PathPilot Tools and Features - 8L

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.

Open

Figure 1: Controller Files window on the File tab.

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 / HUB Files window or the Controller Files window).

Open

Figure 2: File tab.

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 →.

Open

Figure 3: File tab.

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.

Open

Figure 4: File tab.

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.

Open

Figure 5: 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.

Open

Figure 6: Recent Files menu on the Main tab.

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.

Open

Figure 7: Edit G-code button on the File tab.

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.

Open

Figure 8: Job assignment editor.

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.

Open

Figure 9: Window Expander on the Main tab.

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.

Open

Figure 10: Search for a text command.

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

Open

Figure 11: Search for a feed 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.

Open

Figure 12: Accessing the Options menu by right-clicking.

• 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.

Open

Figure 13: Tool Path display on the Main tab.

• Select the View Options tab.

Open

Figure 14: View Options tab on the Main tab.

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

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 an Outside Diameter

Using conversational programming, you can program PathPilot to rough and finish three features: an outside diameter, a fillet (corner radius), or an adjacent face. For information, see "About OD Turning".

Before You Begin

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

• The value used in the Z End DRO field should be less than the value used in the Z Start DRO field.

• The value used in the Filet Radius DRO field should be larger than the radius of the tool.

• The tool is cutting both an outside diameter and a face — valid tools are limited to orientation 2 for a front tool post, 8L tool.

• The face is always on the headstock end of the diameter being cut.

• The fillet calculation doesn't use cutter radius compensation: the middle of the fillet isn't on the true radius for a tool with a tip radius.

To create an outside diameter:

1. From the Conversational tab, select the OD Turn tab.

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

Open

Figure 15: Conversational DROs on the OD Turn tab.

3. Work through the program-specific DRO fields:

   1. In the Tool DRO field, type the currently selected tool as it's defined in the Tool Table window (on the Offsets tab).
      This DRO field is a command value — it sets the tool number for a tool change at the start of the program.

NOTE: This DRO field is a reference value. It's also used with the Tool Clearance DRO field to locate some of the transitions between rapid and feed rate. If the values in the Initial X DRO field and the Final X DRO field are both positive, the tool works on the positive X side of the spindle center (the side toward you). If they're both negative, the tool works the negative side of the spindle (the side away from you). It's an error if there's a positive and a negative value for each DRO field.

NOTE: This DRO field is used with the Tool Clearance DRO field to set the transition between rapid and feed rate on some Z moves.

NOTE: If you type a value that's less than the tip radius, PathPilot drives the cutter to the corner. If you type a value that's larger than the Z range (the distance between the location of the stock's face and the desired location of the part's face) or the X range (half of the distance between the stock's outside diameter and the desired value of the part's outside diameter), the fillet starts or ends outside of the stock perimeter, and it doesn't end at the specified X and Z locations.

NOTE: Use larger values to begin; once you're familiar with how the program works, smaller values may save time. This DRO field is also sometimes used as a location for retracting the tool while making cutting passes.

Open

Figure 16: Program-specific DROs on the OD Turn Tab.

About OD Turning

Outside diameter turning is the process of removing material on the outside of a part.

OD Turning in PathPilot

During an OD turning routine, PathPilot does the following:

1. Roughing starts at the location typed in the Initial X DRO field, and incrementally cuts diameters at an adjusted depth of cut using the value typed in the Roughing DOC DRO field.

2. The finish diameter is started at the following location: (Final X + [2 × Finish DOC]). At this point, a single finishing pass is done at the value typed into the Finish DOC DRO field.
   The finish pass starts at the +Z (tailstock) end of the outside diameter and feeds to the middle of the fillet.

NOTE: Since there is only one finish pass, the value in the Finish DOC DRO field isn't adjusted.

3. The tool retracts to the stock diameter.

4. The face finish pass is cut from the stock diameter to the end of the fillet.

Create an Internal Diameter

Using conversational programming, you can program PathPilot to cut a basic or extended internal diameter on a part. For information, see "About ID Turning".

Before You Begin

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

• Valid tool orientations are limited to orientation 3 for an 8L front tool post.

• The tool path changes by 90° on the same side of the tool, so a form tool (narrow tip angle) and separate roughing DOCs are needed.

