PathPilot Interface - PCNC 1100
Overall Layout
The PathPilot® interface is divided into two sections, the Notebook and the Persistent Controls (see Figure 1). The Persistent Controls make up the bottom half of the screen and include three control groups: the Program Control Group, the Position Status Group, and the Manual Control Group. The top half of the screen is the Notebook, which includes seven tabs including Main, File, Settings, Offsets, Conversational, Probe, and Status. Depending on the mill accessories, there may also be optional tabs including ATC (automatic tool changer), Injection Molder, and Scanner. These tabs are used to select different Notebook pages, each of which displays various buttons, digital readouts (DROs), and information pertinent to the functioning of the PathPilot interface.
For example, the File page of the Notebook is used for tasks like transferring a G-code file from a USB drive to the controller, loading a G-code file into memory, or editing a G-code file.
While the Notebook half of the screen allows you to perform a variety of tasks based on which tab is active (loading G-code file, writing G-code with the Conversational tab, touching off tools), the Persistent Controls half of the PathPilot interface contains the controls used to set up a job and execute G-code. Operators already familiar with Tormach milling machines (or most other CNC machines) will be familiar with many of the Persistent Controls buttons.
For definitions and more information on the terminology used in reference with PathPilot, refer to “Programming”.
Persistent Controls
The Persistent Controls on the lower half of the screen are always present – they don’t move or disappear as you page through the Notebook that makes up the top half of the interface (see Figure 1). These are divided into three logical families: Program Control Group, Position Status Group, and Manual Control Group.
Program Control Group
The buttons, sliders, and DROs of the Program Control Group are functions that relate to tasks the operator might perform while running a G-code program (see Figure 2). They may be used at any time while running a program, or before running a program to set modes like Single Block or M01 Break.
Cycle Start – The Cycle Start button is used to start a program. While running a program the LED in the upper right hand corner of the button illuminates.
If Single Block is active, the Cycle Start button causes the mill to execute one line of G-code per click of the button. When running a program, if motion is paused due to Feedhold, M01 Break, Single Block, or because the mill is waiting on a manual tool change, the Cycle Start button LED flashes on and off until the Cycle Start button is pressed again.
It is an error if:
Cycle Start is pressed when the Main tab of the notebook is not active
Cycle Start is pressed when no G-code program is loaded
Cycle Start is pressed before the mill has been referenced
Single Block – Turns Single Block on (LED illuminated) or off. When Single Block mode is active, the mill executes one block of G-code, then pauses and flashes the Cycle Start button LED on and off, inviting the operator to press the Cycle Start button to execute the next line of G-code. This feature may be turned on or off before running a program or during program execution.
NOTE: Non-motion lines are ignored by Single Block mode. This means that the PathPilot interface will skip comment lines and blank lines.
M01 Break – Turns M01 Break button on (LED illuminated) or off (LED off). When M01 Break is active, and an M01 (optional stop) is programmed in the G-code file, the mill stops when it reaches the M01 line and the Cycle Start button LED flashes on and off. The mill continues to execute the program lines after the M01 when the Cycle Start button is pressed. This feature may be turned on or off before running a program or during program execution.
Feedhold – Turns Feedhold button on (LED illuminated). Turning Feedhold on pauses mill motion, and the Cycle Start button LED flashes on and off. Turning Feedhold on leaves the spindle running (if it is already on). To turn Feedhold off, click the Cycle Start button. The Feedhold button works during program execution or during manual data input (MDI) moves (G-code commands entered into the MDI line below the G-code listing on the Main screen). Feedhold has no effect when the mill is not moving. Also, application of Feedhold is delayed if clicked during a spindle-synchronized move (e.g., G84 tapping cycles) until that spindle-synchronized move is complete. The feedhold function is also connected to the keyboard’s space bar – pressing the spacebar on the keyboard is equivalent to clicking this button with the mouse.
Stop – Stops all mill motion, including spindle motion. If clicked while running a program or during an MDI move, the Stop button stops the mill and rewinds the G-code program. Stop doesn’t change the current modal state of the mill (G54, G01, etc.).
