter (L) which determines the order of the curve (k) and subsequently its degree (k-1).

Using this curve definition the knots of the NURBs curve are not defined by the user they are calculated by the inside algorithm, in the same way as it happens in a great number of graphic applications, where the curve shape can be modified only acting on either control points or weights.

More information on NURBs can be found here:

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

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.

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.

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.

It is an error if:

For more information on cutter orientation used by the Q word, see the Lathe Tool Orientation diagram.

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.

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 (G91) has no effect on G10 L2.

Important Concepts:

It is an error if:

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.

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

The coordinate system is described in the Coordinate System Section.

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 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 G38 section.

It is an error if:

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 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.

It is an error if:

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.

It is an error if:

These codes set the current plane as follows:

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 G2 G3 and Section G81 G89

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

G28 uses the values stored in parameters 5161-5166 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 specifed in the ini file. All axes defined in the ini file will be moved when a G28 is issued.

It is an error if :

G30 functions the same as G28 but uses the values stored in parameters 5181-5186 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 specifed in the ini file. All axes defined in the ini file will be moved when a G30 is issued.

It is an error if :

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.

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.

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.

The pins motion.spindle-at-speed and the encoder.n.phase-Z for the spindle must be connected in your HAL file before G33 will work. See the Integrators Manual for more information on spindle synchronized motion.

It is an error if:

For rigid tapping (spindle synchronized motion with return), code G33.1 X- Y- Z- K- where K- gives the distance moved for each revolution of the spindle. A rigid tapping move consists of the following sequence:

Spindle-synchronized motions wait for spindle index, so multiple passes line up. G33.1 moves end at the original coordinate.

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

It is an error if:

Program G38.x axes to perform a straight probe operation. The axis words are optional, except that at least one of them must be used. The axis words together define the destination point that the probe will move towards, starting from the current location. If the probe is not tripped before the destination is reached G38.2 and G38.4 will signal an error.

The tool in the spindle must be a probe or contact a probe switch.

In response to this command, the machine moves the controlled point (which should be at the center of the probe ball) in a straight line at the current feed rate toward the programmed point. In inverse time feed mode, the feed rate is such that the whole motion from the current point to the programmed point would take the specified time. The move stops (within machine acceleration limits) when the programmed point is reached, or when the requested change in the probe input takes place, whichever occurs first.

After successful probing, parameters 5061 to 5069 will be set to the coordinates of X, Y, Z, A, B, C, U, V, W of the location of the controlled point at the time the probe changed state. After unsuccessful probing, they are set to the coordinates of the programmed point. Parameter 5070 is set to 1 if the probe succeeded and 0 if the probe failed. If the probing operation failed, G38.2 and G38.4 will signal an error by posting an message on screen if the selected GUI supports that. And by halting program execution.

A comment of the form (PROBEOPEN filename.txt) will open filename.txt and store the 9-number coordinate consisting of XYZABCUVW of each successful straight probe in it. The file must be closed with (PROBECLOSE). For more information see the Comments Section.

An example file smartprobe.ngc is included (in the examples directory) to demonstrate using probe moves to log to a file the coordinates of a part. The program smartprobe.ngc could be used with ngcgui with minimal changes.

It is an error if:

See G0 & M2 sections for more information.

It is an error if:

The D word is optional; if there is no D word the radius of the currently loaded tool will be used (if no tool is loaded and no D word is given, a radius of 0 will be used).

If supplied, the D word is the tool number to use. This would normally be the number of the tool in the spindle (in which case the D word is redundant and need not be supplied), but it may be any valid tool number.

To start cutter compensation to the left of the part profile, use G41. G41 starts cutter compensation to the left of the programmed line as viewed from the positive end of the axis perpendicular to the plane.

To start cutter compensation to the right of the part profile, use G42. G42 starts cutter compensation to the right of the programmed line as viewed from the positive end of the axis perpendicular to the plane.

The lead in move must be at least as long as the tool radius. The lead in move can be a rapid move.

Cutter compensation may be performed if the XY-plane or XZ-plane is active.

User M100-M199 commands are allowed when Cutter Compensation is on.

The behavior of the machining center when cutter compensation is on is described in the Cutter Compensation Section along with code examples.

