PathPilot Tools and Features - 1100M
- Sam Bollen
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:
From the File tab, in the Controller Files window, select the desired .nc file.
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:
Either insert a USB drive into any open USB port, or sign in to PathPilot HUB.
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.
Select the location to which you want to copy the transferred file.
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.
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:
From the Main tab, in the G-Code tab, select the Recent Files menu.
The last five program files loaded into PathPilot display.
Select the name of the desired G-code program.
The G-code program loads.
Close the Current Program
From the Main tab, on the G-Code tab, select the Recent Files menu.
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:
From the Controller Files window, highlight the .nc file and select Edit G-code.
The file opens in a text editor.
Make and save the appropriate changes to the file.
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:
From the File tab, select the .nc file.
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.
Edit the file contents as needed. Do any of the following:
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
Select Insert Step.
PathPilot opens the Conversational tab.Create the new job assignment.
Select Insert.
(Optional) Edit the job assignment order in the program.
Load an Existing G-Code File
Select Insert File. You can insert G-code files that are hand-written, generated from CAM software, or generated from conversational programming in PathPilot.
Navigate to and select the .nc file that you want to insert.
Select Open.
(Optional) Edit the job assignment order in the program.
Edit a Job Assignment
Select the job assignment, and then select Conv. Edit.
PathPilot opens the Conversational tab.Edit the job assignment.
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:
From Main tab, on the G-Code tab, select any line of code to use as a starting point.
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.
Select the Enter key.
If PathPilot finds the information, the searched term is scrolled to and highlighted in the G-Code tab.(Optional) Select Enter.
PathPilot finds the next instance of the searched text.(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:
From the Main tab, on the G-Code tab, do one of the following:
Right-click any line in the program.
Tap the line. Then, select the Options menu.
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
From the Main tab, do one of the following:
Right-click the Tool Path display.
Select the View Options tab.
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 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".
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:
From the Conversational tab, select the Face tab.
From the Conversational DROs group, set the parameters for the facing operation.
Work through the program-specific DRO fields:
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.
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.
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".
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.
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:
Moves the machine to the predefined G30 position, or the tool change position.
If required, performs or requests a tool change.
Makes a rapid move in the X and Y direction to the beginning of the workpiece.
Makes a rapid move in the Z direction to the predefined Z Clear position.
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).
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".
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:
From the Conversational tab, select the Profile tab.
From the Conversational DROs group, set the parameters for the profiling operation.
Work through the program-specific DRO fields:
In the X Start DRO field and the X End DRO field, type the location of the workpiece edges.
In the Y Start DRO field and the Y End DRO field, type the location of the workpiece edges.
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.
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.
In the Radius DRO field, type the required radius for the corners of the profile. For no corner radius, type 0.
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.
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:
Retracts the tool to the Z Clear position.
NOTE: The first Z pass cuts at Z Start minus Depth of Cut adjusted.
Makes a rapid movement to the beginning of the section.
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.
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:
From the Conversational tab, select the Pocket tab.
From the Conversational DROs group, set the parameters for the pocket operation.
Work through the program-specific DRO fields:
In the X Center DRO field and the Y Center DRO field, type the location of the pocket's center.
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:
From the Conversational tab, select the Pocket tab.
From the Conversational DROs group, set the parameters for the pocket operation.
Work through the program-specific DRO fields:
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.
In the Radius DRO field, type the required radius for the corners of the pocket. For no corner radius, type 0.
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.
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.
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:
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:
Uses a straight Z plunge into the pocket center. You must use a center-cutting end mill.
Makes a single pass around the perimeter of the pocket at the adjusted Z depth of cut.
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:
Uses a helical entry into the pocket center.
Makes a hole that is two times the diameter of the tool diameter in the pocket center.
Makes a spiral cut out from the pocket center to the pocket diameter.
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:
Uses a straight Z plunge into the pocket center. You must use a center-cutting end mill.
Makes a single pass around the perimeter of the pocket at the adjusted Z depth of cut.
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):
From the Conversational tab, select the Drill/Tap tab.
From the Drill/Tap tab, select the Circular tab.
In the Number of Holes DRO field, type the number of holes (greater than 0) required for the pattern.
In the Start Angle DRO field, type the value of the angle from angle 0 (from -90 to 90).
In the Diameter DRO field, type the size of the circular pattern (as defined by a line through the center point of each hole).
In the Center X DRO field and the Center Y DRO field, type the location for the center of the hole.
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:
From the Conversational tab, select the Drill/Tap tab.
From the Drill/Tap tab, select the Pattern tab.
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.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.
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.
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.
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".
Set the parameters for the hole in the Z range:
In the Z Start DRO field, type the location for the first Z pass.
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".
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.
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.
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.
Set the parameters for the hole in the Z range:
In the Z Start DRO field, type the location for the first Z pass.
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:
From the Conversational tab, select the Thread Mill tab.
From the Conversational DROs group, set the parameters for the thread milling operation.
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.
Work through the program-specific DRO fields:
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".
To create an engraving sequence on a part:
From the Conversational tab, select the Engrave tab.
From the Conversational DROs group, set the parameters for the engraving operation.
Work through the program-specific DRO fields:
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.
From the Conversational tab, select the DXF tab.
Select the File DRO field.
The File Selector dialog box opens.Select the .dxf file, and then select Open.
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".
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.
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%.
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.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:
From the PathPilot interface, on the Status tab, select Internet.
The Network Configuration dialog box displays.
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.
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:
From the PathPilot interface, on the Status tab, select Update.
The Software Update dialog box displays.
From the Software Update dialog box, select the Check online daily for updates; confirmation required for download and installation checkbox.
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:
From the Network Name field, type a new network name.