PathPilot Interface - PCNC 770

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.

Open

Figure 1

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.

Open

Figure 2

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.

Open

Figure 3

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).

Open

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)

Open

Figure 5: Jog Shuttle

Open

Figure 6: Jogging with Keyboard Keys

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).

Open

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).

Open

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:

*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).

Open

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).

Open

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.

Open

Figure 11

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)

Open

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

Open

Figure 13

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.

Open

Figure 14

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

1. Insert a USB drive into any open USB port.

2. Navigate to the file to transfer in the USB Drive Window.

3. In the hard drive window, navigate to the desired location in the PathPilot interface to copy the transferred file from the USB drive.

4. Highlight the file or folder to copy in the USB drive window; click Copy From USB (see Figure 14).

5. 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.

6. When copied to the new location, the file displays in the USB drive window.

7. Click Eject to disconnect the USB drive from the controller (see Figure 14).

Loading G-code

The Load G-code function is only available for files stored on the controller (see Figure 14).

1. Navigate to the desired .nc file in the hard drive window; highlight the file and click Load G-code (see Figure 14).

2. 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

1. Highlight the file and click Edit G-code (see Figure 14).

2. 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.

3. Click the X in the upper right-hand corner of the screen to close the text editor.

4. Click OK when asked to re-load the file.

Editing G-code with Conversational Programming

1. From the File tab, select the file and click Conv. Edit (see Figure 14).
   A job assignment editor opens the file in a new window. The left window displays job assignments of a program. The right window displays a preview of the program (see Figure 15).

Open

Figure 15

2. Edit the file contents as needed:

• To change the order in which the steps of the program occur: Click Move Up, Move Down, Duplicate, or Remove.

• To create a new job assignment using conversational programming:

  • Click Insert Step. PathPilot creates the job assignment and opens the Conversational tab.

  • Click Insert.

  • If necessary, edit the job assignment order in the program.

• To load an existing G-code file into the program:

  • Click Insert File. G-code files that are hand-written, or generated from CAM software or conversational programming in PathPilot, can be inserted.

  • Navigate to and select the .nc file that you want to insert.

  • Click Open.

  • If necessary, edit the job assignment order in the program.

• To edit a job assignment that was created in conversational programming:

  • Select the job assignment and click Conv. Edit. In the Conversational tab, PathPilot opens the relevant tab.

  • Make the desired changes to the job assignment.

  • Click Finish Editing.

3. Click Save.
   The G-code program file is updated.

Tips:

• To restore an edited job assignment to its original parameters: Click Revert.

• To undo all changes made to an entire G-code program: Click Close. When prompted, Close Without Saving.

Settings Tab

The Settings tab displays active settings of the PathPilot controller, allowing you to configure PathPilot to suit your machine configuration (see Figure 16).

Open

Figure 16

The window on the left side of the Settings tab displays a list of available G-code modalities. Active G-codes are highlighted in yellow (see Figure 16).

Specifying the Tool Change Method

Select the ATC (Automatic Tool Changer) or Manual Tool Change option to identify the tool changer type for your specific mill configuration. Mill behavior differs when it encounters an M6 command for an ATC or manual tool change.

If the ATC option is selected, PathPilot searches for an ATC attached to the mill. If the mill is equipped with an ATC, tools that have been assigned to the tray are changed automatically when a Tx M6 command is issued through the MDI line or within a G-code program file. The Tool DRO and M6 G43 button only change the current tool number – neither directly cause an automatic tool change. To request an ATC tool change, either program M6 Tx G43 in the MDI line or type a tool number in the Tool DRO and press Enter. For more information, refer to “ATC”.

If the Manual Tool Change option is selected, the mill pauses at the M6 command during a G-code program file execution, allowing you to manually change tools (see “Operation”, for information on the manual tool change procedure). After changing tools, press Cycle Start to resume program execution with the new tool. When the mill is paused and waiting for a manual tool change in the middle of a G-code program, the Cycle Start LED flashes on and off and a message is displayed with the requested tool number on the tool path display.

Selecting the Spindle Type

Use the Spindle Type drop-down to select spindle scaling if your mill is equipped with a Speeder Series 2 (PN 31350) or a High-speed Spindle (PN 35178).

Changing the Network Name

Use the Network Name field to change the network name of the controller; press Enter. The controller must be restarted for the name change to take effect.

If you are connected to a network using either the Ethernet jack or the optional Wireless Network Adapter (PN 38207), the controller appears on a network as network-attached storage. The controller exports a Windows network share named gcode to the Windows network with a domain name WORKGROUP. The default network name of the controller is TORMACHPCNC. The login name for the share is WORKGROUP\operator and the password is pcnc. The network name must be unique on your network. For more information, refer to the documentation that ships with the Wireless Network Adapter.

Disabling Limit Switches

The Limit Switches checkbox is selected by default. To provide a temporary workaround for a malfunctioning limit switch circuit, clear the checkbox. When cleared, Ref X, Ref Y, Ref Z, and Ref A sets the machine reference position to the mill position at the time it is clicked rather than completing the homing procedure.

NOTE: If desired, use this procedure in conjunction with one or more dial indicators mounted at the ends of mill travel to provide a more accurate method of manually referencing the mill.

Limiting a G30/M998 Move

Select G30/M998 Move in Z Only to move to the tool change position in the Z-axis only when using a G30 or M998 command. Otherwise, a coordinated X, Y, Z move occurs on G30 or M998.

The G30 or M998 G-code commands can be used to move the mill to a pre-set position. The position is settable using the Set G30 button on the Offsets screen. A G30 or M998 command is typically programmed right before a tool change line in G-code program files so that the spindle head clears the workpiece with sufficient distance to be able to change tools. For more information on using a G30 or M998 command, refer to “Programming”.

Enabling Feeds and Speeds Suggestions in Conversational Programming

Select “Conversational Feeds and Speeds” to enable feeds and speeds suggestions in PathPilot when using conversational programming. For more information on use, refer to “Using Feeds and Speeds Suggestions”.