It is an error if:

G41.1 & G42.1 function the same as G41 & G42 with the added scope of being able to program the tool diameter. The L word defaults to 0 if unspecified.

It is an error if:

G43 enables tool length compensation. G43 changes subsequent motions by offsetting the Z and/or X coordinates by the length of the tool. G43 does not cause any motion. The next time a compensated axis is moved, that axis’s endpoint is the compensated location.

G43 without an H word uses the currently loaded tool from the last Tn M6.

G43 Hn uses the offset for tool n.

It is an error if:

It is an error if:

It is OK to program using the same offset already in use. It is also OK to program using no tool length offset if none is currently being used.

To move in the machine coordinate system, program G53 on the same line as a linear move. G53 is not modal and must be programmed on each line. G0 or G1 does not have to be programmed on the same line if one is currently active. For example G53 G0 X0 Y0 Z0 will move the axes to the home position even if the currently selected coordinate system has offsets in effect.

It is an error if:

The coordinate systems store the axis values and the XY rotation angle around the Z axis in the parameters shown in the following table.

It is an error if:

See the Coordinate System Section for an overview of coordinate systems.

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

The G73 cycle is drilling or milling with chip breaking. This cycle takes a Q number which represents a delta increment along the Z axis.

It is an error if:

Optional settings

The tool is moved to the initial X and Z positions prior to issuing the G76. The X position is the drive line and the Z position is the start of the threads.

The tool will pause briefly for synchronization before each threading pass, so a relief groove will be required at the entry unless the beginning of the thread is past the end of the material or an entry taper is used.

Unless using an exit taper, the exit move (traverse to original X) is not synchronized to the spindle speed. With a slow spindle, the exit move might take only a small fraction of a revolution. If the spindle speed is increased after several passes are complete, subsequent exit moves will require a larger portion of a revolution, resulting in a very heavy cut during the exit move. This can be avoided by providing a relief groove at the exit, or by not changing the spindle speed while threading.

The final position of the tool will be at the end of the drive line. A safe Z move will be needed with an internal thread to remove the tool from the hole.

It is an error if:

The pins motion.spindle-at-speed and the encoder.n.phase-Z for the spindle must be connected in your HAL file before G76 will work. See the Integrators Manual for more information on spindle synchronized motion.

The G76 canned cycle is based on the G33 Spindle Synchronized Motion. For more information see the G33 Technical Info.

The sample program g76.ngc shows the use of the G76 canned cycle, and can be previewed and executed on any machine using the sim/lathe.ini configuration.

In the figure the tool is in the final position after the G76 cycle is completed. You can see the entry path on the right from the Q29.5 and the exit path on the left from the L2 E0.045. The white lines are the cutting moves.

The canned cycles G81 through G89 and the canned cycle stop G80 are described in this section.

All canned cycles are performed with respect to the currently-selected plane. Any of the six planes may be selected. Throughout this section, most of the descriptions assume the XY-plane has been selected. The behavior is analogous if another plane is selected, and the correct words must be used. For instance, in the G17.1 plane, the action of the canned cycle is along W, and the locations or increments are given with U and V. In this case substitute U,V,W for X,Y,Z in the instructions below.

Rotary axis words are not allowed in canned cycles. When the active plane is one of the XYZ family, the UVW axis words are not allowed. Likewise, when the active plane is one of the UVW family, the XYZ axis words are not allowed.

All canned cycles use X, Y, Z, or U, V, W groups depending on the plane selected and R words. The R (usually meaning retract) position is along the axis perpendicular to the currently selected plane (Z-axis for XY-plane, etc.) Some canned cycles use additional arguments.

For canned cycles, we will call a number sticky if, when the same cycle is used on several lines of code in a row, the number must be used the first time, but is optional on the rest of the lines. Sticky numbers keep their value on the rest of the lines if they are not explicitly programmed to be different. The R number is always sticky.

In incremental distance mode X, Y, and R numbers are treated as increments from the current position and Z as an increment from the Z-axis position before the move involving Z takes place. In absolute distance mode, the X, Y, R, and Z numbers are absolute positions in the current coordinate system.

