Operator Manual

This reference covers the operation of all NXGEN CNC Controls. For questions not covered in this manual, contact us at support@nxgencnc.com or call us at (888) 949-2939 Ex 2.
Return to nxgencnc.com


The NXGEN Control is an advanced, feature-rich Control designed upon the success and simplicity of the Fadal controls. Any machine operator familiar with old Fadal operation will be able to walk up the Control and use it. All the familiar codes, functions, and commands of the old system are retained, with many new features and performance benefits added.

This manual will provide an outline of the basic operation of the Control. Please note it is designed for a user who has some familiarity with Fadal operation / machine operation in general (familiar with G codes, M codes, etc).



The NXGEN Pendant is an advanced, full-feature pendant modeled after the successful CNC88 pendants. It comes complete with a fully-functional switch panel, touchscreen, and keyboard. 

1.2.Touch Screen

The NXGEN provides the same functionality as the CNC 88 Quick-Key menu system without a need to “drill down” through a series of menus to locate a function. Instead of five selections, the Control reduces the interface to only one or the Touch Keys.

A fully operating touchscreen, all of the following buttons, activities, and functions can be selected by either touching or clicking with a mouse. While you still can use commands like the old system, using the touch keys will quickly perform what actions the commands achieve. The Touch Keys minimize the use of a “back” button, greatly speeding up machine operation. Simply touch what you need to do

Like the CNC 88, press the MANUAL key to abort/ exit such operations as Auto/Single Step, Slide Hold or any waiting mode. If a function blinks red, that indicates the Manual key is needed to abort the current operation mode.

To switch between MDI, Auto or Command modes, press the space bar.

For an outline of the interface, see Interface Overview

Other Tips:

  • The touch screen works in conjunction with a mouse or any other pointing device.
  • The touch screen can be disabled for “mouse only” operation in the parameter settings.
  • The touch screen is best cleaned with a mild cleaner.

1.3.Switch Panel

Designed for the same functionality as with the CNC 88, with an added USB port for convenience, the NXGEN Switch Panel contains all the functionality operators and servicemen need in the day-to-day use of the machine.

Below outlines the basic function of each Switch Panel feature.

Feature Option Function
Memory Lock On/Off When enabled, prevents modification of program
Load Meter LED Array displaying spindle load.
Block skip On/Off Used to activate the block skip code in the program.
Optional Stop On/Off Used to activate the optional stop code in the program
Work Light On/Off Used to active the work light in the machine
Emergency Stop On/Off When pressed, will pause all machine functions and put it in E-TOP mode. Reset by turning the button clockwise and pressing JOG.
Rapid Travel 25%, 50%, 100% Used to select rapid speed by percentage of set value.
Feed Rate Pot 0-250% Used to select Feed Rate speed by percentage of set value.
Spindle Pot 0-250% Used to select spindle speed by percentage of set value (up to max RPM).
Axis Jog Selector X, Y, Z, A, B, Aux, Remote Used to select axis in JOG, or to active remote in JOG.
Increment Jog Selector .01, .001, .0001 Used to select Jog pulse increment.
MPG Wheel Used to pulse axis while in JOG at a set increment.
USB Port Available USB port
Start Button On/Off Used to start program (can also be done on touch screen).
Slide Hold Button On/Off Used to activate slide hold (can also be done on touch screen).



The pendant comes complete with an industrial water-proof Windows keyboard, with the following features:

  • Twelve Function Keys
  • Windows compatible, 88-Key Functionality
  • Polycarbonate Case with Mounting Holes
  • Backlit Keys

The keyboard is designed to meet MIL-STD-461E and NEMA 4X specifications, for military computing applications.

KEY SWITCH MATERIAL: Industrial silicone rubber
FEEDBACK: Tactile with mechanical snap
SEALED: 100% Humidity

  • To right click, hold down the right click key (noted below) and click/touch.
  • To access the Windows 7 system, press the Windows key on the lower left position of the keyboard.
  • To active the backlight, select the backlit key (noted below).

Other Tips:

  • Since the control is based on Windows 7, you can add another keyboard by simply adding a USB interface keyboard and/or mouse. There are open USB ports located at the right hand side of the CPU card cage.
  • Depending on use, can be cleaned with a mild cleaner.

1.5.Remote Handwheel


While in JOG, rotate the Pendant Axis Selector to the REMOTE position and the control then reads the current axis selector on the remote HANDWHEEL.

Remote Functions:

  1. AXIS Selections : AXZ12 is used to select the XYZAB axis.
  2. Increment Selections:  X1, X10 and X100 is used to select .0001, .001 and .01 step size.
  3. The ESTOP button puts the machine in the ESTOP condition.
  4. The START CYCLE works the same as the START button on the pendant.
  5. The FEED HOLD button works the same as the SLIDE HOLD button on the pendant.
  6. REMOTE TOOL IN/OUT is achieved by pressing and hold down both the START CYCLE and the FEED HOLD button.

To switch back to using the Pendant Switches:

Switch the axis selector on the Remote Handwheel to OFF then rotate the Pendant Axis Selector to an active axis.

2.Interface Overview

The NXGEN Interface is divided into the following sections, as described and shown below. Each section is described in detail in this manual.

POSITION DISPLAY WINDOW: this part of the Interface show the axis position, with optional views on the right section of the display. Read more.

TOUCH KEYS: includes an array of one-touch buttons that aid in day-to-day operation, service and setup of the machine. These replace many of the old CNC88 commands (which can still be entered and used, if desired).

OPTIONS WINDOW: a section of the interface that will display optional buttons and functions, depending on the function.

G CODE STATUS WINDOW: a window that displays different statuses of the control, such as active G codes, current RPM, etc. Read more.

ACTIVE LEDS WINDOW: a window of LEDs that light up depending on different statuses. Read more.

ENTER NEXT COMMAND WINDOW: a multi-function window where the operator can enter in commands. This will occasionally display messages. Read more.

FUNCTIONS KEYS: a collection of commands that are crucial to operation of the machine and easily accessed. Read more.

PROGRAM AND MESSAGE DISPLAY WINDOW: a multi-use window that will display program code and messages. Read more.

2.1.Power On/Off

HOW To Power ON

Apply power to the machine using the Main Power Disconnect and the control will start up. There is no use of the green start button as with the CNC 88 control

How To Power OFF

Pressing this button stops the Automatic operation or MD.

Press the RETURN POWER OFF button.

  1. When the machine is not at the Cold Start Position, the Options show PROCEED or CANCEL
    Pressing PROCEED will return the axes to the Cold Start position.
    Pressing CANCEL will abort the operation.
  2. There are two options that appear.
    Goes into ESTOP
    Closes the CNC Control
    Goes to the Windows Desktop
    Note: Shut Down Windows before disconnecting Main Power
    Prepares to shut down all power
    Same as above except shuts down Windows.

2.2.Color Codes

The NXGEN Keys are color coded to reflect their status. They follow the below color scheme.

