AXIS is a graphical front-end for EMC2 which features a live preview and backplot. It is written in Python and uses Tk and OpenGL to display its user interface.

Figure 4.1. AXIS Window

To select AXIS as the front-end for EMC2, edit the .ini file. In the section [DISPLAY] change the DISPLAY line to read

DISPLAY = axis

Then, start EMC2 and select that ini file. The sample configuration sim/axis.ini is already configured to use AXIS as its front-end.

When you start AXIS, a window like the one in Figure [cap:AXIS-Window] is shown.

The AXIS window contains the following elements:

4.3.3. Graphical Display Area

4.3.3.1. Coordinate Display

In the upper-left corner of the program display is the coordinate display. It shows the position of the machine. To the left of the axis name, an origin symbol () is shown if the axis has been properly homed. To the right of the axis name, a limit symbol () is shown if the axis is on one of its limit switches.

To properly interpret these numbers, refer to the "Position:" indicator in the status bar. If the position is "Absolute", then the displayed number is in the machine coordinate system. If it is "Relative", then the displayed number is in the offset coordinate system. When the coordinates displayed are relative and an offset has been set, the display will include a cyan "machine origin" marker (). If the position is "Commanded", then it is the ideal position—for instance, the exact coordinate given in a G0 command. If it is "Actual", then it is the position the machine has actually been moved to. These values can differ for several reasons: Following error, dead band, encoder resolution, or step size. For instance, if you command a movement to X 0.0033 on your mill, but one step of your stepper motor is 0.00125, then the "Commanded" position will be 0.0033 but the "Actual" position will be 0.0025 (2 steps) or 0.00375 (3 steps).

4.3.3.2. Preview Plot

When a file is loaded, a preview of it is shown in the display area. Fast moves (such as those produced by the G0 command) are shown as green lines. Moves at a feed rate (such as those produced by the G1 command) are shown as solid white lines. Dwells (such as those produced by the G4 command) are shown as small "X" marks.

G0 (Rapid) moves prior to a feed move will not show up on the preview plot. Rapid moves after a T<n> (Tool Change) will not show on the AXIS preview until after a feed move. To turn either of these features off program a G1 without any moves prior to the G0 moves.

4.3.3.3. Program Extents

The "extents" of the program in each axis are shown. At each end, the least or greatest coordinate value is indicated. In the middle, the difference between the coordinates is shown. In Figure ( [cap:AXIS-Window]), the X extent of the file is from 0.00 to 6.92 inches, a total of 6.92 inches.

When some coordinates exceed the "soft limits" in the .ini file, the relevant dimension is shown in a different color and enclosed by a box. In Figure ( [cap:Soft-Limit]) the maximum soft limit is exceeded on the X axis as indicated by the box surrounding the coordinate value.

Figure 4.2. Soft Limit

4.3.3.4. Tool Cone

The location of the tip of the tool is indicated by the "tool cone". The cone does not indicate anything about the shape, length, or radius of the tool.

When a tool is loaded (for instance, with the MDI command T1M6 ), the cone changes to a cylinder which shows the diameter of the tool given in the tool table file.

4.3.3.5. Backplot

When the machine moves, it leaves a trail called the backplot. The color of the line indicates the type of motion: Yellow for jogs, faint green for rapid movements, red for straight moves at a feed rate, and magenta for circular moves at a feed rate.

4.3.3.6. Interacting

By left-clicking on a portion of the preview plot, the line will be highlighted in both the graphical and text displays. By left-clicking on an empty area, the highlighting will be removed.

By dragging with the left mouse button pressed, the preview plot will be shifted (panned).

By dragging with shift and the left mouse button pressed, or by dragging with the mouse wheel pressed, the preview plot will be rotated. When a line is highlighted, the center of rotation is the center of the line. Otherwise, the center of rotation is the center of the file as a whole.

By rotating the mouse wheel, or by dragging with the right mouse button pressed, or by dragging with control and the left mouse button pressed, the preview plot will be zoomed in or out.

By clicking one of the "Preset View" icons, or by pressing "V", several preset views may be selected.

4.3.4. Text Display Area

By left-clicking a line of the program, the line will be highlighted in both the graphical and text displays in blue.

When the program is running, the line currently being executed is highlighted in red. If no line has been selected by the user, the text display will automatically scroll to show the current line.

Figure 4.3. Current and Selected Lines

4.3.5. Manual Control

While the machine is turned on but not running a program, the items in the "Manual Control" tab can be used to move the machining center or turn different parts of it on and off.

When the machine is not turned on, or when a program is running, the manual controls are unavailable.

Many of the items described below are not useful on all machines. When AXIS detects that a particular pin is not connected in HAL, the corresponding item in the Manual Control tab is removed. For instance, if the HAL pin motion.spindle-brake is not connected, then the "Brake" button will not appear on the screen. If the environment variable AXIS_NO_AUTOCONFIGURE is set, this behavior is disabled and all the items will appear.

4.3.5.1. The "Axis" group

"Axis" allows you to manually move the machine. This action is known as "jogging". First, select the axis to be moved by clicking it. Then, click and hold the "+" or "-" button depending on the desired direction of motion. The first four axes can also be moved by the arrow keys (X and Y), PAGE UP and PAGE DOWN keys (Z) and the [ and ] keys (A).

If "Continuous" is selected, the motion will continue as long as the button or key is pressed. If another value is selected, the machine will move exactly the displayed distance each time the button is clicked or the key is pressed. By default, the available values are:

0.1000, 0.0100, 0.0010, 0.0001

See the Configure section of the Integrators Manual for more information on setting the increments.

4.3.5.2. Homing

If your machine has home switches and a homing sequence defined for all axes the button will read "Home All". The "Home All" button or the Ctrl-HOME key will home all axes using the homing sequence. Pressing the HOME key will home the current axis, even if a homing sequence is defined.

If your machine has home switches and no homing sequence is defined or not all axes have a homing sequence the button will read "Home" and will home the selected axis only. Each axis must be selected and homed separately.

If your machine does not have home switches defined in the configuration the "Home" button will set the current selected axis current position to be the absolute position 0 for that axis and will set the "is-homed" bit for that axis.

See the Integrators Manual for more information on homing.

4.3.5.3. Touch Off

By pressing "Touch Off" or the END key, the "G54 offset" for the current axis is changed so that the current axis value will be the specified value. Expressions may be entered using the rules for rs274ngc programs, except that variables may not be referred to. The resulting value is shown as a number.

Figure 4.4. Touch Off

4.3.5.4. Override Limits

By pressing "Override Limits", the machine will temporarily be allowed to jog off of a physical limit switch. This check box is only available if a limit switch is tripped.

4.3.5.5. The "Spindle" group

The buttons on the first row select the direction for the spindle to rotate: Counterclockwise, Stopped, Clockwise. Counterclockwise will only show up if the pin motion.spindle-reverse is in the hal file (it can be net trick-axis motion.spindle-reverse ). The buttons on the next row increase or decrease the rotation speed. The checkbox on the third row allows the spindle brake to be engaged or released. Depending on your machine configuration, not all the items in this group may appear. Pressing the spindle start button sets the "S" speed to 1.

4.3.5.6. The "Coolant" group

The two buttons allow the "Mist" and "Flood" coolants to be turned on and off. Depending on your machine configuration, not all the items in this group may appear.

4.3.6. MDI

MDI, allows G-code programs can be entered manually, one line at a time. When the machine is not turned on, or when a program is running, the MDI controls are unavailable.

Figure 4.5. The MDI tab

History

This shows MDI commands that have been typed earlier in this session.

MDI Command

This allows you to enter a g-code command to be executed. Execute the command by pressing Enter or by clicking "Go".

Active G-Codes

This shows the "modal codes" that are active in the interpreter. For instance, "G54" indicates that the "G54 offset" is applied to all coordinates that are entered. When in Auto the Active G-Codes represent the codes after any read ahead by the interpreter.

Almost all actions in AXIS can be accomplished with the keyboard. A full list of keyboard shortcuts can be found in the AXIS Quick Reference, which can be displayed by choosing Help > Quick Reference. Many of the shortcuts are unavailable when in MDI mode.

AXIS includes a program called "emctop" which shows some of the details of EMC’s state. You can run this program by invoking Machine > Show EMC Status

Figure 4.6. EMC Status Window

The name of each item is shown in the left column. The current value is shown in the right column. If the value has recently changed, it is shown on a red background.

AXIS includes a program called "MDI" which allows text-mode entry of MDI commands to a running EMC session. You can run this program by opening a terminal and typing

mdi /path/to/emc.nml

Once it is running, it displays the prompt MDI> . When a blank line is entered, the machine’s current position is shown. When a command is entered, it is sent to EMC to be executed.

This is a sample session of mdi.

$ mdi ~/emc2/configs/sim/emc.nml  +
MDI>  +
(0.0, 0.0, 0.0, 0.0, 0.0, 0.0) +
MDI> G1 F5 X1 +
MDI>  +
(0.5928500000000374, 0.0, 0.0, 0.0, 0.0, 0.0) +
MDI>  +
(1.0000000000000639, 0.0, 0.0, 0.0, 0.0, 0.0)

AXIS includes a program called "axis-remote" which can send certain commands to a running AXIS. The available commands are shown by running axis-remote ---help and include checking whether AXIS is running (---ping), loading a file by name, reloading the currently loaded file (---reload), and making AXIS exit (---quit).

EMC2 includes a userspace hal component called "hal_manualtoolchange", which shows a window (Figure [cap:The-Manual-Toolchange]) when a M6 command is issued. After the OK button is pressed, execution of the program will continue.

The HAL configuration file configs/sim/axis_manualtoolchange.hal shows the HAL commands necessary to use this component.

hal_manualtoolchange can be used even when AXIS is not used as the GUI. This component is most useful if you have presettable tools and you use the tool table.

