PathPilot Tools and Features

In This Section, You'll Learn:

How to use PathPilot, depending on the activity that you want to do.

Create and Load G-Code Files

To get started with PathPilot, you must first load or create a G-code file.

Load G-Code

To run a G-code program on a PathPilot controller, you must first verify that the file is on the controller. For more information on transferring and moving files, see "Transfer Files to and From the Controller".

To load G-code:

1. From the File tab, in the Controller Files window, select the desired .nc file.

2. Select Load G-Code.

NOTE: This function is only available for files stored on the PathPilot controller.

PathPilot loads the G-code file and opens the Main tab.

Transfer Files to and From the Controller

To run a G-code program, you must transfer the files to the PathPilot controller. You can either use a USB drive or PathPilot HUB (our cloud-based simulator) to transfer files. For more information on PathPilot HUB, go to hub.pathpilot.com.

To transfer files to and from the controller:

1. Either insert a USB drive into any open USB port, or sign in to PathPilot HUB.

2. From the File tab, select the file to transfer (either in the USB Files window or the Controller Files window).

NOTE: Select Back to move backward and either Home or USB to move to the highest level.

3. Select the location to which you want to copy the transferred file.

4. Select either Copy <- or Copy ->.

NOTE: The file must have a unique name. If it doesn't, you must either overwrite the file, rename the file, or cancel the file transfer.

5. If you’re using a USB drive, Select Eject.
   It's safe to remove the USB drive from the controller.

Preview G-Code Files

You can preview an .nc file that's either on the PathPilot controller or on a USB drive.

To preview G-code files:

• From the File tab, in the Controller Files window or the USB Files window, select an .nc file.

The text displays in the Preview window.

Access Recent G-Code Files

You can load a recently loaded G-code file from the Main tab. For information, see "About the G-Code Tab".

To access recent G-code files:

1. From the Main tab, in the G-Code tab, select the Recent Files menu.

The last five program files loaded into PathPilot display.

2. Select the name of the desired G-code program.
   The G-code program loads.

Close the Current Program

1. From the Main tab, on the G-Code tab, select the Recent Files menu.

2. Select Clear Current Program.

The currently loaded G-code program closes.

Edit G-Code

In PathPilot, there are two ways to edit G-code:

Edit G-Code with a Text Editor

You can edit .nc files that are on the PathPilot controller. If the .nc file is in the USB Files window, you must first transfer it to the controller; go to "Transfer Files to and From the Controller".

To edit G-code with a text editor:

1. From the Controller Files window, highlight the .nc file and select Edit G-code.

The file opens in a text editor.

2. Make and save the appropriate changes to the file.

3. Close the text editor.

Tip! To quickly edit an already loaded G-code program from the Main tab, you can use a keyboard shortcut: Shift+Alt+E.

Edit G-Code with Conversational Programming

You can edit .nc files that are on the PathPilot controller. If the .nc file is in the USB Files window, you must first transfer it to the controller; go to "Transfer Files to and From the Controller".

To edit G-code with conversational programming:

1. From the File tab, select the .nc file.

2. Select Conv. Edit.
   The file opens in a job assignment editor window: the program's job assignments are on the left and a preview of the program is on the right.

3. Edit the file contents as needed. Do any of the following:

• Change the Step Order

• Create a New Job Assignment

• Load an Existing G-Code File

• Edit a Job Assignment

4. Select Save.
   The G-code program file is updated.

Change the Step Order

• Select Move Up, Move Down, Duplicate, or Remove.

Create a New Job Assignment

1. Select Insert Step.
   PathPilot opens the Conversational tab.

2. Create the new job assignment.

3. Select Insert.

4. (Optional) Edit the job assignment order in the program.

Load an Existing G-Code File

1. Select Insert File. You can insert G-code files that are hand-written, generated from CAM software, or generated from conversational programming in PathPilot.

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

3. Select Open.

4. (Optional) Edit the job assignment order in the program.

Edit a Job Assignment

1. Select the job assignment, and then select Conv. Edit.
   PathPilot opens the Conversational tab.

2. Edit the job assignment.

3. Select Finish Editing.

Tips

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

NOTE:  Revert is only available for individual job assignments created in conversational programming.

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

Read G-Code

Once your G-code file is loaded into PathPilot, you can read it in the following ways:

Expand the G-Code Tab

You can change the size of the G-Code tab if you need more space to view the code. For more information on using the G-Code tab, see "About the G-Code Tab".

To expand the G-Code tab:

• Select the Window Expander.

The Tool Path display shrinks.

About the G-Code Tab

The G-Code tab displays the code of the currently loaded program file. Use the scroll bars to view the entire file. You can make the G-Code tab larger. For information, see "Expand the G-Code Tab".

PathPilot highlights certain lines of code of interest. When running a G-code program in single block mode, there may be as many as two lines of G-code highlighted, both with a different color:

• Green Line Indicates the start line (the line from which PathPilot starts the program).
  To change the start line, go to "Set a New Start Line".

• Orange Line Indicates the line of code that PathPilot is currently executing.

Search in the Code

You can use PathPilot to search the text of a G-code program file for specific numbers, codes, or other items of interest (like tools, feeds, and speeds).

To search in the code:

1. From Main tab, on the G-Code tab, select any line of code to use as a starting point.

2. In the MDI Line DRO field, type Find followed by one of the following:

• Any text. PathPilot searches for instances of the specific number or code.

• Feed. PathPilot searches for instances of the actual word Feed and any F G-code command.

• Speed. PathPilot searches for instances of the actual word Speed and any S G-code command.

• Tool. PathPilot searches for instances of the word Tool and any T G-code command.
  NOTE: The find command is not case-sensitive.

3. Select the Enter key.
   If PathPilot finds the information, the searched term is scrolled to and highlighted in the G-Code tab.

4. (Optional) Select Enter.
   PathPilot finds the next instance of the searched text.

5. (Optional) Select Enter+Shift.
   PathPilot finds the previous instance of the searched text.

NOTE: When the search reaches the end of the G-code file, it starts again from the beginning.

Set a New Start Line

The start line (the line from which PathPilot starts the program) is, by default, the first line of code in the program.

To set a new start line:

1. From the Main tab, on the G-Code tab, do one of the following:

   1. Right-click any line in the program.

• Tap the line. Then, select the Options menu.

2. Select the desired lead-in move. For information, see "Lead-In Moves".

Lead-In Moves

• Set start line (no preparation) Keep the current tool in the spindle, with the current tool length applied. The machine executes the start line from the current position.

NOTE: We don't recommend this option for starting partway through a cut.

Example

Starting the program at a tool change.

Starting the program with a different tool in the spindle than the program calls for (like if your tool broke, which you've replaced, but you'd rather not edit the entire program or the tool table entry).

• Set start line (restore with linear lead-in) Perform a tool change (as required). The machine rapids in X and Y, then Z to the current position, then feeds in a straight linear line to the start line position.

NOTE: This option assumes that the current position is the lead-in position.

Example
Quickly resuming work after stopping the program to make an adjustment to the machine setup (like clearing chips, removing an object, or turning on the coolant pump). Because the machine's already set up, you can position the tool near the stopping point.

• Set start line (restore with Z plunge lead-in) Perform a tool change (as required). The machine rapids in Z to G30 clearance height, rapids in X and Y to the start line position, then feeds in Z to the start line position.

Example
Running a sub-section of a large program when the correct tool isn't loaded (and positioning the tool tip near the starting point is difficult, like with a long tool or fly cutter loaded). This option doesn't require you to jog to the exact lead-in position.

Change the View of the Tool Path Display

1. From the Main tab, do one of the following:

• Right-click the Tool Path display.

• Select the View Options tab.

2. Select a new view.
   For information, see "About the Tool Path Display" (page 10).

About the Tool Path Display

The Tool Path display is a graphical representation of the currently loaded G-code file's tool path.

There are four available views:

• Front

• Iso

• Side

• Top

You can see grid lines behind the tool path while you are using either a Top, Front, or Side view. Depending on which programming mode you're in (G20 or G21), PathPilot defaults to one of the following grid line spacings:

• G20 Mode 1/2 in. intervals

• G21 Mode 5 mm intervals

In the Tool Path display, there are four different line types:

• Dotted Blue Lines Indicate the boundary box (the ends of travel of the axes).

• Red Lines Indicate the tool path as it is cut.

NOTE: The Tool Path display shows the program extents — the furthest points to which the tool will travel while running the program — of the currently loaded G-code file alongside the tool path lines.

• White Lines Indicate the preview lines.

• Yellow Lines Indicate the jogging moves.

To erase the jogging moves (yellow line) or the tool path (red lines), do one of the following:

• Double-click anywhere in the Tool Path display.

• Select Reset.

Use Conversational Programming

To create simple parts, use the conversational programming feature in PathPilot.

About Conversational Programming

PathPilot includes G-code generators intended to make simple G-code programs:

• Programs for simple parts.

• Programs for parts made up of a collection of simple features.

NOTE: For complex parts, or parts with complex shapes, we recommend you use a CAD/CAM program.

The Conversational tab is divided into two sections:

• Parameters common to most operations, like speeds and feeds.

NOTE: DRO fields that are grayed out are not available for the specific conversational features.

• Parameters specific to each operation, like part geometry.

Create a Face on a Part

Using conversational programming, you can program PathPilot to take multiple cuts — each following the last — on an X/Y plane over a Z range. For information, see "About Facing" (page 12).

Before You Begin

Before you begin, you must verify that you enter the program values considering the following:

• The area from the rear, left corner of the workpiece to the rear, right corner of the workpiece must be clear of any obstructions from the Z Start position to the Z End position.

• The top of the workpiece must be free of any workholding devices.

• The value used in the Z End DRO field must be such that it is above the workholding device.

• The value used in the Z Clear DRO field must be such that it is above any obstruction in the tool path between the end of one pass and the beginning of the next.

