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.

Los valores que siguen a las letras a menudo se dan como números explícitos. A menos que se indique lo contrario, los números explícitos pueden ser valores reales. Por ejemplo, G10 L2 podría igualmente escribirse G[2*5] L[1+1]. Si el valor del parámetro 100 era 2, G10 L#100 también significaría lo mismo.

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

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.

For linear (straight line) motion at programmed 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).

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) at the current 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 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:

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 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:

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

It is an error if:

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:

It is an error if:

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.

More information on NURBS can be found here:

https://wiki.linuxcnc.org/cgi-bin/wiki.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 L0 reload all tool table data. Requires that there is no current tool loaded in spindle.

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 for the specified tool.

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 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 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 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.

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 Arcs 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 5161-5169 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 machine origin.

It is an error if :

G30 functions the same as G28 but uses the values stored in 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 machine origin.

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.

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.

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 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.

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.n 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 X, Y, Z, A, B, C, U, V, W coordinates of the location of the controlled point at the time the probe changed state (in the current work coordinate system). 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.

Here is an example formula to probe tool height with conversion from a local coordinate system Z offset to machine coordinates which is stored in the tool table. The existing tool height compensation is first cancelled with G49 to avoid including it in the calculation of height, and the new height is loaded from the tool table. The start position must be high enough above the tool height probe to compensate for the use of G49.

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

G43 Hn uses the offset for tool n.

The active tool length compensation values are stored in the numbered parameters 5401-5409.

It is an error if:

It is an error if:

You can sum together an arbitrary number of offsets by calling G43.2 more times. There are no built-in assumptions about which numbers are geometry offsets and which are wear offsets, or that you should have only one of each.

Like the other G43 commands, G43.2 does not cause any motion. The next time a compensated axis is moved, that axis’s endpoint is the compensated location.

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.

G52 is used in a part program as a temporary "local coordinate system offset" within the workpiece coordinate system. More information on G52 is in the Local and Global Offsets section.

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.

See G0 section for more information.

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 G70 cycle is intended to be used after the shape of the profile given in the subroutine with number Q has been cut with G71 or G72.

It is an error if:

The G71/G72 cycle is intended to rough cut a profile on a lathe. The G71 cycles remove layers of the material while traversing in the Z direction. The G72 cycles remove material while traversing the X axis, the so called facing cycle. The direction of travel is the same as in the path given in the subroutine. For the G71 cycle the Z coordinate must be monotonically changing, for the G72 this is required for the X axis.

The profile is given in a subroutine with number Q-. This subroutine may contain G0, G1, G2 and G3 motion commands. All other commands are ignored, including feed and speed settings. The [gcode:g0] commands are interpreted as G1 commands. Each motion command may also include an optional A- or C- number. If the number A- is added a fillet with the radius given by A will be inserted at the endpoint of that motion, if this radius is too large the algorithm will fail with a non-monotonic path error. It is also possible to use the C- number, which allows a chamfer to be inserted. This chamfer has the same endpoints as a fillet of the same dimension would have but a straight line is inserted instead of an arc.

When in absolute mode the U (for X) and W (for Z) can be used as incremental displacements.

The G7x.1 cycles do not cut pockets. The G7x.2 cycles only cut after the first pocket and continue where G7x.1 stopped. It is advisible to leave some additional material to cut before the G7x.2 cycle, so if G7x.1 used a D1.0 the G7x.2 can use D0.5 and 0.5mm will be removed while moving from one pocket to the next.

The normal G7x cycles cut the entire profile in one cycle.

It is an error if:

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. Peck clearance can be specified by optional P number.

It is an error if:

The G74 cycle is intended for tapping with floating chuck and dwell at the bottom of the hole.

The length of the dwell is specified by a P- word in the G74 block. The feed rate F- is spindle speed multiplied by distance per revolution (thread pitch). In example S100 with 1.25MM per revolution thread pitch gives a feed of F125.

Optional settings

Thread entries and exits can be programmed tapered with the E and L values.

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 is not synchronized to the spindle speed and will be a rapid move. 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 spindle.N.at-speed and the encoder.n.phase-Z for the spindle must be connected in your HAL file before G76 will work. See the spindle pins in the Motion section for more information.

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 nine 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.

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 preceding 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 following moves take place:

Suppose the current position is (X1, Y2, Z3) and the preceding 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 maximum rapid move 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 rapid moves 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 rapid moves to that location as in Example 4. After that initial Z move, the rapid 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.

This will be similar to example 3 above, just with an added dwell of 2 seconds at the bottom of the hole.

The G83 cycle (often called peck drilling) is intended for deep drilling ormilling 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. Peck clearance can be specified by optional P number.

It is an error if:

The G84 cycle is intended for tapping with floating chuck and dwell at the bottom of the hole.

The length of the dwell is specified by a P- word in the G84 block. The feed rate F- is spindle speed multiplied by distance per revolution (thread pitch). In example S100 with 1.25MM per revolution thread pitch gives a feed of F125.

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 offset for that axis will be zero.

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 of the coordinate system’s origins (G53-G59.3) are offset this same distance.

G92 uses the values stored in parameters 5211-5219 as the X Y Z A B C U V W offset values for each axis. 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 offset when G92 is active. If an axis was not entered following the G92, that axis' offset will be zero.

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 (G91 instead of G90) 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 all axis words are omitted.

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 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:

When using G96, ensure that X0 in the current coordinate system (including offsets and tool lengths) is the center of rotation or LinuxCNC will not give the desired surface speed. G96 is not affected by radius or diameter mode.

To achieve CSS mode on selected spindles programme successive G96 commands for each spindle prior to issuing M3.

It is an error if:

When spindle retracts during canned cycles, there are two options to choose from for the way it does it:

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, 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.