Important Note: Rapids will not show on the preview after a T<n> is issued until the next feed move after the M6. This can be very confusing to most users. To turn this feature off for the current tool change program a G1 with no move after the T<n>.

Figure 4.7. The Manual Toolchange Window

AXIS includes several Python modules which may be useful to others. For more information on one of these modules, use "pydoc <module name>" or read the source code. These modules include:

To use these modules in your own scripts, you must ensure that the directory where they reside is on Python’s module path. When running an installed version of EMC2, this should happen automatically. When running "in-place", this can be done by using scripts/emc-environment.

By including the line

LATHE=1

in the [DISPLAY] section of the ini file, AXIS selects lathe mode. The "Y" axis is not shown in coordinate readouts, the view is changed to show the Z axis extending to the right and the X axis extending towards the bottom of the screen, and several controls (such as those for preset views) are removed.

Pressing "V" zooms out to show the entire file, if one is loaded.

When in lathe mode, the shape of the loaded tool (if any) is shown.

Figure 4.8. Lathe Tool Shape

For more information on ini file settings that can change how AXIS works see the INI File/Sections/[DISPLAY] Section of Configuration chapter in the Integrators manual.

4.11.1. Program Filters

AXIS has the ability to send loaded files through a "filter program". This filter can do any desired task: Something as simple as making sure the file ends with 'M2 ', or something as complicated as detecting whether the input is a depth image, and generating g-code to mill the shape it defines.

The [FILTER] section of the ini file controls how filters work. First, for each type of file, write a PROGRAM_EXTENSION line. Then, specify the program to execute for each type of file. This program is given the name of the input file as its first argument, and must write rs274ngc code to standard output. This output is what will be displayed in the text area, previewed in the display area, and executed by EMC when "Run". The following lines add support for the "image-to-gcode" converter included with EMC2:

[FILTER] +
PROGRAM_EXTENSION = .png,.gif Greyscale Depth Image +
png = image-to-gcode +
gif = image-to-gcode

It is also possible to specify an interpreter:

PROGRAM_EXTENSION = .py Python Script +
py = python

In this way, any Python script can be opened, and its output is treated as g-code. One such example script is available at nc_files/holecircle.py . This script creates g-code for drilling a series of holes along the circumference of a circle.

Figure 4.9. Circular Holes

If the environment variable AXIS_PROGRESS_BAR is set, then lines written to stderr of the form

FILTER_PROGRESS=%d

will set the AXIS progress bar to the given percentage. This feature should be used by any filter that runs for a long time.

xrdb -merge /usr/share/doc/emc2/axis_light_background

xrdb -merge /usr/share/doc/emc2/axis_big_dro

*Axis*optionLevel: widgetDefault

root_window.bind("<Control-q>", "destroy .") +
help2.append(("Control-Q", "Quit")) +
vars.show_distance_to_go.set(1)

Touchy requires you to create a file named "touchy.hal" in the same folder as your ini file to make these connections. Touchy executes the hal commands in this file after it has made its pins available for connection.

To use Touchy in the [DISPLAY] section of your ini file change the DISPLAY = touchy

Font Configuration is done on the Preferences Tab. Changes will be saved to the current computer in a hidden file.

TkEMC is one of the most traditional graphical front-ends for EMC. It is written in Tcl and uses the Tk toolkit for the display. Being written in TCL makes it very portable (runs on a multitude of platforms). A separate backplot window can be displayed as shown in Figure( [cap:TkEMC-Window]).

Figure 6.1. TkEMC Window

To select TkEMC as the front-end for EMC2, edit the .ini file. In the section [DISPLAY] change the DISPLAY line to read

DISPLAY = tkemc

Then, start EMC2 and select that ini file. The sample configuration sim/tkemc.ini is already configured to use TkEMC as its front-end.

When you start EMC2 with TkEMC, a window like the one in Figure [cap:TkEMC-Window] is shown.

The TkEMC window contains the following elements:

6.3.4. Automatic control

Figure 6.2. TkEMC Interpreter / program control

6.3.4.1. Buttons for control

The buttons in the lower part of TkEMC (seen in Figure [cap:TkEMC-Interpreter]) are used to control the execution of a program: “Open” to load a program, “Verify” to check it for errors, “Run” to start the actual cutting, “Pause” to stop it while running, “Resume” to resume an already paused program, “Step” to advance one line in the program and “Optional Stop” to toggle the optional stop switch (if the button is green the program execution will be stopped on any M1 encountered).

6.3.4.2. Text Program Display Area

When the program is running, the line currently being executed is highlighted in white. The text display will automatically scroll to show the current line.

6.3.5. Manual Control

6.3.5.1. Implicit keys

TkEMC allows you to manually move the machine. This action is known as “jogging”. First, select the axis to be moved by clicking it. Then, click and hold the “+” or “-” button depending on the desired direction of motion. The first four axes can also be moved by the arrow keys (X and Y), PAGE UP and PAGE DOWN keys (Z) and the [ and ] keys (A).

If “Continuous” is selected, the motion will continue as long as the button or key is pressed. If another value is selected, the machine will move exactly the displayed distance each time the button is clicked or the key is pressed. The available values are:

1.0000 0.1000 0.0100 0.0010 0.0001

By pressing “Home” or the HOME key, the selected axis will be homed. Depending on your configuration, this may just set the axis value to be the absolute position 0.0, or it may make the machine move to a specific home location through use of “home switches”. See the Integrators Manual for more information on homing.

By pressing “Override Limits”, the machine will temporarily be permitted to jog outside the limits defined in the .ini file. (Note: if “Override Limits” is active the button will be displayed using a red colour).

1. TkEMC Override Limits & Jogging increments example

6.3.5.2. The “Spindle ” group

The button on the first row select the direction for the spindle to rotate: Counterclockwise, Stopped, Clockwise. The buttons next to it allow the user to increase or decrease the rotation speed. The button on the second row allows the spindle brake to be engaged or released. Depending on your machine configuration, not all the items in this group may have an effect.

6.3.5.3. The “Coolant ” group

The two buttons allow the “Mist” and “Flood” coolants to be turned on and off. Depending on your machine configuration, not all the items in this group may appear.

6.3.6. Code Entry

Manual Data Input (also called MDI), allows G-code programs to be entered manually, one line at a time. When the machine is not turned on, and not set to MDI mode, the code entry controls are unavailable.

Figure 6.3. The Code Entry tab

6.3.6.1. MDI:

This allows you to enter a g-code command to be executed. Execute the command by pressing Enter.

6.3.6.2. Active G-Codes

This shows the “modal codes” that are active in the interpreter. For instance, “G54” indicates that the “G54 offset” is applied to all coordinates that are entered.

Almost all actions in TkEMC can be accomplished with the keyboard. Many of the shortcuts are unavailable when in MDI mode.

The most frequently used keyboard shortcuts are shown in Table [cap:Most-Common-Keyboard].

Figure 7.1. The Mini Graphical Interface

Mini was designed to be a full screen graphical interface. It was first written for the Sherline CNC but is available for anyone to use, copy, and distribute under the terms of the GPL copyright.

Rather than popup new windows for each thing that an operator might want to do, Mini allows you to display these within the regular screen. Parts of this chapter are copied from the instructions that were written for that mill by Joe Martin and Ray Henry.

Figure 7.2. Mini Display for a Running EMC

 The Mini screen is laid out in several sections. (See Figure
<<fig:startmini>> ) These include a menu across the top, a set of main
control buttons just below the menu and two rather large columns of
information that show the state of your machine and allow you to enter
commands or programs.

When you compare figure [fig:startmini] with figure [fig:runmini] you will see many differences. In the second figure

Once you start working with Mini you will quickly discover how easily it shows the conditions of the EMC and allows you to make changes to it.

The first row is the menu bar across the top. Here you can configure the screen to display additional information. Some of the items in this menu are very different from what you may be acustomed to with other programs. You should take a few minutes and look under each menu item in order to familiarize yourself with the features that are there.

The menu includes each of the following sections and subsections.

You will notice between the info menu and the help menu there are a set of four buttons. These are called check buttons because they have a small box that shows red if they have been selected. These four buttons, Editor, Backplot, Tools, and Offsets pop in each of these screens. If more than one pop-in is active (button shown as red) you can toggle between these pop-ins by right clicking your mouse.

Below the menu line is a horizontal line of control buttons. These are the primary control buttons for the interface. Using these buttons you can change mode from [MANUAL] to [AUTO] to [MDI] (Manual Data Input). These buttons show a light green background whenever that mode is active.

You can also use the [FEEDHOLD], [ABORT], and [ESTOP] buttons to control a programmed move.

7.4.1. MANUAL

This button or pressing <F3> sets the EMC to Manual mode and displays an abreviated set of buttons the operator can use to issue manual motion commands. The labels of the jog buttons change to match the active axis. Whenever Show_Mode_Full is active in in manual mode, you will see spindle and lube control buttons as well as the motion buttons. A keyboard <i> or <I> will switch from continuous jog to incremental jog. Pressing that key again will toggle the increment size through the available sizes.

Figure 7.3. Manual Mode Buttons

 A button has been added to designate the present position as the home
position. We felt that a machine of this type (Sherline 5400) would be
simpler to operate if it didn't use a machine home position. This
button will zero out any offsets and will home all axes right where
they are.

 Axis focus is important here. Notice (in figure  <<fig:startmini>>)
that in manual mode you see a line or 'groove'  around the X axis to
highlight its position display. This groove says
that X is the active axis. It will be the target for jog moves made
 with the 'plus' and 'minus'  jog buttons. You can change axis focus by
clicking on any other axis
display. You can also change axis focus in manual mode if you press its
name key on your keyboard. Case is not important here. [Y] or [y] will
shift the focus to the Y axis. [A] or [a] will shift the focus to the A
axis. To help you remember which axis will jog when you press the jog
buttons, the active axis name is displayed on them.