 Blue indicates the button is not active.

 Green indicates the button is active.

 Red flashes if the button action is not available. 

 Grey indicates the button is an option. 

2.3.Position Display Window

The Position Display window is located on the upper right side of the interface, and is divided into left and right sections. The left section is always the Axis Display (ABS), and the right section has the following three options: Distance to Go, Incremental Distance, and Machine Zero.

To alternate between the three options on the right section, simply touch/click the active title (only Distance to Go shown).

Axis Display Window (ABS)

The left section of the Position Display is the Axis Display window (ABS) and shows the XYZAB axis position. The number of axes shown depends on the axis configuration set in the parameters (three axis shown).

The numeric values displayed are the actual encoder positions, unlike with the CNC 88 (which only displayed the program position, not the real position). The number of decimals positions can be changed in the parameter settings.

In the CNC 88, the minimum resolution was .0001 inches, but the NXGEN resolution is much higher. The actual minimum resolution depends on the ball screw pitch, that is, the encoder counts per turn, described below.

  • For DC machines: With a .200” pitch ballscrew, the smallest resolution is .000024”
  • For AC machines: With a .3937 (10mm) pitch ballscrew, the smallest resolution is .0000125”.

To see the smallest increment, start JOG mode and press the T key, the smallest resolution becomes the JOG increment.

Distance to Go (DIS TO GO)

Distance to Go displays the countdown from the current position to the desired position.

Next Incremental Distance (INCR)

Next Incremental Distance displays the incremental distance of the last move that was made, relative to the direction.

Machine Zero (MACHZERO)

Machine Zero displays the current position’s distance from cold start position (the machine zero)



Press the F1 key to change the display to the large Position Display, press F1 again to restore the normal screen.

2.4.Program and Message Display Window

The lower left portal labeled “CNC PROGRAM” displays the currently loaded program as well as system information and warning messages.

Other Tips:

  • During AUTO, the program display window, when clicked on allows the scrolling ahead into 48K of the up and coming program.

2.5.Function Keys

Located in the lower center part of the touchscreen are the function keys.  They are designed to work identical to the Legacy controls keys, and have familiar commands like Start, Auto, Single Step, and Manual.  These functions are standard and work just as they would on any CNC88. The operator can use key callers to help indicate the operational conditions.

The Keys are explained in depth below.



Press Start to begin a program or command from a waiting mode; after AUTO, the Start key has an embedded single stepping program.

Instead of having to put the machine in single step and repeatedly push the key, you can just hold the Start key down and the control will automatically continue at a single step pace.



Auto to begin running a program or cancel Single Step mode. The control will continue to process the program until the buffer is filled and the program continues (or until the Slide Hold key is pressed).

Pressing Auto while in command mode initiates the Auto Mode screen. The program will be initiated once the Auto key is pressed again.  If not, the control is in the Waiting state.



Manual interrupts the current activity of the machine and enters the COMMAND mode, allowing the operator to toggle between Manual Data Input (MDI) and enter next command. The key is however ignored if pressed when the machine is running a program.

Double clicking the key puts the machine in MDI mode

2.5.4.Single Step

Single Step

Single Step puts the machine in a Waiting state in between each program block.  This allows the operator to run the machine through the program step by step.

An alternate way to run the machine in Single Step is to simple hold down the Start key.

The Single Step state is exited through pushing any of the following keys:

  • Start: starts one block of the program.
  • Auto:  resumes continuous running of the program
  • Jog: initiates the Jog mode
  • Manual:- terminates the program and enters command mode.


Other Tips: 

  • During Single Step Mode, hold down the START key to quickly step through the SINGLE STEP process rather than having to push START for each block.



The JOG function is designed to operate the same as with the CNC 88. The NXGEN also has many new features.

Pressing the JOG key begins the JOG mode and used to restore and recover from an ESTOP condition.

To exit Jog, push the Manual key.



Once in Jog, the operator can move the axis motors by selecting an axis in two ways:

1) Selecting an axis via the axis selector switch on the Pendant control panel

2) Selecting an axis by entering X, Y, Z, A, B, or C on the keyboard.

The jog direction is selected by either entering the “-” or “+” key on the keyboard or by the rotation direction on the pendant hand wheel (clockwise = positive, counterclockwise = negative), or the hand held remote hand wheel if applicable.

The speed of the jog increment is set by pressing H, M, L, or T (High, Medium, Low, or Tiny respectively) on the keyboard, or by selecting the increment value on the selector switch on the pendant control panel.

H = .01            M = .001         L = .0001             T = .00001

The speed of the jog can also be set via the feed rate pot on the pendant control panel.  The feed rate speed is only used when in jog, and is overrode when using the hand wheel.

Short moves can be made by pressing the Jog key repeatedly.  Holding the Jog key down jogs the machine in a continuous motion, at the set increment and feed rate. Jog

Advanced Jog

The NXGEN comes with many improvements to the standard CNC88 JOG.


Once in JOG, the Program and Message Display window displays a JOG: Hot Key List that shows all the available keyboard functions.

  • XYZAB – Selects Axis
    Overrides current axis selection and is in effect until rotating the Axis Selection knob.
  • The original H,M,L keys are used to override the increment selection. We have added a new selection key that sets the increment to the smallest resolution which is one motor encoder count.
  • 1,2,3,4,5 keys select increments that are between .001 and .01 jog step increments. This improves the functionality of machining with the Hand Wheel when .001 is too slow and .01 is too fast.
  • Pressing the following keys 1 to 5 changes the increment and feed feedrate:
    1 = .001 – 15 IPM
    2 = .002 – 30 IPM
    3 = .003 – 45 IPM
    4 = .004 – 60 IPM
    5 = .005 – 75 IPM
  • The “J” key is a short cut to the new JOG MENU (see below)
  • The “P” key brings up the FEED TO POSITION.
  • The “R” key is a short cut to the RIGID TAP IN JOG.
  • The “S” key is a short cut to JOG TEACH.
  • The + and – keys are used to change the JOG axis direction, normally set with the handwheel direction of rotation.



Once in JOG, a new JOG MENU key becomes available in the G-Code Status Window. Pressing this key will display JOG features in the OPTIONS window. This is the same as pressing the “J” shortcut key.

The Jog Menu options are described below. Jog Fixture

Create Jog Fixture

Used to turn on a Fixture Offset while in JOG or temporally zero an axis position display like a Digital Read Out while in JOG.  Press this button and the options will be displayed. to Position

Feed to Position 

Same as using the “P” short cut described above.

Pressing this key brings up a prompt that allows the entry of a desired positioning move. This allows moves like MDI while still in JOG. The move will be made at the current feedrate displayed in the status window. The value entered is absolute and can be overridden with G91 added with the axis move. To move all axis to their zero positions, enter G28 in the prompt line. Tap Retract

Rigid Tap Retract

Same as using the “R” short cut described above.