To create a face on a part:

1. From the Conversational tab, select the Face tab.

2. From the Conversational DROs group, set the parameters for the facing operation.

3. Work through the program-specific DRO fields:

   1. In the X Start DRO field and the X End DRO field, type the location of the workpiece edges. We recommend using the rear left corner of the part for the X Start value.

   2. In the Y Start DRO field and the Y End DRO field, type the location of the workpiece edges. We recommend using the front right corner of the part for the Y End value.

   3. In the Stepover DRO field, type the required distance between tool paths. To prevent uncut areas in the spiral corners, we recommend limiting this value to 80% of the tool diameter. For information, see "Facing Reference".

   4. In the Z Start DRO field and the Z End DRO field, type the location of the first and last Z passes. For a single Z pass at the location typed in the Z End DRO field, type a value of 0 or a full Z range value into the Depth of Cut DRO field.

   5. In the Depth of Cut DRO field, type the desired amount of material to remove.

NOTE: The depth of cut is later adjusted within the Z range so that each pass in the Z range has the same depth (rather than the last Z pass having a short depth of cut).

About Facing

Face milling is the process of cutting a surface that's perpendicular to the axis of the cutting tool. A facing program is usually used to cut an accurate, finished top surface on a rough piece of stock material. After a facing program is complete, tool marks remain — creating a fairly flat surface, with microscopic height differences.

Facing in PathPilot

When using a facing routine, each tool pass along the X-/Y-axis begins off to the side of the workpiece to avoid plunging into the workpiece. To compensate for this procedure, PathPilot sets lead-in tool paths outside of the workpiece using the part's work offsets, the tool's diameter, and the predetermined stepover value. PathPilot also adjusts the depth of cut to make sure each tool pass has the same depth, rather than cutting a short depth on the last pass of the program.

During a facing routine, PathPilot does the following:

1. Moves the machine to the predefined G30 position, or the tool change position.

2. If required, performs or requests a tool change.

3. Makes a rapid move in the X and Y direction to the beginning of the workpiece.

4. Makes a rapid move in the Z direction to the predefined Z Clear position.

5. Begins the cut in the X/Y plane at an adjusted Z depth of cut.

NOTE: The value entered into the Depth of Cut DRO field is adjusted within the Z range (the value entered into the Z End DRO field minus the value entered into the Z Start DRO field).

6. Makes cuts in a rectangular spiral from the workpiece perimeter to the workpiece center.

For information on using conversational programming in PathPilot to face a part, see "Create a Face on a Part" (page 11).

Facing Reference

PathPilot uses the following terms when creating a face on a part in conversational programming:

• Stepover Indicates how much space PathPilot creates between each spiral tool path.

• Z Clear Indicates the Z location that the tool moves (retracts) to when starting or ending a tool pass.

Create a Profile on a Part

Using conversational programming, you can program PathPilot to take multiple cuts — each following the last — on an X/Y plane over a Z range to form a boss. For information, see "About Profiling".

Before You Begin

Before you begin, you must verify that you enter the program values considering the following:

• The value used in the Radius DRO field must be between 0 and either:

  • One half of the boss' narrow width, or

  • The full radii on the long ends of the boss

• The value used in the Z Clear DRO field must be set to clear any obstructions between path changes.

To create a profile on a part:

1. From the Conversational tab, select the Profile tab.

2. From the Conversational DROs group, set the parameters for the profiling operation.

3. Work through the program-specific DRO fields:

   1. In the X Start DRO field and the X End DRO field, type the location of the workpiece edges.

   2. In the Y Start DRO field and the Y End DRO field, type the location of the workpiece edges.

   3. In the X Profile Start DRO field, the X Profile End DRO field, the Y Profile Start DRO field, and the Y Profile End DRO field, type the location of the profile's outer edges.

   4. In the Stepover DRO field, type the required distance between tool paths. If you want a single cut in the workpiece (to create a slot), type 0.

   5. In the Radius DRO field, type the required radius for the corners of the profile. For no corner radius, type 0.

   6. In the Z Start DRO field and the Z End DRO field, type the location for the first and last Z passes. For a single Z pass at Z End, type 0 — or a full Z range value — in the Z DOC DRO field.

   7. In the Z DOC DRO field, type the desired amount of material to remove.

NOTE: The depth of cut is later adjusted within the Z range so that each pass in the Z range has the same depth (rather than the last Z pass having a short depth of cut).

About Profiling

A profiling program is usually used to create a circular or rectangular boss within a larger piece of stock material. The outer bound of the area is the stock material's perimeter. The inner bound of the area is the boss' perimeter.

Profiling in PathPilot

When using a profile routine, each tool pass along the X-/Y-axis begins off to the side of the workpiece to avoid plunging into the workpiece. To compensate for this procedure, PathPilot sets lead-in tool paths outside of the workpiece using the part's work offsets, the tool's diameter, and the predetermined stepover value. PathPilot also adjusts the depth of cut to make sure each tool pass has the same depth, rather than cutting a short depth on the last pass of the program.

When you're creating a profile on a part using conversational programming, PathPilot does the following in the order listed:

1. Retracts the tool to the Z Clear position.

NOTE: The first Z pass cuts at Z Start minus Depth of Cut adjusted.

2. Makes a rapid movement to the beginning of the section.

3. If required, makes a tool path around the perimeter of the boss to cut the programmed radii.

NOTE: Radius cuts use an adjusted feed rate to compensate for the difference between the tool's control point rate (at the tool center) and the actual rate at the radius surface.

4. Repeats Steps 1-3 for each predefined Z Depth of Cut.

NOTE: The last Z pass will cut at the Z End location.

For information on using conversational programming in PathPilot to create a profile, see "Create a Profile on a Part".

Profiling Reference

PathPilot uses the following terms when creating a profile on a part in conversational programming:

• Stepover Indicates the tool path offset between section sweeps.

• Z Clear Indicates the Z location the tool moves to or retracts to when starting or ending a section change, section sweep, or Z pass.

Create a Pocket on a Part

Using conversational programming, you can program PathPilot to take multiple cuts — each following the last — on an X/Y plane over a Z range to form a circular or rectangular pocket. For information, see "About Pockets".

Before You Begin

Before you begin, you must verify that you enter the program values considering the following:

• The value used in the Radius DRO field must be between 0 and either:

  • One half of the pocket's narrow width, or

  • The full radii on the long ends of the pocket

To create a circular pocket on a part:

1. From the Conversational tab, select the Pocket tab.

2. From the Conversational DROs group, set the parameters for the pocket operation.

3. Work through the program-specific DRO fields:

   1. In the X Center DRO field and the Y Center DRO field, type the location of the pocket's center.

   2. In the Pocket Dia. DRO field, type the required diameter for the pocket.

NOTE: The radius of the tool is used to set the tool path diameter.

c. In the Stepover DRO field, type the required distance between each rotation of the spiral cut. For a single cut around the inside perimeter of the pocket (to create a slot), type 0.

d. In the Z Start DRO field and the Z End DRO field, type the location of the first and last Z passes. For a single Z pass at the location typed in the Z End DRO field, type a value of 0 or a full Z range value into the Depth of Cut DRO field.

e. In the Z DOC DRO field, type the desired amount of material to remove.

NOTE: The depth of cut is later adjusted within the Z range so that each pass in the Z range has the same depth (rather than the last Z pass having a short depth of cut).

To create a rectangular pocket on a part:

1. From the Conversational tab, select the Pocket tab.

2. From the Conversational DROs group, set the parameters for the pocket operation.

3. Work through the program-specific DRO fields:

   1. In the X Start DRO field, the X End DRO field, the Y Start DRO field, and the Y End DRO field, type the location of the pocket edges.

   2. In the Radius DRO field, type the required radius for the corners of the pocket. For no corner radius, type 0.

   3. In the Stepover DRO field, type the required distance between adjacent tool paths. For a single cut around the inside perimeter of the pocket (to create a slot), type 0.

   4. In the Z Start DRO field and the Z End DRO field, type the location of the first and last Z passes. For a single Z pass at the location typed in the Z End DRO field, type a value of 0 or a full Z range value into the Depth of Cut DRO field.

   5. In the Z DOC DRO field, type the desired amount of material to remove.

NOTE: The depth of cut is later adjusted within the Z range so that each pass in the Z range has the same depth (rather than the last Z pass having a short depth of cut).

About Pockets

A pocket program is usually used to remove a large amount of material from a part.

Creating Pockets in PathPilot

For more information about creating a pocket on a part using conversational programming, see of the following sections, depending on the shape of the pocket:

• "About Circular Pockets"

• "About Rectangular Pockets"

For information on using conversational programming in PathPilot to make a pocket on a part, see "Create a Pocket on a Part".

About Circular Pockets

PathPilot does one of the following, depending on the diameter of the tool:

• Tool Diameter Larger Than Pocket Diameter PathPilot displays an error and does not create any G-code. You must select a different tool or edit the diameter of the pocket.

• Tool Diameter Just Small Enough to Fit Within Pocket Diameter PathPilot does the following in the order listed:

1. Uses a straight Z plunge into the pocket center. You must use a center-cutting end mill.

2. Makes a single pass around the perimeter of the pocket at the adjusted Z depth of cut.

3. Continues to make single passes around the perimeter of the pocket.

• Pocket Diameter More Than Two Times Tool Diameter PathPilot does the following in the order listed:

1. Uses a helical entry into the pocket center.

2. Makes a hole that is two times the diameter of the tool diameter in the pocket center.

3. Makes a spiral cut out from the pocket center to the pocket diameter.

4. Makes a cut around the perimeter of the pocket.

About Rectangular Pockets

PathPilot does one of the following, depending on the diameter of the tool:

• Tool Diameter Larger Than Pocket Width PathPilot displays an error and does not create any G-code. You must select a different tool or edit the width of the pocket.

• Tool Diameter Just Small Enough to Fit Within Pocket Parameters PathPilot does the following in the order listed:

1. Uses a straight Z plunge into the pocket center. You must use a center-cutting end mill.

2. Makes a single pass around the perimeter of the pocket at the adjusted Z depth of cut.

3. Continues to make single passes around the perimeter of the pocket.

• Length of Pocket More Than Two Times Diameter of Tool PathPilot uses a linear ramp entry.