Coolant – Turns coolant on (LED illuminated) or off (LED off). Clicking this button turns power on or off to the coolant accessory port on the side of the electrical cabinet – so long as the Coolant switch on the operator panel is in Auto mode. This button is the equivalent to M8/M9 G-code commands. It may be clicked before, after, or during program execution, or an MDI move.
Reset – Brings the mill out of an E-stop condition, resets G-code modalities, clears alarm messages, and rewinds the G-code program. When the mill is first powered on, or after an emergency stop (E-stop), the Reset button flashes back and forth between red and white. When this button is flashing (after power has been restored to the mill), clicking the Reset button starts and verifies communication between the mill and the controller. Reset may be clicked any time after the mill is powered on. Reset does the following:
Resets all modal G-codes to their normal state including work offset to G54 default
Rewinds a G-code program
Stops a program, MDI move, or homing move if one is currently in progress
Clears alarms (for more information on alarms, see the Status tab section)
Clears the tool path backplot
Spindle Override – The Spindle Override Slider and RPM 100% button (see Figure 2) allow you to override the commanded spindle speed by percentages ranging from 1 percent to 150 percent. The RPM 100% button returns the override to 100 percent of the commanded value or no override. The spindle must be running for these controls to have a noticeable effect. If overriden when the spindle is stopped, the speed is overridden the next time spindle starts. The override doesn’t drive the spindle past its maximum speed. The Spindle Override setting is ignored during spindle-synchronized (e.g., G84 tapping cycle) moves or any time M48 (disable feed and speed overrides) is in effect.
Feedrate Override – The Feedrate Override Slider and Feed 100% button (see Figure 2) work similarly to the spindle override controls. They affect the commanded feedrate by a percentage ranging from 1 percent to 150 percent. The feedrate override works for MDI, jogging, and G-code program G01/G02/G03 moves. The override has no effect on G00 (rapid) moves. The Feedrate Override setting is ignored during spindle-synchronized (e.g. G84 tapping cycle) moves or any time M48 (disable feed and speed overrides) is in effect.
Maxvel Override – The Maxvel Override and Maxvel 100% button (see Figure 2) work similarly to the Feedrate Override controls, except that these controls affect both G00 and G01 moves. They clamp the mill velocity to a percentage of the maximum velocity. The Maxvel slider can be very useful when running a G-code program for the first time. You can use it to stop the mill by sliding it down to 0 percent and verifying the Distance to Go and X/Y/Z/A DROs look appropriate before continuing. The Maxvel Override is a safety feature, and as such is not inhibited during spindle- synchronized moves or with M48. Make sure that Maxvel is at a value that allows the mill to achieve the programmed feed rate during spindle synchronized moves (e.g. G84 tapping) or the move may fail to produce the intended results.
Position Status Group
The buttons, labels, and DROs of the Position Status Group pertain to mill position, active G-code modalities, and feed/speed settings (see Figure 3). These controls may be used at any time before or after running a G-code program or MDI move. They are unavailable for operator input while mill is moving.
Axes Work Offset DROs – The X, Y, Z, and A work offset DROs display the current mill position expressed in the currently active work offset coordinate system (G54, G55, etc.).
When the mill is at rest, these readouts are also operator entry fields. Change the current work offset position by clicking in the DRO field, which illuminates. Type a number, for example 4.0, and click Enter on keyboard. Press the Esc key to return to the original value.
This technique is used for setting any DRO. Remember to click Enter after any DRO change. If you forget and just click on another DRO, any value you have just entered is discarded. This is designed to avoid accidental changes.
For convenience, the Zero button to the left of the axis DROs can be used to set the current work offset position for that axis to 0.000.
DTG (Distance to Go) – Just to the right of the axis DROs are the DTG (see Figure 2) or Distance to Go labels (light blue) that are read-only and display the distance remaining in any single move.
If you feedhold the mill in the middle of a move, or turn the Maxvel or Feedrate overrides to 0 percent, these labels display the distance left in the commanded move. These labels are useful when proving out a part.
Ref Axes Buttons – Ref X, Ref Y, Ref Z, and Ref A buttons reference the axes to their home switch locations. This must be done after power on and before running a part program or using MDI commands. The axes may be referenced simultaneously, though it is common practice to reference the Z-axis first to clear the spindle or tool from the area of the workpiece or vise. When referenced, the LED is illuminated.