This is used to retract a Thread Tap from the part or to do Rigid Tap while in JOG.

To Retract a Tap:

  1. During a RT process, if the Slide Hold/Manual is used or the ESTOP Button is pressed or the Power is lost. Simply restore power and press JOG to start the amplifiers.
  2. Press the R key to begin RT retract. This will bring up a dialog box – enter Y to begin.
  3. Select the Z axis and JOG the Z in the positive direction and the spindle will follow. Tap in JOG

Rigid Tap in JOG

This feature allows the operator to Rigid Tap while in JOG. 

To Rigid Tap in Jog:

  1. Start JOG by pressing the JOG key
  2. Press the “r” key begin Rigid Tap. This will bring up a dialog box – enter Y to begin. 
  3. Once RT is activated, switching from Z axis to another axis will suspend the RT and allow normal JOG for all axes except the Z axis. For example, switch from Z to X and you can jog X to a desired location then switch back to Z and tap the hole.

To change Z position while in RT:
a) Press the SPINDLE FWD button to cancel the RT mode and return the Z axis to normal operation.
b) After re-positioning Z, press the R key to return to the RT mode. Teach

Jog Teach

Same as using the “S” short cut described above.

The “S” key stores current location in a file named JOG TECH (date).NC in the CNC PROGRAMS folder. Every time the “S” is pressed.
Once your press MANAUL, the OPTIONS keys are display that allow you to open the saved positions in the Editor and save the file to your desired location.



Spindle Off turns the spindle on at the current RPM setting. The Spindle key on the top right of the function keys displays the status of the spindle.

The Spindle Off blue key indicates that the spindle is off and ready to be enabled.  Tapping this key enables the spindle at the preset RPM.

Note that to enable the spindle there is a two-factor saftey built into the system. Once tapped, the key will turn greed and the Control will ask you to “Confirm Spindle On” by selecting either the Proceed or Cancel key in the Option window.

To override this safety, simply hold Shift and tap the Spindle key to immediately start the spindle.

The other two forms of the key, Spindle FWD and Spindle REV, indicate that the spindle is enabled and the direction it is rotating.


Tapping the Spindle key when it is enabled in either direction disables the Spindle.

For more information on the Spindle, see Spindle Functions.

2.5.7.Slide Hold

Slide Hold

Slide Hold stops the movement of the X, Y, Z, A and B axis.  Note that neither the Spindle nor the coolant are affected.  Slide Hold will be overrode when either the Start or Auto key is pushed.

2.5.8.Coolant #1 and # 2

Coolant #1 and #2

The coolant is off when the button is blue and displays “Off.”  To turn the coolant on, touch the key.  The key turns green and it shows “On” when the coolant is enabled.   Click the key again to turn it off.

Note that to enable either of the coolants there is a two-factor safety built into the system. Once tapped, the key will turn green and the Control will ask you to “Confirm Coolant On” by selecting either the Proceed or Cancel key in the Option window.

To override this safety, simply hold Shift and tap the Coolant key to immediately start the coolant.

Both Coolant #1 and #2 function the same. M7 and M8 configuration is determined in parameter settings.

2.5.9.Tool In/Out

Tool In/Out

Tool In/Out commands the machine to release the current mounted tool.  A blue key indicates the tool is available to be removed.  A green key indicates that the machine is releasing the tool.

To remove a tool, hold down the key, and manually remove the tool.

The control automatically checks to see if the draw bar is down.  Any errors preventing the tool from being removed (i.e., if the machine does not have adequate air pressure) will be displayed in the Status Window.

2.5.10.Turret CCW / CW

Turret CCW / CW

The turret keys rotate the tool turret either CW or CCW. The turret will rotate as long as the key is pressed.

A blue key indicates that the turret is not rotating but is ready to rotate.  A green key indicates that the turret is currently rotating in a counterclockwise direction.

2.6.Enter Next Command Window

Enter Next Command Window

The Enter Next Command Window is a multi-use window where many commands can be performed. Here, instead of using the Touch Keys, you can enter commands such as AU, BL, SETP, etc., the same as the CNC 88.

The Window will also at times display certain messages important for the operator, such as “CONFIRM SPINDLE ON”.

Enter the command MU to display a list of the commands supported and new ones that have be added.

Other Tips:

  • Press the space bar to switch between the MDI, Command modes.

2.7.Status Window

Status Window

The Status Window displays the active G-code, Tool, Spindle Speed and values such as RPM and FEEDRATE, as Outlined below.

2.8.Active Window LEDs

Active Window LEDs

The LEDs in the Active Window display shows the current status of the Control.

LED ON indicates Active, OFF indicates not active.

  • ALARM and FAULT indicates an ESTOP condition. Press JOG to reset.
  • CLAMP 1 and 2 are used for the A/B axis brake.
  • DRY RUN led is lit when Dry Run mode is active.
  • FEED OFF is lit when the feed pot is off and prohibiting motion.
  • ORIENT is lit when the spindle is oriented and locked,
  • REMOTE is lit when in JOG mode and the Remote Handwheel is active.

2.9.Graphic View Port

Graphic View Port

The NXGEN Real-time Modeling is a dynamic, real-time tool that can be used either before you run the part for an accurate representation of how the part will be machined, or while machining a part.

The system runs two blocks ahead of the actual machining process, and displays a real time of the position of the tool.  If you enter JOG while in the display and jog any direction, that movement will be displayed in real time.

To view the Graphic View Port, click the “View Graphics” key on the Touch Keys window.

To return to the Touch Keys windows, simply click anywhere on the Graphic View Port.

With the NXGEN modeling, the model will turn red wherever the machine rapids through the material.

For more information on graphics, see View Graphics.

3.Memory Keys

Memory Keys

The Memory Key section of the Interface is used to perform actions that have to do with program memory.

We will discuss each key, and their options, in depth in this section.

3.1.Load Program

Load Program

To load a previously loaded program:

Press the LOAD PROGRAM key to show the 8 last programs loaded in the OPTIONS category on the right. The last program loaded will be on the top of the list. Simply tap on the desired program to load.

To load a program on USB, disk or network:

Press the LOAD PROGRAM key a second time to bring up a Windows dialog and navigate as you would on your PC to locate the file.

Where to Store:

The NXGEN comes with a folder on the C: hard drive named CNC PROGRAMS. You can use this folder or create your own just as you would on your PC.

File Names:

Use any standard Windows 7 file names.
Individual components of a filename (i.e. each subdirectory along the path, and the final filename) are limited to 255 characters, and the total path length is limited to approximately 32,000 characters.