• Pocket Parameters More Than Two Times Diameter of Tool PathPilot uses a helical entry.

Create Hole Locations on a Part (Drill/Tap)

Using conversational programming, you can program PathPilot to make multiple holes on a part. For information, see "About Drilling and Tapping".

Before You Begin

Before you begin, you must verify that you enter the program values considering the following:

• In the Conversational DROs group, the value in the Z Clear DRO field must be set to clear any obstructions between hole changes.

To make a specific hole pattern of evenly spaced holes around a circumference (also know as a bolt pattern):

1. From the Conversational tab, select the Drill/Tap tab.

2. From the Drill/Tap tab, select the Circular tab.

3. In the Number of Holes DRO field, type the number of holes (greater than 0) required for the pattern.

4. In the Start Angle DRO field, type the value of the angle from angle 0 (from -90 to 90).

5. In the Diameter DRO field, type the size of the circular pattern (as defined by a line through the center point of each hole).

6. In the Center X DRO field and the Center Y DRO field, type the location for the center of the hole.

7. Depending on if you're drilling or tapping the holes, do one of the following:

• Go to "Create a Drilling Sequence".

• Go to "Create a Tapping Sequence".

Use the Location table to make a list of X and Y locations for each hole using the same tool, the same Z location, and the same values in the Conversational DROs group.

NOTE: You can create holes using different tools or different parameters. You must first post the first group of hole locations, enter the second group of hole locations, and then append the second group to the existing posted file.

To make a hole pattern based on X and Y locations on a part:

1. From the Conversational tab, select the Drill/Tap tab.

2. From the Drill/Tap tab, select the Pattern tab.

3. In the Location table, select the row, then select the cell to edit.
   Holes indicated in the Location table are completed from top to bottom.

4. Depending on if you're drilling or tapping the holes, do one of the following:

• Go to "Create a Drilling Sequence".

• Go to "Create a Tapping Sequence".

Tips

• To rearrange the row order, select a row, and then select Raise or Lower.

• To clear all values in the table, select Clear All.

• To make sure that the value is a valid number, leave the cell. If the value isn't a valid number, it's erased, and an error displays on the Status tab.

• Before posting the file, make sure that there are none of the following:

  • X values without a Y value

  • Y values without an X value

  • An empty row before the last row with values

About Drilling and Tapping

A drilling and tapping program is used to create a series of holes in defined locations on a part.

Drilling and Tapping in PathPilot

PathPilot has the following options to define the locations:

• Pattern Use X and Y locations to make a list of hole locations.

• Circular Use a circumference to make a specific pattern of evenly spaced holes.

For information on using conversational programming in PathPilot to drill and tap holes, see "Create Hole Locations on a Part (Drill/Tap)".

During a drilling routine, PathPilot uses one of the following canned G-code cycles, depending on the entries in each DRO field:

• G81 Drill

• G82 Drill with dwell

• G83 Drill with peck

NOTE: The features can't be combined, because peck cancels dwell.

When using a tapping routine, PathPilot uses the G84 canned G-code cycle. G84 is similar to G81, but it commands a spindle reverse once it gets to the bottom of the hole.

It's 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 selected in one of the RPM, Pitch, or TPU DRO fields.

NOTE: An auto-reversing tapping head typically uses a drilling cycle.

Create a Drilling Sequence

The Drill tab uses one of the following canned G8x cycles to drill a hole at each identified location:

• G81 Drill

• G82 Drill with dwell

• G83 Drill with peck

NOTE: The features can't be combined, because peck cancels dwell.

Hole depth is usually defined as the full diameter portion of the hole, so you may need to consider the Z length from the drill point to the corner.

1. In the Spot Tool # DRO field, type the number of the spot drill.
   If a valid tool number is used in the Spot Tool # DRO field, PathPilot makes a spot drilling sequence before the drilling sequence. In the spot drilling sequence, PathPilot uses the values indicated in the Feedrate DRO field, the Spindle RPM DRO field, and the Z Clear DRO field.

NOTE: To skip a spot drilling sequence, leave the Spot Tool # DRO field blank.

2. In the Spot Tool DOC DRO field, type the depth of cut for the spot drilling sequence.

NOTE: To skip a spot drilling sequence, leave the Spot Tool DOC DRO field blank.

3. In the Peck DRO field, type the distance for each peck.

NOTE: Any entry greater than 0 typed in the Peck DRO field replaces G81 with G83 in the G-code. For information, see "Drilling and Tapping Reference".

4. Set the parameters for the hole in the Z range: 

   1. In the Z Start DRO field, type the location for the first Z pass.

   2. In the Z End DRO field, type the location for the last Z pass.

Create a Tapping Sequence

The Tap tab uses the G84 canned cycle — it's similar to the G81 drill cycle, but it commands a spindle reverse once it reaches the bottom of the hole.

NOTE: If you're using an auto-reversing tapping head, use a drilling sequence. Go to "Create a Drilling Sequence".

1. In the Dwell DRO field, type the time — in seconds — for the tool to pause at the bottom of the hole before retracting.
   A dwell gives the tool time to completely cut the bottom of the hole.

NOTE: Any entry greater than 0 typed in the Dwell DRO field replaces G81 with G82 in the G-code — unless there is an entry greater than 0 in the Peck DRO field.

2. Set the parameters for the threads: In the Pitch (In) DRO field or the Threads/In DRO field, type either the required pitch or the threads per inch.

NOTE: The Pitch (In) DRO field and the Threads/In DRO field are linked — after you type a value in one and press Enter on the keyboard, the other is auto-filled.

3. In the Conversational DROs group, make sure that the value in the Z Feedrate DRO field is the same as the value that you set in Step 2.

4. Set the parameters for the hole in the Z range:

   1. In the Z Start DRO field, type the location for the first Z pass.

   2. In the Z End DRO field, type the location for the last Z pass.

Drilling and Tapping Reference

PathPilot uses the following terms when drilling and tapping on a part in conversational programming:

• 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:

  • Positive or negative

  • Up to 90 degrees (or -90 degrees)
    A negative angle produces a clockwise rotation; a positive angle produces a counterclockwise rotation.

  • Rotates the pattern either clockwise or counterclockwise
    For example, to create a hex pattern with flats on the top and bottom, use a value of 0 in the Start Angle DRO field. To create a hex pattern with flats on the left and right sides, use a value of 30 (or -30) in the Start Angle DRO field.

• Peck The value isn't adjusted: the G83 routine feeds at the Z Feedrate, starting from Z Clear down to the Peck distance, then rapid retracts to Z Clear, and rapid returns to start the next Peck.

NOTE: The first and last peck will likely be shorter than the value typed into the Peck DRO field.

Create Threads on a Part

Using conversational programming, you can program PathPilot to take helical tool paths around a boss or inside a hole to create external or internal threads. For information, see "About Thread Milling".

Before You Begin

Before you begin, you must verify that you enter the program values considering the following:

• The auto-filled DRO field values assume a full-form threaded tool. If you're using a fine-point threaded tool to cut coarse threads, you must modify the root diameter to account for the tool's smaller nose radius.

• The value used in the Z Clear DRO field must be such that it can clear any blockages in the path between the end of one Z pass and the beginning of the next.

To create threads on a part:

1. From the Conversational tab, select the Thread Mill tab.

2. From the Conversational DROs group, set the parameters for the thread milling operation.

3. Depending on the type of threads, do one of the following:

• For external threading (creating threads on a boss, for example), select External.

• For internal threading (creating threads inside a hole, for example), select Internal.

4. Work through the program-specific DRO fields:

   1. From the Quick Reference drop-down, select the thread size.
      The Threads/In DRO field, Pitch (In) DRO field, Major Dia. DRO field, and Minor Dia. DRO field auto-fill.

NOTE: The threads listed follow the current unit setting: either inches (G20) or millimeters (G21).

b. In the Z Start DRO field, type the location of the first Z pass (where you want the thread to start).

c. In the Z End DRO field, type the location of the last Z pass (where you want the thread to end).

NOTE: The tool actually goes beyond the value entered in the Z End DRO field, due to the cutting tip width and the Z component of the compound feed angle and thread depth.

d. In the Depth of Cut DRO field or the Number of Passes DRO field, type a value to represent the amount of material to remove in each helical pass. For information, see "Thread Milling Reference".

NOTE: The Depth of Cut DRO field and the Number of Passes DRO field are linked — after you type a value in one and press Enter on the keyboard, the other is auto-filled.

About Thread Milling

Thread milling is used to make helical tool paths on a part — either externally, like on a boss, or internally, like in a hole. The right-handed threads are based on pitch, diameter, and length.

Thread Milling in PathPilot

For information on using conversational programming in PathPilot to do thread milling, see "Create Threads on a Part".

Thread Milling Reference

PathPilot uses the following terms when creating a thread mill on a part using conversational programming:

• Major Dia. and Minor Dia. Set 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 is the distance (the 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 degrees, keeping the cuts to one face of the tool.

NOTE: The Depth of Cut DRO field and the Number of Passes DRO field are linked — after you type a value in one and press Enter on the keyboard, the other is auto-filled.

• Z Clear The location the tool moves or retracts to when starting or ending a Z pass.

Create Text to Engrave on a Part

Using conversational programming, you can program PathPilot to engrave a single line of text on a part. For example, you could use this feature to engrave True Type stick or outline fonts into things like simple plaques, control panels, or data plates. For information, see "About Engraving" (page 28).

To create an engraving sequence on a part:

1. From the Conversational tab, select the Engrave tab.

2. From the Conversational DROs group, set the parameters for the engraving operation.

3. Work through the program-specific DRO fields:

   1. In the Text DRO field, type the desired text to engrave.
      The text appears in the Preview window.

b. From the Font list, select the desired font for the engraved text.

NOTE: To search the Font list, select a font and begin typing the font's name. PathPilot scrolls to the result.