Use a USB Camera

After plugging in the USB camera, navigate to the camera settings. From the PathPilot interface, in the Settings tab, open the Camera(s) tab. Identify the Camera Status read-only dialog box.

Open

Figure 56: USB Camera status.

As cameras are plugged in and unplugged, the Camera Status area is refreshed. To test compatibility of any USB camera, plug it in and watch the Camera Status area for the camera name and details.

NOTE:  If a camera isn't shown after plugging it in or starting a video recording, it might require too much power from the USB ports on the controller. This is very likely when more than one camera is used. Try using a powered USB hub to add the camera(s).

When a USB camera is plugged in, it's analyzed for supported video and audio formats, frame sizes, and frame rates. If the camera supports it, PathPilot uses H.264 compression; otherwise, it uses Motion JPEG.

If the USB camera has a microphone, PathPilot records audio as well as video. The preferred format is compressed AAC, but uncompressed PCM is used as a fallback.

About USB Cameras

Recording video and audio from USB cameras is supported in PathPilot v2.10.0 and later. You can use up to four cameras simultaneously to record from different vantage points.

NOTE: All cameras are started and stopped at the same time — if you don't want a camera to record, you must unplug it.

USB cameras are compatible with all machine types, but older controllers may lack the processing power and memory needed for camera support. Controllers require 4GB of memory for camera functionality. Use the ADMIN MEMORY MDI command to verify the memory size of a controller.

You can purchase a Tormach USB Camera (PN 51240) with a metal case, mounting bracket, and 15-foot USB cable. Other USB cameras may work (see below), but do not include any technical support.

Manual Recording

To start or stop a manual recording, either:

• Use the controls in the Manual Recording area of the Camera(s) tab.
  When a manual recording is stopped, a file save-as dialog appears prompting you for the file name base to use.

Open

Figure 57: Manual recording controls.

• Select the Video Camera Recording button in the Persistent Controls section.

Open

Figure 58: Video Camera Recording button.

Whenever PathPilot is recording from a USB camera and/or the virtual screen camera, the LED on this button is green. If PathPilot is recording and the button is pressed:

• If a program is running and not paused at an M00/M01, the recording is aborted.

• If a program is not running, but the machine is moving, the recording is aborted.

• Otherwise, if a manual recording is in progress, it is stopped and a file save as dialog will appear. If an automatic e-stop loop recording is in progress, it is aborted since no e-stop occurred.

To include a screen recording:

1. Toggle the Include PathPilot screen in recordings checkbox in the Camera Settings area of the Camera(s) tab to enable or disable screen recording.

Open

Figure 59: Camera settings.

To take a picture (using all of the USB cameras at once):

1. Select Snapshot in the Manual Recording area of the Camera(s) tab.
   The Main tab displays.

2. Review the camera images, which display on top of the Tool Path area. The camera images refresh every 0.5 seconds.

3. Align the cameras or adjust lighting to your preference, and then select the Shutter button.

Open

Figure 60: Example of taking a photo.

Automatic E-Stop Loop Recording ("Dashcam")

E-stop loop recording enables analysis of the previous 30 seconds after an E-stop. When enabled, recording is automatically started after reset.

To enable or disable the recording of emergency stops:

1. Toggle the Automatic e-stop loop recording checkbox in the Camera Settings area of the Camera(s) tab.

NOTE: This feature is enabled by default.

Automatic E-stop loop recording starts when the Reset button is selected. If you selected Video Camera Recording to abort a previous E-stop loop recording, select Reset to start it again.

To view E-stop videos:

1. A slight delay occurs after an E-stop while the video is saved to the E-stop Videos folder. Select the video file, and then select Load G-Code to view it.

NOTE: The E-Stop Videos folder is automatically monitored for internal drive space use. If the folder size grows beyond 5 GB, the oldest video files are automatically deleted until the folder size becomes less than 5 GB.

Review Video and Image Files

1. On the File tab, select the video or image file and select Load G-Code.
   A video player application starts or the image preview is displayed.
   Alternatively, you could transfer the video or image files to a Windows or macOS computer for review.

File Naming Convention

For manual and automatic E-stop recordings, the base file name for the recording has automatically chosen suffixes appended for each camera.

For example, if you stop a manual recording of two cameras, specify “Left Bracket Op1” as the name, and enabled screen recording, you'll see the following files:

G-Code Commands

PathPilot supports three new M-codes to control cameras within G-code programs: M301, M302, and M303. Example use cases:

• Record only across each M01 stop where the operator needs to flip a workpiece or change a tool.

• Create short videos that focus on unique aspects of the program to reduce later video editing.

• Record USB IO integration operations with robots or other devices (pneumatic vises, etc.).

• Monitor progress on a workpiece by including M303 throughout the program.

File Naming Conventions

Recordings or pictures created by M301/M302/M303 have automatically generated file names, with the base file name taken from the running G-code file. Video files are saved alongside the G-code file. The suffix for each file uses a time stamp format. This makes it easy to distinguish multiple runs of the same G-code program.

For example, if engrave.nc is running and uses M301 and M302 to create one recording on a machine with one camera, and screen recording is enabled, you'll see the following files:

Use M01 to Take Pictures

In addition to displaying information like pictures or messages during an M01 break, you can also use a USB camera (if installed) to take a picture.

To use M01 to take pictures:

1. Add M01 (op1_setup.jpg) into your G-code program.

2. Run the G-code program.

3. When PathPilot executes the M01 it looks to see if the comment contains a file name.

• If there isn't a file name: The comment is shown as instructional text across the tool path.

• If there is a file name, but the file doesn’t exist yet and the extension is .jpg, .png, or .jpeg: The USB cameras are initialized and shown in the tool path display.

4. Select the Shutter button to take the picture and create the op1_setup.jpg file.
   In future runs of the G-code program, op1_setup.jpg will display to the operator for instructional purposes on the workpiece.

Enabling Accessories

Use the Settings tab to enable optional accessories that work with PathPilot.

4th Axis Homing

Select 4th Axis Homing if you are using an optional 4th Axis Homing Kit (PN 31921). For information on installation and use, refer to the documentation that ships with the product.