The following are legal and illegal characters in a filename:

Legal:  A-Z 0-9 $#&+@!()-{}’`_~, and the space

Illegal: |<>\^=?/[]”;* plus control characters

If you prefer, you can still follow the CNC 88 program storage system that was using O-words such as “O9999”, but now you can add more data such as:

O9999 (Program to rough out material)

O123456-1 (Tool #1, Finishing)

1234567-1 Finishing Tool – ET Phone Home

File Extensions:

The control does not require any specific file name extension. Use any common Windows extension names for text files such as .TX, TXT, CAM systems commonly use .NC or .CNC

For more information, see Naming Files, Paths, and Namespaces, see the following:


3.2.Auto Options

Auto Options

Pressing the AUTO OPTIONS key will turn it green and show the following auto options available on your machine:




MST LOCK DRY RUN (under development)


We will discuss these options in this section. To cancel any of the options set in this section, simply press “Cancel All Options”. To go back to the Auto Options menu, press the Auto Options key again.

3.2.1.Mid-Program Start

Mid-Program Start

Mid-Program Start allows the operator to start the program at a specified block number. Selecting this key brings up the Mid-Program Start Menu.

Modal search allows you to start search for the block number, or simply enter the block number into the Enter Next Command window. 

Disable the Mid-Program start by selecting Turn Off or pressing Manual. 

This is the same as the “AU” command, which can also be entered in the Enter Next Command window instead of using the touch key. 



3.2.2.Graphic Dry Run

Graphic Dry Run

Touching Dry Run key enables a graphic dry run of the loaded program.

Selecting the Graphics Dry Run key turns it green, showing that it is active. Once active, simply press the AUTO key to watch the graphic simulation of machining the part, as fast as possible.

The following adjustments can be made to the Dry Run before running the program:

  • The Feed Override key permits a custom feed rate to be entered.
  • The Rapid Override key allows the user to set a desired rapid speed.

The screen then indicates your selections. For example, in the screen below, note that the – ACTIVE – LEDs on the right shows DRY RUN as active and the FEED indicator shows 75 IPM in green (normally white), indicating the feed rate override is in effect and the RAPID OVERRIDE is set to 300 IPM.

With a simple touch of the AUTO key, the machine will begin with the current dry run settings.

3.2.3.Feed Override

Feed Override

This function allows you to enter in a custom feed rate for your program. The Control comes with preset suggested overrides of 75 IPM and 150 IPM. Select either of these, or enter in a custom value using the Custom Feed Rate button. Once pressed, the Control will prompt you to enter in the desired feed rate into the Enter Next Command window. 

Once successfully overridden, the Feed section of the G Code Status Window will display the custom feed rate in green. 

To cancel the feed rate, press Clear Override in the Feed Override menu, or Cancel All Options in the Auto Options menu. 


3.2.4.Rapid Override

Rapid Override

This function allows you to enter in a custom rapid rate for your program. The Control comes with preset suggested overrides of 150 IPM and 300 IPM. Select either of these, or enter in a custom value using the Custom Rapid Rate button. Once pressed, the Control will prompt you to enter in the desired rapid rate into the Enter Next Command window. The window will briefly turn blue if successfully overridden. 

To cancel the rapid override, press Clear Override in the Rapid Override menu, or Cancel All Options in the Auto Options menu. 

3.2.5.Rapid to Zero

Rapid to Zero

Press this key to easily rapid all axes to their zero positions.

3.3.Manual Data Input

Manual Data Input (MDI) 

The NXGEN is compatible with many of the familiar codes used on the Legacy control, and MDI accepts all different command inputs.  For example, the “M9” command orients the spindle, a G00 command moves the machine to a certain place, or the M3S500 command will start the spindle at 500 RPM.

To Enter MDI

There are three ways to begin MDI
1. Press the MDI key
2. Enter the command MD
3. Press the Space Bar

To Exit, press the MANUAL key

How to Use MDI

Enter in a desired command in the Enter Next Command and push enter.  The Start key will turn green, indicating that it is ready to proceed.  Push Start, and the machine will execute the move. Once executed, all the commands are displayed in their own line in the blue command screen.

Unique NXGEN MDI Features

The NXGEN comes with many new features that enhance the MDI functionality.

For example, if there a typo in your command, instead of having to retype the entire line, you can simply insert the key indicator into the line and correct the typo.

To enter in a command entered in previously, there are two options:

  1. Type the command again in the Enter Next Command Window and press Start
  2. Touch/click the desired command line in the blue command screen, and it will be reloaded in the Enter Next Command Window. Note that touching a previous command just loads it into the Enter Next Command Window; it does not start the command. Thus, the command can be edited if necessary, then executed.

Lines of code entered are retained until power off. If you exit MDI and return to MDI, the previous entries still in the history. You can also scroll through all the MDI data once the screen is filed.

Another useful feature is cutting and pasting code from a program. Once in the Program editor, highlight a line of code, press Ctrl-C to copy the line of code. Start MDI and press Ctrl-V to paste that line into MDI. Press ENTER to run that line of code.

3.4.Program Edit


The Edit key allows the operator to edit the program via a full featured editor, with features including file, search, view, and language settings. You can enter multiple instances of the same program, allowing you to look at both at the same time.

Programs can be edited at any time, even when the machine is running.

3.5.Return for Power Off

Return for Power Off

Pressing this button will move the slides to the Cold Start posing in preparation for Power Off.
Three options will then appear in the Options section:

  1. Shut Down NXGEN
    This exits the CNC Control and returns to the Windows Desktop.
  2. Shut Down Windows
    Shuts down everything in preparation for Power Off
  3. Cancel
    Aborts options 1 and 2

3.6.View Graphics

View Graphics

Select this key to switch to a graphic view of the loaded program. Note that a program must be loaded first before any graphics can be viewed.

Once in the graphic view, a new key called Move Graphics becomes available adjacent to the Status Window. Press this key to load a menu of selectors to move the graphic image, according to the following selectors.  This menu is also displayed in the CNC Program Window.

To stop moving graphics, select the Move Graphics key again. The key will turn blue, indicating that it is no longer active.

Arrow Keys ⭠⭡⭢⭣ Move part up, down, left, and right in the 2D plane.
Shift + Arrow Keys Rotate part in the 3D plane.
+/- Keys Zoom part in/out
1 Key Show Isometric view (default)
2 Key Show XY-Plane View
3 Key Show XZ-Plane View
4 Key Show YZ-Plane View
0 Key Reset the View to Default

4.Setup Mode

Setup Mode

The Setup Mode section of the Interface contains a series of functions used to set-up the tools offsets.


4.1.Get Next Tool

Get Next Tool

This key will automatically do the following to get the next tool in the spindle.

  1. Cancel JOG and turn off the spindle.
  2. Move the Z axis to the tool change position.
  3. Orientate the spindle and get the next tool in the TC carousel.

Once complete, the machine is ready to install the correct tool. Press JOG to establish the new tool length offset.

4.2.Get Specific Tool

Get Specific Tool

This button allows you to select a specific tool in the turret and load it into the spindle. Once selected, the Control will prompt you for the next desired tool number then preform the same operation as above to get that tool.