 The EMC can jog (move a particular axis) as long as you hold the
button down when it is set for 'continuous', or it can jog for a preset
distance when it is set for 'incremental' . You can also jog the active
axis by pressing the plus [+] or minus
[-] keys on the keyboard. Again, case is not important for keyboard
jogs. The two small buttons between the large jog buttons let you set
which kind of jog you want. When you are in incremental mode, the
distance buttons come alive. You can set a distance by pressing it with
the mouse. You can toggle between distances by pressing [i] or [I] on
the keyboard. Incremental jog has an interesting and often unexpected
effect. If you press the jog button while a jog is in progress, it will
add the distance to the position it was at when the second jog command
was issued. Two one-inch jog presses in close succession will not get
you two inches of movement. You have to wait until the first one is
complete before jogging again.

 Jog speed is displayed above the slider. It can be set using the
slider by clicking in the slider's open slot on the side you want it to
move toward, or by clicking on the [Default] or [Rapid] buttons. This
setting only affects the jog move while in manual mode. Once a jog move
is initiated, jog speed has no effect on the jog. As an example of
this, say you set jog mode to 'incremental'  and the increment to 1
inch. Once you press the [Jog] button it will
travel that inch at the rate at which it started.

7.4.2. AUTO

When the Auto button is pressed, or <F4> on the keyboard, the EMC is changed into that mode, a set of the traditional auto operation buttons is displayed, and a small text window opens to show a part program. During run the active line will be displayed as white lettering on a red background.

In the auto mode, many of the keyboard keys are bound to controls. For example the numbers above the querty keys are bound to feed rate override. The 0 sets 100%, 9 sets 90% and such. Other keys work much the same as they do with the tkemc graphical interface.

Figure 7.4. Auto Mode

Auto mode does not normally display the active or modal codes. If the operator wishes to check these, use menu Info → Active_G-Codes. This will write all modal codes onto the message scratch pad.

If abort or estop is pressed during a run a set of buttons displays to the right of the text that allows the operator to shift the restart line forward or backwards. If the restart line is not the last active line, it will be highlighted as white letters on a blue background. Caution, a very slow feed rate, and a finger poised over the pause button is advised during any program restart.

 The real heart of CNC machine tool work is the auto mode. Sherline's
auto mode displays the typical functions that people have come to
expect from the EMC. Along the top are a set of buttons which control
what is happening in auto mode. Below them is the window that shows the
part of the program currently being executed. As the program runs, the
active line shows in white letters on a red background. The first three
buttons, [Open], [Run], and [Pause] do about what you'd expect. [Pause]
will stop the run right where it is. The next button, [Resume], will
restart motion. They are like feedhold if used this way. Once [Pause]
is pressed and motion has stopped, [Step] will resume motion and
continue it to the end of the current block. Press [Step] again to get
the motion of the next block. Press [Resume] and the interpreter goes
back to reading ahead and running the program. The combination of
[Pause] and [Step] work a lot like single block mode on many
controllers. The difference is that [Pause] does not let motion
continue to the end of the current block. Feed rate Override ... can be
very handy as you approach a first cut. Move in quickly at 100 percent,
throttle back to 10% and toggle between [Feedhold] and 10% using the
pause button. When you are satisfied that you've got it right, hit the
zero to the right of nine and go.

 The [Verify] button runs the interpreter through the code without
initiating any motion. If Verify finds a problem it will stop the read
near the problem block and put up some sort of message. Most of the
time you will be able to figure out the problem with your program by
reading the message and looking in the program window at the
highlighted line. Some of the messages are not very helpful. Sometimes
you will need to read a line or two ahead of the highlight to see the
problem. Occasionally the message will refer to something well ahead of
the highlight line. This often happens if you forget to end your
program with an acceptable code like %, m2, m30, or m60.

There are two columns below the control line. The left side of the screen displays information of interest to the operator. There are very few buttons to press here.

The right column is a general purpose place to display and work. Here you can see the modal buttons and text entry or displays. Here you can view a plot of the tool path that will be commanded by your program. You can also write programs and control tools and offsets here. The modal screens have been described above. Each of the popin displays are described in detail below.

7.6.1. Program Editor

Figure 7.5. Mini Text Editor

The editor is rather limited compared to many modern text editors. It does not have undo nor paste between windows with the clipboard.These were eliminated because of interaction with a running program. Future releases will replace these functions so that it will work the way you’ve come to expect from a text editor. It is included because it has the rather nice feature of being able to number and renumber lines in the way that the interpreter expects of a file. It will also allow you to cut and paste from one part of a file to another. In addition, it will allow you to save your changes and submit them to the EMC interpreter with the same menu click. You can work on a file in here for a while and then save and load if the EMC is in Auto mode. If you have been running a file and find that you need to edit it, that file will be placed in the editor when you click on the editor button on the top menu.

7.6.2. Backplot Display

Figure 7.6. Minis Backplotter

 Backplot [Backplot] will show the tool path that can be viewed from a
chosen direction. '3-D' is the default. Other choices and controls are
displayed along the top and right side of the pop-in. If you are in the
middle of a cut when you press one of these control buttons the machine
will pause long enough to re-compute the view.

Along the right side of the pop-in there is a small pyramid shaped graphic that tries to show the angle you are viewing the tool path from. Below it are a series of sliders that allow you to change the angle of view and the size of the plot. You can rotate the little position angle display with these. They take effect when you press the [Refresh] button. The [Reset] button removes all of the paths from the display and readies it for a new run of the program but retains your settings for that session.

If backplot is started before a program is started, it will try to use some color lines to indicate the kind of motion that was used to make it. A green line is a rapid move. A black line is a feed rate move. Blue and red indicate arcs in counterclockwise and clockwise directions.

The backplotter with Mini allows you to zoom and rotate views after you have run your program but it is not intended to store a tool path for a long period of time.

7.6.3. Tool Page

The tool page is pretty much like the others. You can set length and diameter values here and they become effective when you press the [Enter] key. You will need to set up your tool information before you begin to run a program. You can’t change tool offsets while the program is running or when the program is paused.

Figure 7.7. Mini Tool Display

The [Add Tools] and [Remove Tools] buttons work on the bottom of the tool list so you will want to fill in tool information in decending order. Once a new tool has been added, you can use it in a program with the usual G-code commands. There is a 32 tool limit in the current EMC configuration files but you will run out of display space in Mini long before you get there. (Hint You can use menu → view → show popin full to see more tools if you need.)

7.6.4. Offset Page

The offset page can be used to display and setup work offsets. The coordinate system is selected along the left hand side of the window. Once you have selected a coordinate system you can enter values or move an axis to a teach position. .Mini Offset Display

 You can also teach using an edgefinder by adding the radius and length
to the offset_by widgets. When you do this you may need to add or
subtract the radius depending upon which surface you choose to touch
from. This is selected with the add or subtract radiobuttons below the
offset windows.

The zero all for the active coordinate system button will remove any offsets that you have showing but they are not set to zero in the variable file until you press the write and load file button as well. This write and load file button is the one to use when you have set all of the axis values that you want for a coordinate system.

A number of the bindings used with tkemc have been preserved with mini. A few of the bindings have been changed to extend that set or to ease the operation of a machine using this interface. Some keys operate the same regradless of the mode. Others change with the mode that EMC is operating in.

One of the features of Mini is that it displays any axis above number 2 as a rotary and will display degree units for it. It also converts to degree units for incremental jogs when a rotary axis has the focus.

The Mini Graphical Interface. Keystick is a minimal text based interface.

To use keystick change the DISPLAY ini file setting to:

DISPLAY = keystick

Keystick is very simple to use. In the MDI Mode you simply start typing the g code and it shows up in the bottom text area. The “?” key toggles help.

A CNC machine has many mechanical components that may be controlled or may affect the way in which control is exercised. This section describes the subset of those components that interact with the Interpreter. Mechanical components that do not interact directly with the Interpreter, such as the jog buttons, are not described here, even if they affect control.

The Interpreter interacts with several switches. This section describes the interactions in more detail. In no case does the Interpreter know what the setting of any of these switches is.

A tool file is required to use the Interpreter. The file tells which tools are in which carousel slots and what the length and diameter of each tool are.

The file consists of any number of header lines, followed by one blank line, followed by any number of lines of data. The header lines are ignored by the interpreter. It is important that there be exactly one blank line (with no spaces or tabs, even) before the data. The header line shown in Table [cap:Sample-Tool-File] describes the data columns, so it is suggested (but not required) that such a line always be included in the header.

Each data line of the file contains the data for one tool. The line may contain 4 or 5 elements (“mill format”) or 8 or 9 elements (“lathe format”).

The units used for the length and diameter are in machine units.

The lines do not have to be in any particular order. Switching the order of lines has no effect unless the same slot number is used on two or more lines, which should not normally be done, in which case the data for only the last such line will be used.

In emc, the location of the tool file is specified in the ini file. See the Integrator Manual for more details.

A tool file may have a mixture of “mill format” and “lathe format” lines, though usually the “lathe format” lines are only required for lathe-type tooling.

9.4.2. Lathe Format Tool Files

The “lathe format” of a tool file is shown in Table [cap:Lathe-Tool-File].

Table 9.2. Sample Tool File (lathe format)

Pocket	FMS	ZOFFSET	XOFFSET	DIA	FRONTANGLE	BACKANGLE	ORIENTATION
Comment
		1	1	0.0	0.0	0.1	95.0
155.0	1		2	2	0.5	0.5	0.1

The Pocket, FMS, DIA and Comment fields are as for mill format tool files. The ZOFFSET field is the same as the TLO field of mill format tool files. The DIA is also used by the AXIS gui display.