Basic Internal Diameters

To create a basic internal diameter:

1. From the Conversational tab, select the ID Turn tab.

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

Open

Figure 17: ID Turn tab on the Conversational tab.

3. Work through the program-specific DRO fields:

   1. In the Tool DRO field, type the currently selected tool as it's defined in the Tool Table window (on the Offsets tab).
      This DRO field is a command value — it sets the tool number for a tool change at the start of the program.

   2. In the Initial X DRO field, type the diameter of the pilot hole. Make sure that the diameter is large enough to clear the tool holder's X width.

   3. In the Final X DRO field, type the desired final diameter of the internal diameter.

   4. In the Z Start DRO field, type the location of the stock's face.

NOTE: This DRO field is used with the Tool Clearance DRO field to set the transition between rapid and feed rate on some Z moves.

NOTE: Use larger values to begin; once you're familiar with how the program works, smaller values may save time. Larger values bring the back of the tool holder closer to the ID wall on the end of facing cuts.

Open

Figure 18: Program-specific DROs on the ID Turn tab.

Extended Internal Diameters

To create an extended internal diameter:

1. From the Conversational tab, select the ID Turn tab.

2. Select the button to toggle from Basic to Extended mode.

Open

Figure 19: ID Turn tab in Extended mode.

3. From the Conversational DROs group, set the parameters for the ID turning operation.

Open

Figure 20: ID Turn tab on the Conversational tab.

4. Work through the program-specific DRO fields:

   1. In the Tool DRO field, type the currently selected tool as it's defined in the Tool Table window (on the Offsets tab).
      This DRO field is a command value — it sets the tool number for a tool change at the start of the program.

   2. In the Initial X DRO field, type the diameter of the pilot hole. Make sure that the diameter is large enough to clear the tool holder's X width.

   3. In the Final X DRO field, type the desired final diameter of the internal diameter. The value must be greater than twice the tool holder’s X width plus tool clearance.

   4. In the Z Start DRO field, type the location of the stock's face.

NOTE: This DRO field is used with the Tool Clearance DRO field to set the transition between rapid and feed rate on some Z moves.

NOTE: The fillet calculation does not use CRC, so the middle of the fillet may not be on the true radius for a tool with a tip radius. Valid values are 0 or positive. Values larger than the Z range (Z START - Z END) or the X range ((INITIAL X - FINAL X) / 2) are valid, but will have a fillet start or end short of the finish locations, which may not be practical.

NOTE: Use larger values to begin; once you're familiar with how the program works, smaller values may save time. Larger values bring the back of the tool holder closer to the ID wall on the end of facing cuts.

NOTE: The reverse or back cutting direction is sensitive to depth of cut. Form tools with a small angle between cutting edges allows for a larger depth of cut.

Open

Figure 21: Program-specific DROs on the ID Turn tab.

About ID Turning

Internal diameter turning is the process of removing material from the inside of a part.

ID Turning in PathPilot

There are two versions of ID turning in PathPilot: basic and extended. Both versions use CSS for spindle speed control and FPR for feed control. The fillet does not use CRC so the fillet will not follow a true radius for tools with a tip radius.

• Basic Mode
  Basic mode does one operation, which roughs and finishes from an initial pilot hole diameter to a final internal diameter without cutting a face at the bottom of hole. Use Basic mode for through holes or holes that don’t need a finished face. Each pass ends at Z End.
  Roughing starts at the pilot hole diameter (the value in the X Start DRO field), and incrementally cuts diameters with an adjusted depth of cut until the start of the finish diameter (X End - [2 × Finish DOC]). Finishing is done in one pass.

• Extended Mode
  Extended mode does three operations: ID roughing, face roughing, and an ID, fillet, and face finish pass. The extended ID roughing passes stop at the bottom of the pilot hole in order to prevent engaging too much of the tool cutting edge. Once the rough ID is cut to the pilot hole bottom, rough facing is started. There are two DRO fields for depth of cut, since, depending on the tool geometry, ID roughing and face roughing may need different depth of cuts.
  For each face pass, the tool tip cuts to the hole center + Tool Clearance which requires a rough hole diameter (which was cut in the first operation) that is a little more than twice the tool’s X width. Caution is needed to prevent hitting the back of the tool holder on the side of the hole.