The L number is optional and represents the number of repeats. L=0 is not allowed. If the repeat feature is used, it is normally used in incremental distance mode, so that the same sequence of motions is repeated in several equally spaced places along a straight line. When L- is greater than 1 in incremental mode with the XY-plane selected, the X and Y positions are determined by adding the given X and Y numbers either to the current X and Y positions (on the first go-around) or to the X and Y positions at the end of the previous go-around (on the repetitions). Thus, if you program L10 , you will get 10 cycles. The first cycle will be distance X,Y from the original location. The R and Z positions do not change during the repeats. The L number is not sticky. In absolute distance mode, L>1 means do the same cycle in the same place several times, Omitting the L word is equivalent to specifying L=1.

The height of the retract move at the end of each repeat (called clear Z in the descriptions below) is determined by the setting of the retract mode: either to the original Z position (if that is above the R position and the retract mode is G98, OLD_Z), or otherwise to the R position. See the G98 G99 Section.

It is an error if:

If the XY plane is active, the Z number is sticky, and it is an error if:

If other planes are active, the error conditions are analogous to the XY conditions above.

Preliminary motion is a set of motions that is common to all of the milling canned cycles. If the current Z position is below the R position, the Z axis is traversed to the R position. This happens only once, regardless of the value of L.

In addition, at the beginning of the first cycle and each repeat, the following one or two moves are made

If another plane is active, the preliminary and in-between motions are analogous.

There are at least two reasons for using canned cycles. The first is the economy of code. A single bore would take several lines of code to execute.

The G81 Example 1 demonstrates how a canned cycle could be used to produce 8 holes with ten lines of G code within the canned cycle mode. The program below will produce the same set of 8 holes using five lines for the canned cycle. It does not follow exactly the same path nor does it drill in the same order as the earlier example. But the program writing economy of a good canned cycle should be obvious.

The G98 to the second line above means that the return move will be to the value of Z in the first line since it is higher that the R value specified.

This example demonstrates the use of the L word to repeat a set of incremental drill cycles for successive blocks of code within the same G81 motion mode. Here we produce 12 holes using five lines of code in the canned motion mode.

The second reason to use a canned cycle is that they all produce preliminary moves and returns that you can anticipate and control regardless of the start point of the canned cycle.

It is an error if:

The following code produces the same final position and machine state as the previous code.

The advantage of the first set is that, the G80 line clearly turns off the G81 canned cycle. With the first set of blocks, the programmer must turn motion back on with G0, as is done in the next line, or any other motion mode G word.

If a canned cycle is not turned off with G80 or another motion word, the canned cycle will attempt to repeat itself using the next block of code that contains an X, Y, or Z word. The following file drills (G81) a set of eight holes as shown in the following caption.

The use of G80 in line N200 is optional because the G0 on the next line will turn off the G81 cycle. But using the G80 as shown in Example 1, will provide for easier to read canned cycle. Without it, it is not so obvious that all of the blocks between N120 and N200 belong to the canned cycle.

The G81 cycle is intended for drilling.

The cycle functions as follows:

Suppose the current position is (X1, Y2, Z3) and the following line of NC code is interpreted.

This calls for absolute distance mode (G90) and OLD_Z retract mode (G98) and calls for the G81 drilling cycle to be performed once.

The X value and X position are 4.

The Y value and Y position are 5.

The Z value and Z position are 1.5.

The R value and clear Z are 2.8. OLD_Z is 3.

The following moves take place:

Suppose the current position is (X1, Y2, Z3) and the following line of NC code is interpreted.

This calls for incremental distance mode (G91) and OLD_Z retract mode (G98). It also calls for the G81 drilling cycle to be repeated three times. The X value is 4, the Y value is 5, the Z value is -0.6 and the R value is 1.8. The initial X position is 5 (=1+4), the initial Y position is 7 (=2+5), the clear Z position is 4.8 (=1.8+3), and the Z position is 4.2 (=4.8-0.6). OLD_Z is 3.

The first preliminary move is a traverse along the Z axis to (X1,Y2,Z4.8), since OLD_Z < clear Z.

The first repeat consists of 3 moves.

The second repeat consists of 3 moves. The X position is reset to 9 (=5+4) and the Y position to 12 (=7+5).

The third repeat consists of 3 moves. The X position is reset to 13 (=9+4) and the Y position to 17 (=12+5).