4.3.Set Length Offset

Set Length Offset

Select this button to set length offsets. This will bring up a selection of settings that are discussed below.

Press to select which length or diameter offset number to use for this tool.

Records the current Z axis position into the length offset table.

Press to see the table of tool offsets both diameter and length. Press the MANUAL key when finished reviewing the table and return to this option button page.


Press this key to quickly modify the length offset that was just recorded in the length offset table. The Control will prompt ENTER LENGTH INCREMENT in the Enter Next Command window.
This lets the operator modify the length offset by a gauge used to establish the length offset.
For example, if using a 1” gauge block, enter -1 to add that value to the length offset and set the length offset to the bottom of the gauge block.

4.4.Diameter Offset

Diameter Offset

Use this setting to set the diameter offset for the tool loaded in the spindle. The options are outlined below:

Press to select which length or diameter offset number to use for this tool

Press this key to quickly enter the diameter offset of the tool if using CRC.
You’ll see the prompt ENTER NEW DIAMETER.

Press this key to quickly enter the diameter offset of the tool if using Solid Modeling instead of Wire Frame graphics. This is the actual tool diameter for graphics, not related to the CRC diameter for cutter compensation.
You’ll see the prompt ENTER NEW DIAMETER.


See Tool Offset Table for more information.

Use this setting to quickly adjust the current diameter offset by entering the desired amount to adjust.
For Example:
IF using a .75” diameter offset, enter a value of -.001 to change the offset to .749

Adjusts the offset for the Rendered Diameter same as above.

Press to see the Tool Usage table that keeps track of the tool usage.
USED displays the total time used for each tool.
HR. MAX displays the maximum time for each tools usages,
Once the MAX time is exceeded, the operator is notified and prompted for three options:
1) Remind Me Later
2) Open Tool Time Menu
3) Reset Tool Times

See Tool Info Table for more information.

Press the MANUAL key when finished reviewing the table and return to this option button page.

4.5.Spindle Functions

Spindle Functions

This button is designed to be used as a quick access to changing spindle operations that normally would be done in MDI. While you can still use MDI, this setup option is available, except during AUTO and MDI

Pressing this key brings up the following Spindle Functions Menu.

Simply press the button and enter the desired spindle speed in the Enter Next Command window and press enter. The S-work is not required, just a number.  

Press this button and the spindle will stop and orient the spindle.
This operates like M19 in MDI but faster.

Turns the spindle on at the current RPM setting in the M3 direction.

Temporarily sets the Maximum programmable Spindle speed to the desired value. Enter in the desired value in the Enter Next Command window and press enter. This is in effect until reset or power off.

Retracts the spindle orientation locking mechanism.

Turns the spindle on at the current RPM setting in the M4 direction.

  • Other Tips:
    You can use the normal CNC88 speed override (for example, 500.2) to set the spindle RPM to 500 in high range.

4.6.Return Home

Return Home 

Press this button to move all axes to the current zero position. The speed is subject to the Feedrate Override Pot. The design is to provide the operator with the ability to easily slow and speed up the return to home moves.
If the Z is negative, the Z will move to zero first, then return the other axes to zero.
100% on the Feedpot provides rapid speed.



This section of the interface contains selectors that help establish and adjust machine and offset related settings.

We will discuss these buttons in detail below.

5.1.Offset Tables

Offset Tables

This button brings quick access to all offset tables, all described below.

5.1.1.Tool Offset Table


Displays 99 tool offsets settings
Touch or Click on any value you want to change then select NEW to enter a new value or select MODIFY to adjust a current value

Press to mass edit the length offsets. You are prompted the Starting and Ending tool number and the amount you want to add too all the tools.
This is a fast way to adjust all the length offsets after setting the lengths.

Select the offset number to enter both the Diameter and Length offset value then press Enter to input the values and the next entry will come up.

Press the MANUAL key when finished reviewing the table and return to Adjustment page.

5.1.2.Fixture Offset Tables


Displays 48 fixture offset settings
Touch or Click on any value you want to change then select NEW to enter a new value or select MODIFY to adjust a current value

Multiple Entry:
Select the offset number to enter both XYZAB value as #,# then press Enter to input the values and the next entry will come up.

Press the MANUAL key when finished reviewing the table and return to Adjustment page.

5.1.3.Tool Info Table


Press to see the Tool Usage table that keeps track of the tool usage.
USED displays the total time used for each tool.
HR. MAX displays the maximum time for each tools usages.
Once the MAX time is exceeded, the operator will be notified and prompted for three options:

  1. Remind Me Later
  2. Open Tool Time Menu
  3. Reset Tool Times

Press the MANUAL key when finished reviewing the table and return to Adjustment page.

5.2.Set Axes

Set Axes

This button works same as with the Command SETX SETY with the CNC 88.
SET H sets the current position for all axes.
SET SC Cancels previous SET axis and restore position zero to the Cold Start position.

5.3.Set Fixtures

Set Fixtures

Press to select which fixture offset number to adjust.

Stores the current position into the Selected Fixture Offset Table (X-Z Shown).


Short cut to the offset table for easy verification and adjustment. See Fixture Offset Table for more information. 

5.4.Set Turret Number

Set Turret Number

This function is similar to the SETTO command except it allows for a combination of settings. Here the operator can define, for example, that Tool 5 is in the spindle and the turret is at position 10. At the next tool change, the turret will move to #5, put the tool away in slot #5, then get the specified tool.

Press the button to define which tool is in the spindle.

Press the button to define which turret pocket is at the spindle load position.



This button brings up various functions for setting up, testing and maintaining the machine. All are discussed in this section.

After selecting a function, press the SERVICE button to return to the options menu.

5.5.1.SETP Settings

SETP Settings

Accesses the SETP.CFG file in the MACHINE SETTINGS folder that contains all the parameters that are specific to the machine and operator preferences. Access requires the same password used in the CNC 88.



This function brings up a Diagnostic window used by service support for serving the machine and control.



Pressing this button brings up a menu to adjust the backlash settings for all axes.
This functions same as the BL command, but is accessible directly from JOG.

To Set Backlash

To set a backlash for an axis, select the desired axis from the menu in the Options panel. This will bring up a dialouge box where you can enter in a backlash value for that axis between 0 – 0.003 Inches. Click “OK” and the backlash value will be saved.



Pressing this button actives the following Reset menu: 


Press this button to restart the NXGEN software.


Press this button to revert the NXGEN software to the power-on state.

5.5.5.Message Log

Message Log

Selecting this button opens the log of program warnings/errors and machine related messages. This is especially helpful to reference when having a problem loading a program.
The log stores the following data:

  • Date and Time
  • Reason
  • Data
  • Program Name
  • Block Number

5.5.6.Remote Support

Remote Support

Pressing this button activates the support link to the NXGEN office over the Internet.

5.5.7.Tool Changer

Tool Changer

Once activated (Green), the tool change operation goes into a Single Step type of mode that prompts the serviceman at each step of the Tool Change, helping diagnose any error.
This mode is canceled by pressing the button again and turning gray.