Create a Profile on a Part

Using conversational programming, you can program PathPilot to rough and finish an arbitrary internal or external profile on a part. For information, see "About Profiling" (page 20).

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

• The Tool Clear Dia X DRO field has a value of larger diameter than first X value on the Profile Point table.

• Verify that the X-axis direction matches your specific lathe.

X-Axis Differences Between Lathes

IMPORTANT! The X-axis direction differs between the 15L lathe and the 8L lathe. Where X-axis values are mentioned in this documentation, verify the intended movement direction based on your lathe model. Adjust clearances, cutting directions, and tool paths accordingly.

• 15L X+ moves away from the operator, X- moves toward the operator.

• 8L X+ moves toward the operator, X- moves away from the operator.

Open

Figure 22: X-axis movement on an 8L lathe.

Complete the following steps in the order listed:

Describe the Stock

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

2. (Optional) To create an internal profile, select the button to toggle from External mode to Internal mode.

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

Open

Figure 23: Conversational DROs on the Profile tab.

4. Work through the program-specific DRO fields:

   1. In the Stock Dia DRO field, type the diameter of the stock.

   2. In the Tool Clearance Z DRO field, type the incremental Z value for the tool clearance on the Z-axis.
      Tool Clearance Z is the Z plane the tool goes from rapid to feed.

   3. In the Stock Z DRO field, type the starting Z value for the profile.

   4. In the Tool Clear Dia X DRO field, type the X value — as a diameter — for the tool clearance on the X-axis.

      1. For External Profiles You must make sure the value typed in the Tool Clear Dia X DRO field is a smaller diameter than the value typed in the Stock Dia DRO field.

      2. For Internal Profiles You must make sure the value typed in the Tool Clear Dia X DRO field is a larger diameter than the first diameter (specified in the Profile Point table).

Open

Figure 24: Program-specific DROs on the Profile tab.

Identify the Profile Points

Use the Profile Point table to describe the point-to-point values of a profile — from a larger Z value to a smaller Z value. As you work through the Profile Point table, PathPilot displays a graphical representation of the profile on your part.

Click on any segment in the graphic to highlight the corresponding row in the Profile Point table. Alternately, you may click on any row in the Profile Point table to highlight the corresponding segment in the graphic.

Point the mouse toward any area in the graphic and use the scroll wheel to zoom in and out to enlarge small features. To quit zooming, either select the Esc key or select another line in the Profile Point table.

To identify the profile points:

1. Select the Profile Point tab.

2. In the Profile Point table, type the X and Z values for the profile. X values are in diameters terms. Make sure that the X values are entered correctly based on your lathe model: for 8L lathes, the X+ values decrease toward the spindle.

NOTE: If the value is unchanged from the previous row in the Profile Point table, PathPilot assumes the value is repeated. If you are using the same value, you can leave the cell empty.

3. (Optional) In the Radius column, type a value to X and Z end points to create an arc.

   1. For a Center Point Above and/or to the Right of the Start Point Type a positive radius value.

   2. For a Center Point Below and/or to the Left of the Start Point Type a negative radius value.

Open

Figure 25: Profile Points table on the Profile tab.

Identify the Tool

1. In the Tool DRO field, type the number of the tool to use for creating the profile.
   Tool Geometry displays a graphical representation of the selected tool.

2. On the graphical representation of the profile on your part, make sure there are no red line segments. If there are red line segments, you must specify a new tool or edit the fields in the Profile Point table.
   A red line segment indicates that the geometry of the selected tool cannot cut the programmed angle without gouging the part profile — typically, when feature entry or exit angles are too steep for the tool geometry to clear.
   The back angle of the tool will not clear the entry to the arc feature.

Identify the Roughing and Finishing

Use the Roughing / Finishing tab to describe the required roughing and finishing for the part’s profile.

NOTE: You can use only roughing or only finishing. It is an error if all three of the following DRO fields are empty: Finishing Passes, Roughing DOC, and Finishing DOC.

To identify the roughing and finishing:

1. Select the Roughing / Finishing tab.
   PathPilot updates the graphical representation of the profile depending on which DRO field you select:

• Select inside the Roughing DOC DRO field to display a roughing graphic.