Enabling CNC Scanner

Select CNC Scanner if you are using an optional CNC Scanner. The Scanner tab displays. For information on installation and use, refer to the documentation that ships with the product.

Enabling Enclosure Door Switch

Select Enclosure Door Switch if you are using an optional Enclosure Door Switch Kit (PN 35550). The installed enclosure door switch is activated, and, when the front doors are opened:

• All axis motion stops

• Spindle speed reduces to 1000 RPM

For more information on installation and use, refer to the documentation that ships with the product.

Enabling Injection Molder

Select Injection Molder if you are using an optional Injection Molder. The Injection tab displays. For information on installation and use, refer to the documentation that ships with the product.

Enabling Soft Keyboard

Select Soft / Onscreen Keyboard to use a soft keyboard with the optional Touch Screen Kit (PN 35575). For information on setup and calibration, refer to the documentation that ships with the product.

When you select a DRO field, a numeric keypad opens on screen (see Figure 17). When you select either the MDI line, the Save field, the Save As field, or the conversational title DRO, a QWERTY keyboard opens on screen (see Figure 18). Press Enter to accept the value typed; press ESC to exit the soft keyboard and restore the previous value.

Open

Figure 17

Open

Figure 18

Enabling Probes

Identify the probe type if you are using one of the two optional probe options — a Passive Probe (PN 32309) and an industrial-grade Digitizing Probe (PN 31858).

IMPORTANT! Do not use probing features in PathPilot before selecting this setting. Refer to chapter 8, Accessories, to make sure the correct probe is selected.

Enabling USB I/O Board

Select Use USB IO Kit if you are using an optional USB M-code I/O Interface Kit (PN 32616). For information on installation and use, refer to the documentation that ships with the product.

Switching to RapidTurn

Click Switch to RapidTurn to close the PathPilot interface for the mill and open PathPilot interface for the RapidTurn^™ (PN 32901). For information on operating the RapidTurn and related interface, refer to the RapidTurn operator manual.

Offsets Tab

The Offsets tab reveals two sub tabs: Tool and Work (see Figure 19).

Open

Figure 19

Work offsets are a concept that allow the operator to think in terms of X/Y/Z coordinates with respect to the part instead of thinking of them with respect to the mill position. Up to nine work offsets can be saved in the control. These are selected either by typing G54, G55, ... (up to G59, G59.1, G59.2, G59.3) into the MDI line, or by including them in a G-code program.

Tool offsets allow the operator to use tools of different lengths or – when using G41/G42 cutter radius compensation – different diameters, while still programming with respect to the workpiece. The most common tool offset is the tool length offset, which is applied by the G43 command.

Tool Tab

The Tool tab displays a tool table on the right with fields available to input tool information (see Figure 19).

NOTE: Fields are only editable if the mill is powered on and not in Reset mode.

For a given machining operation, the X and Y position of the workpiece are fixed. If you are using multiple tools of differing lengths, you will need to change the Z offset for each tool. PathPilot allows you to switch tools quickly, without the need to set up the mill every time a tool is mounted. Each tool and holder only needs to be measured once, either offline or in the mill.

Tool Measuring Techniques

Different tool measuring techniques may be used, but the three most common methods are:

• Offline measurement with a height gauge

• Automated measurement with an electronic tool setter

• Touching off tool to a reference surface

Measuring Offline with a Height Gauge

The Tormach Tool Assistant Set (PN 31988) includes an 8” digital height gauge and a USB interface cable with touch trigger (see Figure 20).

1. Connect the USB interface cable to any available USB port on the controller.

2. Move the digital height gauge to a block and press Zero on the touch trigger. The device is zeroed.

NOTE: Granite Surface Plate with Integrated Tool Hole (PN 31713), as shown in Figure 20, helps accurately measure tool length.

3. To measure tool height, mount the tool in a TTS tool holder and place on a block (see Figure 20). The tool height measurement is the distance from the block surface to the end of the tool tip.

Open

Figure 20

4. From the PathPilot interface, click the appropriate line in the tool table (see Figure 19); the line is highlighted.

5. Press Data on the USB interface cable to transfer measurement information to the Length field in the tool table (see Figure 19).

Measuring Automatically with an Electronic Tool Setter

Before using an electronic tool setter:

• Set the work offset such that the surface upon which the electronic tool setter sits is Z zero. A quick way to do this is to use the Move And Set Work Offset button on the Offsets screen’s Work tab, with either a tool of known length in the spindle or with no tool in the spindle (and Tool Zero in the tool DRO).
  
  By doing this setup step, you are measuring true tool lengths, and can interchange tools measured in the height gauge with tools measured with the electronic tool setter.

To measure a tool with the electronic tool setter: Put the tool in the spindle, type the tool number in the tool DRO, and then, with the tool centered over the electronic tool setter, click the Move And Set Tool Length button on the Offsets screen’s Tool tab.

Measuring by Touching Off Tool

This method was covered in chapter 5, Intro to PathPilot, in your operator manual. It is not as accurate as the previously described methods, but works in many situations.

Creating Tool Descriptions

PathPilot uses keywords and patterns in the tool description to recognize tooling features. Refer to the section Using Tool Keywords later in this chapter for more information.

Example: "Dia:.3125 4FL R:03 AlTiN CRB variable loc:.75"

This description provides the following information for PathPilot to calculate machining information:

• 0.3125 tool diameter

• Four flutes

• 0.03 radius, or "bullnose"

• Aluminum-titanium nitrade coating

• Carbide

• Variable helix

• 0.75 length of cut (loc)

To get accurate machining information, all tooling must be described with detail: the more detail, the better the results. Using a personal description likely won’t contain meaningful information for PathPilot.

Open

Figure 21

Example: "Gold colored end mill from middle drawer"

This description provides virtually no information. PathPilot defaults to basic cutter features about this tool:

• Two flutes

• Uncoated, high-speed steel end mill

• Length of cut based on the diameter

Manually Entering Tool Descriptions

You can manually enter tool descriptions in the Tool Table window. Descriptions are not case sensitive.