5.5.8.Internal Diagnostics

Internal Diagnostics

Pressing this button brings up a list of three internal diagnostics, all very helpful aids in examining Control function. Used for service and internal diagnostics by NXGEN, the widows below can be displayed anytime while the machine is running or not running

Pressing the Toggle All Windows key will bring up all three diagnostics at once.

NOTE: the Control will prompt the user for a passcode to access these diagnostics. Window

Diagnostic Window

This window displays Axis Position Error, software and motion control board diagnostics and status of integral software and hardware. Window

Watch Window

This window provides a wide range of information on the Control status:

  • Provides motor encoder information.
  • Voltage information from the Feed and Spindle override pots.
  • Status of integral software and hardware / Output Window

Input / Output Window

This window displays all the controls inputs and outputs in a LED style display. When you hover over the LED with the mouse pointer the description of the IO is displayed.

The LEDs that have a black box around them are outputs that control the Solid State relays on the 1100-1 and 1100-2 boards.

The output state can be changed by clicking on the LED. This provides a serviceman the means of actuating the Solid State Relay during servicing.

Clicking on an Input LED will generate an alarm message.



Displays the RI options that existed on the CNC 88. With the NXGEN you can use touch screen or the RI command to access this option page.

The 5 gray option buttons display “KEEP” OFFSETS, “KEEP” MEMORY, “KEEP” INFO or “KEEP” POSITIONS.

When you click on a option button, it will switch from “KEEP” to “ZERO”. Click again and it switches back.

Make the selections you want to clear then press the green REINITIALIZE button to proceed with clearing the selections.

5.6.Cold Start

Cold Start

Performs the Cold Start command at the current location.
Same as the CS command.

Press to first move to the current zero position of the Axis Display window then performs a Cold Start to locate the machine zero.

6.Work and Tool Offset Setup

Our work and tool offset setup is designed to be as quick and easy as possible to setup your parts.
To achieve this, we intergraded the setup function with JOG and designed it to easily work with a common Edge Finder, Haimer 3D-Sensor or a Probe (Table or Spindle).

Below shows the SETUP Tools highlighted in red. These tools are activated and made available in JOG.


Below shows the Main SETUP Tools Menu, with seven functions for quick and easy setting of the Fixture offsets and the Tool Length offsets.

6.1.The SETTINGS Button

Pressing the SETTINGS button brings up the Settings menu and shows the following buttons.

Press one of the four options according to below:

  • NEXT OFFSET to increment to the next Fixture Offset Number (1-48)
  • OFFSET NUMBER to enter a Fixture Offset number
  • PROBE ON/OFF to toggle the touch probe status
  • PROBE TIP DIA to enter a new diameter for Edge Finder or Probe. The setting Diameter setting can be made permanent using SETP

Press the FINISH button to return to the Main SETUP Tool Menu.

6.2.Function Buttons

The Function Buttons (top row) cover four handy calculations: CENTER, CORNER, MIDWAY, and ANGLE. We’ll cover them in this section and give an example of how to use them.

When active, the SETUP Tool Menus will display the current function in an enlarged, green cell as sampled below:

6.2.1.Circle Center

Pressing the CIRCLE CENTER button opens the function, ready to locate points.

See below for an example usage.


Pressing the CORNER button opens the function and provides four inside and four outside configurations, as displayed below:

Selecting the desired key will activate the function. Pictured below is the after pressing the upper left corner button for finding an outside, upper left corner position:

See below for an example usage.


Pressing the MIDWAY button opens the function and provides three configurations for locating the middle between positions in X, Y or both X and Y. This is commonly used for either inside a pocket or outside a rectangle.

Selecting the desired key will activate the function. Pictured below is the after pressing the upper left MIDWAY button for finding a midway position in the X axis.

See below for an example usage.


Pressing the ANGLE button opens the function and can provide the angle of a side defined by two points. This is used with G68 to rotate the program XY coordinate to synchronize with the actual part.

See below for an example usage.

6.2.5.Example Usage

The CENTER, CORNER, MIDWAY, and ANGLE functions operate the same. Below is an example finding the center of a circle using the CENTER function.

Press the CENTER Button.

Pressing the button shows the Circle function:

Computing the center XY location requires three XY points. To enter the points into the software and compute the desired Center, complete the following:

  1. JOG XY to the Point 1
  2. Press RECORD PNT 1 Button
  3. Repeat steps 1 and 2 for the remaining two XY Positions

The Data window on the left will show the stored positions when recorded.
After all points are stored, the Calculated Circle Center and Radius will automatically be displayed.

Press the FINISHED button when all positions have been recorded to store the computed value.

The below Info Request window will then appear. This prompt provides the opportunity to move to the computed XY position.

Options for moving to position:

  1. Press OK and the XY axes will feed to position at the current feed rate.
  2. Move Z to clearance.
    Enter a value in the data input to raise or lower the Z axis before moving to the XY position.
    Example: Enter 1.5 and press OK to rapid the Z axis up 1.5 inches before feeding to XY
    Enter a 0 value for no Z move.

If you do not want to move to the computed position, simply press Cancel.

Once either has been selected, the function is complete and will return to the Main SETUP Tool Menu. The computed value is stored.

6.3.Tool Length Offsets

Pressing the TOOL LENGTH button begins the function to set the Length Offsets (H1-H99).

One of two images will appear depending if a Touch Probe is ON or OFF.

Image below indicates that the Touch Probe is ON, and a Probe touch is required to store Z length.

Image below indicates that the Touch Probe is OFF, and the length setting will be using a manual Height gauge.

The RECORD OFFSET button is used to Record the Tool Length Offset when the tool is touching the Probe or the Height gauge.

The OFFSET NUMBER button is used to enter a length offset number (1-99).

The procedure for setting length offsets is as follows:

1) JOG the tool to the Table Probe or Height block.
2) Press the RECORD Z PROBE Button.
3) Press the GET NEXT TOOL button.
4) Repeat steps 1 and 3 as needed or FINISHED when completed.

6.3.1.Calibrating Height Block or Table Probe for Z Tool Length

The calibration process establishes the distance from the Probe or the Height block to the program Z0 Datum (see below diagrams).
Once established it can be saved in the SETP parameters for permanent use.

Calibration Procedure:

  1. Jog Tool to the Top of the Probe or Height block.
  2. Press RECORD Z PROBE button.
  3. Jog Tool to Program Z0 Datum.
  4. Press RECORD PART Z0 button.

The Calibration value will be added to the Z position when storing a value in the Tool Offset Table.
When using a Height Gauge such as a 1-2-3 block, the value is negative and increases the final tool offset value.
With the Table mounted probe (Renishaw TS-20), the value is positive and reduces the final tool offset value.

The PROBE ON/OFF button toggles the touch probe status. It is retained until power off.