• Click inside the Finishing DOC DRO field or the Finish Passes DRO field to display a finishing graphic.

2. In the Roughing DOC DRO field, type the depth of cut for each roughing pass.

NOTE: The default value is 0.02 inches.

3. In the Finishing DOC DRO field, type the depth of cut for each finishing pass.

NOTE: The default value is 0.003 inches.

4. In the Finishing Passes DRO field, type the number – from 0-2 – of finishing passes.

NOTE: The default value is 2 (passes).

A finishing pass is a continuous pass from the start of the profile (toward the tailstock) to the end of the profile (toward the headstock).

Open

Figure 26: Roughing/Finishing tab on the Profile tab.

Describe the Tool Geometry

Use the Tool Geometry tab to describe the front and rear profiling angles. Because there are many tool and tool holder geometries, the Tool Geometry tab allows you to properly describe each tool and avoid part gouging.

To describe the tool geometry, first determine the cutting direction: either X+ or X-, based on the tool orientation and an internal or external profile. (For 8L lathes, an X+ cutting direction moves toward the operator.)

Use the table below to select the correct tool orientation for your machine.

To describe the tool geometry:

• X- Cutting Tool In the Front Angle DRO field and the Back Angle DRO field, type the value of the tool geometry expressed as a negative angle in the counterclockwise direction from 0˚.

Open

Figure 27: Tool Geometry tab on the Profile tab.

NOTE: The Tool Geometry graphic preview (to the right of the Tool DRO field) updates as angles are changed.

• X+ Cutting Tool In the Front Angle DRO field and the Back Angle DRO field, type the value of the tool geometry expressed as a negative angle in the clockwise direction from 0˚.

About Profiling

The profile is created from a list of points that describes the part geometry. A profile can have both forward (toward the tailstock) and rear (toward the headstock) facing features, and can also start behind the highest Z plane (the feature that is closest to the tailstock).

On the Profile tab, you can also specify things like:

• Tool geometry

• Feeds and speeds

• Finish depth

• Number of finish passes

• Roughing depth of cut (roughing DOC)

Create a Face on a Part

Using conversational programming, you can program PathPilot to cut a face with tool paths from the stock's outer diameter to the spindle center or an inner diameter (with each pass progressing in Z toward the headstock). For information, see "About Facing".

Before You Begin

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

• To cut with a rear tool, the values used in the Initial X DRO field and the Final X must be positive. The tool works on the positive X side of the spindle center (the side toward you).

• To cut with a front tool, the values used in the Initial X DRO field and the Final X must be negative. The tool works on the negative side of the spindle (the side away from to you).

• The value used in the Roughing DOC DRO field must be positive.

• The value used in the Finish DOC DRO field must be positive.

• Spindle speed control: CSS.

• Feed rate control: FPR.

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.

Open

Figure 28: Conversational DROs on the Face tab.

3. Work through the program-specific DRO fields:

   1. In the Tool DRO field, type the tool number for use with the program. This sets the tool number for a tool change at the start of the program.

   2. In the Initial X DRO field, type the stock diameter. This value is also used with the value in the Tool Clearance DRO field to locate some of the transitions between rapid and feed rate.

   3. In the Final X DRO field, type the location of the face inside diameter. The tool path goes beyond this diameter by the tool clearance. For tools with a tip radius, the control point and face contact point aren't the same, so the tool clearance value, if greater than the tool tip radius, can be used to extend the path to the contact point.

   4. In the Z Start DRO field, type the location of the stock face. Roughing passes start here. It is also used with Tool Clearance to set the transition between rapid and feed rates on some moves.

   5. In the Z End DRO field, type the finished face location.

   6. In the Tool Clearance DRO field, type the desired space required for tool retracting and transitions between rapid and cutting feed rate. Since there's one value used for X and Z moves, set the value to the greater of the two clearances. Larger values may be safer, but brings the back of the tool holder closer to the inner diameter wall on the end of facing cuts. Smaller values may save time once you're familiar with how well the program works.

   7. In the Roughing DOC DRO field, type the depth of the material being cut. This depth of cut is adjusted to get the value used in the G-code.

   8. In the Finish DOC DRO field, type the desired amount of material required for one finish pass (after roughing).

Open

Figure 29: Program DROs on the Face tab.

