Menus ----- File->Run... : prompts for an NC program to run. You need to be in Auto mode, or you'll get an error. File->Reset : resets the interpreter. The modal G and M codes are set to their defaults. File->Quit : quits the Tkemc graphical application. The controller will also shut down. View->Tools : shows the tool table. You can edit the table. Selecting the Done button will save the table and reload it into the controller. Note that Tab and Return affect the text, so you have to click the Done button with the mouse. View->Offsets and Variables : shows the interpreter parameters, which hold the work offsets and user variables. You can edit the file. Selecting the Done button will save the file and reload it into the controller. Note that Tab and Return affect the text, so you have to click the Done button with the mouse. Settings->Relative Display, Actual Display : sets the display to show positions as relative to the current work offset, or in absolute machine coordinates. In relative display mode, the work offsets are shown also. Settings->Actual Position, Commanded Position : sets the display to show either the actual position of the axes, as reported by their feedback, or the commanded position, which is where the controller is commanding them to go. Help->Help... : brings up this help window. Help->About... : brings up a credits window. Status Command Buttons ---------------------- The buttons in the next two rows are labeled according to the current EMC status. Click on them to pop up menus that send commands to the EMC. The labels on these buttons will change to reflect the new status. ON/ESTOP-RESET/ESTOP : changes the power state of the machine. At startup the machine is in ESTOP. Selecting Estop Reset will enable the estop circuitry, but the servos will not yet be enabled. Selecting Machine On will enable the servos. Selecting Machine Off will disable the servos. Selecting Estop at any time will return the machine to the initial estopped state. Function keys F1 and F2 will toggle the states of the estop and servo systems, respectively. The Function Keys are listed completely below. (!) SAFETY NOTE: ESTOP will put the machine into the estopped state, but should not be relied on for this action in the event of an emergency. Always use the hardware estop to assure physical disabling of the machine. MANUAL/AUTO/MDI : changes the execution mode of the machine. Manual mode allows the operator to jog and home the axes, and control the coolant and spindle. Auto mode allows the operator to load programs into the machine, run them, and pause/step/resume them. Manual Data Input (MDI) mode allows the operator to type in blocks of NC code interactively. Function key F3 puts the controller into manual mode. F4 puts the controller into Auto mode. F5 puts the controller into MDI mode. MIST ON/OFF, FLOOD ON/OFF : turns mist or flood coolant on or off. Function key F7 toggles the state of the mist coolant; F8 toggles the flood coolant. These buttons and function keys only work in Manual mode. SPINDLE FORWARD/REVERSE/OFF : turns the spindle on forward, reverse, or off. Function key F9 turns the spindle on forward if it's off, or off if it's on. F10 turns the spindle on reverse if it's off, or off it it's on. These buttons and function keys only work in Manual mode. The speed of the spindle can be decreased or increased using the < and > buttons to the left and right of the spindle control button, respectively. F11 and F12, while pressed, decrease or increase the spindle speed, respectively, until they are released. These buttons and function keys work in manual, auto, or MDI mode. They are not active when the spindle is off. BRAKE ON/OFF : puts the spindle brake on, or releases it. This can be used to manually operate the spindle brake for maintenance or tramming operations. The 'B' and 'b' key, in manual mode, ABORT : stops all motion and any program that is running. The Escape key accomplishes the same result. Use ABORT or the Escape key to stop machine motions while testing programs. (!) NOTE: ABORT will not affect the estop state of the machine. Tool and Tool Offset -------------------- At the left, below the command buttons, is a display of the currently loaded tool and the tool offset, if any. A value of 0 for the Tool means that no tool is in the spindle. The offset is non-zero if a tool length offset is