If a pattern or word in the description is recognized, PathPilot uses syntax highlighting to indicate a valid description (see Figure 21).

Refer to the section Using Tool Keywords later in this chapter for more information on tool description keywords.

Using Tool Keywords

Generating Automatic Tool Descriptions

If you are using a Tormach tool, you can enter the part number to automatically generate tool descriptions in the Tool Table window (see Figure 22).

Open

Figure 22

NOTE: If you're unsure of the part number, you can search for the tool at tormach.com.

1. From the PathPilot interface, on the Offsets tab, in the Tool Table window, select a blank line.

2. Type the part number for the tool.

3. You must enter the value for the Length.

Work Tab

The Work tab displays a read-only table of work offsets. The active work offset is highlighted in this table.

NOTE: The table cannot be edited directly. To change the current work offset value, either type into an Axis DRO or use Zero button next to the Axis DRO.

Working with Backups

Make a periodic backup of the tool offset and fixture information and machine settings to store externally should the controller get replaced or need to be restored to factory settings.

Create a tool offset and fixture information backup on a PathPilot controller as follows:

1. Insert a USB drive into any open USB slot on the controller.

2. On the Main screen, type ADMIN SETTINGS BACKUP in the MDI line.

3. In the dialog box, navigate to a location to store the backup .zip file on the USB drive and rename if desired; click Save.

NOTE: Keep this file somewhere safe and easily accessible.

Restore tool offset and fixture information backup on a PathPilot controller as follows:

1. Transfer the tool offset and fixture information and machine settings backup to a USB drive; insert into any open USB slot on the controller.

2. On the Main screen, type ADMIN SETTINGS RESTORE in the MDI line.

3. In the dialog box, navigate to the backup .zip file on the USB drive; click Open. PathPilot exits, restores from the backup file, and then restarts PathPilot.

Conversational Tab

The Conversational tab provides an interface for programming at the controller. Use Conversational to machine simple parts without the use of CAD/CAM.

Using Feeds and Speeds Suggestions

You can use PathPilot to automatically calculate feeds and speeds: from the Conversational tab, in the Conversational DROs group, select a material, a sub-type, and a tool (see Figure 23).

Open

Figure 23

To calculate feeds and speeds, you must first make sure PathPilot has relevant details about the tooling. For more information, go to the section Creating Tool Descriptions earlier in this chapter.

1. From the PathPilot interface, on the Conversational tab, locate the Material dropdowns in the Conversational DROs group.

2. From the Material dropdown, select your material.
   Examples:

• Aluminum

• Plastic

3. If required, from the Sub-type dropdown, select the material sub-type.
   Examples:

• -any-

• 6061

4. In the Tool DRO, type the assigned tool number.

5. Click Refresh (to the right of the Sub-type dropdown). The following machining-related DROs are calculated:

• Spindle RPM

• Feedrate

• Z Feedrate

• Depth of Cut (if milling)

• Stepover (if milling)

• Peck (if drilling)

NOTE: After PathPilot calculates values for the machining-related DROs, the background turns green (see Figure 23).

Adjusting DRO Values

After selecting the material and tool, you can adjust the values in the calculated DROs, like Feedrate or Stepover. Adjusting the value in one of these DROs does not change the value in the other machining- related DROs.

Once you adjust the value in the DRO, the background switches from green back to white (see Figure 24). This helps you identify which DROs have suggested values (those with a green background), and which DROs have values you've supplied (white background).

Open

Figure 24

Refreshing DRO Values

The suggested feeds and speeds are no longer valid if:

• You select different material or sub-type values, or if you type a new value in to the Tool DRO.
  The suggested feeds and speeds are made by taking into account all of these values. Changing any value requires you to refresh.

• You select a different Conversational tab.
  The suggested feeds and speeds are made by taking into account the current, specific conversational operation — like Face, or Pocket. Changing your conversational operation requires you to refresh.

When the feeds and speeds are no longer valid, the Refresh button turns green, and the machining-related DRO backgrounds switch from green to white (see Figure 25).

Open

Figure 25

Using Additional Provided Information

On the Conversational tab, in the Conversational DROs group, there are tips that are displayed based on the calculations that PathPilot is performing (see Figure 26):

• Chip load information
  Chip load — the amount of material removed per tooth — is based on the number of flutes, RPM, and feedrate.
  Chip thinning takes the stepover (the horizontal depth of cut into the workpiece) into account, and provides the actual chip load.
  As the stepover value decreases, the actual chip load decreases. If the stepover is too small, the cutter may not have enough contact with the material to cut — effectively resulting in pre-mature tool wear.

Open

Figure 26

• Cutting speed information
  Cutting speed is the speed that a given tooth (flute) on the cutter will be moving when it cuts through the material. All materials have a documented cutting speed.
  In imperial units, cutting speed is measured as surface feet per minute (SFM). In metric units, cutting speed is measured as surface meters per minute (SMM).

• Material removal information
  The material removal rate (MRR) indicates how much material is removed by the tool per minute while cutting.
  In imperial units, cutting speed is measured as cubic inches per minute.
  In metric units, cutting speed is measured as cubic centimeters per minute.

Face Tab

Face is generally used for cutting an accurate top surface from rough stock, cutting successive XY-planes over a Z range (see Figure 27).

Open

Figure 27

It is assumed that the top of the stock is free of any clamps or other work holding devices, such as when the stock is held in a vise. The start of each Z pass is intended to be off to the side of the workpiece then move in XY to start cutting at the X Start, Y Start corner. This avoids the need for plunging the Z Depth of Cut move into the workpiece.

Therefore, the area around this corner must be clear of obstructions down to Z End. The tool diameter also extends beyond the workpiece X and Y edges by an amount dependent on the tool diameter and the stepover values, so Z End must be above the vise jaws.

The G-code routine starts with a move to G30, which typically is the park, or tool change position. Next comes a tool change if needed, a rapid move in XY to the workpiece start, and a rapid down in Z to Z Clear. An XY pass starts with an adjusted Z Depth of Cut, then a rectangular spiral from the workpiece perimeter, ending at the center. If a finish pass with different parameters is needed, save the current file, edit the current screen to the finish configuration and append to the saved file.