About Facing

During a facing routine, PathPilot does the following:

1. Rough facing starts at Z Start and incrementally cuts at the depth of cut until the start of the finish face pass (Z End + Finish DOC).

2. The start of each pass is at the Initial X diameter + Tool Clearance and moves in the minus X direction until the Final X diameter – Tool Clearance is reached.
   If the value in the Final X DRO field is zero, the end of the pass will go beyond the spindle center.

3. Finishing is done in one pass at the value entered into the Finish DOC DRO field.

Create a Chamfer or Radius on a Part

Using conversational programming, you can program PathPilot to cut a chamfer, taper, or corner radius. For information, see "About Chamfer and Radius".

Before You Begin

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

• Uses cutter compensation (G41, G42), so that tools with a nose radius can cut to the correct profile.

• Radii are limited to 90° arcs that start on the outside diameter (the Initial X DRO field and the Z End DRO field). Be careful when using chamfer angles less than 30° or greater than 60°, due to the extra travel involved in traversing the tool clearance space at an angle. The path may take the tool into the chuck, spindle, or adjacent workpiece features.

• The value used in the Rouging DOC DRO field must be positive.

• The value used in the Finish DOC DRO field must be positive.

• Spindle speed control: CSS.

• Tool feed control: FPR.

To create a chamfer or radius on a part:

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

2. From the Conversational DROs group, set the parameters for the chamfer or radius operation.

Open

Figure 30: Conversational DROs on the Chamfer tab.

3. Work through the program-specific DRO fields:

   1. In the Tool DRO field, type the tool number for use with the program. This sets the tool number for a tool change at the start of the program.

   2. In the X DRO field, type the stock diameter. This value is also used with the Tool Clearance DRO field to locate some of the transitions between rapid and feed rates.

   3. In the Z Start DRO field, type the stock face or the end of the chamfer or radius. This value is also used with the Tool Clearance DRO field to set the transition between rapid and feed rates on some Z moves.

   4. In the Z End DRO field, type the location of the start of the chamfer or radius. The Z width of a chamfer or the radius of a corner equals (Z End - Z Start).

   5. (Optional) In the Chamfer Angle DRO field, type the angle between the workpiece centerline and the chamfer.

   6. In the Tool Clearance DRO field, type the desired space beyond the stock outside diameter and face that's required for some movements to clear the workpiece. Since there is one value used for X and Z moves, set the value to the greater of the two clearances. Larger values may be safer; smaller values may save time once you're familiar with how well the program works. This field is also sometimes used as a location for retracting the tool while making cutting passes.

   7. In the Rouging DOC DRO field, type the depth of cut during roughing. The depth of cut is adjusted. In this case, the roughing range is the distance from the workpiece corner (the intersection of the face and outer diameter) and the closest point on the chamfer or radius minus the finish depth of cut.

   8. In the Finish DOC DRO field, type the desired amount of material required for one finish pass (after roughing).

Open

Figure 31: Program DROs on the Chamfer tab.

About Chamfer and Radius

During a routine to create a chamfer or a radius, PathPilot does the following:

1. Roughing starts at the corner of X and Z Start in adjusted depth of cut increments perpendicular to the chamfer angle or incremental arcs for radius.

2. The last roughing pass leaves enough material for the finish pass; finishing is done with a single pass.

3. Passes start and end on the perimeter of the tool clearance space, which is set by adding the tool clearance DRO value to the stock OD, X, and the face location, Z Start.

Create a Groove or Part a Workpiece

Using conversational programming, you can program PathPilot to create a groove or to part a workpiece from stock. For information, see "About Grooving and Parting".

Before You Begin

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

• Grooving paths are based on Z Start and Z End values:

  • If the value in the Z Start DRO field is greater than the value in the Z End DRO field, the tool’s control point is set to the +Z side of the tool.

  • If the value in the Z Start DRO field is less than the value in the Z End DRO field, the control point is set to the -Z side of the tool.

• Groove roughing is done with plunge cuts in the X direction. Each plunge is incremented in the Z direction from Z Start ± Finish DOC to Z End ± (Tool Width + Finish DOC).