The XOFFSET field gives an offset for the X coordinate when tool length offsets are in effect.

The ORIENTATION field gives the orientation of the lathe tool, as illustrated in [cap:Tool-Orientations]. The red cross is the controlled point. See [sub:Controlled-Point].

The FRONTANGLE and BACKANGLE fields are used by some user interfaces to display a fancy representation of the lathe tool.

Figure 9.1. Tool Orientations

In the RS274/NGC language view, a machining center maintains an array of numerical parameters defined by a system definition (RS274NGC_MAX_PARAMETERS). Many of them have specific uses especially in defining coordinate systems. The number of numerical parameters can increase as development adds support for new parameters. The parameter array persists over time, even if the machining center is powered down. EMC2 uses a parameter file to ensure persistence and gives the Interpreter the responsibility for maintaining the file. The Interpreter reads the file when it starts up, and writes the file when it exits.

All parameters are avalible for use in G Code programs.

The format of a parameter file is shown in Table [cap:Parameter-File-Format]. The file consists of any number of header lines, followed by one blank line, followed by any number of lines of data. The Interpreter skips over the header lines. It is important that there be exactly one blank line (with no spaces or tabs, even) before the data. The header line shown in Table [cap:Parameter-File-Format] describes the data columns, so it is suggested (but not required) that that line always be included in the header.

The Interpreter reads only the first two columns of the table. The third column, "Comment," is not read by the Interpreter.

Each line of the file contains the index number of a parameter in the first column and the value to which that parameter should be set in the second column. The value is represented as a double-precision floating point number inside the Interpreter, but a decimal point is not required in the file. All of the parameters shown in Table [cap:Parameter-File-Format] are required parameters and must be included in any parameter file, except that any parameter representing a rotational axis value for an unused axis may be omitted. An error will be signalled if any required parameter is missing. A parameter file may include any other parameter, as long as its number is in the range 1 to 5400. The parameter numbers must be arranged in ascending order. An error will be signalled if not. Any parameter included in the file read by the Interpreter will be included in the file it writes as it exits. The original file is saved as a backup file when the new file is written. Comments are not preserved when the file is written.

A permissible line of input code consists of the following, in order, with the restriction that there is a maximum (currently 256) to the number of characters allowed on a line.

Any input not explicitly allowed is illegal and will cause the Interpreter to signal an error.

Spaces and tabs are allowed anywhere on a line of code and do not change the meaning of the line, except inside comments. This makes some strange-looking input legal. The line "G0X +0. 12 34Y 7" is equivalent to "G0 x+0.1234 Y7", for example.

Blank lines are allowed in the input. They are to be ignored.

Input is case insensitive, except in comments, i.e., any letter outside a comment may be in upper or lower case without changing the meaning of a line.

A line number is the letter N followed by an integer (with no sign) between 0 and 99999 written with no more than five digits (000009 is not OK, for example). Line numbers may be repeated or used out of order, although normal practice is to avoid such usage. Line numbers may also be skipped, and that is normal practice. A line number is not required to be used, but must be in the proper place if used.

A word is a letter other than N followed by a real value.

Words may begin with any of the letters shown in Table [cap:Words-and-their]. The table includes N for completeness, even though, as defined above, line numbers are not words. Several letters (I, J, K, L, P, R) may have different meanings in different contexts. Letters which refer to axis names are not valid on a machine which does not have the corresponding axis.

The following rules are used for (explicit) numbers. In these rules a digit is a single character between 0 and 9.

Notice that initial (before the decimal point and the first non-zero digit) and trailing (after the decimal point and the last non-zero digit) zeros are allowed but not required. A number written with initial or trailing zeros will have the same value when it is read as if the extra zeros were not there.

Numbers used for specific purposes in RS274/NGC are often restricted to some finite set of values or some to some range of values. In many uses, decimal numbers must be close to integers; this includes the values of indexes (for parameters and carousel slot numbers, for example), M codes, and G codes multiplied by ten. A decimal number which is supposed be close to an integer is considered close enough if it is within 0.0001 of an integer.

A numbered parameter is the pound character # followed by an integer between 1 and 5399. The parameter is referred to by this integer, and its value is whatever number is stored in the parameter.

A value is stored in a parameter with the = operator; for example "#3 = 15 " means "set parameter 3 to 15." A parameter setting does not take effect until after all parameter values on the same line have been found. For example, if parameter 3 has been previously set to 15 and the line "#3=6 G1 x#3 " is interpreted, a straight move to a point where x equals 15 will occur and the value of parameter 3 will be 6.

The # character takes precedence over other operations, so that, for example, "#1+2 " means the number found by adding 2 to the value of parameter 1, not the value found in parameter 3. Of course, #[1+2] does mean the value found in parameter 3. The # character may be repeated; for example ##2 means the value of the parameter whose index is the (integer) value of parameter 2.

The interpreter maintains a number of readonly parameters for a loaded tool:

Named parameters work like numbered parameters but are easier to read. All parameter names are converted to lower case and have spaces and tabs removed. Named parameters must be enclosed with < > marks.

#<named parameter here> is a local named parameter. By default, a named parameter is local to the scope in which it is assigned. You can’t access a local parameter outside of its subroutine - this is so that two subroutines can use the same parameter names without fear of one subroutine overwriting the values in another.

#<_global named parameter here> is a global named parameter. They are accessible from within called subroutines and may set values within subroutines that are accessible to the caller. As far as scope is concerned, they act just like regular numeric parameters. They are not stored in files.

Examples:

Notes:

The global parameters _a, _b, _c, … _z have been reserved for special use. In the future, they may provide access to the last Aword, Bword, Cword, etc.

Two global read only named parameters are available to check which version is running from G Code.

An expression is a set of characters starting with a left bracket [ and ending with a balancing right bracket ] . In between the brackets are numbers, parameter values, mathematical operations, and other expressions. An expression is evaluated to produce a number. The expressions on a line are evaluated when the line is read, before anything on the line is executed. An example of an expression is [1 + acos[0] - [#3 ** [4.0/2]]].

Binary operators only appear inside expressions. There are four basic mathematical operations: addition (+), subtraction (-), multiplication (*), and division (/). There are three logical operations: non-exclusive or (OR), exclusive or (XOR), and logical and (AND). The eighth operation is the modulus operation (MOD). The ninth operation is the "power" operation (** ) of raising the number on the left of the operation to the power on the right. The relational operators are equality (EQ), inequality (NE), strictly greater than (GT), greater than or equal to (GE), strictly less than (LT), and less than or equal to (LE).

The binary operations are divided into several groups according to their precedence. (see table [cap:Operator-Precedence]) If operations in different precedence groups are strung together (for example in the expression [2.0 / 3 * 1.5 - 5.5 / 11.0] ), operations in a higher group are to be performed before operations in a lower group. If an expression contains more than one operation from the same group (such as the first / and * in the example), the operation on the left is performed first. Thus, the example is equivalent to: [[[2.0 / 3] * 1.5] - [5.5 / 11.0]] , which is equivalent to to [1.0 - 0.5] , which is 0.5.

The logical operations and modulus are to be performed on any real numbers, not just on integers. The number zero is equivalent to logical false, and any non-zero number is equivalent to logical true.

A function is either "ATAN " followed by one expression divided by another expression (for example "ATAN[2]/[1+3]") or any other function name followed by an expression (for example "SIN[90] "). The available functions are shown in table [cap:Functions]. Arguments to unary operations which take angle measures (COS, SIN, and TAN ) are in degrees. Values returned by unary operations which return angle measures (ACOS, ASIN, and ATAN) are also in degrees.

The FIX function rounds towards the left (less positive or more negative) on a number line, so that FIX[2.8] =2 and FIX[-2.8] = -3, for example. The FUP operation rounds towards the right (more positive or less negative) on a number line; FUP[2.8] = 3 and FUP[-2.8] = -2, for example.

The EXISTS function checks for the existence of a single named parameter. It takes only one named parameter and returns 1 if it exists and 0 if it does not exist. It is an error if you use a numbered parameter or an expression.

A line may have any number of G words, but two G words from the same modal group (see Section [sec:Modal-Groups]) may not appear on the same line.

A line may have zero to four M words. Two M words from the same modal group may not appear on the same line.

For all other legal letters, a line may have only one word beginning with that letter.

If a parameter setting of the same parameter is repeated on a line, "#3=15 #3=6 ", for example, only the last setting will take effect. It is silly, but not illegal, to set the same parameter twice on the same line.

If more than one comment appears on a line, only the last one will be used; each of the other comments will be read and its format will be checked, but it will be ignored thereafter. It is expected that putting more than one comment on a line will be very rare.

The three types of item whose order may vary on a line (as given at the beginning of this section) are word, parameter setting, and comment. Imagine that these three types of item are divided into three groups by type.

The first group (the words) may be reordered in any way without changing the meaning of the line.

If the second group (the parameter settings) is reordered, there will be no change in the meaning of the line unless the same parameter is set more than once. In this case, only the last setting of the parameter will take effect. For example, after the line "#3=15 #3=6 " has been interpreted, the value of parameter 3 will be 6. If the order is reversed to "#3=6 #3=15" and the line is interpreted, the value of parameter 3 will be 15.

If the third group (the comments) contains more than one comment and is reordered, only the last comment will be used.

If each group is kept in order or reordered without changing the meaning of the line, then the three groups may be interleaved in any way without changing the meaning of the line. For example, the line "g40 g1 #3=15 (foo) #4=-7.0 " has five items and means exactly the same thing in any of the 120 possible orders (such as "#4=-7.0 g1 #3=15 g40 (foo)") for the five items.