XY DROs

Start and End – These DROs should be set to the location of the workpiece edges. Tool paths, such as a lead-in, that are normally outside of the workpiece area are set in reference to these values, so no adjusting beyond the actual location of these edges should be needed.

Stepover – This is the space between spiral tool paths. To prevent uncut areas in the spiral corners, the stepover value should be limited to 80 percent of the tool diameter (see Figure 28). A stepover of 0 may be entered which invokes a center only cut. This is more formally called by X or Y values that create a workpiece width less than 70 percent of the tool diameter.

Open

Figure 28

Z DROs

Z Start and End – The first Z pass will cut at Z Start – Depth of Cut adjusted. The last Z pass will cut at the Z End location. For a single Z pass at Z End, enter 0 or a full Z range value into the Depth of Cut DRO.

Depth of Cut – The Depth of Cut entered into the DRO is later adjusted within the Z range, Z End – Z Start, so each Z pass has the same depth instead of having a short depth on the last pass. For a single pass at Z End enter 0 or a full Z range value into the Depth of Cut DRO.

Z Clear – This is the Z location the tool moves or retracts to when starting or ending a Z pass. This should be set to clear any obstructions in the path between the end of one Z pass and the beginning of the next.

Profile Tab

Profile cuts an XY area with successive Z Depth of Cuts to form a rectangular island (see Figure 29).

Open

Figure 29

The outer bound of the area is the stock material's outer edges. The inner bound is the island perimeter. For the cutting routine, the area is divided into four sections (north, east, south, and west). As with Face, the starting position for cutting each section is off the workpiece with an X or Y feed into the workpiece, thus avoiding a Z plunge cut. Cutting paths are restricted to climb cutting, so the tool is retracted to Z Clear at the end of each sweep of a section, with a rapid move to the beginning of the section for the next sweep. After each section is cut, the corner radii, if any, are cut with a tool path that travels around the perimeter of the island. This process is repeated for each Z Depth of Cut pass. If a finish pass is needed, leave enough material, then append your finishing G-code (usually a single pass around the perimeter) to this file later. Feed rate on the radius cuts are adjusted to compensate for the difference between the tool control point rate (at the tool center) and the actual rate at the radius surface.

X and Y Start and End DROs

Start and End – These DROs should be set to the location of the workpiece edges. Tool paths outside of the workpiece area are set in reference to these values so no adjusting beyond the actual location of these edges should be needed.

Profile Start and End – The tool radius is used to create the tool path, so these DROs should be set to the location of the profile outer edges.

Radius – Enter 0 if no corner radius is desired. Valid radii values are from 0 to one half of the island’s narrow width (or limited to full radii on the long ends of the island).

Stepover – This is the tool path offset between section sweeps. A stepover of 0 creates a single pass (or rectangular slot) around the perimeter (outside) of the boss.

Z Start and End – The first Z pass cuts at Z Start – Depth of Cut adjusted. The last Z pass will cut at the Z End location. For a single Z pass at Z End, enter 0 or a full Z range value into the Depth of Cut DRO.

Depth of Cut – The Depth of Cut entered into the DRO is later adjusted to fit evenly within the Z range (Z End – Z Start), so each Z pass has the same depth instead of having a short depth on the last pass. For a single Z pass at Z End, enter 0 or a full Z range value into the Depth of Cut DRO.

Z Clear – Z location the tool moves or retracts to when starting or ending a Z pass, a section sweep, or a section change. This should be set to clear any obstructions between path changes.

Pocket Tab

Pocket cuts a rectangular or circular pocket (cavity). The rectangular pocket can have a corner radius specified, or otherwise the tool paths have sharp corners (see Figure 30).

Open

Figure 30

Rectangular

The general tool path pattern for Pocket-Rectangular depends on the size of the width (width being considered the smaller of X or Y widths) and length of the pocket relative to tool diameter. The pattern within each Z Depth of Cut pass is repeated within the Z range (Z End – Z Start), but the entry and clearing patterns may be different. There are three sub-patterns: entry, clear (out material), and perimeter.

If tool diameter is bigger than pocket width no G-code being produced, an error appears on the Status tab.

If the tool just fits within the pocket width and length, a straight Z plunge in the pocket center is used, therefore a center cutting end mill is needed. Next comes a single pass around the perimeter. This is repeated for each Z Depth of Cut pass.

If the tool just fits within the pocket width, but length is greater than 2x tool diameter, this allows a linear ramp entry which also does the material clearing. The linear ramp is limited to a Z slope of 2° or less (the angle is adjusted smaller to fit the slot length). A single perimeter cut is done next.

If the pocket width and length are greater than 2x tool diameter, this allows a helical entry which cuts a hole of 2x tool diameter in the center of the pocket. Material clearing is done by squaring up the hole, then cutting wings to each side of the pocket length. Finally, a perimeter cut is done.

X and Y Start and End DROs

Start and End – These DROs should be set to the location of the pocket edges.

Radius – Enter 0 if no corner radius is desired. Valid radii values are from 0 up to one half of the pocket’s narrow width (or limited to full radii on the long ends of the pocket). The actual corner radii must be larger than or equal to the tool’s radius, but Pocket tolerates radius entries less than the tool radius – the tool path will just be a sharp corner.

Stepover – This is the offset between adjacent tool paths. A stepover of 0 creates a single pass (or rectangular slot) around the perimeter (inside) of the pocket.

Z DROs

Z Start and End – The first Z pass will cut at Z Start – Depth of Cut adjusted. The last Z pass cuts at the Z End location. For a single Z pass at Z End, enter 0 or a full Z range value into the Depth of Cut DRO.

Depth of Cut – The Depth of Cut entered into the DRO is later adjusted to fit evenly within the Z range (Z End – Z Start), so each Z pass has the same depth instead of having a short depth on the last pass. For a single Z pass at Z End, enter 0 or a full Z range value into the Depth of Cut DRO.

Z Clear – Z location the tool moves or retracts to when starting or ending the Pocket routine.