Now suppose that you execute the first G81 block of code but from (X0, Y0, Z0) rather than from (X1, Y2, Z3).

Since OLD_Z is below the R value, it adds nothing for the motion but since the initial value of Z is less than the value specified in R, there will be an initial Z move during the preliminary moves.

This is a plot of the path of motion for the second g81 block of code.

Since this plot starts with (X0, Y0, Z0), the interpreter adds the initial Z0 and R1.8 and rapids to that location. After that initial Z move, the repeat feature works the same as it did in example 3 with the final Z depth being 0.6 below the R value.

Since this plot starts with (X0, Y0, Z0), the interpreter adds the initial Z0 and R1.8 and rapids to that location as in Example 4. After that initial Z move, the rapid traverse move to X4 Y5 is done. Then the final Z depth being 0.6 below the R value. The repeat function would make the Z move in the same location again.

The G82 cycle is intended for drilling with a dwell at the bottom of the hole.

The motion of a G82 canned cycle looks just like G81 with the addition of a dwell at the bottom of the Z move. The length of the dwell is specified by a P- word in the G82 block.

The G83 cycle (often called peck drilling) is intended for deep drilling or milling with chip breaking. The retracts in this cycle clear the hole of chips and cut off any long stringers (which are common when drilling in aluminum). This cycle takes a Q number which represents a delta increment along the Z-axis. The retract before final depth will always be to the retract plane even if G98 is in effect. The final retract will honor the G98/99 in effect. G83 functions the same as G81 with the addition of retracts during the drilling operation.

It is an error if:

This code is currently unimplemented in LinuxCNC. It is accepted, but the behavior is undefined. See section G33.1

The G85 cycle is intended for boring or reaming, but could be used for drilling or milling.

The G86 cycle is intended for boring. This cycle uses a P number for the number of seconds to dwell.

It is an error if:

This code is currently unimplemented in LinuxCNC. It is accepted, but the behavior is undefined.

This code is currently unimplemented in LinuxCNC. It is accepted, but the behavior is undefined.

The G89 cycle is intended for boring. This cycle uses a P number, where P specifies the number of seconds to dwell.

G92 makes the current point have the coordinates you want (without motion), where the axis words contain the axis numbers you want. All axis words are optional, except that at least one must be used. If an axis word is not used for a given axis, the coordinate on that axis of the current point is not changed.

When G92 is executed, the origins of all coordinate systems move. They move such that the value of the current controlled point, in the currently active coordinate system, becomes the specified value. All coordinate system’s origins are offset this same distance.

For example, suppose the current point is at X=4 and there is currently no G92 offset active. Then G92 x7 is programmed. This moves all origins -3 in X, which causes the current point to become X=7. This -3 is saved in parameter 5211.

Being in incremental distance mode has no effect on the action of G92.

G92 offsets may be already be in effect when the G92 is called. If this is the case, the offset is replaced with a new offset that makes the current point become the specified value.

It is an error if:

LinuxCNC stores the G92 offsets and reuses them on the next run of a program. To prevent this, one can program a G92.1 (to erase them), or program a G92.2 (to remove them - they are still stored).

See the Coordinate System Section for an overview of coordinate systems.

See the Offsets Section for more information.

See the Parameters Section for more information.

You can set axis offsets in one program and use the same offsets in another program. Program G92 in the first program. This will set parameters 5211 to 5219. Do not use G92.1 in the remainder of the first program. The parameter values will be saved when the first program exits and restored when the second one starts up. Use G92.3 near the beginning of the second program. That will restore the offsets saved in the first program.

It is an error if:

It is an error if:

Program a G98 and the canned cycle will use the Z position prior to the canned cycle as the Z return position if it is higher than the R value specified in the cycle. If it is lower then the R value will be used. The R word has different meanings in absolute distance mode and incremental distance mode.

The G98 to the second line above means that the return move will be to the value of Z in the first line since it is higher that the R value specified.

The initial (G98) plane is reset any time cycle motion mode is abandoned, whether explicitly (G80) or implicitly (any motion code that is not a cycle). Switching among cycle modes (say G81 to G83) does NOT reset the initial plane. It is possible to switch between G98 and G99 during a series of cycles.