Many commands cause the controller to change from one mode to another, and the mode stays active until some other command changes it implicitly or explicitly. Such commands are called "modal". For example, if coolant is turned on, it stays on until it is explicitly turned off. The G codes for motion are also modal. If a G1 (straight move) command is given on one line, for example, it will be executed again on the next line if one or more axis words is available on the line, unless an explicit command is given on that next line using the axis words or canceling motion.

"Non-modal" codes have effect only on the lines on which they occur. For example, G4 (dwell) is non-modal.

Modal commands are arranged in sets called "modal groups", and only one member of a modal group may be in force at any given time. In general, a modal group contains commands for which it is logically impossible for two members to be in effect at the same time - like measure in inches vs. measure in millimeters. A machining center may be in many modes at the same time, with one mode from each modal group being in effect. The modal groups are shown in Table [cap:Modal-Groups].

For several modal groups, when a machining center is ready to accept commands, one member of the group must be in effect. There are default settings for these modal groups. When the machining center is turned on or otherwise re-initialized, the default values are automatically in effect.

Group 1, the first group on the table, is a group of G codes for motion. One of these is always in effect. That one is called the current motion mode.

It is an error to put a G-code from group 1 and a G-code from group 0 on the same line if both of them use axis words. If an axis word-using G-code from group 1 is implicitly in effect on a line (by having been activated on an earlier line), and a group 0 G-code that uses axis words appears on the line, the activity of the group 1 G-code is suspended for that line. The axis word-using G-codes from group 0 are G10, G28, G30, and G92.

It is an error to include any unrelated words on a line with O- flow control.

Comments can be added to lines of G code to help clear up the intention of the programmer. Comments can be embedded in a line using parentheses () or for the remainder of a line using a semi-colon. The semi-colon is not treated as the start of a comment when enclosed in parentheses.

G0 (Rapid to start) X1 Y1 +
G0 X1 Y1 (Rapid to start; but don't forget the coolant) +
M2 ; End of program.

The interpreter and task are carefully written so that the only limit on part program size is disk capacity. The TkEMC and Axis interface both load the program text to display it to the user, though, so RAM becomes a limiting factor. In Axis, because the preview plot is drawn by default, the redraw time also becomes a practical limit on program size. The preview can be turned off in Axis to speed up loading large part programs. In Axis sections of the preview can be turned off using special comments.

Use at least 3 digits after the decimal when milling in millimeters, and at least 4 digits after the decimal when milling in inches. In particular, arc tolerance checks are made to .001 and .0001 depending on the active units.

G-code is most legible when at least one space appears before words. While it is permitted to insert white space in the middle of numbers, there is no reason to do so.

Center-format arcs (which use I- J- K- instead of R- ) behave more consistently than R-format arcs, particularly for included angles near 180 or 360 degrees.

When correct execution of your program depends on modal settings, be sure to set them at the beginning of the part program. Modes can carry over from previous programs and from the MDI commands.

As a good preventative measure, put a line similar to the following at the top of all your programs:

G17 G20 G40 G49 G54 G80 G90 G94

(XY plane, inch mode, cancel diameter compensation, cancel length offset, coordinate system 1, cancel motion, non-incremental motion, feed/minute mode)

Perhaps the most critical modal setting is the distance units—If you do not include G20 or G21, then different machines will mill the program at different scales. Other settings, such as the return mode in canned cycles may also be important.

Ignore everything in Section [sec:Order-of-Execution], and instead write no line of code that is the slightest bit ambiguous.

Don’t use and set a parameter on the same line, even though the semantics are well defined. Updating a variable to a new value, such as #1=[#1+#2] is ok.

Line numbers offer no benefits. When line numbers are reported in error messages, the numbers refer to the line number in the file, not the N-word value.

Because the meaning of an F-word in feed-per-minute mode varies depending on which axes are commanded to move, and because the amount of material removed does not depend only on the feed rate, it may be easier to use G93 inverse time feed mode to achieve the desired material removal rate.

You have seen how handy a tool length offset can be. Having this allows the programmer to ignore the actual tool length when writing a part program. In the same way, it is really nice to be able to find a prominent part of a casting or block of material and work a program from that point rather than having to take account of the location at which the casting or block will be held during the machining.

This chapter introduces you to offsets as they are used by the EMC. These include;

Regardless of any offsets that may be in effect, putting a G53 in a block of code tells the interpreter to go to the real or absolute axis positions commanded in the block. For example

g53 g0 x0 y0 z0

will get you to the actual position where these three axes are zero. You might use a command like this if you have a favorite position for tool changes or if your machine has an auto tool changer. You might also use this command to get the tool out of the way so that you can rotate or change a part in a vice.

G53 is not a modal command. It must be used on each line where motion based upon absolute machine position is desired.

Fixture Offsets. Work or fixture offset are used to make a part home that is different from the absolute, machine coordinate system. This allows the part programmer to set up home positions for multiple parts. A typical operation that uses fixture offsets would be to mill multiple copies of parts on multiple part holders or vises.

The values for offsets are stored in the VAR file that is requested by the INI file during the startup of an EMC. In our example below we’ll use G55. The values for each axis for G55 are stored as variable numbers.

5241    0.000000

5242    0.000000

5243    0.000000

5244    0.000000

5245    0.000000

5246    0.000000

In the VAR file scheme, the first variable number stores the X offset, the second the Y offset and so on for all six axes. There are numbered sets like this for each of the fixture offsets.

Each of the graphical interfaces has a way to set values for these offsets. You can also set these values by editing the VAR file itself and then restarting EMC so that the EMC reads the new values however this is not the recommended way. G10, G92, G28.1, etc are better ways to affect variables. For our example let’s directly edit the file so that G55 takes on the following values.

5241    2.000000

5242    1.000000

5243   -2.000000

5244    0.000000

5245    0.000000

5246    0.000000

You should read this as moving the zero positions of G55 to X = 2 units, Y= 1 unit, and Z = -2 units away from the absolute zero position.

Once there are values assigned, a call to G55 in a program block would shift the zero reference by the values stored. The following line would then move each axis to the new zero position. Unlike G53, G54 through G59.3 are modal commands. They will act on all blocks of code after one of them has been set. The program that might be run using figure [cap:Fixture-Offsets] would require only a single coordinate reference for each of the locations and all of the work to be done there. The following code is offered as an example of making a square using the G55 offsets that we set above.

G55 G0 x0 y0 z0

g1 f2 z-0.2000

x1

y1

x0

y0

g0 z0

g54 x0 y0 z0

m2

"But," you say, "why is there a G54 in there near the end." Many programmers leave the G54 coordinate system with all zero values so that there is a modal code for the absolute machine based axis positions. This program assumes that we have done that and use the ending command as a command to machine zero. It would have been possible to use g53 and arrive at the same place but that command would not have been modal and any commands issued after it would have returned to using the G55 offsets because that coordinate system would still be in effect.

(((G54)))G54     use preset work coordinate system 1

(((G55)))G55     use preset work coordinate system 2

(((G56)))G56     use preset work coordinate system 3

(((G57)))G57     use preset work coordinate system 4

(((G58)))G58     use preset work coordinate system 5

(((G59)))G59     use preset work coordinate system 6

G59.1(((G59.1)))   use preset work coordinate system 7

G59.2(((G59.2)))   use preset work coordinate system 8

G59.3(((G59.3)))   use preset work coordinate system 9

The way that it works has changed just a bit from the early days to the current releases. It should be thought of as a temporary offset that is applied to all other offsets.

 A user must understand the correct ways that the g92 values work. They
are set based upon the location of each axis when the g92 command is
invoked. The NIST document is clear that, "To make the  current point
have the coordinates" x0, y0, and z0 you would use g92
 x0 y0 z0. G92 'does not work from absolute machine coordinates'. It
works from 'current location'.

 G92 also works from current location as modified by any other offsets
that are in effect when the g92 command is invoked. While testing for
differences between work offsets and actual offsets it was found that a
g54 offset could cancel out a g92 and thus give the appearance that no
offsets were in effect. However, the g92 was still in effect for all
coordinates and did produce expected work offsets for the other
coordinate systems.

 It is likely that the absence of home switches and proper home
procedures will result in very large errors in the application of g92
values if they exist in the var file. Many EMC users do not have home
switches in place on their machines. For them home should be found by
moving each axis to a location and issuing the home command. When each
axis is in a known location, the home command will recalculate how the
g92 values are applied and will produce consistent results. Without a
home sequence, the values are applied to the position of the machine
when the EMC begins to run.

 Issuing g92 x y z a b c does in fact set values to the g92 variables
such that each axis takes on the value associated with its name. These
values are assigned to the current position of the machine axis. These
results satisfy paragraphs one and two of the NIST document.

 G92 commands work from current axis location and add and subtract
correctly to give the current axis position the value assigned by the
g92 command. The effects work even though previous offsets are in.

5211    0.000000

5212    0.000000

5213    0.000000

5214    0.000000

5215    0.000000

5216    0.000000

This sample engraving project mills a set of four .1 radius circles in roughly a star shape around a center circle. We can setup the individual circle pattern like this.

G10 L2 P1 x0 y0 z0 (ensure that g54 is set to machine zero)

g0 x-.1 y0 z0

g1 f1 z-.25

g3 x-.1 y0 i.1 j0

g0 z0

m2

We can issue a set of commands to create offsets for the four other circles like this.

G10 L2 P2 x0.5 (offsets g55 x value by 0.5 inch)

G10 L2 P3 x-0.5 (offsets g56 x value by -0.5 inch)

G10 L2 P4 y0.5 (offsets g57 y value by 0.5 inch)

G10 L2 P5 y-0.5 (offsets g58 y value by -0.5 inch)

We put these together in the following program.