• Even though a grooving/parting tool may be considered to have two tips, valid tool orientation is limited to:

  • Groove on the positive side of Z Start, Front Tool = Type 3

  • Groove on the negative side of Z Start, Front Tool = Type 4

  • Part on the negative side of Z Start, Front Tool = Type 4

• CSS is used for spindle speed control.

• FPR is used for feed rate control.

• CRC is not used.

To create a groove on a part, or to part a workpiece:

1. From the Conversational tab, select the Groove/Part tab.

2. From the Conversational DROs group, set the parameters for the grooving or parting operation.

Open

Figure 32: Conversational DROs on the Groove/Part tab.

3. If required, toggle the Groove/Part button. Then, do one of the following:

• Go to "Create a Groove on a Part".

• Go to "Part a Workpiece from the Stock”.

Create a Groove on a Part

Work through the program-specific DRO fields:

1. In the Tool DRO field, type the tool number for use with the program. This sets the tool number for a tool change at the start of the program.

2. In the Initial X DRO field, type the stock diameter. This value is also used with the Tool Clearance DRO field to locate some of the transitions between rapid and feed rates.

3. In the Final X DRO field, type the diameter of the new groove bottom or the end of the parting.

4. In the Z Start DRO field, type the location of the groove start. For parting, this field sets the location of the +Z side of the slot.

5. In the Z End DRO field, type the location of the groove end.

6. In the Tool Width DRO field, type the groove or parting tool's width.

7. In the Rough DOC DRO field, type the depth of the material being cut. In this case, for groove, it is the Z offset for each plunge cut. The depth of cut is adjusted. Valid values are positive and normally should be less than the full depth width of the tool tip (usually the distance between tip radii centers).

8. In the Finish DOC DRO field, type the desired amount of material required for one finish pass (after roughing).

9. In the Tool Clearance DRO field, type the desired space beyond the stock outside diameter for rapid movements to clear the workpiece. Larger values may be safer; smaller values may save time once you're familiar with how well the program works. This field is also sometimes used as a location for retracting the tool between cutting passes.

Open

Figure 33: Program-specific DROs on the Groove/Part tab.

Part a Workpiece from the Stock

Work through the program-specific DRO fields:

1. In the Tool DRO field, type the tool number for use with the program. This sets the tool number for a tool change at the start of the program.

2. In the Initial X DRO field, type the stock diameter. This value is also used with the Tool Clearance DRO field to locate some of the transitions between rapid and feed rates.

3. In the Final X DRO field, type the diameter of the new groove bottom or the end of the parting.

4. In the Z Start DRO field, type the location of the groove start. For parting, this field sets the location of the +Z side of the slot.

5. In the Tool Width DRO field, type the groove or parting tool's width.

6. In the Tool Clearance DRO field, type the desired space beyond the stock outside diameter for rapid movements to clear the workpiece. Larger values may be safer; smaller values may save time once you're familiar with how well the program works. This field is also sometimes used as a location for retracting the tool between cutting passes.

Open

Figure 34: Program-specific DROs on the Groove/Part tab.

About Grooving and Parting

1. Groove finishing is done with a plunge cut down the Z End side.

2. When the tool reaches the bottom, the tool is moved in the Z direction toward the center of the groove, then retracts.

3. The tool is plunged on the Z Start side of the groove, then again is moved in Z toward the groove center and retracted. This requires a grooving tool, which can side cut. Part does one plunge cut at Z Start. The tool’s control point is on the +Z side of the tool. The plunge cannot be set to go beyond the spindle center (X = 0).

Create Holes on a Part or Tap a Hole

Using conversational programming, you can program PathPilot to drill holes on a part, or use rigid tapping to thread 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:

• The value used in the Z Start DRO field must be larger than the value in the Z End DRO field.

• For tapping, the value used in the Z End DRO should allow for extra threading while the spindle comes to a stop and reverses.

• The value used in the Peck Depth DRO field needs a direction, so should have a negative value.

• Drilling is limited to the -Z direction, toward the spindle.

• Use the RPM DRO field instead of CSS.

To create holes on a part, or to tap a hole:

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

2. From the Conversational DROs group, set the parameters for the drilling or tapping operation.

Open

Figure 35: Conversational DROs on the Drill/Tap tab.

3. If required, toggle the Drill/Tap button. Then, do one of the following:

• Go to "Create a Hole on a Part".