Status – The Status line displays the currently active G-code modalities and the active tool. A more detailed description of these active G-codes is provided on the Settings tab.
Jog Active LEDs – Between the (Zero) Axis and DROs are LEDs. If the mill is equipped with an optional Jog Shuttle (PN 30616), the active jog axis is indicated by an illuminated LED (see Figure 3).
Manual Control Group
The Manual Control Group's buttons, slider, and DROs allow the operator to perform tasks related to manual control of the mill, including jogging the mill axes, changing the current tool number, feed rate, or spindle speed, and starting or stopping the spindle (see Figure 4).
Tormach mills can be jogged with either the Jog Shuttle shown in Figure 5 or with the keyboard’s arrow keys (see Figure 6):
The right arrow jogs X-axis in the positive X direction (moves table left of operator)
The left arrow jogs X-axis in the negative X direction (moves table right of operator)
The up arrow jogs Y-axis in the positive Y direction (moves table toward operator)
The down arrow jogs Y-axis in the negative Y direction (moves table away from operator)
The Page Up key jogs the Z-axis in the positive Z direction (moves spindle up)
The Page Down key moves the Z-axis in the negative Z direction (moves spindle down)
NOTE: Jogging is not permitted during G-code program execution or during MDI moves.
The Jog Shuttle is an optional accessory (see Figure 5) that may increase productivity, especially on short-run jobs requiring extensive setting up of the workpiece and tooling.
The X, Y, Z and A buttons are used to jog axes X, Y, Z and A respectively (the LED light beside an axis DRO in the PathPilot interface indicates which axis is selected for jogging). The Step button cycles through the available jog step sizes (the LED on a Step Size Button in the PathPilot interface indicates which size is active). Continuous jogging is done with the Shuttle Ring by turning it counterclockwise (minus) and clockwise (plus). There are seven speeds to position any axis with speed and precision. Step jogging is done with the Jog Wheel (with finger dimple) by turning it counterclockwise in the minus direction and clockwise in the plus direction. The move will be made at the current feed rate.
Whether using the jog shuttle or the keyboard arrow keys, there are two modes of jogging, continuous and step. When using the keyboard to jog, switch between modes using the Jog Cont/ Step button (see Figure 7).
Step Mode – In Step mode the mill jogs in steps, where the step size is controlled by the four buttons to the right of the Step label (see Figure 7).
Notice that in imperial units (type G20 in the MDI Line) the step sizes range from 0.0001” to 0.1” (see Figure 7), whereas in metric mode (type G21 in the MDI Line) the step sizes range from .01 mm to 10 mm. The illuminated LED in the upper right corner of each Step button indicates active step size.
Continuous Mode – In Continuous mode the mill jogs at a continuous velocity when you press and hold any one keyboard arrow key; stop the mill by releasing the key. Axis motion is key specific as shown in Figure 6. The velocity is set using the Jog Speed Slider (see Figure 7). To set jogging velocity to the maximum speed, click and drag the Jog Speed Slider to the far right position.
Feed Rate DRO – Feed rate is the velocity at which the workpiece can be fed against the machine tool. The DRO, or digital read out, is the field that displays this velocity.
Spindle Controls – The REV, Stop, and FWD buttons can be used to manually control the spindle (see Figure 8). Rev is the equivalent of typing M04 in the MDI Line – it starts the spindle counter clockwise at the RPM specified in the Spindle RPM DRO (see Figure 8).
The Stop button stops the spindle, similar to the M5 command. The FWD button starts the spindle clockwise at the set RPM. These buttons are unavailable when running a G-code program or in the middle of an MDI move. Pressing REV or FWD triggers an alarm if the commanded spindle speed is outside of the valid spindle speed range for the mill's current belt position.
The Spindle RPM DRO is used to display the current spindle speed command (see Figure 8). You may change the current spindle speed command by typing a value into this DRO and pressing Enter. Values above the maximum RPM or below the minimum RPM for the current belt position triggers an alarm.
The Spindle Range button toggles between the two belt/pulley settings with an LED indicating which position is active (see Figure 8). For more information on spindle belt/pulley settings see, “Operation”.