(a program for milling five small circles in a diamond shape)

G10 L2 P1 x0 y0 z0 (ensure that g54 is machine zero)

G10 L2 P2 x0.5 (offsets g55 x value by 0.5 inch)

G10 L2 P3 x-0.5 (offsets g56 x value by -0.5 inch)

G10 L2 P4 y0.5 (offsets g57 y value by 0.5 inch)

G10 L2 P5 y-0.5 (offsets g58 y value by -0.5 inch)

g54 g0 x-.1 y0 z0 (center circle)

g1 f1 z-.25

g3 x-.1 y0 i.1 j0

g0 z0

g55 g0 x-.1 y0 z0 (first offset circle)

g1 f1 z-.25

g3 x-.1 y0 i.1 j0

g0 z0

g56 g0 x-.1 y0 z0 (second offset circle)

g1 f1 z-.25

g3 x-.1 y0 i.1 j0

g0 z0

g57 g0 x-.1 y0 z0 (third offset circle)

g1 f1 z-.25

g3 x-.1 y0 i.1 j0

g0 z0

g58 g0 x-.1 y0 z0 (fourth offset circle)

g1 f1 z-.25

g3 x-.1 y0 i.1 j0

g54 g0 x0 y0 z0

m2

Now comes the time when we might apply a set of G92 offsets to this program. You’ll see that it is running in each case at z0. If the mill were at the zero position, a g92 z1.0000 issued at the head of the program would shift everything down an inch. You might also shift the whole pattern around in the XY plane by adding some x and y offsets with g92. If you do this you should add a G92.1 command just before the m2 that ends the program. If you do not, other programs that you might run after this one will also use that g92 offset. Furthermore it would save the g92 values when you shut down the EMC and they will be recalled when you start up again.

The "Tool Table" is a text file that contains information about each tool. The file is located in the same directory as your configuration and is called "tool.tbl". The tools might be in a tool changer or just changed manually. The file can be edited with a text editor or be updated using G10 L1. See the Lathe Specifics Section for lathe tool table example. The maximum number of entries in the tool table is 56. The maximum tool and pocket number is 99999.

In general new tool table line format is:

Cutter Radius Compensation allows the programmer to program the tool path without knowing the exact tool diameter. The only caveat is the programmer must program the lead in move to be at least as long as the largest tool radius that might be used.

There are two possible paths the cutter can take while cutter radius compensation is on to the left or right side of a line when facing the direction of cutter motion from behind the cutter. To visualize this imagine you were standing on the part walking behind the tool as it progresses across the part. G41 is your left side of the line and G42 is the right side of the line.

The end point of each move depends on the next move. If the next move creates an outside corner the move will be to the end point of the compensated cut line. If the next move creates in an inside corner the move will stop short so to not gouge the part. The following figure shows how the compensated move will stop at different points depending on the next move.

Figure 14.2. Compensation End Point

14.3.1. Overview

14.3.1.1. Tool Table

Cutter radius compensation uses the data from the tool table to determine the offset needed. The data can be set at run time with G10 L1.

14.3.1.2. Programming Entry Moves

Any move that is long enough to perform the compensation will work as the entry move. The minimum lenght is the cutter radius. This can be a rapid move above the work piece. If several rapid moves are issued after a G41/42 only the last one will move the tool to the compensated position.

In the following figure you can see that the entry move is compensated to the right of the line. This puts the center of the tool to the right of X0 in this case. If you were to program a profile and the end is at X0 the resulting profile would leave a bump due to the offset of the entry move.

Figure 14.3. Entry Move

14.3.1.3. Z Motion

Z axis motion may take place while the contour is being followed in the XY plane. Portions of the contour may be skipped by retracting the Z axis above the part and by extending the Z-axis at the next start point.

14.3.1.4. Rapid Moves

Rapid moves may be programed while compensation is turned on.

14.3.1.5. Good Practices

• Start a program with G40 to make sure compensation is off.

14.3.2. Examples

14.3.2.1. Outside Profile

Figure 14.4. Outside Profile

14.3.2.2. Inside Profile

Figure 14.5. Inside Profile

Polar Coordinates can be used to specify the XY coordinate of a move. The @n is the distance and ^n is the angle. The advantage of this is for things like bolt hole circles which can be done very simply by moving to a point in the center of the circle, setting the offset and then moving out to the first hole then run the drill cycle. Polar Coordinates always are from the current XY zero position. To shift the Polar Coordinates from machine zero use an offset or select a coordinate system.

In Absolute Mode the distance and angle is from the XY zero position and the angle starts with 0 on the X Positive axis and rotates in a CCW direction about the Z axis. The code G1 @1^90 is the same as G1 Y1.

In Relative Mode the distance and angle is also from the XY zero position but it is cumulative. This can be confusing at first how this works in incremental mode.

For example if you have the following program you might expect it to be a square pattern.

F100 G1 @.5 ^90
G91 @.5 ^90
@.5 ^90
@.5 ^90
@.5 ^90
G90 G0 X0 Y0 M2

You can see from the following figure that the output is not what you might expect. Because we added .5 to the distance each time the distance from the XY zero position increased with each line.

Figure 15.1. Polar Spiral

The following code will produce our square pattern.

F100 G1 @.5 ^90
G91 ^90
^90
^90
^90
G90 G0 X0 Y0 M2

As you can see by only adding to the angle by 90 degrees each time the end point distance is the same for each line.

Figure 15.2. Polar Square

It is an error if:

G0 axes

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 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 radius compensation is active, the motion will differ from the above; see Section [sec:Cutter-Radius-Compensation].

If G53 is programmed on the same line, the motion will also differ; see Section [sub:G53:-Move-in].

It is an error if:

G1 axes

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 radius compensation is active, the motion will differ from the above; see Section [sec:Cutter-Radius-Compensation].

If G53 is programmed on the same line, the motion will also differ; see Section [sub:G53:-Move-in].

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 rotation occours. 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.

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

If cutter radius compensation is active, the motion will differ from what is described here. See Section [sec:Cutter-Radius-Compensation].

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

It is an error if:

`G2 or G3` `axes` `I- J-`

`G2 or G3` `axes` `I- K-`

`G2 or G3` `axes` `J- K-`

15.5.2. Examples

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

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

The code for the example:

G2 X1 Y1 I1 F10

Figure 15.3. 

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 g code for the following example:

G2 X0 Y1 I1 J0.5 F25
G3 X0 Y0 I1 J-0.5 F25

Figure 15.4. 

Here is an example of a center format command to mill a spiral arc:

That means to 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.

G2 or G3 I- J- K-

G4 P[seconds]

For a dwell, program G4 P- . This will keep the axes unmoving for the period of time in seconds specified by the P number.

It is an error if:

G5.1 Xn Yn I[X offset] J[Y offset]

G5.1 creates a quadratic B-spline in the XY plane with the X and Y axis only.

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.

Sample NURBs Code

G0 X0 Y0
F10
G5.2 X0 Y1 P1 L3
     X2 Y2 P1
     X2 Y0 P1
     X0 Y0 P2
G5.3
/ The rapid moves show the same path without the NURBs Block
G0 X0 Y1
   X2 Y2
   X2 Y0
   X0 Y0
M2

Figure 15.5. Sample NURBs Output

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 P[tool number] R[radius] X[offset] Y[offset] Z[offset] A[offset] B[offset] C[offset] U[offset] V[offset] W[offset] I[frontangle] J[backangle] Q[orientation]

Program a G10 L1 to set a tool table entry from a program or the MDI window. G10 L1 reloads the tool table.

It is an error if:

For more information on tool orientation see figure ( [cap:Tool-Orientations])

G10 L2 P[coordinate system] R[rotation about Z]

The coordinate system is described in Section [cha:Coordinate-System].

To set the origin of a coordinate system, program G10 L2 P- R- axes , where the P number is in the range 0 to 9. For the currently active coordinate system program P0. To specify a coordinate system program 1 to 9 corresponding to G54 to G59.3 . Optionally program R to indicate the rotation of the XY axis around the Z and all axis words are optional. The origin of the coordinate system specified by the P number is set to the given values (in terms of the not offset machine coordinate system). Only those coordinates for which an axis word is included on the line will be set. Being in incremental distance mode (G91) has no effect on G10 L2. The direction of rotation is CCW as viewed from the Top View.

Important Concepts:

It is an error if:

If a G92 origin offset was in effect before G10 L2, it will continue to be in effect afterwards.

The coordinate system whose origin is set by a G10 command may be active or inactive at the time the G10 is executed. If it is currently active, the new coordinates take effect immediately.

Examples:

G10 L10 P[tool number] R[radius] X[offset] Z[offset] Q[orientation]

G10 L10 is just like G10 L1 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:

G10 L20 P[coordinate system]

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 effects of having a plane selected are discussed in Section [sub:G2,-G3:-Arc] and Section [sub:G81-to-G89:]

Program G20 to use inches for length units.

Program G21 to use millimeters for lenght units.

It is usually a good idea to program either G20 or G21 near the beginning of a program before any motion occurs, and not to use either one anywhere else in the program.

G28 uses the values in parameters 5161-5166 as the absolute values to make a rapid traverse move to from the current position. The parameter values are in terms of the absolute coordinate system and the machine’s native coordinate system.

G28 axes will make a rapid traverse move to the position specified by axes , then will make a rapid traverse move to the predefined position in parameters 5161-5166.

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

It is an error if :

G30 uses the values in parameters 5181-5186 as the absolute values to make a rapid traverse move to from the current position. The parameter values are in terms of the absolute coordinate system and the machine’s native coordinate system.

G30 axes will make a rapid traverse move to the position specified by axes , then will make a rapid traverse move to the predefined position in parameters 5181-5186.

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

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

It is an error if :

G33 X- Y- Z- K-

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.

Note: K follows the drive line described by X- Y- Z- and is not parallel to the Z axis.