The Preview window updates to display the font selected.

NOTE: You can add True Type font files to the PathPilot controller. For information, see "Transfer Files to and From the Controller".

c. Use the Alignment radio buttons to select the desired alignment of the text: either Left, Center, or Right.
The Preview window updates to display the font selected.

d. In the Height DRO field, type the distance in the Y direction from the top of the text to the bottom of the text.
PathPilot uses the height value, along with font data, to calculate scale for character paths in the G-code program.

NOTE: The value typed in the Height DRO field includes ascenders and descenders, but no the tool cutting diameter. For a more accurate value, subtract the diameter from the overall height.

e. In the X Base DRO field and the Y Base DRO field, type the location of the left side of the first character’s baseline.

NOTE:   If any characters in the text have descenders, like y or g, they extend below the baseline.

f. In the Z Start DRO field, type the location of the surface on which to engrave.

g. In the Z Depth of Cut DRO field, type the desired depth the that the cutting tool is fed into the workpiece.

h. In the Z Clear DRO field, type the value for the tool to move or retract to — in the Z direction — at the start and end of the engraving sequence and between characters.

About Engraving

Engraving is used to engrave a single line of text cut in a single horizontal pass along the X-axis of a part.

Import a DXF File

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. From the Conversational tab, select the DXF tab.

2. Select the File DRO field.
   The File Selector dialog box opens.

3. Select the .dxf file, and then select Open.

4. The shapes from the selected file are loaded into the Preview window.

NOTE: The .dxf file must already be transferred to the PathPilot controller. For information, see "Transfer Files to and From the Controller".

5. In the X Offset DRO field and the Y Offset DRO field, type the offset value added in the XY direction from the bottom left corner of the .dxf drawing.

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

Example
If you type 1.0 in the Scale DRO field, the .dxf is scaled at 100%.
If you type 2.0 in the Scale DRO field, the .dxf is scaled at 200%.

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

8. Select one of the following to set the cutter compensation to be applied to the tool path:

• 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: 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.

Change the Layer or Shape Cut 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 is the same as the order of the enabled shapes in the tree view window and the cyan path in the Preview window.

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

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:

• Cyan Selected paths

• Gray Disabled paths

• White Drawing path

• Magenta Cut path

• Dark Cyan Stippled Line Tool path between cuts

• The coordinates use the following colors:

  • Red X-axis

  • Green Y-axis

  • Blue Z-axis

Machine Settings and Accessories

Before running a G-code program, you must first make sure that the machine settings are properly configured.

Enable an Internet Connection

If desired, you can enable an internet connection on your PathPilot controller. An internet connection allows you to receive automatic PathPilot updates and transfer files with PathPilot Hub instead of a USB drive.

To enable an internet connection:

1. From the PathPilot interface, on the Status tab, select Internet.

The Network Configuration dialog box displays.

2. From the Network Configuration dialog box, in the Networks list, select the network you want to use. Then, select Connect.

NOTE: Wi-Fi connection signal strengths are indicated on a scale of 0 to 100, with 100 being the strongest. PathPilot continually refreshes the signal levels to help you find the best placement for your Wi-Fi network adapter. Ethernet connections are indicated by a prefix in the following format: eth[NUMBER]. For example, eth1.

The PathPilot operating system connects to the internet using the network you specified. It continues to detect and connect to the Wi-Fi network, even after power cycles.

3. Once connected, you can use the PathPilot Hub and automatic updates features.

Enable Automatic Updates

NOTE: Automatic updates require an internet connection. If you haven't yet enabled it, go to "Enable an Internet Connection".

If desired, you can enable automatic updates for PathPilot.

To enable automatic updates:

1. From the PathPilot interface, on the Status tab, select Update.
   The Software Update dialog box displays.

2. From the Software Update dialog box, select the Check online daily for updates; confirmation required for download and installation checkbox.

3. Select Close.
   When future updates are available, the Status tab displays a notification.

Change the Network Name

If you're connected to a network using either the Ethernet jack or the (optional) Wireless Network Adapter (PN 38207), the PathPilot controller appears on your network as network-attached storage. The default network name of the controller is TORMACHPCNC.

To change the network name:

1. From the Network Name field, type a new network name.

NOTE: The network name must be unique within your network.

2. Select the Enter key.

3. For the change to take effect, you must restart the controller.

Select the Spindle Type

If you have an additional spindle (separate from the standard spindle), you must first select it in PathPilot.

To select the spindle type:

• From the Settings tab, from the Spindle Type drop-down, select the appropriate spindle option.

Change the Screen Orientation

A vertical orientation for 1920 × 1080 monitors is supported in PathPilot v2.10.0 and later. For more information on the portrait layout, go to "About Portrait Screen Layout" (page 37).

To change the screen orientation:

1. From the PathPilot interface, on the Settings tab, select Portrait from the Layout drop-down menu. Restart the controller.

2. Rotate the monitor to the portrait orientation. You can rotate it either left or right, depending on what's easier for your setup.

3. While the controller is restarting, specify which direction you've rotated the monitor. Select Apply. If the result is unexpected, click Restore Previous Configuration on the confirmation dialog and choose a rotation direction again.

The controller restarts in portrait layout.

About Portrait Screen Layout

Portrait layout provides some key advantages:

• A larger tool path window that's always visible at the top of the screen, regardless of which tab you have active.

• A wider G-code window to more easily read the loaded G-code file and, if enabled, line numbers.

• The tool path window's view options are always visible for much easier access.

• When browsing G-code files using the File tab, file previews display on the top portion of the screen.

Specify the Tool Change Method

When PathPilot finds an M06 command in a G-code program, it has different behaviors depending on the specified tool change method.

To specify the tool change method:

• From the Settings tab, select the appropriate tool change method for your machine.

About Automatic Tool Changes

If you're using an Automatic Tool Changer (ATC) to make tool changes, PathPilot does the following:

1. Looks for an ATC.
   In the PathPilot interface, the ATC tab displays.

2. When PathPilot finds a Txx M06 command in the G-code program, the ATC loads the specified tool into the spindle.

About Manual Tool Changes

If you're making manual tool changes, PathPilot pauses when it finds an M06 command in the G-code program. While it's paused, PathPilot does the following:

1. The Cycle Start button flashes.

2. The Tool Path display shows the requested tool number.

Disable Hard Stop Referencing

To provide a temporary workaround for a malfunctioning limit switch circuit, you can disable the limit switches.

NOTE: By default, the Hard Stop Referencing checkbox is selected.

To disable hard stop referencing:

1. From the Settings tab, clear the Hard Stop Referencing checkbox.

2. Select OK.
   The machine completes a unique referencing procedure after selecting the axis reference buttons: rather than moving each axis to the end of its travel, the reference position is set as the machine's current position.

Tip! This is useful for troubleshooting, because you're now able to move the axis.

Limit G30 Moves

You can limit G30 moves so that only the Z-axis moves. For information, see "About G30".

To limit G30 moves:

• From the Settings tab, select G30/M998 Move in Z Only.

About G30

A G30 command in a G-code program moves the machine to a preset position. For more information on setting a G30 position, see "Use a G30 Position".

Use a G30 move to start a coordinated movement of the axes. You can limit the movement to only the Z-axis. For information, see "Limit G30 Moves".

Tip! It's useful to program a G30 move right before a tool change so that the machine can jog to a safe tool change position.

Enable the On-Screen Keyboard

If you have an (optional) Touch Screen Kit (PN 35575), you can use a soft keyboard to type information in the PathPilot interface. For information, see "About Soft Keyboards".

To enable and use the soft (on-screen) keyboard:

1. From the Settings tab, select Soft / On-Screen Keyboard.

2. To resize the keyboard, select a corner of the keyboard and drag.

3. To reposition the keyboard, select the Anchor key and drag the keyboard anywhere on the screen.

4. To close the keyboard, select the X key.

About Soft Keyboards

If you enabled a soft keyboard (on-screen keyboard) in the PathPilot interface to use with an optional touch screen or operator console, a keyboard opens when you select any field where keyboard input is required.

The keyboard displays a wide range of keys: both uppercase and lowercase, symbols, arrow keys, caps lock, backspace and delete, and more.

Enable the USB M-Code I/O Interface Kit

If you have a USB M-Code I/O Interface Kit (PN 32616), you must first enable it in the PathPilot interface.

To enable the USB M-Code I/O Interface Kit:

• From the Settings tab, select USB IO Kit (PN 32616).

Enable Tooltips

PathPilot displays expandable tooltips for many areas of the interface. Hovering over an item, like a DRO field or a button, displays helpful information about the item.

To enable or disable tooltips:

1. From the Settings tab, select or clear Show Tooltips.

NOTE: If you disable the tooltips, you can still display them for specific items. Hover over an area of the interface, and select the Shift key on the keyboard.

Enable the Door Lock Switch Kit

If you have a Door Lock Switch Kit, you must first enable it in PathPilot.

To enable the Door Lock Switch Kit:

1. On the Settings tab, select Enclosure Door Switch.

On the Status tab, the Door Locked / Open LEDs display.

2. Reference the machine: select Ref Z, Ref X, and Ref Y.

3. Open the enclosure doors.

4. From the PathPilot interface, on the Status tab, make sure that the Door Open LED is on, and the Door Locked LED is off.

5. Close the enclosure doors and verify that the Door Open LED is off. Then, push in the Emergency Stop button on the operator box.
   The doors lock, and the Door Locked LED comes on.

6. From the PathPilot interface, on the Status tab, make sure that the Door Open LED is off.

7. Unlock the enclosure doors: twist out the Emergency Stop button and press the Reset button on the operator box.
   The doors unlock.

Enable Feeds and Speeds Suggestions in Conversational Routines

You can use PathPilot to automatically calculate feeds and speeds. For more information, see "Use Feeds and Speeds Suggestions".

• From the Settings tab, select Conversational Feeds and Speeds.