Circular

Pocket-Circular has a different entry for cutting a circular pocket dependent on the pocket diameter and the tool diameter (see Figure 31).

• If the tool diameter is bigger than pocket diameter:

  • This produces an error with no G-code being produced.

• If the tool just fits within the pocket diameter:

  • A straight Z plunge in the pocket center is used, therefore a center cutting end mill is needed. Next comes a single pass around the perimeter. This is repeated for each Z Depth of Cut pass.

Open

Figure 31

• If the pocket diameter is greater than 2x tool diameter:

XY DROs

X and Y Center – These DROs should be set to the location of the pocket center.

Pocket Dia. – Enter the value of the pocket diameter. The tool radius is used to set the tool path diameter.

Stepover – This is the tool path offset between each rotation of the spiral cut. A stepover of 0 creates a single pass (or circular slot) around the perimeter (inside) of the pocket.

Z DROs

Z Start and End – The first Z pass cuts at Z Start – Depth of Cut adjusted; last Z pass cuts at the Z End location. For a single Z pass at Z End, enter 0 or a full Z range value into the Depth of Cut DRO.

Depth of Cut – The Depth of Cut entered into the DRO is later adjusted to fit evenly within the Z range (Z End – Z Start), so each Z pass has the same depth instead of having a short depth on the last pass. For a single Z pass at Z End, enter 0 or a full Z range value into the Depth of Cut DRO.

Z Clear – Z location the tool moves or retracts to when starting or ending the Pocket routine.

Drill/Tap Tab

Drill/Tap provides a means to create a hole location list, then, based on DRO entries, configures an appropriate canned cycle G-code to create holes – either Pattern or Circular (see Figure 32).

Open

Figure 32

The Drill/Tap tab contains a separate, smaller notebook consisting of two tabs: Pattern and Circular.

Pattern DROs

Hole Location Table – This table should be used for making a list of X and Y locations for each hole using the same tool, Z, and common DRO entries (see Figure 32). To create holes using different tools or other parameters, post the first group, clear the table, enter the next group of locations and other parameters, then append the new list to the existing posted file.

Holes in a list are completed in order from top to bottom. You can rearrange the row order by using the Raise and Lower buttons. To move a row, first activate it by clicking anywhere on the desired row, which highlights it in blue, then select either Raise or Lower. To edit an X or Y cell, click on the desired row, then click the desired cell. An active cell shows up as a white box with a cursor marker (which looks like | ) on a blue row. If there is already a number in the selected cell, it is blocked in blue and is replaced with any number typed in.

To edit an existing number, click on the number until a cursor appears. The Clear All button clears all entries in the table. Leaving a cell checks the entry to see if it is a valid number. If not, the entry is erased and an error shows up in the Status tab. Rows are checked when Post to File is clicked. Any missing entries (an X without a Y, a Y without an X, or an empty row before the last row with an entry) stop the posting and insert the text “??” in the cells with missing entries. Fill in the missing entries, delete any “??” entries and Lower any empty rows past the last row with an entry, then try posting again.

The Circular tab creates a specific hole pattern of evenly spaced holes around a circumference, also know as a bolt pattern (see Figure 33). As with the Pattern tab, all features and corresponding DROs, like Spot and Peck, are retained.

Open

Figure 33

Circular DROs

Number of Holes – Specifies the number of holes in the pattern. This must be greater than zero.

Start Angle – Specifies the angle from angle 0. Angle 0 is a base (horizontal) line from the center point going right (east) to the circumference. The angle from the base line can be either positive or negative, up to 90 degrees (or -90 degrees) and rotates the pattern either clockwise or counterclockwise. A negative angle produces a clockwise rotation; a positive angle produces a counterclockwise rotation. For example, to create a hex pattern with flats on the top and bottom, enter 0 into the Start Angle DRO. To create a hex pattern with flats on the left and right sides, enter 30 (or -30) into the Start Angle DRO.

Diameter – The size of the circular pattern as defined by a line through the center point of each hole.

Center X, Center Y – Defines the center point of the circular pattern.

Spot Tool # – If this DRO contains a valid tool number when Post To File is clicked, a spot drilling sequence using this tool number will occur prior to the drilling sequence. The Feedrate, Spindle RPM, and Z Clear from the drilling sequence will be used for the spot drilling operation. The depth of cut for the spot drilling will be taken from the Spot Drill DOC DRO.

Spot Tool DOC – If the drilling operation includes spot drilling, this DRO will be used to determine the depth of cut for the spot drilling operation (for more information on defining a tool for a spot drilling operation, refer to Spot Tool # earlier in this section).

Drill

The Drill tab uses one of the canned G8x cycles to drill a hole at each location called out in the Hole Location Table (see Figure 32). The drill cycles available are: G81 – Drill, G82 – Drill with Dwell, and G83 – Drill with Peck (features can not be combined; peck cancels dwell).

Since it is usually more convenient to touch-off a drill on its point, that configuration is presented in the graphics. Hole depth is usually defined as the full diameter portion of the hole, so the Z length from the drill point to the corner may need to be considered.

Dwell – An entry greater than 0 replaces G81 with G82 in the G-code, unless there is an entry greater than 0 in Peck. The G82 routine feeds at the Z Feedrate (a DRO in the left panel) until reaching the bottom of the hole, then the position is maintained during the period set by Dwell.

This is usually used to let the tool complete the cutting of the hole bottom before retracting. A revolution calculation is presented in the graphics to aid in setting an appropriate dwell value (such as half revolution for a two flute drill).

Peck – An entry greater than 0 replaces G81 with G83 in the G-code. The G83 routine feeds at the Z Feedrate starting from Z Clear down a Peck distance, then rapid retracts to Z Clear, and rapid returns to start the next peck. The peck distance is not adjusted so the first and last peck will likely be shorter than the Peck setting.

Z DROs

Z Start and End – G8x starts at the Z Clear location and ends at Z End location.

Z Clear – This is the Z location the tool moves or retracts to at the start, end, and while pecking, as well as moving between holes, so it must clear any obstructions along the path between holes.