The ENTER VALUE button allows you to manually enter a value. Note that the value could be from a previous setup or a different Height Gauge.

6.4.Z Fixture Offset

The Z Fixture function provides a quick and easy method to establish multiple Z fixture offsets.
The process uses the G54 offset value and creates G55-G59 (E2 – E48) with values adjusted relative to the G54 Offset.

For Example: With a G54 having a Z-1.000 value
   G55 is higher than G54 so G55 would be less negative than -1.000 by the difference in height between G54 and G55
   G56 would be more negative than -1.000
   G57 would be less negative than -1.000

Setting Procedure:

  1. Jog tool or indicator to the top of G54 surface and press SET Z RELATIVE.
  2. Jog to top of next Z fixture offset
  4. Press NEXT OFFSET
    Repeat process from step 2 until complete then press FINISHED.


7.NC Word Summary

NC Word Summary Definition
A A axis angular motion command (or optional Servo Coolant)
B B axis angular motion command
C C axis angular motion command
D Tool diameter offset
E Fixture offset
F Feed rate, or spindle speed for tapping
G Preparatory function
H Tool length offset or Length and diameter offset for Format 1
I X axis distance to arc center or Initial peck size for drilling (G73 G83) or X axis shift in boring cycle (G76) JY axis distance to arc center or Reducing value of the initial peck (G73, G83) or Y axis shift in boring cycle (G76)
J Y axis distance to arc center or Reducing value of the initial peck (G73, G83) or Y axis shift in boring cycle (G76)
K Z axis distance to arc center or Minimum peck size for drilling (G73, G83)
L Subroutine definition or call or Subprogram repeat function(M98) or Programmable data input function(G10) or Line repeat function or Fixed cycle repetitions
M Machine function code
N Program sequence number
O Program identification number
P Dwell time in milliseconds (G04) or Percentage factor for retracting feed on tapping cycles or Fixture and tool offset number (G10) or Subprogram number (M98) or Value for R0-R9 (G10) or Sequence/ line number jump (M99) or Feed distance before peck (G73 G83) or P1 with G17 Q to use B axis during mapping or Angular tolerance for Feed Forward
Q Peck size in drill cycles (G73, G83) or Thread lead in tapping cycles (G74, G75, G84) or Diameter for automatic tool diameter override (H99) or Scale factor for Flat Cam programming on the rotary table or Length tolerance to ignore Feed Forward
R Subroutine parameter input R0 through R9 R0 Plane for fixed cycle or Radius designation (circular interpolation, G2 & G3) or Tool offset value amount (G10) Parametric Variables R0, R1 – R9
S Spindle speed (RPM)
S.1 Set belt range to low
S.2 Set belt range to high
T Tool number selector for turret
V Variables in Macros (V1-V100)
X X axis motion command
Y Y axis motion command
Z Z axis motion command

8.Character Summary

Character Definition
0-9 Numerical digits
A-Z Alphabetical characters
% Program start or end, rewind to start
+ Plus, positive
Minus, negative
( Comment start (standard NC program), or Engraving text start (L9201 Fixed Subroutine), or Mathematical operator (Macro Programming)
. Decimal point
, Comma
EOB ENTER key, carriage return / line feed (ASCII 13,10)
* Comment start
/ Optional block skip
: Program identification number (Format 2)
# Macro Line Identification

9.G Codes

Preparatory Functions

Codes are divided into groups or families to distinguish which codes can function simultaneously in a program. Codes belonging to a similar group cannot function together. Codes from different families or groups can function together

EXAMPLE:    N11 G90 G0 G1 X1. F40.

The G0 and G1, from group A, cannot be programmed in the same line because they are both from the same group. The G90, from group F, can be with the G0 or the G1, if they were on separate lines, because it is from a different group

Exception: A G90 and G91 can appear on the same line. Each will affect the motion words to the right of the G90 or G91 codes.

EXAMPLE:    N14 G90 X5.321 G91 Y.25 G90

The X move will be made in absolute and the Y move will be made in incremental. The G90 at the end of the line places the machine back in absolute for the next line of the program.

Modal & Non Modal Functions

Modal: These codes remain in effect until modified or canceled by another modal code with the same group designation code letter.

Non Modal: These codes only affect the line in which they appear and do not cancel modal codes.

Code Group Designation Modal Non Modal Description
G0 A Yes Rapid Travel (Point-to-Point Positioning)
G1 A Yes * see note Linear Interpolation
G2 A Yes * see note Circular Interpolation Clockwise
G3 A Yes * see note Circular Interpolation Counterclockwise
Note: G2 and G3 cancel G0 and remain active until canceled by each other. With G2 or G3 active, a move without I, J, K, or R is considered linear (G1).
G4 B Yes Dwell
G5 A Yes Non Modal Rapid Travel
G8 D Yes Acceleration (No Feed Ramps)
G9 D Yes Deceleration (Feed Ramps & In-Position Check)
G10 I Yes Programmable Data Input
G15 C Yes YZ Circular plane with simultaneous A axis
G17 C Yes XY plane selection
G17.1 C* Yes AB word swap
G17.2 C Yes AB word swap cancel
G18 C Yes XZ plane selection
G19 C Yes YZ plane selection
G20 M Yes Check parameters for inches mode set in SETP
G21 M Yes Check parameters for metric mode set in SETP
G28 I Yes Return to current zero(set home) position
G28.1 I Yes Return from Jog Away
G29 I Yes Return from current zero (set home) position
G31 I Yes Probe touch function (Skip Function)
G31.1 I Yes Probe no touch function
G40 D Yes Cutter compensation canceled
G41 D Yes Cutter compensation left (climb)
G42 D Yes Cutter compensation right (conventional)
G43 J Yes Tool length compensation positive
G44 J Yes Tool length compensation negative
G45 I Yes Tool offset single expansion
G46 I Yes Tool offset single reduction
G47 I Yes Tool offset double expansion
G48 I Yes Tool offset double reduction
G49 J Yes Tool length offset cancel
G50 J Yes Ramp slope control cancel
G50.1 J Yes Mirror image cancel
G51 J Yes Ramp slope control
G51.1 J* Yes Mirror image
G51.2 J* Yes Tool Load Compensation
G51.3 J* Yes Axis Scaling
G52 I Yes Coordinate system shift
G53 I Yes Machine coordinate system
G54 O Yes Fixture offset 1 (E1)
G55 O Yes Fixture offset 2 (E2)
G56 O Yes Fixture offset 3 (E3)
G57 O Yes Fixture offset 4 (E4)
G58 O Yes Fixture offset 5 (E5)
G59 O Yes Fixture offset 6 (E6)
G66 C Yes Modal subroutine
G67 C Yes Modal subroutine cancel
G68 C Yes Rotation
G69 C Yes Rotation cancel
G70 M Yes Check parameters for inches mode set in SETP
G71 M Yes Check parameters for metric mode set in SETP
G73 E Yes Peck drill cycle
G74 E Yes Left hand tapping with compression holder
G74.1 E Yes Left hand Rigid tapping
G74.2 E Yes Prepare for Left hand Rigid tapping (optional)
G75 E Yes Tapping cycle with self-reversing head
G76 E Yes Fine bore cycle
G80 E Yes Fixed cycle cancel
G81 E Yes Spot drill cycle
G82 E Yes Counter bore cycle
G83 E Yes Deep hole drill cycle
G84 E Yes Right hand tapping with compression holder
G84.1 E Yes Right hand Rigid tapping
G84.2 E Yes Prepare for Right hand Rigid tapping (optional)
G85 E Yes Bore in, Bore out
G86 E Yes Bore in, Spindle off, Rapid out
G87 E Yes Bore in, Bore out
G88 E Yes Bore in, Dwell, Bore out
G89 E Yes Bore in, Dwell, Bore out
G90 F Yes Absolute programming
G91 F Yes Incremental programming
G91.1 P Yes High speed execution
G91.2 P Yes High speed execution cancel (Format 2 only)
G92 I Yes Programmed coordinate system preset
G93 K Yes Rotary axis 1/T feed rate specification
G94 K Yes Rotary axis DPM, IPM feed rate specification
G98 G Yes Return to initial plane after final Z
G99 G Yes Return to R0 plane after final Z