Tool DRO (T) – Displays the tool currently in the spindle. To change the spindle tool and apply its tool length offset, type a number (valid range is 0–256) in the Tool DRO and press Enter key or click the M6 G43 button.
M6 G43 Button – Causes the system to change the number of the tool that is currently in the spindle to the number typed in the DRO, as well as apply the length offset for that tool. M6 is the G-code command that requests a tool change and G43 is the command that applies a tool length offset (for more information on these commands, Programming).
Tool Length Label – Displays the current tool length offset. This display is normal (light blue text on grey background) when the tool offset number matches the tool number. But an alarm appears (orange text on red background) if the offset number does not match the current tool number.
Go to G30 Button – Causes the mill to move to a pre-defined G30 position, and is equivalent to typing G30 in the MDI Line. This G30 position can be set using the Set G30 button on the Offsets tab. Operators familiar with M998 will notice that the behavior of G30 is identical to M998. By default, the move to the G30 position is in Z only. This can be changed on the Settings tab.
To set the G30 position, jog the mill to the desired position and click the Set G30 Position button on the Offsets tab. Subsequent uses of the G30 command in G-code or the Go To G30 button will cause the mill to move to this position.
Keyboard Shortcuts
Several keyboard shortcuts are provided for operator convenience. Below is a list of shortcuts used in the PathPilot interface:
Spacebar | Feedhold | Alt + R | Cycle Start |
|---|---|---|---|
ESC | Stop | Alt + F | Coolant |
Alt + Enter | Give Focus to MDI line | Alt + E | Edit currently loaded G-code program* |
*Use the Alt+E command on any PathPilot screen to edit G-code.
Main Tab
The Main tab is active by default when the PathPilot controller first powers on, and contains four controls: recent files, G-code window, MDI line, and tool path display (see Figure 9).
Selecting a Recent G-code Program File
The recent files drop-down menu displays the currently loaded G-code program file (see Figure 9). Click the drop-down menu to display the last five program files loaded into PathPilot; select the name of the program from the menu to load the G-code.
Select Clear Current Program in the recent files drop-down menu to close the currently loaded G-code program file.
Working in the G-code Window
The G-code window displays the G-code of the currently loaded program file. Use the scroll bars to view the entire file.
PathPilot highlights certain lines of code of interest. When running a G-code program in single block mode, there may be as many as three lines of G-code highlighted, each with a different color:
Green line: indicates the start line, which is the first line in the program (unless this has been changed with the Set Start Line feature)
Blue line: indicates the line of code that is currently executing
Brown line: indicates the move that will occur the next time Cycle Start is pressed
Setting a New Start Line
The start line is the line at which the G-code program begins. By default, this is the first line of code in the G-code program. Right-click the preferred start line of code in the program and select Set Start Line to change the start line.
When using the Set Start Line option, the operator is responsible for making sure that the mill is in the proper state before the code executes.
To set a start line in the middle of a G-code program file, make sure that any preparatory moves (like turning the spindle and coolant on) are manually completed before clicking Cycle Start.
The mill reads backwards through the beginning of the G-code program file to do things like set the appropriate G5x active work offset, G61/64 setting, and other modal states. It will not turn the spindle or coolant on.
Expanding the G-code Window
Double-click the G-code window to expand the G-code window and shrink the tool path display. Double-click the G-code window again to return the display to its original size.
Manually Entering Commands
When running a G-code program, commands to the mill are read from a file. You can also send G-code commands to the mill directly with the MDI line (see Figure 10).
Click the MDI field to use the MDI line; the line is highlighted. Type the command, using the Backspace, Delete, Left and Right arrow keys to correct typing errors. Press Enter to execute the command; press Esc to abandon it.
Click the MDI field and use the Up or Down arrow keys to copy a recent MDI command into the MDI line. Up to 100 MDI commands are stored for reuse; these commands are saved between sessions. Command history is available after a power cycle.
NOTE: When the MDI line is open, all keystrokes are registered as a typed command. Jogging is not possible when you are clicked inside the MDI field.
Searching in the Code
MDI has the ability to search the text of a G-code program file for specific numbers, codes, or items of interest like tools, feeds, and speeds.
Type FIND followed by the text to be searched in the MDI line (see Figure 11). Pressing Enter finds the next instance of the searched text; pressing Enter while holding down the Shift key finds the previous instance.