Tap

Tap uses the G84 canned cycle which is similar to the G81 drill cycle, except a spindle reversal is commanded at the bottom of the hole (see Figure 34). It is important that the Z Feedrate matches the spindle RPM and tap pitch, so the rate is calculated from the pitch and RPM DRO entries. The result is displayed in the Z Feedrate DRO (in the left panel) after the Enter key is pressed in one of the RPM, Pitch, or TPU DROs. Note that an auto-reversing tapping head typically uses a drilling cycle.

Open

Figure 34

Dwell – Allows for tapping with a tension/compression tapping head. A calculation is presented as a guide to how much the tapping head may need to extend while the Z-axis is stopped during spindle reversal at the bottom of the hole. Dwell travel is half the distance the tap would travel at the selected RPM. This assumes half the dwell time is on the down stroke and half up. It is also assumed the RPM is constant during the down stroke, but since the spindle is actually decelerating to a stop, the actual travel should be considerably less.

Pitch and Threads/Unit – These DROs are linked; enter whichever value is handy. When the Enter key is pressed, the corresponding DRO is calculated and updated.

Z DROs

Z Start and End – G84 starts at the Z Clear location, reverses the spindle at the Z End location, and ends back at the Z Clear location. Note that the tap continues a little bit beyond Z End during the dwell period.

Z Clear – This is the Z location the tool moves or retracts to at the start and end of a hole, as well as moving between holes, so it must clear any obstructions along the path between holes.

Thread Mill Tab

The thread milling routine produces helical tool paths needed for milling straight external or internal right-handed threads based on pitch, diameter, and length (see Figures 6.35 and 6.36).

Open

Figure 35

Open

Figure 36

Thread Table – Contains values for some common threads. The threads listed follow the current unit setting (inch or millimeter). Once a selection is made, the data from the selected thread is copied to the appropriate DROs. This table is stored in user-editable text files found in the thread_data subdirectory of the G-code folder on the controller's hard drive; to edit (e.g., to add to or modify the defaults), highlight the file and click Edit G-code. For more information on files stored on the controller's hard drive, refer to File Tab section earlier in this chapter.

NOTE: The values entered in these tables assume a full form thread tool. If using a fine point threading tool to cut coarse threads, the root diameter must be modified to account for the smaller tool nose radius of the fine point threading tool.

XY DROs

X and Y – These DROs locate the center of the threaded stud or hole.

Major and Minor Diameter – Sets the start and end diameter of the thread peak and valley.

Depth of Cut – Sets the amount of material cut in each helical pass. The value entered is the distance (change in radius) the tool is fed on the first pass. This first pass cuts a triangular area which is related to the chip load. Subsequent cut depths are set to cut the same amount of area, so the linear feed gets smaller for each pass. The tool is also fed in on a compound angle of 30°, keeping the cuts to one face of the tool. The number of passes that fit in a thread depth is calculated and presented in the Number of Passes DRO.

Number of Passes – This DRO value is either calculated from the Depth of Cut value or can be entered here, which invokes (upon pressing the Enter key) a calculation and entry to the Depth of Cut DRO.

Z DROs

Z Start and End – Sets the location of the thread start and end. The tool will actually go beyond Z End due to the cutting tip width and the Z component of the compound feed angle and thread depth.

Z Clear – This is the Z location the tool moves or retracts to when starting or ending a Z pass. This should be set to clear any obstructions in the path between the end of one Z pass and the beginning of the next.

Threads/Unit and Pitch – Pitch is used to set the helix feed in Z per turn. An entry in one of these DROs will invoke a calculation and entry into the other, so enter whichever type of setting that is handy.

Engrave Tab

The Engrave tab (see Figure 37) contains functions to engrave a single line of text cut in a single horizontal pass (along the X-axis). This is a basic text engraving routine best suited for engraving True Type stick or outline fonts into things like simple plaques, control panels, or data plates.

Open

Figure 37

Fonts describe paths of the tool control point; therefore, the tool’s effective cutting diameter may need to be considered for overall character size.

Serial numbers – a number that sequentially increases with each Cycle Start – can be engraved alone or added to the end of any desired text. Serial numbers use their own non-proportional font and are scaled to match the defined font extents. For more information on adding serial numbers to an engraving routine, refer to SN Start later in this section.

X and Y Start – Sets the location of the left side of the first character’s baseline. If any characters in the text have descenders, such as y or g, they extend down below the baseline. The tool’s effective cutting diameter may cut an area before or beyond the start location (see Figure 38).

Open

Figure 38

Height – Sets the Y distance from bottom to top of text. This includes ascenders and descenders, but not the tool cutting diameter (subtract this diameter from the overall desired height to get a more accurate value to enter). Height is used with the font data to calculate a scale value that is applied to the character paths in the G-code. The actual height may vary and need adjustment.

Text DRO – Is the text to be engraved. A sample of the text in the selected font is updated when the Enter key is pressed.

SN Start – Sets a starting serial number. Add zeros in front of the first digit as a hint to the number of decimals to be engraved in the series (including leading zeros). For example, if '0012' is entered, '0012,' '0013,' '0014,' '…' will be engraved. If '99' is entered, '99,' '100,' '101,' '…' will be engraved. The current serial number is stored internally; to view, hover over the SN Start DRO.

NOTE: Leave the Text DRO blank to only engrave a set of sequential serial numbers; likewise, leave SN Start blank to only engrave a line of text. It is an error if both the Text DRO and SN Start are blank.

Font – Lists the True Type font files found in the font directory. Scroll through and click on the desired font; clicking presents a sample in the Text DRO. Some font files do not render in this box, but may be viewed by posting the file and checking the font in the Main tab’s preview window (see Figure 38). True Type font files may be added to the Font list by transferring font files to the gcode/engraving_ fonts sub-directory in the controller's home directory (for more information, refer to File Tab section earlier in this chapter). Power the controller off and back on to refresh new files in the Font list.

Z DROs

Z Start – Sets the location of the surface to engrave.

Depth of Cut – Is the depth the cutter is fed into the workpiece.