Specify Probing and Tool Measuring Options

If you have any of the following accessories, you must first specify which you're using in the PathPilot interface:

• Active Probe (PN 31858)

• Passive Probe (PN 32309)

• Electronic Tool Setter (PN 31875)

To specify a probe or a tool setter:

• From the Settings tab, select the correct probing or tool measuring options for both Accessory Input 1 and Accessory Input 2.

Use the RapidTurn Interface

If you have a RapidTurn, you must first change the PathPilot interface.

To use the RapidTurn interface:

• From the Settings tab, select Switch to RapidTurn.

The PathPilot interface for the mill closes, and the PathPilot interface for the RapidTurn opens.

Specify the 4th Axis Rotary Type

To select the 4th axis that you're using:

• From the Settings tab, select the 4th Axis Rotary tab. Then, from the 4th Axis Type drop-down menu, select 4" 4th Axis.

NOTE: Once you change the axis scale, you may see a message indicating a Joint 3 following error. If you do, select Reset, and the new axis will function as normal.

Enable the 4th Axis Homing Kit

If you have a 4th Axis Homing Kit (PN 31921), you must first enable it in the PathPilot interface.

To enable the 4th Axis Homing Kit:

• From the Settings tab, select the 4th Axis Rotary tab. Then, select 4th Axis Homing (PN 31921).

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.

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.

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

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.

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.

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.

For more information, see Display Information and Capture Images During an M00 or M01 Break.

Set Up G-Code Programs

Before running a G-code program, you must first make sure that the machine is properly set up for the specific G-code program.

Use a Probe with PathPilot

Use the Probe tab in the PathPilot interface to automate functions with a probe.

Set Up the Probe

Before using the functions on the Probe tab, you must first do the following:

1. Verify that tool number 99 (the probe tool) is in the spindle.

2. Disable the spindle to prevent any accidental spindle starts with the probe in the spindle.

3. Verify that the feed rate is appropriate for probing moves.

NOTE: All probing moves occur at a feed rate specified by the DRO fields on the Probe Setup tab.

4. Press the probe tip and make sure that, from the PathPilot interface, on the Probe tab, the Accessory Input light comes on.
   This indicates that the probe polarity is correctly specified.
   If the Accessory Input light does not come on, you must change the probe polarity setting. For information, see "Specify Probing and Tool Measuring Options".

Use a Probe to Find a Feature's Location

To find the location of a workpiece or vise in the current work offset coordinates:

1. From the PathPilot interface, on the Probe tab, select the X/Y/Z Probe tab.

2. Position the probe near the workpiece or vise.

3. One at a time, select Find X+, Find X-, Find Y+, Find Y-, or Find Z-.

The axis is probed, and the location of the probed surface is displayed.

Use a Probe to Set Work Offset Zeroes

You can set the work offsets of a workpiece or vise jaw using a probe.

Set the X and Y Work Offset Zero on the Corner of a Feature

1. From the PathPilot interface, on the Probe tab, select the X/Y/Z Probe tab.

2. Position the probe so that it is below the surface of the feature and 1 in. away from the vice jaw corner in the X and Y directions.

3. Select Find Corner, Set Work Origin.

The axes are probed, and the location of the probed surface is set as the current work offset's X/Y origin.

NOTE: Select Change Corner to change the corner on which to probe.

Set the Work Offset Zeroes on a Feature

1. From the PathPilot interface, on the Probe tab, select the X/Y/Z Probe tab.

2. Position the probe near the workpiece or vise.

3. One at a time, select Probe X+, Set Work Origin, Probe X-, Set Work Origin, Probe Y+, Set Work Origin, Probe Y-, Set Work Origin, or Probe Z-, Set Work Origin.

The axis is probed, and the location of the probed surface is set as the current work offset's origin.

Use a Probe to Find the Center of a Feature

You can find the center of a pocket, slot, or boss on a part using a probe.

Find the Center of a Pocket

1. From the PathPilot interface, on the Probe tab, select the Rect/Circ tab.

2. Position the probe near the center of the pocket.

3. Select Find Center, Set Work Origin as shown in the following image.

Find the Center of a Slot

1. From the PathPilot interface, on the Probe tab, select the Rect/Circ tab.

2. Position the probe near the center of the slot.

3. Depending on the slot, do one of the following:

   1. To probe the slot in the X direction only, select Find Center, Set Work Origin as shown in the following image.

b. To probe the slot in the Y direction only, select Find Center, Set Work Origin as shown in the following image.

Find the Center of a Rectangular Boss

1. From the PathPilot interface, on the Probe tab, select the Rect/Circ tab.

2. Position the probe below the top surface of the boss and on the left-hand side.

3. Select Find Center, Set Work Origin as shown in the following image.

The probe moves around the edge of the workpiece to find the center.

Find the Center of a Circular Boss

1. From the PathPilot interface, on the Probe tab, select the Rect/Circ tab.

2. Position the probe below the top surface of the boss and on the left-hand side.

3. Select Find Center, Set Work Origin as shown in the following image.

The probe moves around the workpiece three times to determine the approximate center of the curve, and then makes four additional move to confirm the center of the circle.

Find the Center Rotation of an A-Axis

1. From the PathPilot interface, on the Probe tab, select the Rect/Circ tab.

2. Position the probe directly above the A-axis center of rotation.

3. Select Find A Axis Center & Set Work Origin.

The probe moves around the round workpiece mounted in the A-axis to find the center rotation of the A-axis.

Set Tool Length Offsets

Before running a G-code program, PathPilot must know the length of the tools that are required for the program. For more information on using tool length offsets, see "About Tool Offsets".

NOTE: You can import a .csv file with tool length offset data. For information, see "Import and Export the Tool Table".

To set tool length offsets:

1. Verify that the machine is powered on and out of reset.

2. Put a tool into a tool holder, and set it aside to measure.
   For information, see Set Up Tooling.

3. From the PathPilot interface, on the Offsets tab, verify that the Tool tab is selected.

4. Find the Tool Table window.

5. Depending on your workflow, you can measure your tools using any of the following methods:

• Use a Tool Height Setter For information, see "Use a Tool Height Setter to Measure Tools".

• Use an Electronic Tool Setter For information, see "Use an Electronic Tool Setter to Measure Tools".

• Touch Off of a Known Reference Height For information, see “Touch Off the Tool Length Offsets”.

About Tool Offsets

Tool offsets allow you to use various tools while still programming with respect to the workpiece. Tools can have different lengths (and, while using cutter radius compensation, different diameters).

The most common tool offset is the tool length offset: when you change tools, PathPilot must account for the difference in tool length. In CNC machines, the tool length offset is applied using a G43 command.

The tool length offset is the distance from the cutting edge of the tool to the shoulder of the tool holder.

Before you begin a G-code program, you must verify the lengths of the tools in the program, and make sure that the lengths agree with the tool length offsets set in PathPilot:

• Each time you change tools, you must apply a new tool length offset in PathPilot.

• Each time you replace a tool, you must remeasure its length, and apply a new tool length offset in PathPilot.

NOTICE! You must always verify that the physical length of a tool agrees with the tool length offset value set in PathPilot. If you don't, there's a risk that the tool length offset misrepresents the currently active tool in the spindle, which may result in a machine crash or damaged tooling, workpieces, or fixtures.

Touch Off the Tool Length Offsets

Touch off the tool length offsets by using a reference surface with a known height, which gives you a basis to measure any other tool lengths. Use any surface that is parallel (within 0.02 mm) to the machine table. For example:

• A 1-2-3 Block Set (PN 31950)

• Box parallel

There are two steps to touch off the tool offsets. Complete the following steps in the order listed:

Set a Known Reference Height

This procedure sets a new Z zero position for the currently selected work offset.

To set a known reference height:

1. Identify a precision surface to use as a reference surface (like a 1-2-3 Block Set), and put it below the spindle on the machine table. Verify that there's a clear path from the spindle to the machine table.

2. Set a new, unused work offset (like G55). From the PathPilot interface, on the Main tab, in the MDI Line DRO field, type a work offset. Then select the Enter key.
   For information, see "Set Work Offsets".

3. If there's already a tool in the spindle, remove it.

4. From the PathPilot interface, in the Tool DRO field, type 0. Then select the Enter key.

5. Slowly jog the Z-axis down (-Z) until it's 0.04 in. (1 mm) from the reference surface.

6. Measure the thickness of a piece of paper, and put the paper on the reference surface. Note the thickness of the paper for later.

7. While moving the paper back-and-forth across the reference surface, slowly step the Z-axis down (-Z) until you feel a light pull on the piece of paper. This indicates that the paper is contacting the spindle.

NOTE: It's easier to use step jogging for this task. For information on step jogging, see "About Step Jogging".

8. From the PathPilot interface, in the Z-axis work offset DRO field, type the thickness of the piece of paper. Then select the Enter key.

The reference surface is now set as the Z zero position in the current coordinate system.

9. To set the tool length offset, go to “Measure Tools Using a Known Reference Height”.

Measure Tools Using a Known Reference Height

This procedure sets the tool length offset using a known reference height. If you have not yet done so, you must first set the Z zero position; go to Set a Known Reference Height.

To measure tools using a known reference height:

1. Verify that the reference surface is still on the machine table with the piece of paper.

2. From the PathPilot interface, on the Offsets tab, find an unused tool number in the Tool Table window. Then, type a description for the tool you're measuring.

3. Put the tool holder into the spindle.

4. From the PathPilot interface, in the Tool DRO field, type the number of the tool. Then select the Enter key.

5. Slowly jog the Z-axis down (-Z) until it is 0.04 in. (1 mm) from the reference surface.

6. Continue to slowly jog the Z-axis while slowly moving the piece of paper back-and-forth on the reference surface.

7. Stop jogging the Z-axis when you feel a light pull on the piece of paper, which indicates that it is in contact with the tool.

8. From the PathPilot interface, on the Offsets tab, in the Tool Table, select the tool for which you previously wrote a description.