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

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

It is an error if:

G33.1 X- Y- Z- K-

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:

Example:

;move to starting position
G0 X1.000 Y1.000 Z0.100
;rigid tapping a 20 TPI thread
G33.1 Z-0.750 K0.05

Program G38.2 axes, G38.3 axes, G38.4 axes, or G38.5 axes to perform a straight probe operation. The axis words are optional, except that at least one of them must be used. The tool in the spindle must be a probe.

It is an error if:

In response to this command, the machine moves the controlled point (which should be at the end of the probe tip) 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.

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 probe failed, G38.2 and G38.4 will signal an error.

A comment of the form (PROBEOPEN filename.txt) will open filename.txt and store the 9-number coordinate consisting of X, Y, Z, A, B, C, U, V, W of each successful straight probe in it. The file must be closed with (PROBECLOSE).

Program G40 to turn cutter radius compensation off. The next move must be a straight move. It is OK to turn compensation off when it is already off.

It is an error if:

G41 or G42 D[tool]

G41 start cutter radius compensation to the left of the programmed line as viewed from the positive end of the axis perpendicular to the plane.

G42 start cutter radius 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 and can be a rapid move.

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

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

The behavior of the machining center when cutter radius compensation is on is described in Section [sec:Cutter-Radius-Compensation]

G41.1 or G42.1 D[diameter] <L[orientation]>

To turn cutter radius compensation on left, program G41.1 D- L-.

To turn cutter compensation on right, program G42.1 D- L-.

The D word specifies the cutter diameter. The L word specifies the cutter orientation, and defaults to 0 if unspecified. For more information on cutter orientation see Section ( [cap:Tool-Orientations]).

It is an error if:

To move in absolute coordinates from the machine origin, 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:

To select coordinate system 1, program G54, and similarly for other coordinate systems. The system-number-G-code pairs are: (1-G54), (2-G55), (3-G56), (4-G57), (5-G58), (6-G59), (7-G59.1), (8-G59.2), and (9-G59.3 ). The coordinate systems store the values for each system in the variables shown in the following table.

It is an error if:

See Section [cha:Coordinate-System] for an overview of coordinate systems.

G61 Exact Path Mode

G61.1 Exact Stop Mode

G64 Best Possible Speed

G64 P- (motion blending tolerance) Q- (naive cam tolerance)

G61 visits the programmed point exactly, even though that means temporarily coming to a complete stop.

G64 without P means to keep the best speed possible, no matter how far away from the programmed point you end up.

G64 P- Q- is a way to fine tune your system for best compromise between speed and accuracy. The P- tolerance means that the actual path will be no more than P- away from the programmed endpoint. The velocity will be reduced if needed to maintain the path. In addition, when you activate G64 P- Q- it turns on the "naive cam detector"; when there are a series of linear XYZ feed moves at the same feed rate that are less than Q- away from being collinear, they are collapsed into a single linear move. On G2/3 moves in the G17 (XY) plane when the maximum deviation of an arc from a straight line is less than the G64 P- tolerance the arc is broken into two lines (from start of arc to midpoint, and from midpoint to end). those lines are then subject to the naive cam algorithm for lines. Thus, line-arc, arc-arc, and arc-line cases as well as line-line benefit from the "naive cam detector". This improves contouring performance by simplifying the path. It is OK to program for the mode that is already active. See also Section [sub:Path-Control-Mode] for a discussion of these modes. If Q is not specified then it will have the same behavior as before and use the value of P-.

`G73 X- Y- Z- A- B- C- R- L- Q-`

The G73 cycle is intended for deep drilling or milling with chip breaking. The retracts in this cycle 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.

It is an error if:

`G76 P- Z- I- J- R- K- Q- H- E- L- `

It is an error if:

Figure 15.6. G76 Threading

Optional settings

Tapered entry and exit moves can be programmed using E- and L-.

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.

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.

The following example shows the result of running this G-Code:

G0 Z-.5 X .2
G76 P0.05 Z-1 I-.075 J0.008 K0.045 Q29.5 L2 E0.045

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.

Figure 15.7. Threading Example

Program G80 to ensure no axis motion will occur. It is an error if:

The canned cycles G81 through G89 are described in this section. Two examples are given with the description of G81 below.

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.

Rotational 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.

The G81 cycle is intended for drilling.

Example 1. Suppose the current position is (1, 2, 3) and the XY-plane has been selected, and the following line of NC code is interpreted.

G90 G81 G98 X4 Y5 Z1.5 R2.8

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 number and X position are 4. The Y number and Y position are 5. The Z number and Z position are 1.5. The R number and clear Z are 2.8. Old Z is 3. The following moves take place.

Example 2. Suppose the current position is (1, 2, 3) and the XY-plane has been selected, and the following line of NC code is interpreted.

G91 G81 G98 X4 Y5 Z-0.6 R1.8 L3

This calls for incremental distance mode (G91) and OLD_Z retract mode (G98) and calls for the G81 drilling cycle to be repeated three times. The X number is 4, the Y number is 5, the Z number is -0.6 and the R number 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 move is a traverse along the Z-axis to (1,2,4.8), 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).

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

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.

It is an error if:

This code is currently unimplemented in EMC2. It is accepted, but the behavior is undefined. See section [sec:G33,-G33.1:-Spindle-Synchronized]

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.

The spindle must be turning before this cycle is used. It is an error if:

This code is currently unimplemented in EMC2. It is accepted, but the behavior is undefined.

This code is currently unimplemented in EMC2. 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.

G90 is Absolute Distance Mode

G91 is Incremental Distance Mode

Interpretation of G Code can be in one of two distance modes: absolute or incremental.

To go into absolute distance mode, program G90 . In absolute distance mode, axis numbers (X, Y, Z, A, B, C, U, V, W) usually represent positions in terms of the currently active coordinate system. Any exceptions to that rule are described explicitly in this Section [sub:G81-to-G89:].

To go into incremental distance mode, program G91 . In incremental distance mode, axis numbers usually represent increments from the current coordinate.

G90.1 Absolute Distance Mode for I, J & K offsets.

G91.1 Incremental Distance Mode for I, J & K offsets.

G92 X- Y- Z- A- B- C- U- V- W-

See Section [cha:Coordinate-System] for an overview of coordinate systems.

See Section [sec:G92-Offsets] for more information on Offsets.

To make the current point have the coordinates you want (without motion), program G92 X- Y- Z- A- B- C- U- V- W- , 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. It is an error if:

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.

To reset axis offsets to zero, program G92.1 or G92.2. G92.1 sets parameters 5211 to 5219 to zero, whereas G92.2 leaves their current values alone.

To set the axis offset to the values saved in parameters 5211 to 5219, program G92.3.

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.

EMC2 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).

G93 is Inverse Time Mode

G94 is Units per Minute Mode

G95 is Units per Revolution Mode.

Three feed rate modes are recognized: units per minute, inverse time, and units per revolution. Program G94 to start the units per minute mode. Program G93 to start the inverse time mode. Program G95 to start the units per revolution mode.

In units per minute feed rate mode, an F word is interpreted to mean the controlled point should move at a certain number of inches per minute, millimeters per minute, or degrees per minute, depending upon what length units are being used and which axis or axes are moving.

In units per revolution mode, an F word is interpreted to mean the controlled point should move a certain number of inches per revolution of the spindle, depending on what length units are being used and which axis or axes are moving. G95 is not suitable for threading, for threading use G33 or G76.

In inverse time feed rate mode, an F word means the move should be completed in [one divided by the F number] minutes. For example, if the F number is 2.0, the move should be completed in half a minute.

When the inverse time feed rate mode is active, an F word must appear on every line which has a G1, G2, or G3 motion, and an F word on a line that does not have G1, G2, or G3 is ignored. Being in inverse time feed rate mode does not affect G0 (rapid traverse) motions.

It is an error if:

 G96 D[max spindle speed] S[units per minute] is Constant Surface Speed
Mode

G97 is RPM Mode

Two spindle control modes are recognized: revolutions per minute, and CSS (constant surface speed). Program G96 D- S- to select constant surface speed of S feet per minute (if G20 is in effect) or meters per minute (if G21 is in effect). The maximum spindle speed is set by the D- number in revolutions per minute. When using G96, ensure that X0 in the current coordinate system (including offsets and tool lengths) is the center of rotation or emc will not give the desired spindle speed. G96 is not affected by radius or diameter mode.

Program G97 to select RPM mode.

It is an error if:

When the spindle retracts during canned cycles, there is a choice of how far it retracts: (1) retract perpendicular to the selected plane to the position indicated by the R word, or (2) retract perpendicular to the selected plane to the position that axis was in just before the canned cycle started (unless that position is lower than the position indicated by the R word, in which case use the R word position).

To use option (1), program G99. To use option (2), program G98 . Remember that the R word has different meanings in absolute distance mode and incremental distance mode.

To pause a running program temporarily (regardless of the setting of the optional stop switch), program M0. EMC2 remains in the Auto Mode so MDI and other manual actions are not enabled.

To pause a running program temporarily (but only if the optional stop switch is on), program M1. EMC2 remains in the Auto Mode so MDI and other manual actions are not enabled.

It is OK to program M0 and M1 in MDI mode, but the effect will probably not be noticeable, because normal behavior in MDI mode is to stop after each line of input, anyway.

To exchange pallet shuttles and then stop a running program temporarily (regardless of the setting of the optional stop switch), program M60.

If a program is stopped by an M0, M1, or M60 , pressing the cycle start button will restart the program at the following line.

To end a program, program M2. To exchange pallet shuttles and then end a program, program M30. Both of these commands have the following effects.

No more lines of code in an RS274/NGC file will be executed after the M2 or M30 command is executed. Pressing cycle start will start the program back at the beginning of the file.

To start the spindle turning clockwise at the currently programmed speed, program M3.

To start the spindle turning counterclockwise at the currently programmed speed, program M4.

To stop the spindle from turning, program M5.