active. Position Display Options and Work Offsets ----------------------------------------- At the right, below the command buttons, is a display showing how to interpret the position numbers. There are two sources of position feedback, either Commanded or Actual. Commanded numbers are what the motion system asks for, and is not necessarily what the machine axes positions are (servo lag may mean they are different). Actual numbers reflect the current position of the axes. Normally, actual numbers are what you want. In some cases, for example running a program in simulation with the axes inhibited or disconnected, commanded numbers are what you want. Position numbers can also be Absolute or Relative. Absolute numbers are not affected by any work offsets in a program. They are relative to the machine home position. Relative numbers include any work offset. If Relative numbers are selected, the applicable Work Offsets are shown. To change these settings, use the '@' key for Commanded/Actual, and the '#' key for Absolute/Relative. The default values can be set in the INI file, e.g., [DISPLAY] POSITION_OFFSET = RELATIVE POSITION_FEEDBACK = ACTUAL or [DISPLAY] POSITION_OFFSET = ABSOLUTE POSITION_FEEDBACK = COMMANDED Axis Positions -------------- Axis positions are displayed in a large font in the middle of the display. The values are interpreted in units, commanded/actual, and absolute/relative, as described above. The color of the numbers shows the state of each axis. Yellow numbers mean the axis has not yet been homed. Green numbers mean the axis has been homed and is within limits. Red numbers mean the axis is at a soft or hard limit. Axis Command Buttons -------------------- Below the axis position numbers is a row of command buttons that affect axis motion. The Axis Speed setting, displayed in units/minute, can be changed by clicking and holding the < or > buttons until the desired setting is reached. The Increment button shows the current value of the jog increment, or "continuous" for continuous jogging. Clicking on this button brings up a menu that changes the jog increment or selects continuous jogging. The Axis Motion buttons jog an axis in the negative direction using the "-" button, positive direction using the "+" button, or home the axis using the "home" button. The Feed Override value in percent is displayed, and can be changed by clicking and holding the < or > buttons until the desired setting is reached. Manual Data Input (MDI) Box --------------------------- Below the axis command buttons is an input box labeled "MDI:" that is active when the machine is in manual data input (MDI) mode. You can type NC code statements into this box, and hit Enter to send the command. Note that many of the function and alphanumeric accelerator keys don't work as accelerator keys, so that they can be used to compose MDI statements. Keys F1-F5 (estop state and manual/auto/mdi mode), and F11-F12 (spindle speed control) do work; others do not. Below the MDI box is a display of the current modal settings for G, M, F, and S codes. These are only valid when in MDI mode. In Auto mode, they hold the modal values up to the point where the interpreter has read, usually far ahead of the executing line in the program. They do, however, always show the modal groups that are applicable when you next enter an MDI line. Program Display --------------- At the bottom of the main screen is a label showing the current program, or the last program loaded. Below this is a row of command buttons to Open, Run, Pause, Resume, or Step the program. The Open button is identical to the File->Open... menu at the top, as is the 'o' or 'O' accelerator. The run, pause, resume, and step accelerators are 'r', 'p', 's', and 'a', respectively, lower or upper case. The window at the bottom shows a few lines of text of the currently loaded program. The display window is moved through the program so that the currently executing line is always at the top. Function and Accelerator Keys ----------------------------- Escape abort motion <-| F1 toggle estop/estop reset state | F2 toggle machine off/machine on state |- work in MDI mode also F3 manual mode | F4 auto mode | F5 MDI mode <-| F6 reset interpreter F7 toggle mist on/mist off F8 toggle flood on/flood off F9 toggle spindle forward/off F10 toggle spindle reverse/off F11 decrease spindle speed <-|- work in MDI