9. In the Touch Z DRO field, type the thickness of the piece of paper. Then select the Enter key.

10. Select Touch Z.
    The length of the tool is stored in the Tool Table window.

11. From the Tool Table window, in the Length column, verify that the length of the tool is correct.

12. In the Diameter column, type the diameter of the tool. Then select the Enter key.

13. Jog the Z-axis up (+Z).
    You've completed the procedure to measure a tool offset. Repeat this procedure for any remaining tooling you have. Once you're done adding tool length offsets, switch back to your work coordinate system.

Use an Electronic Tool Setter (ETS) to Measure Tools

An ETS is a device used to measure the length of a cutting tool.

To use an ETS to measure tools:

1. Plug in the ETS to the Accessory 2 port.

2. Put the ETS on the known reference surface below the spindle.

3. From the PathPilot interface, on the Offsets tab, in the Tool Table window, in the Description column, type a description for the tool.

4. In the Diameter column, type the diameter of the tool. Then select the Enter key.

5. Put a tool holder into the spindle.

6. From the PathPilot interface, type the tool number in the Tool DRO field. Then select the Enter key.

7. Jog the Z-axis down (-Z) until it is above the ETS.

8. From the Offsets tab, on the Tool tab, select Move and Set Tool Length.

NOTE: Regardless of the initial feed rate, the final touch off feed rate while using an ETS is 2-1/2 in. per minute (IPM).

9. From the Tool Table window, in the Length column, verify that the length of the tool is correct.

Use a Tool Height Setter to Measure Tools

This procedure sets the tool length offset using a known reference height and a Tool Height Setter (PN 39682).

Complete the following steps in the order listed:

Set a Known Reference Height

This procedure sets a new Z zero position for the currently selected work offset.

To set a known reference height:

1. Identify a precision surface to use as a reference surface (like a 1-2-3 Block Set), and put it below the spindle on the machine table. Verify that there's a clear path from the spindle to the machine table.

2. Set a new, unused work offset (like G55). From the PathPilot interface, on the Main tab, in the MDI Line DRO field, type a work offset. Then select the Enter key.
   For information, see "Set Work Offsets".

3. If there's already a tool in the spindle, remove it.

4. From the PathPilot interface, in the Tool DRO field, type 0. Then select the Enter key.

5. Slowly jog the Z-axis down (-Z) until it's 0.04 in. (1 mm) from the reference surface.

6. Measure the thickness of a piece of paper, and put the paper on the reference surface. Note the thickness of the paper for later.

7. While moving the paper back-and-forth across the reference surface, slowly step the Z-axis down (-Z) until you feel a light pull on the piece of paper. This indicates that the paper is contacting the end face of the spindle.

NOTE: It's easier to use step jogging for this task. For information on step jogging, see "About Step Jogging".

8. From the PathPilot interface, in the Z-axis work offset DRO field, type the thickness of the piece of paper. Then select the Enter key.

The reference surface is now set as the Z zero position in the current coordinate system.

Verify the Calibration of the Tool Height Setter

The higher side of the Tool Height Setter is precision ground. You can use it as a reference surface to calibrate the tool.

1. Use the provided dowel pin to compress the setting face of the Tool Height Setter to the level of the ground reference surface.

2. Adjust the indicator dial's bezel to read zero. Make note of how many times the indicator rotates around the dial.

3. Measure the height of the ground reference surface from the bottom surface of the Tool Height Setter with a calipers. Note the measured height for later.

4. Carefully, without moving the bezel, put the Tool Height Setter on the reference surface that's on the machine table.

Measure Tools Using a Known Reference Height

This procedure sets the tool length offset using a known reference height. If you have not yet done so, you must first set the Z zero position; go to Set a Known Reference Height.

To measure tools using a known reference height:

1. From the PathPilot interface, on the Offsets tab, find an unused tool number in the Tool Table window. Then, type a description for the tool you're measuring.

2. Put the tool holder into the spindle.

3. From the PathPilot interface, in the Tool DRO field, type the number of the tool. Then select the Enter key.

4. Slowly jog the Z-axis down (-Z) to contact the Tool Height Setter. Stop jogging when the Tool Height Setter reads zero, which indicates that it's compressed to the height of the ground surface. Verify that the indicator rotated around the dial the same number of times as when you calibrated the Tool Height Setter.

5. From the PathPilot interface, on the Offsets tab, in the Tool Table, select the tool for which you previously wrote a description.

6. In the Touch Z DRO field, type the height of the Tool Height Setter. Then select the Enter key.

7. Select Touch Z.
   The length of the tool is stored in the Tool Table window.

8. From the Tool Table window, in the Length column, verify that the length of the tool is correct.

9. In the Diameter column, type the diameter of the tool. Then select the Enter key.

10. Jog the Z-axis up (+Z).
    You've completed the procedure to measure a tool offset. Repeat this procedure for any remaining tooling you have. Once you're done adding tool length offsets, switch back to your work coordinate system.

Set Work Offsets

To set the current axis location to zero in the active work coordinate system:

• Select Zero [Axis].

To change work offsets:

1. On the Main tab, in the MDI Line DRO field, type the new work offset to activate (for example, G55). Then select the Enter key.

2. The new work offset displays in the following locations in the PathPilot interface:

   1. The Status read-only DRO field.

   2. Above the Work Offset DRO fields.

NOTE: The values in the Work Offset DRO fields update to indicate the new location of each axis in the new work offset.

For more information on using work offsets, see "About Work Offsets".

About Work Offsets

Work offsets allow you to think in terms of X, Y, and Z coordinates with respect to the part, rather than thinking of them with respect to the machine position. This means that you can jog the machine to an arbitrary location (like the end of a workpiece) and call that location zero.

You can save up to 500 work offsets in PathPilot. The naming structure varies based on the offset number, as detailed in the following table.

View Work Offsets

To view the current work offset:

• From the Offsets tab, on the Work tab, identify the Work Offsets Table window.

The active work offset is highlighted.

To change the current work offset, go to "Set Work Offsets".

View Available G-Code Modes

The G-Code Description window shows a list of all available G-code modes.

To view available G-code modes:

• From the Settings tab, find the G-Code Description window.

Run G-Code Programs

While running a G-code program, use the following controls:

Bring the Machine Out of Reset

• Select Reset.

For more information on reset mode, see "About Reset Mode".

About Reset Mode

When the machine is first powered on, or after an emergency stop, the Reset button flashes. When you select the flashing Reset button, PathPilot verifies communication to the machine and does the following activities:

• Brings the machine out of an emergency stop condition

• Clears alarms

• Clears the tool path backplot

• Resets all modal G-codes to their normal state

• Rewinds the currently loaded G-code program

• Stops machine motion, but is not a replacement for the Emergency Stop button

You can select the Reset button any time while the machine is on.

View the Active Axis to Jog

To find which axis is active while jogging your machine:

• Identify the light next to the Work Offset DRO fields.

For information, see "Jog the Machine".

Jog the Machine

To switch between jogging modes:

• From the Manual Control area, in the Jog group, select Jog.
  PathPilot toggles between continuous velocity mode and step mode.

When the Cont green light is on, continuous velocity mode is selected.

When the Step green light is on, step mode is selected.

To use continuous velocity mode:

• Set the velocity: drag the Jog Speed slider.

For more information on continuous velocity mode, see "About Continuous Velocity Jogging".

To use step mode, select the step size. Do one of the following, depending on your accessories:

• In the Manual Control Area, in the Jog group, select the step size.
  The Step button's light comes on, indicating which step size is active.

• On the (optional) Jog Shuttle, press the Step button to toggle the currently selected step size.
  In the PathPilot interface, the Step button's light comes on, indicating which step size is active.

For more information on step mode, see "About Step Jogging".

Jog in Continuous Velocity Mode

In continuous mode, the machine jogs at a continuous velocity.

To select continuous velocity mode:

• In the Manual Control area, select Jog.

When the Cont green light is on, continuous velocity mode is selected.

When the Step green light is on, step mode is selected.

To set the velocity:

• Drag the Jog Speed slider.

About Continuous Velocity Jogging

While jogging in continuous velocity mode, the machine moves at a constant speed for as long as:

• A keyboard key is pressed

• The Jog Shuttle outer ring is twisted away from the neutral position

This is useful when you're doing things like:

• Roughly positioning the machine (for example, to move the spindle head away from the workpiece).

• Moving the machine a certain distance at a constant speed (for example, to align a vise).

Jog in Step Mode

In step mode, the machine jogs in steps, which range based on the programming mode you're using:

• Imperial (G20) Mode 0.0001 in. to 0.1000 in.

• Metric (G21) Mode 0.01 mm to 10 mm

To select the step size:

• In the Manual Control Area, select the step size.
  The Step button's light comes on, indicating which step size is active.

About Step Jogging

While jogging in step mode, the machine moves one step each time you either press a jog key on the keyboard or click the inner wheel of the Jog Shuttle. The jog step sizes range depending on the programming mode you are using:

• Imperial (G20) Mode 0.0001 in. to 0.1000 in.

• Metric (G21) Mode 0.01 mm to 10 mm

Step jogging mode is useful to finely move the machine, like when you're indicating a workpiece or manually setting tool lengths.

The jog keys on the keyboard only move the machine in steps when step mode is indicated in PathPilot. The inner wheel on the jog shuttle always moves the machine in steps, regardless of which mode is indicated in PathPilot.

View the Current Machine Position

• Identify the Work Offset DRO fields.

The position is expressed by the currently active work offset coordinate system (like G54 or G55).

When the machine isn't moving, you can edit the DRO fields. For more information on setting work offsets, go to "Set Work Offsets".

Reference the Machine

1. Verify that the machine can freely move to its reference position (at the ends of travel).

2. To verify that the tooling is clear of any possible obstructions, reference the Z-axis before referencing the other axes: from the PathPilot interface, select Ref Z.

3. Once the spindle is clear of any possible obstructions, continue referencing all axes.

NOTE: You can select the buttons one after another. Once the machine references one axis, it'll move on to the next.

After each axis is referenced, its button light comes on.

For more information on referencing the machine, see "About Referencing".

