PathPilot Tools and Features - 1100M
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.