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:
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 / HUB 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 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:
From the Conversational tab, select the OD Turn tab.
From the Conversational DROs group, set the parameters for the OD turning operation.
Work through the program-specific DRO fields:
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.
b. In the Initial X DRO field, type the value of the stock's outside diameter.
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.
c. In the Final X DRO field, type the desired value of the part's final outside diameter.
d. 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.
e. In the Z End DRO field, type the desired location of the part's face.
f. In the Fillet Radius DRO field, type the desired radius between the part's outside diameter and its face. For no radius, type 0.
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.
g. In the Tool Clearance DRO field, type the distance required for clearance when the machine makes rapid movements between the stock's outside diameter its face. Because there's only one value used for X and Z moves, use the greater of the two clearances.
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.
h. In the Roughing DOC DRO field, type the desired amount of material to remove from the radius of the stock on each roughing pass. The depth of cut is adjusted to get the value used in the G-code.
i. In the Finish DOC DRO field, type the desired amount of material required for one finish pass (completed after roughing).
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:
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.
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.
The tool retracts to the stock diameter.
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:
From the Conversational tab, select the ID Turn tab.
From the Conversational DROs group, set the parameters for the ID turning operation.
Work through the program-specific DRO fields:
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.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.
In the Final X DRO field, type the desired final diameter of the internal diameter.
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.
e. In the Z End DRO field, type the desired final location for the part's face.
f. In the Tool Clearance DRO field, type the distance required to retract the tool and transition between rapid and cutting feed rate. Because there's only one value used for X and Z moves, use the greater of the two clearances.
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.
g. In the ID Rough DRO field, type the depth of material to cut on the radius of the bore. The depth of cut is adjusted to get the value used in the G-code.
h. In the Finish DOC DRO field, type the desired amount of material required for one finish pass on the ID, fillet, and face (completed after roughing).
Extended Internal Diameters
To create an extended internal diameter:
From the Conversational tab, select the ID Turn tab.
Select the button to toggle from Basic to Extended mode.
From the Conversational DROs group, set the parameters for the ID turning operation.
Work through the program-specific DRO fields:
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.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.
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.
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.
e. In the Fillet Radius DRO field, type the desired radius between the finished inside diameter and the face.
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.
f. In the Z End DRO field, type the desired final location for the part's face.
g. In the Tool Clearance DRO field, type the distance required to retract the tool and transition between rapid and cutting feed rate. Because there's only one value used for X and Z moves, use the greater of the two clearances.
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.
h. In the ID Rough DRO field, type the depth of material to cut on the radius of the bore. The depth of cut is adjusted to get the value used in the G-code.