About Referencing

You must reference the machine to establish a known position for PathPilot. The position that's set while referencing the machine is the origin of the machine coordinate system. Without referencing the machine, PathPilot won't know the current position of the machine axes.

You must reference the machine at the following times:

• After you power on the machine

• After you push in the Emergency Stop button

• Before running a G-code program

• Before using MDI commands

• Before setting work or tool offsets

• After a collision or an axis stall/fault

When referencing, the machine moves each axis to the end of its travel. The machine stops at the limit switch, which sets the axis’ reference position.

Start a Program

• From the PathPilot interface, in the Main tab, select Cycle Start.

For more information on starting a program, see "About Cycle Start".

If you can't start a program, go to "Cycle Start Reference".

About Cycle Start

While a program is running, the Cycle Start button's light is on.

The Cycle Start button's light flashes if motion is paused during the program. The following modes may pause motion during a program:

• Single block

• Feed hold

• M01 break

If machine motion pauses a single block, feed hold, or M01 break, the Cycle Start button flashes until it's selected again.

Cycle Start Reference

The Cycle Start button doesn't operate if you select it:

• While you're not in the Main tab. For information, see Main Tab.

• Before you've loaded a G-code program. For information, see "Load G-Code".

• Before referencing the machine. For information, see "Reference the Machine".

Stop Machine Motion

• From the Program Control area, select Stop.

Operate the Coolant Pump

To turn coolant on or off:

• Select Coolant.

For more information on turning on and off coolant, see "About Coolant".

About Coolant

In the PathPilot interface, the Coolant button controls the machine's coolant pump power outlet. The Coolant button’s light shows the current state of the outlet: the light is on when the outlet has power; the light is off when the outlet does not have power.

NOTE: The Coolant button is equivalent to using an M08 (coolant on) or M09 (coolant off) command in the G-code program.

Use the Coolant button before or after a program is running, while a program is running, or while you are using manual data input (MDI) commands.

View the Active G-Code Modes

To find the currently active G-code modes and the currently active tool at a glance:

• Identify the Status read-only DRO field.

For more information on G-code modes, go to "View Available G-Code Modes".

View the Distance to Go

To view the distance to go:

• Identify the DTG read-only DRO fields.

The value is the remaining distance in any programmed move.

For more information on using the DTG read-only DRO fields, see "About Distance to Go".

About Distance to Go

While a program is running, the DTG read-only DRO fields show the remaining distance in each move.

After using the feed hold function or the maxvel override function, look at the distance to go. This read-only DRO field is useful to prove out a part program.

Control G-Code Programs

If necessary, use the following controls to add to your G-code program:

Use the Feed Hold Function

• Select Feed Hold.

Tip! Use the Spacebar key to quickly activate the feed hold function.

For more information on using the feed hold function, see "About Feed Hold".

About Feed Hold

When the feed hold function is active, the Feed Hold button's light is on.

The feed hold function pauses machine motion — aside from the spindle — and the Cycle Start button flashes. For information, see "About Cycle Start".

NOTE: If the machine isn't moving, the feed hold function doesn't have an effect.

You can use the feed hold function either while a program is running or while you are using manual data input (MDI) commands. If the program is running a spindle-synchronized move, the feed hold function is delayed until the move is complete.

Use the Feed Rate Override Function

To use the feed rate override function:

• Using the Feed Rate Override slider, change the programmed feed rate by a specific percentage.

NOTE: Percentages range from 1-200%.

To remove the feed rate override function:

• Select Feed 100%.
  The feed rate returns to 100% of its programmed value (it's no longer overriden).

For more information on the feed rate override function, see "About Feed Rate Override".

About Feed Rate Override

You can use the feed rate override function while you're doing any of the following activities:

• Using manual data input (MDI) commands

• Jogging

• Running a program with G01, G02, or G03 commands

The feed rate override function does not affect G00 (rapid) commands. It's ignored if:

• The program is running a spindle-synchronized move

• An M48 (disable feed and speed overrides) command is used

To indicate lack of motion or unusual levels, the slider turns yellow when it's either at 0% or above 100%.

The Feed Rate Override slider and Feed 100% button work similarly to the spindle override controls. They affect the commanded feed rate by a percentage from 1-200%. The feed rate override works for MDI, jogging, and G-code program G01/G02/G03 moves. The override has no effect on G00 (rapid) moves.

Use M01 Break Mode

• Select M01 Break.

For more information on using M01 break mode, see "About M01 Break".

About M01 Break

When the M01 break mode is active, the M01 Break button's light is on. When the M01 break mode is inactive, the M01 Break button's light is off.

M01 break mode enables any M01 (optional stop) commands that are programmed in the G-code file. You can turn M01 break mode on or off either before starting a program or while a program is running.

• When M01 Break is Active Machine motion stops after PathPilot reaches an M01 command, and the Cycle Start button flashes. For information, see "About Cycle Start".

• When M01 Break is Inactive PathPilot ignores all programmed M01 commands.

Display Information and Capture Images During an M00 or M01 Break

Display Information with Images

If the comment occurs on a line with M00 or M01, and contains a file name with a .jpg or .png extension, PathPilot displays the image in the Tool Path display when the program reaches the M00 or M01 break.

To display an image during an M00 or M01 break:

1. Move an image file with a .jpg or .png extension to the PathPilot controller in one of the following locations:

• In the same folder as the G-code program

• In an images folder within the G-code program's folder

• In an images folder within the home directory

2. Program an M00 or M01 break, and, using parentheses, type the full file name of the image (including its extension).

Example
M01 (Op1_Setup.jpg) displays the image file on the Tool Path display.

Display Information with Text

To display a message on the Tool Path display:

1. Program an M00 or M01 break, and, using parentheses, type a message that you’d like to display on the screen.

Example
M01 (Check coolant nozzles are pointed correctly) displays Check coolant nozzles are pointed correctly across the bottom of the Tool Path display.

2. The message displays on the Tool Path display.

Capture Images with a USB Camera

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 us 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.

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

   2. 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.

Use the Maxvel Override Function

To use the maxvel override function:

• Using the Maxvel Override slider, change the maximum velocity by a specified percentage.

To remove the maxvel override function:

• Select Maxvel 100%.

For more information on using the maxvel override function, see "About Maxvel Override".

About Maxvel Override

The maxvel override function affects G00 and G01 commands, and it's useful for:

• Running a Program for the First Time Drag the Maxvel Override slider to 0% to verify that all DRO fields look appropriate.

• Safety If you're running a spindle-synchronized move, a maxvel override isn't ignored.
  Verify that the maxvel override value allows the machine to use the programmed feed rate during spindle-synchronized moves. If it can't, the spindle-synchronized move won't produce the results you want.

To indicate lack of motion or unusual levels, the slider turns yellow when it's either at 0% or above 100%.

Use Single Block Mode

• Select Single Block.

For more information on using single block mode, see "About Single Block".

About Single Block

While single block mode is active, the Single Block button's light is on.

Single block mode runs one line of G-code at a time. After each line, motion is paused, and the Cycle Start button flashes. For information, see "About Cycle Start".

NOTE: Single block mode ignores non-motion lines, like comment lines or blank lines.

Use the Spindle Override Function

To use the spindle override function:

• Using the Spindle Override slider, change the programmed spindle speed by a specific percentage.

NOTE: Percentages range from 1-200%.

To remove the spindle override function:

• Select RPM 100%.
  The spindle speed returns to 100% of its programmed value (it's no longer overriden).

For more information on using the spindle override function, see "About Spindle Override".

About Spindle Override

The spindle override function won't command the spindle to move past the maximum allowable speed. If the spindle isn't moving, the spindle override function is delayed until the next time spindle starts. The override doesn’t drive the spindle past its maximum speed. It does affect the speed of a spindle command limited by a D word.

You can use the spindle override function while you're doing any of the following activities:

• Running a program

• Using manual data input (MDI) commands

The spindle override function is ignored in the following situations:

• If the program is running a spindle-synchronized move

• If an M48 (disable feed and speed overrides) command is used

To indicate lack of motion or unusual levels, the slider turns yellow when it's either at 0% or above 100%.

Change the Feed Rate

• In the Feed Rate DRO field, type in a feed rate. Then select the Enter key.

For information, see "About Feed Rates".

About Feed Rates

A feed rate is the velocity at which the workpiece can be fed against the tool in the machine's spindle.

Change the Spindle Speed

• In the Spindle RPM DRO field, type in a spindle speed. Then select the Enter key.

NOTE: Verify that the spindle speed is within the specified range for the spindle belt's position. For information, see Change the Spindle Speed Range.

For information, see "About Spindle Controls".

About Spindle Controls

A spindle speed is the rate at which the spindle rotates.

Use the FWD, REV, and Stop buttons to manually control the spindle.

The FWD and REV buttons and the Spindle RPM DRO field don't operate if selected when:

• A G-code program is running.

• Using manual data input (MDI) commands.

• You type a value outside of the specified range for the spindle belt's position into the Spindle RPM DRO field.

For information, see Change the Spindle Speed Range.

Spindle Controls Reference

The spindle speed is measured in revolutions per minute (RPM).

Two speed ranges are available:

• Low 70 rpm to 2,000 rpm

• High 250 rpm to 10,000 rpm

Change the Tool Number

The Tool DRO field shows the tool currently in the spindle.

To change the tool number (and apply its tool length offset):

1. In the Tool DRO field, type a number (the valid range is from 0-1000). Then select the Enter key.

NOTE: You can also select M6 G43. For information, see "About M6 G43".

About M6 G43

The M6 G43 button is a shortcut used to do the following:

• Change the number of the currently-loaded tool in the spindle to the number typed in the Tool DRO field. This is the equivalent of an M06 command.

• Apply the tool length offset for that tool typed in the Tool DRO field. For more information on tool length offsets, see "Set Tool Length Offsets". This is the equivalent of a G43 command.

Use a G30 Position

The Go to G30 button moves the machine to a predefined G30 position. For information, see "About G30".