If found, PathPilot scrolls to the line containing the searched text and highlights it in yellow (see Figure 11). When the search reaches the end of the G-code file, it wraps and starts again from the beginning.
Change the starting point of the search by clicking on any line in the G-code window.
When used in conjunction with the FIND command, certain search terms (listed below) initiate a search through the G-code file to find more than just the actual search term:
FIND TOOL: Searches for instances of the actual word Tool in the G-code and any T G-code command which calls up a tool (e.g., T12)
FIND SPEED: Searches for instances of the actual word Speed in the G-code and any S G-code command
FIND FEED: Searches for instances of the actual word Feed in the G-code and any F G-code command (see Figure 12)
NOTE: Search text ignores case, so the command FIND TOOL will match TOOL, Tool, tool, etc.
The FIND command simplifies searching of a G-code file to verify speed and feed values and tool calls before cutting a part, or to find a specific set start line point in a large G-code file. For more information on using set start line, refer to “Setting a New Start Line” section earlier in this chapter.
Working in the Tool Path Window
The tool path window displays a graphic representation of the tool path that is executed for the currently loaded G-code file (see Figure 13), each with a different color:
White lines: indicates the preview lines
Red lines: indicates the tool path as it is cut
Yellow lines: indicates jogging moves
Dotted blue lines: indicates the boundary box, which represents the ends of travel of the axes
Double-click the tool path window, or click Reset, to erase the jogging or tool path lines.
Changing the View of the Tool Path Window
Four views are available: top, front, right, and ortho. By default, the view is top. Right-click anywhere in the tool path display and select a different view to change the view of the window.
Grid lines are visible behind the tool path when the view is top, front, or right. Grid lines are not available in ortho. By default, grid lines are drawn at 0.5” intervals when in G20 mode (5 mm intervals when in G21 mode). Right-click anywhere in the tool path display and select a different grid spacing to change the resolution of the grid lines. When a program is loaded, the program extents (furthest points to which the tool will travel while executing the G-code) are displayed to the left and bottom of the tool path (see Figure 13).
File Tab
The File tab is used to transfer files to and from a USB drive, copy, delete, and rename files and folders (see Figure 14). The left window shows files and folders on the controller hard drive; the middle window shows files and folders on a removable USB drive.
Managing Files
Use the New Folder, Rename, and Delete buttons below the respective USB Drive Window and Hard Drive Window for file management (see Figure 14). To move files into a folder, right-click on the file and select cut or copy from the pop-up menu.
Transferring Files or Folders from a USB Drive
Insert a USB drive into any open USB port.
Navigate to the file to transfer in the USB Drive Window.
NOTE: Use Back to navigate backwards; use USB to jump to the highest (home) level (see Figure 14).
In the hard drive window, navigate to the desired location in the PathPilot interface to copy the transferred file from the USB drive.
Highlight the file or folder to copy in the USB drive window; click Copy From USB (see Figure 14).
If the file to be transferred has the same name as an existing file on the controller, you can either overwrite the file, give it a different name, or cancel the file transfer.
When copied to the new location, the file displays in the USB drive window.
Click Eject to disconnect the USB drive from the controller (see Figure 14).
NOTE: Ejecting the USB drive this way helps to avoid corrupting data on the USB drive.
Loading G-code
The Load G-code function is only available for files stored on the controller (see Figure 14).
Navigate to the desired .nc file in the hard drive window; highlight the file and click Load G-code (see Figure 14).
Click on the Main tab; verify G-code file name appears in recent files drop-down menu. For more information on selecting a recent G-code program file, refer to Main Tab section earlier in this chapter.
Editing G-code
The G-code File Preview window displays the contents of the selected .nc file (see Figure 14). You can edit G-code in two ways on your PathPilot controller:
Using a text editor
Using the Conversational tab to edit a file created in PathPilot's conversational programming
NOTE: For information, refer to Conversational Tab section later in this chapter.
Editing G-code with a Text Editor
Highlight the file and click Edit G-code (see Figure 14).
A text editor opens the file in a new window for editing the contents of the file. Make the appropriate changes to the file and click Save.
Click the X in the upper right-hand corner of the screen to close the text editor.