* Modal Code but not cancelled by similar group designation.

10.Default Code Status

The codes below are the default codes utilized by the control. They are in effect at power on, the beginning of program execution, when entering MDI, and after M2.

Reset: Format 1 will default to this status automatically. Format 2 will use this default status after the HO command is used. Use HO like a reset button when in the Format 2 mode. By typing the command HO then pressing the enter button, the control will go into the WAITING stage. At this point the control is reset. If it is desired to move to home, press the START button, if not, press the MANUAL button. The SU (Sum) command will reset and use the default status from the SETP parameters in both format 1 and 2.

G/M code At beginning of program, upon entering MDI, after M2 By reset only
G0 – P 1 2
G1 – P 1 2
G8 Format 2 2 (Unless G9 is used in Auto – Then by reset)
G9 Format 1 1
G17 – P 1 2
G18 – P 1 2
G19 – P 1 2
G40 1 & 2
G49 1 2
G50 1 2
G80 1 2
G67 1 & 2
G69 1 2
G98 1
M5 1 & 2
M9 1 & 2
M10 1 & 2
M47 1 2
M48 1 2
M96 – P 1 & 2
M97 – P 1 & 2

Note: The 1 indicates the code is in effect in Format 1. The 2 indicates the code is in effect in Format 2. The P indicates that these codes may be established by the parameters established with the SETP command.

11.M Functions

Below is a summary table of the M Functions used in this controller.

Modal: These codes remain in effect until canceled by another modal code.

Non Modal :These codes only affect the line in which they appear and do not cancel modal codes

Note: Some M Functions start with motion commanded in a line. Some M Functions start after motion has been completed.

Note: For M60 through M64 only, the use of a minus sign before the number (M-60) will cause the function to occur after motion. This allows the rotary motion and brake application prior to any fixed cycle execution.


Code Starts with Motion Starts after Motion Modal Non Modal Description
M0 Yes Yes Program stop
M1 Yes Yes Optional program stop
M2 Yes Yes End of program
M3 Yes Yes Spindle on clockwise
M3.1 Yes Yes Sub-Spindle on clockwise
M3.2 Yes Yes Return to Main Spindle
M4 Yes Yes Spindle on counterclockwise
M4.1 Yes Yes Sub-Spindle on counterclockwise
M4.2 Yes Yes Return to Main Spindle
M5 Yes Yes Spindle (and Sub-Spindle) stop
M6 Yes Yes Tool change
M7 Yes Yes Coolant 1 on
M7.1 Yes Yes Servo Coolant 1 on
M8 Yes Yes Coolant 2 on
M8.1 Yes Yes Servo Coolant 2 on
M9 Yes Yes Coolant / Servo Coolant 1 & 2 off
M10 Yes Yes Reciprocation cancel
M11 Yes Yes Reciprocate X axis
M12 Yes Yes Reciprocate Y axis
M13 Yes Yes Reciprocate Z axis
M14 Yes Yes Reciprocate A axis
M15 Yes Yes Reciprocate B axis
M16 Yes Yes Reciprocate C axis (VMC45 only)
M17 Yes End of subroutine(see M30)
M18 Yes Yes Cushman® or Erickson® indexer next step
M19 Yes Yes Spindle orient & lock
M20 Yes Yes General purpose indexer next step or Auto. Doors Close
M30 Yes End of all subroutines (see M17) or End of program (Format 2)
M31 Yes Exchange Pallets
M32 Yes Store and Load Pallet A
M32.1 Yes Store and Load Pallet A- Test
M33 Yes Store and Load Pallet B
M33.1 Yes Store and Load Pallet B – Test
M41 Yes Low RPM range
M42 Yes High RPM range Auto Hi/Low
M43 Yes High RPM range Manual change
M45 Yes Execute fixed cycle
M46 Yes Yes Positive approach activate
M47 Yes Yes Positive approach cancel
M48 Yes Yes Potentiometer control on
M48.1 Yes Yes Servo coolant override Pot on
M48.2 Yes Yes Pallet A Rotary override Pot on
M48.3 Yes Yes Pallet B Rotary override Pot on
M49 Yes Yes Potentiometer control off
M49.1 Yes Yes Servo coolant override Pot off
M49.2 Yes Yes Pallet A rotary override Pot off
M49.3 Yes Yes Pallet B rotary override Pot off
M60 Yes Yes A Axis Brake On
M61 Yes Yes A Axis Brake Off
M62 Yes Yes B Axis Brake On
M63 Yes Yes B Axis Brake Off
M64 Yes Activate MP8 Probe
M65 Yes Activate TS-20, TS-27 Probe
M66 Yes User Attached Device
M67 Yes User Attached Device
M68 Yes User Attached Device
M69 Yes User Attached Device
M80 Yes Automatic Doors Open
M81 Yes Automatic Doors Close (Optional)
M90 Yes Yes Default Gain Setting
M91 Yes Yes Normal Gain Setting
M92 Yes Yes Intermediate Gain Setting
M93 Yes Yes High Gain Setting
M94 Yes Yes Feed Forward Function
M94.1 Yes Yes Feed Rate Modification
M94.2 Yes Yes Advanced Feed Forward (Optional)
M95 Yes Yes Feed Forward Cancel
M95.1 Yes Yes Feed Rate Modification Cancel
M95.2 Yes Yes Advanced Feed Forward Cancel
M96 Yes Yes Intersectional CRC Cancel
M97 Yes Yes Intersectional CRC
M98 Yes Execute subprogram
M99 Yes End of subprogram or Line jump
Suggest Edit

Last Updated: June 23, 2022