It is OK to use M3 or M4 if the spindle speed is set to zero. If this is done (or if the speed override switch is enabled and set to zero), the spindle will not start turning. If, later, the spindle speed is set above zero (or the override switch is turned up), the spindle will start turning. It is OK to use M3 or M4 when the spindle is already turning or to use M5 when the spindle is already stopped.

To turn mist coolant on, program M7.

To turn flood coolant on, program M8.

To turn all coolant off, program M9.

It is always OK to use any of these commands, regardless of what coolant is on or off.

To change the current tool number while in MDI or Manual mode program a M61 Qxx in the MDI window. One use is when you power up EMC with a tool currently in the spindle you can set that tool number without doing a tool change.

It is an error if:

To control a digital output bit, program M- P- , where the M-word ranges from 62 to 65, and the P-word ranges from 0 to a default value of 3. If needed the the number of I/O can be increased by using the num_dio parameter when loading the motion controller. See the Integrators Manual Configuration Section EMC and HAL section for more information.

The M62 & M63 commands will be queued. Subsequent commands referring to the same output number will overwrite the older settings. More than one output change can be specified by issuing more than one M62/M63 command.

The actual change of the specified outputs will happen at the beginning of the next motion command. If there is no subsequent motion command, the queued output changes won’t happen. It’s best to always program a motion g-code (G0, G1, etc) right after the M62/63.

M64 & M65 happen immediately as they are received by the motion controller. They are not synchronized with movement, and they will break blending.

To read the value of an analog or digital input pin, program M66 P- E- L- Q- , where the P-word and the E-word ranges from 0 to 3. If needed the the number of I/O can be increased by using the num_dio or num_aio parameter when loading the motion controller. See the Integrators Manual Configuration Section EMC and HAL section for more information.Only one of the P or E words must be present. It is an error if they are both missing.

M66 wait on an input stops further execution of the program, until the selected event (or the programmed timeout) occurs.

It is an error to program M66 with both a P-word and an E-word (thus selecting both an analog and a digital input).In EMC2 these inputs are not monitored in real time and thus should not be used for timing-critical applications.

To control an analog output synchronized with motion, program M67 E- Q- , where the E word ranges from 0 to the default maximum of 3 and Q is the value to set. The number of I/O can be increased by using the num_aio parameter when loading the motion controller. See the "EMC2 and HAL" chapter in the Configuration Section of the Integrators Manual for more information on the Motion Controller. M67 functions the same as M62-63. See the M62-65 section for information about queuing output commands synchronized with motion.

To control an analog output immediately, program `M68 E- Q-, ` where the E word ranges from 0 to the default maximum of 3 and Q is the value to set. The number of I/O can be increased by using the num_aio parameter when loading the motion controller. See the "EMC2 and HAL" chapter in the Configuration Section of the Integrators Manual for more information on the Motion Controller. M68 functions the same as M64-65. See the M62-65 section for information about immediate output commands.

To invoke a user-defined command, program M1nn P- Q- where P- and Q- are both optional and must be a number. The external program "M1nn" must be in the directory named in [DISPLAY]PROGRAM_PREFIX in the ini file and is executed with the P and Q values as its two arguments. Execution of the RS274NGC file pauses until the invoked program exits. Any valid executable file can be used.

The error "Unknown M code used" denotes one of the following

For example to open and close a collet closer that is controlled by a paraport pin using a bash script file using M101 and M102. Create two files called M101 and M102. Set them as executable files (typically right click/properties/permissions) before running EMC2. Make sure the paraport pin is not connected to anything in a hal file.

M101 (file name)

#!/bin/sh
# file to turn on paraport pin 14 to open the collet closer
halcmd setp parport.0.pin-14-out True
exit 0

M102 (file name)

#!/bin/sh
# file to turn off paraport pin 14 to open the collet closer
halcmd setp parport.0.pin-14-out False
exit 0

To pass a variable to a M1nn file you use the P and Q option like this

M100 P123.456 Q321.654

In your M100 file it might look like this:

#!/bin/sh
voltage=$1
feedrate=$2
halcmd setp thc.voltage $voltage
halcmd setp thc.feedrate $feedrate
exit 0

Subroutines extend from a O- sub to an O- endsub . The lines inside the subroutine (the "body") are not executed in order; instead, they are executed each time the subroutine is called with O- call.

O100 sub (subroutine to move to machine home)
G0 X0 Y0 Z0
O100 endsub
(many intervening lines)
O100 call

Inside a subroutine, O- return can be executed. This immediately returns to the calling code, just as though O- endsub was encountered.

O- call takes up to 30 optional arguments, which are passed to the subroutine as #1, #2 , …, #N. Parameters from #N+1 to #30 have the same value as in the calling context. On return from the subroutine, the values of parameters #1 through #30 (regardless of the number of arguments) will be restored to the values they had before the call. Parameters #1 - #30 are local to the subroutine.

Because "1 2 3 " is parsed as the number 123, the parameters must be enclosed in square brackets. The following calls a subroutine with 3 arguments:

O200 call [1] [2] [3]

Subroutine bodies may not be nested. They may only be called after they are defined. They may be called from other functions, and may call themselves recursively if it makes sense to do so. The maximum subroutine nesting level is 10.

Subroutines do not have "return values", but they may change the value of parameters above #30 and those changes will be visible to the calling code. Subroutines may also change the value of global named parameters.

The "while loop" has two structures: while/endwhile, and do/while. In each case, the loop is exited when the "while" condition evaluates to false.

(draw a sawtooth shape)
F100
#1 = 0
O101 while [#1 lt 10]
G1 X0
G1 Y[#1/10] X1
#1 = [#1+1]
O101 endwhile

Inside a while loop, O- break immediately exits the loop, and O- continue immediately skips to the next evaluation of the while condition. If it is still true, the loop begins again at the top. If it is false, it exits the loop.

The "if" conditional executes one group of statements if a condition is true and another if it is false.

(Set feed rate depending on a variable)
O102 if [#2 GT 5]
F100
O102 else
F200
O102 endif

The "repeat" will execute the statements inside of the repeat/endrepeat the specified number of times. The example shows how you might mill a diagonal series of shapes starting at the present position.

(Mill 5 diagonal shapes)
G91 (Incremental mode)
O103 repeat [5]
... (insert milling code here)
G0 X1 Y1 (diagonal move to next position)
O103 endrepeat
G90 (Absolute mode)

The O-number may be given by a parameter or calculation.

O[#101+2] call

In O-words, Parameters (section [sub:Numbered-Parameters]), Expressions (section [sub:Expressions]), Binary Operators (section [sub:Binary-Operators]) and Functions (table [cap:Functions]) are particularly useful.

To call a separate file with a subroutine name the file the same as your call and include a sub and endsub in the file. The file must be in the directory pointed to by PROGRAM_PREFIX. The file name can include lowercase letters, numbers, dash, and underscore only.

o<myfile> call (a named file)

or

o123 call (a number file)

In the called file you must include the oxxx sub and endsub and the file must be a valid file.

myfile.ngc
o<myfile> sub
...
o<myfile> endsub
M2

To set the feed rate, program F<n> where "n" is a number. The application of the feed rate is as described in Section [sub:Feed-Rate], unless inverse time feed rate mode is in effect, in which case the feed rate is as described in Section [sub:G93,-G94:-Set].

To set the speed in revolutions per minute (rpm) of the spindle, program S- . The spindle will turn at that speed when it has been programmed to start turning. It is OK to program an S word whether the spindle is turning or not. If the speed override switch is enabled and not set at 100%, the speed will be different from what is programmed. It is OK to program S0; the spindle will not turn if that is done.

It is an error if:

As described in Section [sub:G84:-Right-Hand-Tapping], if a G84 (tapping) canned cycle is active and the feed and speed override switches are enabled, the one set at the lower setting will take effect. The speed and feed rates will still be synchronized. In this case, the speed may differ from what is programmed, even if the speed override switch is set at 100%.

To select a tool, program T<n> , where the <n> number is the carousel slot for the tool. The tool is not changed until an M6 is programmed (see Section [sub:M6:-Tool-Change]). The T word may appear on the same line as the M6 or on a previous line. It is OK, but not normally useful, if T words appear on two or more lines with no tool change. The carousel may move a lot, but only the most recent T word will take effect at the next tool change. It is OK to program T0 ; no tool will be selected. This is useful if you want the spindle to be empty after a tool change.

It is an error if:

On some machines, the carousel will move when a T word is programmed, at the same time machining is occurring. On such machines, programming the T word several lines before a tool change will save time. A common programming practice for such machines is to put the T word for the next tool to be used on the line after a tool change. This maximizes the time available for the carousel to move.

Rapid moves after a T<n> will not show on the AXIS preview until after a feed move. This is for machines that travel long distances to change the tool like a lathe. This can be very confusing at first. To turn this feature off for the current tool change program a G1 without any move after the T<n>.

Printable characters and white space inside parentheses is a comment. A left parenthesis always starts a comment. The comment ends at the first right parenthesis found thereafter. Once a left parenthesis is placed on a line, a matching right parenthesis must appear before the end of the line. Comments may not be nested; it is an error if a left parenthesis is found after the start of a comment and before the end of the comment. Here is an example of a line containing a comment: "G80 M5 (stop motion)". Comments do not cause a machining center to do anything.

A comment contains a message if "MSG, " appears after the left parenthesis and before any other printing characters. Variants of "MSG, " which include white space and lower case characters are allowed. The rest of the characters before the right parenthesis are considered to be a message. Messages should be displayed on the message display device. Comments not containing messages need not be displayed there.

A comment can also be used to specify a file for the results of G38.x probing. See section [sub:G38.2:-Straight-Probe].

Often, general logging is more useful than probe logging. Using general logging, the format of the output data can be controlled.

General Logging