Z Clear – This is the Z location the tool moves or retracts to at the start and end of the engraving routine, and when moving between characters.

DXF Tab

You can import a .dxf file (Drawing Exchange Format) into PathPilot to generate G-code, which can then cut the shape (or shapes) described in the .dxf file. For example, you could use this feature to engrave logos or artwork.

1. Click the File DRO.
   The File Selector dialog box opens.

2. Select the .dxf file, and then click Open.
   The shapes from the selected file are loaded into the Preview window in the DXF tab.

3. Set the offsets: In the X Offset DRO and the Y Offset DRO, type the offset value added in the XY direction from the bottom left corner of the .dxf drawing.

4. In the Scale DRO, type the scale factor for the drawing. The value typed in the Scale DRO is used as a multiplier for the .dxf dimensions.

5. In the Rotate DRO, type the rotation angle in degrees.
   The rotation angle is applied around the Z-axis of the drawing’s origin.

6. Select the cutter compensation to be applied to the tool path: Click one of the following radio buttons:

• On: the tool moves along the path.

• Outside / Right: offsets the tool path right of the drawing path, seen from the direction where the tool enters the path.

• Inside / Left: is the opposite of Outside / Right.

Working with Layers and Shapes

The .dxf file contains shapes grouped into layers.

In the Shape Selection tree view window, you can enable or disable individual layers and complete layers. You can select shapes either from the tree view window or in the Preview window.

To Change the Layer or Shape Cut Order

To change the shape order, use the Up Arrow and Down Arrow buttons above the shape selection tree view window. Shapes or layers higher in the tree view window are cut earlier than those below it.

The order in which the shapes are cut matches the order of the enabled shapes in the tree view window and the cyan path in the Preview window.

If a layer is selected, the whole layer is moved up or down. Shapes can’t be moved between layers.

To Adjust the Tree View Window

Use the Fold and Unfold buttons to collapse and expand the layer and shape tree in the tree view window.

Working in the Preview Window

The Preview window uses the following colors:

• Selected paths are cyan

• Disabled paths are gray

• The drawing path is white

• The cut path is magenta

• The tool path between cuts is a dark cyan stippled line

• The coordinates are identified as follows:

• The X-axis is red

• The Y-axis is green

• The Z-axis is blue

Probe Tab

The Probe tab of the notebook contains automated functions to find X/Y/Z locations, set work offsets, probe pockets, slots or bosses, as well as instructions on probe and toolsetter setup and calibration. The Probe tab contains a separate, smaller notebook that consists of three tabs:

• X/Y/Z Probe

• Rect/Circ Probe

• Probe/ETS Setup

Tool 99 (the probe tool) must be the current tool in spindle before using any of the probing functions. All probing moves occur at a feed rate specified by the current F command. This can be viewed and modified in the feed rate DRO. For more information, see Feed Rate DRO earlier in this chapter. Disable the spindle (Spindle Lockout Key off) to prevent accidental spindle start with probe in spindle.

NOTE: Check that probe polarity is set correctly on Settings screen (before using the probing buttons) by pressing probe tip while looking at Accessory Input LED on Probe screen (see Figure 39).

Open

Figure 39

XYZ Probe Tab

The X/Y/Z Probe tab of the Probe notebook allows the user to quickly touch off a workpiece or vise jaw to find that feature’s location in current work offset coordinates, or to touch off that feature and set the work offset zero to the feature’s surface (see Figure 39).

The Find Corner, Set Work Origin button is used to probe the corner of a vise jaw or rectangular workpiece, and set that corner to X/Y zero.

NOTE: To change the corner on which to probe a part, click Change Corner.

To use this button, first position the probe below the surface of the vise jaw and roughly 1” away from the vice jaw corner in X and Y (see Figure 39). Upon completion of the probing moves, the current active work offset system (e.g. G54) is set such that the vise jaw corner is 0, 0 (the X/Y origin).

The Probe (Axis), Set Work Offset buttons will probe in one axis only and set the current work offset origin to the probed surface for that axis. The direction of probing is specified by the + or – sign on the button and is described by the accompanying graphic.

The Probe (AXIS) buttons cause a probing move similar to the Probe (AXIS), Set Work Offset buttons, but will not change the work offset value. Instead, the location of the probed surface is displayed in the label below the button.

Rect/Circ Tab

The Rect/Circ tab of the Probe notebook contains buttons that automate tasks like finding the center of a pocket, slot, or bore, as well as finding the center of a circular or rectangular boss (see Figure 40). As the on-screen instructions suggest, first jog the probe below the top surface of the feature to be probed.

Open

Figure 40

The Find Pocket Center, Set Work Origin button works in either a round or rectangular pocket. The probe moves in both X and Y to find the pocket center. The Find Center, Set Work Origin buttons perform a similar probing operation, but in X or Y only, and are intended to be used to find the center of a slot.

The rectangular boss center finding routine hunts around the edge of a square or rectangular workpiece to find the center. To use this routine, start with the probe below the top surface of the boss and on the left-hand side. Similarly, the circular boss center finding routine probes three times to find an approximate center of curvature, then confirms the circular boss center with four additional moves. To use this feature, start with the probe below the top surface of the boss and on the left-hand side.

The Find A Axis Center & Set Work Origin button (see Figure 40) is available for use with a 4th axis mounted in the A-axis orientation. The function probes a round workpiece mounted in the A-axis to find the center rotation of the A-axis. Move the probe to a point approximately directly above the A-axis center of rotation, and click the Find A Axis Center & Set Work Origin button (see Figure 40).

Probe/ETS Setup Tab

The Probe/ETS Setup tab is used to align and set the probe and ETS heights (see Figure 41). For information on probe and ETS setup, refer to chapter 8, Accessories, in your operator manual.

Open

Figure 41

ADMIN Commands

Several ADMIN commands are provided for operator use.

Looking for more information?

This is a section of the PCNC 770 operator's manual. To view the whole manual, go to Tormach document UM10350.

If you have additional questions, we can help. Create a support ticket with Tormach Technical Support at http://tormach.com/how-to-submit-a-support-ticket for guidance on how to proceed.