To set a G30 position:

1. Jog the machine to the desired G30 position.

2. From the Offsets tab, select Set G30.

To go to a set G30 position:

• Do one of the following:

  • Use a G30 command in a G-code program.

  • Select Go To G30.
    

    

NOTE: The G30 position defaults to only moving the Z-axis.

About G30

A G30 command in a G-code program moves the machine to a preset position. For more information on setting a G30 position, see "Use a G30 Position".

Use a G30 move to start a coordinated movement of the axes. You can limit the movement to only the Z-axis. For information, see "Limit G30 Moves".

Tip! It's useful to program a G30 move right before a tool change so that the machine can jog to a safe tool change position.

View the Tool Length

• Identify the Tool Length read-only DRO field.

If the tool offset matches the number of the tool in the Tool DRO field, the text is light blue on a gray background.

If the tool offset doesn't match the number of the tool in the Tool DRO field, the text is orange on a red background.

Manually Enter Commands

You can send G-code commands directly to the machine by using the MDI Line DRO field. For information, see "About the MDI Line DRO Field".

To manually enter commands:

1. Select the MDI Line DRO field.

The DRO field highlights.

2. Type the command.

NOTE: You can use the Backspace, Delete, Left Arrow, and Right Arrow keys to correct typing errors.

3. You must press the Enter key to execute the command. To abandon the command, press Esc.

About the MDI Line DRO Field

The MDI Line DRO field allows you to send commands (or, manual data input) directly to PathPilot. For information, see "Manually Enter Commands".

The MDI Line DRO field saves up to 100 of your most recent commands, which are saved after a power cycle.

When you select the MDI Line DRO field, all keystrokes are used within the field — so, you can't jog the machine.

Admin Commands Reference

Use the following commands in PathPilot:

Copy Recently Entered Commands

1. From the MDI Line DRO field, press either the Up Arrow key or the Down Arrow key.
   The previously entered command displays.

2. You must press the Enter key to execute the command. To abandon the command, press Esc.

For information, see "Manually Enter Commands".

Use Feeds and Speeds Suggestions

NOTE: Calculating feeds and speeds requires that PathPilot has relevant details about the tooling. If you haven't yet done so, go to "Create Tool Descriptions".

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.

1. If you haven't yet done so, enable the conversational feeds and speeds setting. From the Settings tab, select Conversational Feeds and Speeds.

2. From the Conversational tab, locate the Material dropdowns in the Conversational DROs group.

3. From the Material dropdown, select your material (like Aluminum or Plastic).

4. If required, from the Sub-Type dropdown, select the material sub-type (like -any- or 6061).

5. In the Tool DRO field, type the assigned tool number.

6. Select Refresh (to the right of the Sub-Type dropdown).

The following machining-related DRO fields are calculated:

• Spindle RPM

• Feedrate

• Z Feedrate

• Depth of Cut

• Stepover

• Peck (if drilling)

NOTE: After PathPilot calculates values for the machining-related DRO fields, the background turns green.

7. (Optional) You can adjust the values in the calculated DRO fields. Adjusting the value in one of these DRO field doesn't change the value in the other machining-related DRO fields.

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

Refresh DRO Field Values

The suggested values 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 field.
  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. Changing your conversational operation requires you to refresh the feeds and speeds values.

When the feeds and speeds are no longer valid, the Refresh button turns green, and the machining-related DRO field backgrounds switch from green to white, as shown in the following image.

Use Additional Provided Information

The following tips are displayed based on the calculations that PathPilot is performing:

• Chip Load Information Chip load — the amount of material removed per tooth — is based on the number of flutes, RPM, and feed rate.
  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 premature tool wear.

• 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.

Create Tool Descriptions

If desired, you can create tool descriptions in PathPilot. Detailed tool descriptions allow you to receive feeds and speeds suggestions in conversational programming. For information, see "Use Feeds and Speeds Suggestions".

Manually Enter Tool Descriptions

PathPilot uses keywords and patterns in the tool description to recognize tooling features. For information, see "Tool Keywords Reference".

To manually enter tool descriptions:

1. From the PathPilot interface, on the Offsets tab, identify the Tool Table window.

2. Select a blank line.

3. Type a description for the tool. Descriptions are not case sensitive.
   If a pattern or word in the description is recognized, PathPilot uses syntax highlighting to indicate a valid description.

Examples

To get accurate machining information, all tooling must be described with detail: the more detail, the better the results.

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

This description provides the following to 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)

Using a personal description likely won’t contain meaningful information for PathPilot.

Example
Gold colored end mill from middle drawer

This description provides very little information, and PathPilot defaults to basic cutter features:

• Two flutes

• Uncoated, high-speed steel end mill

• Length of cut based on the diameter

Automatically Generate Tool Descriptions

If you're using a Tormach tool, you can enter the part number to automatically generate tool descriptions in the Tool Table window.

NOTE: If you don't know 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, like 35571.
   The full description and tool diameter for a ShearHog (PN 35571) displays.

3. You must enter the value for the Length.

Tool Keywords Reference

PathPilot uses keywords and patterns in the tool description to recognize tooling features.

Use Cycle Counters (M30 and M99)

On the Main tab, the Tool Path display shows M30 and M99 cycle counters. They're useful to count parts completed during unattended operation. For each M-code, there's an A and B counter. This provides more flexibility, because you can reset them to 0 independently.

For example, you could use M30 A to count parts each shift, and M30 B to count parts each week. The cycle counters persist across the controller's power cycles.

Monitor Cycle Counters

• In the MDI Line DRO field, type ADMIN CYCLECOUNTER to show or hide the counters and to reset them to 0.

Change Cycle Counter Values

The cycle counters are implemented as read-only persistent G-code numbered parameters, as detailed in the following table. If needed, the cycle counter value can be read in G-code.

To change a counter value explicitly, use a G10 command: G10 L99 P~ Q~

• P~ selects the cycle counter to change. Use any of the values detailed in the following table.

• Q~ specifies the value to set the cycle counter. If Q~ is omitted, the cycle counter is incremented by 1.

For example, if you program G10 L99 P2, the M99 A cycle counter increments by 1.

System File Management

To keep the files on your system backed up and organized, use the following controls:

Manage System Files

Use the File tab to manage system files on the PathPilot controller. For information, see "Transfer Files to and From Controller".

To manage system files:

• From the PathPilot interface, on the File tab, do any of the following from the Controller Files window:

  • Select a file, and then select New Folder, Rename, or Delete.

  • Select a file, and go to the Options

    menu. Then, select Copy, Cut, or Paste.

To navigate through the system files:

• Select Back or Home.

Create Backup Files

1. Insert a blank, formatted USB drive into the PathPilot controller.

NOTE: To prevent errors when backing up and restoring files, only use a blank, formatted USB drive.

2. From the PathPilot interface, on the Main tab, in the MDI Line DRO field, type ADMIN SETTINGS BACKUP. Then select the Enter key.
   PathPilot generates a backup .zip file, and the Admin Settings Backup dialog box displays.

3. From the Admin Settings Backup dialog box, specify where (on the PathPilot controller or on a USB drive) to save the backup .zip file.

4. Select Save.
   The backup .zip file is saved in the location you specified in Step 3.

5. If you saved the backup .zip file on the PathPilot controller, you must manually transfer it — along with other files you want to back up (like G-code programs) — to a USB drive. From the PathPilot interface, on the File tab, in the Controller Files window, select the backup .zip file and any other files you want to back up.

NOTE: Files must have unique names. If they don't, PathPilot prompts you to overwrite or rename files, or cancel the file transfer.

6. To prevent errors, make sure you don't include the following folders:

• logfiles

• media

• ReleaseNotes

• subroutines

• USB

7. Select Copy to USB.
   The files are copied and display in the USB Files window.

8. Eject the USB drive from the PathPilot controller.

9. From the PathPilot interface, select Exit.

10. Verify that all files are properly saved: insert the USB drive on a device other than the PathPilot controller, and review the list of files on the USB drive.

11. (Optional) As an extra precaution, copy all the files onto the device.

About Backup Files

Make a regular backup of all tool offset and fixture information and machine settings stored on your PathPilot controller. Store the file externally to use if you replace your controller or restore it to factory settings.

Restore Backup Files

1. Insert the USB drive with your backup files into the PathPilot controller.

2. From the PathPilot interface, on the Main tab, in the MDI Line DRO field, type ADMIN SETTINGS RESTORE. Then select the Enter key.
   The Admin Settings Restore dialog box displays.

3. From the Admin Settings Restore dialog box, navigate to the backup .zip file on the USB drive, and then select OK.
   The PathPilot operating system restores the backup, then restarts.

4. If you backed up any other files onto the USB drive, you must manually transfer the files to the PathPilot controller. From the PathPilot interface, on the File tab, in the USB Files window, select the files you want to transfer.

NOTE: To navigate backward, select Back. To navigate to the top level, select USB.

5. From the Controller Files window, select the folder into which you want to copy the files.

6. Select Copy From USB.
   The files display in the Controller Files window.

NOTE: Files must have unique names. If they don't, PathPilot prompts you to overwrite or rename files, or cancel the file transfer.

Import and Export the Tool Table

You can manage the tool table using an external .csv file.

Import a .csv File

1. Transfer the .csv file to a USB drive.

2. Insert the USB drive into the PathPilot controller.

3. Confirm that the PathPilot controller is on.

4. From the Offsets tab, select Import.
   The Import dialog box displays.

5. Navigate to the .csv file on the USB drive. Then, select OK.
   The .csv file updates the tool table.

Export the Tool Table as a .csv File

1. From the Offsets tab, select Export.
   PathPilot generates the .csv file, and the Export dialog box displays.

1. In the Name DRO field, type the name for the .csv file.

2. Select Save.
   The .csv file is saved in the File tab.

3. From the File tab, select the newly created .csv file, and then select Copy to USB.

4. Select Eject.
   It's safe to remove the USB drive from the controller.

Looking for more information?

This is a section of the 1100MX operator's manual. To view the whole manual, go to Tormach document UM10586.

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