mode also F12 increase spindle speed <-| x select X axis y select Y axis z select Z axis Left, Right Arrow jog X axis Up, Down Arrow jog Y axis Page Up, Down jog Z axis Home home selected axis <, > decrement or increment axis speed c/C select continuous jogging i/I select incremental jog, and toggle through increments 1-9,0 set feed override to 10%-90%, 0 is 100% @ toggle commanded/actual position display # toggle absolute/relative position display o/O open a program r/R run an opened program p/P pause an executing program s/S resume a paused program a/A step one line in a paused program b take spindle brake off Alt-b put spindle brake on Note that MDI mode disables most of the keys, since they are valid symbols that can be typed in. F1-F5 work in MDI, as do the spindle speed change keys F11 and F12. The RS-274-NGC Interpreter -------------------------- The EMC runs a dialect of RS-274 "G codes" that originated from Allen-Bradley as part of their work for the National Center for Manufacturing Sciences (NCMS) on the Next Generation Controller (NGC) project. The dialect is similar to the Fanuc series of CNCs. G codes: G00 X Y Z rapid feed G01 X Y Z linear feed, e.g., G01 X10 Y20 Z30 F60 for 60 ipm G02 X Y Z I J clockwise circular feed (helical with Z) G03 X Y Z I J counterclockwise circular feed (helical with Z) G04 P<#> dwell # of seconds G10 L2 P<#> X Y Z set coordinates for system #1-9, 1 = G54, 9 = G59.3 G17 XY plane circular interpolation G18 ZX plane circular interpolation G19 YZ plane circular interpolation G20 English units (inches) G21 metric units (millimeters) G40 cancel cutter compensation G41 D<#> cutter compensation for tool <#>, tool on left G42 D<#> cutter compensation for tool <#>, tool on right G43 H<#> use tool length offset for tool #, 0 = no offset G49 cancel tool length offset G53 turn any coordinate offsets off for this block G54 use coordinate offsets for system #1, from G10 L2 P1 G55 "" for system #2, from G10 L2 P2 G56 "" for system #3, from G10 L2 P3 G57 "" for system #4, from G10 L2 P4 G58 "" for system #5, from G10 L2 P5 G59 "" for system #6, from G10 L2 P6 G59.1 "" for system #7, G10 L2 P7 G59.2 "" for system #8, G10 L2 P8 G59.3 "" for system #9, G10 L2 P9 G61 exact stop mode G64 cutting mode G76 threading canned cycle G80 cancel fixed (canned) cycle G81 drilling cycle, no dwell, rapid out G82 drilling cycle, dwell, rapid out G83 deep hole peck drilling cycle G84 tapping cycle G85 boring cycle, no dwell, feed out G86 boring cycle, spindle stop, rapid out G87 back boring cycle G88 boring cycle, spindle stop, manual out G89 boring cycle, with dwell, feed out G90 non-incremental programming (the usual) G91 incremental programming G93 inverse time feed mode G94 feed per minute mode (the usual) G98,G99 set canned cycle return level M codes: M0 optional program stop M1 program stop M2 program end M3 turn spindle clockwise, e.g., S1000 M3 for 1000 rpm M4 turn spindle counterclockwise M5 turn spindle off M6 tool change, e.g., T1 M6 for tool 1 M7 mist coolant on M8 flood coolant on M9 all coolant off M48 disable override control for M50-51 switches M49 enable override control for M50-51 switches M50 enable/disable feed override M51 enable/disable spindle speed override M52 enable/disable adaptive feed override M53 enable/disable feed hold M62 <| .. |- digital IO control M65 <| M100..M199 user defined commands (check the user manual for details). Frequently Asked Questions (FAQ) -------------------------------- Q. The axes don't move when I try to jog them. A. Make sure you're out of estop, in manual mode. Q. Software limits don't work. I can jog past a soft limit. A. Software limits only work when an axis has been homed, since otherwise the machine doesn't know where the limits really are. Q. Why doesn't the mouse or return key work? A. Sometimes the cursor needs to be in the part of the window with the text in it. Move the cursor to a different region and try it. Q. Why are the modal G and M codes not correct in Auto mode? A. The modes that will be active when you enter MDI mode are shown. These are read ahead of actual program execution. Q. How can I change the fonts/colors/sizes in the Tkemc display? A. The "Tkemc" file in the emc/ directory contains the X resources used by the program. Almost nothing is hard coded in the program itself. You can change any of these values and see the effects.