• Go to "Create Threads in a Hole".

Create a Hole on a Part

Work through the program-specific DRO fields:

1. In the Tool DRO field, type the tool number for use with the program. This sets the tool number for a tool change at the start of the program.

2. In the Z Start DRO field, type the stock face location. This field is also used with the Tool Clearance DRO field to set the transition between rapid and the feed for drilling or tapping.

3. In the Z End DRO field, type the final depth. This is the location where the drill feed stops and optionally dwells.

4. In the Peck Depth DRO field, type an incremental depth for retracting the drill to clear chips from the hole, if required. If drilling the hole doesn't need a peck, type 0. To make each peck depth equal, the value is adjusted to fit an integer number of pecks within the hole depth.

5. In the Tool Clearance DRO field, type the desired space required for tool retraction and transitions between rapid and cutting feed rate.

6. In the Spindle RPM DRO field, type the RPM (G97) desired.

7. In the Dwell at Bottom (Sec) DRO field, type the length of time that Z motion should pause so that the drill can finish cutting the hole bottom before retracting.

Open

Figure 36: Program-specific DROs on the Drill/Tap tab.

Create Threads in a Hole

Work through the program-specific DRO fields:

1. In the Tool DRO field, type the tool number for use with the program. This sets the tool number for a tool change at the start of the program.

2. In the Z Start DRO field, type the stock face location. This field is also used with the Tool Clearance DRO field to set the transition between rapid and the feed for drilling or tapping.

3. In the Z End DRO field, type the final depth. This is the location where the spindle rotation is reversed.

4. In the Peck Depth DRO field, type an incremental depth for retracting the drill to clear chips from the hole, if required. If drilling the hole doesn't need a peck, type 0. To make each peck depth equal, the value is adjusted to fit an integer number of pecks within the hole depth.

5. In the Tool Clearance DRO field, type the desired space required for tool retraction and transitions between rapid and cutting feed rate.

6. In the Spindle RPM DRO field, type the RPM (G97) desired.

7. In the Threads/Inch (/mm) DRO field, type the Z motion to spindle ratio that matches the thread pitch required. This field is also used with the Pitch (Inches) DRO field, so entering a value in either field calculates and inserts a value in the other.

8. In the Pitch (Inches) DRO field, type the Z motion to spindle ratio that matches the required thread pitch. This field is also used with the Threads/Inch (/mm) DRO field, so entering a value in either field calculates and inserts a value in the other.

Open

Figure 37: Program-specific DROs on the Drill/Tap tab.

About Drilling and Tapping

Drilling

1. For feed rate control, drill uses a millimeter or inch feed per revolution (G95) to feed from Z Start + Tool Clearance until Z End.

2. Rapids back to Z Start + Tool Clearance.

Dwell allows a pause for the drill to stay at Z End long enough to cut a full revolution at the bottom of the hole (rather than immediately retracting the drill, which could leave an irregular bottom).

Pecking can help clear chips before they bind in the hole during drilling. The peck motion retracts to Z Start + Tool Clearance on each cycle.

NOTE: Due to motion control limits, the retract to Z Start + Tool Clearance may not retract fully before starting the next drilling feed. You must verify that the pecking retract motion meets requirements for your application.

Tapping

Tap uses electronic gearing (G33.1, Rigid Tapping) to lock the Z-axis and spindle motion together for rigid tapping.

1. Tapping starts with the tap at Z Start + Tool Clearance.

2. Z motion waits until the spindle encoder index is tripped. Then, the gears are engaged and Z feeds at the rate set by the pitch or threads per unit (TPU) and spindle encoder count. The Z motion follows the spindle motion no matter what the spindle does.

3. For tapping, the spindle is run forward until Z End is reached, the spindle is reversed, which causes it to slow to a stop, then reverse. During this time, the tap continues to follow the spindle motion and continues to make threads until the spindle reverses.

NOTE: These extra threads needs to be considered when setting the Z End DRO field.

4. The reverse motion continues until reaching Z Start + Tool Clearance where the gearing is disengaged.

Create Threads on a Part

Using conversational programming, you can program PathPilot to single point an external or an internal thread on an existing outer diameter. For information, see "About Threading”.

Before You Begin

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