Tormach 15L and 15LX · A primer for experienced pen makers new to CNC
This lesson walks you through the instructor’s eight-tool gang arrangement, tool configuration, and offset-setting method. By the end, you will have established Tool 2 as the master tool, referenced the other tools to the same workpiece, and centered the three drills.
The setup and methods below describe this particular machine arrangement. Dimensions and settings must match the actual tooling and clearances on the machine being used.
Terms used in this lesson: OD means outside diameter; ID means inside diameter. Tool numbers identify the eight physical tools. Orientation numbers identify their cutting-point configurations in PathPilot.
Setup order: Check the physical layout, assign all eight tools, establish Tool 2, complete every tenon-based touch-off, then remove the reference workpiece and center the drills in X. All offset-setting entries use millimeters; inch mode is used only for the soft-limit adjustment.
1 - Prepare the machine and tooling
Provide the travel needed for this arrangement
The instructor’s eight-tool arrangement requires adjusting the X-axis soft limit. Follow Tormach’s Adjusting Lathe Soft Limits guide for the adjustment and display commands.
Record the existing soft limits before changing them.
Although the course uses metric units, enter G20 in the MDI field for this adjustment to select inch mode.
Following the guide, set the X-axis soft limit to 12 inches by entering 12 while in inch mode. The instructor identifies this as the maximum setting for their setup.
Display the current soft limits and confirm the change.
Enter G21 to return to metric mode before continuing.
15LX clearance requirement for the instructor’s setup: Remove the bottom trim plate from the carriage before using this extended travel. The instructor reports that it will collide with the angled pan wall on the 15LX; the 15L pan has straight walls. Check clearance on the actual machine throughout the required movement.
Tormach cautions that changing soft limits increases collision risk and requires cautious test runs. Its linked guide mentions the 15L and 8L; the 12-inch setting and 15LX trim-plate requirement above are instructor-provided setup details.
Position the tools within the available X travel
Establish the physical layout by positioning Tool 1 first. Place the cutoff/grooving tool on the gang plate so its cutting tip can travel slightly past X zero, the spindle centerline. This allows the tool to pass through center for a clean cutoff.
At the other end of the arrangement, check Tool 8, the 8.2 mm body drill. Its tip must be able to reach the spindle centerline and travel slightly past X zero as well, so the drill can be aligned on center.
Use these two end positions to establish the usable span of the layout, then arrange Tools 2 through 7 between them. Confirm that all eight tools can reach their required X positions within the available travel, with clearance for every tool and holder throughout the movements. Complete these physical travel checks before setting tool offsets.
Check the physical installation
Secure the tools and holders, check cutting-tool center height, align the drills with the spindle centerline, and check tool projection and clearances. Every gang-plate movement moves all eight tools, so clearance checks must include neighboring tools and holders as well as the tool being used.
Course development note: Add step-by-step instructions and close-up photos for setting center height, aligning drills, securing holders, choosing tool projection, and checking clearance against stock, workholding, carriage, enclosure, and adjacent tools throughout the required movements.
Tormach guidance on center height and drill alignment
Center height and mounting: The Setup section of the 15L Gen 2 Turret Installation Manual discusses shimming cutting tools to the spindle axis, keeping projection short, and the sensitivity of parting tools to alignment. These mounting principles are useful here; its turret alignment steps and shim locations apply to that turret, not this gang plate.
Drill alignment:Touching Off Drills on a Tormach Lathe provides alternative touch-off methods for the 8L and 15L and notes their differing X sign conventions. Use it alongside the method taught in Section 11.
Instructor note: I consider the Tormach approach probably the better way to establish drill alignment and touch-off. The centering-tool and loupe method I demonstrate in Section 11 has given me no issues in my own setup.
Physical drill height and alignment must be correct before relying on X-zero touch-off. Setting X zero locates the drill in X; it does not mechanically adjust holder height or straighten a tilted drill. A holder-specific demonstration for this gang setup remains to be added.
2 - Identify the eight tools
In the annotated photograph, tools run from 1 through 8, top to bottom.
Tool
Function
Use or role
1
Cutoff and grooving
Parting and grooving
2
OD turning
OD turning and master tool
3
7 mm drill
Drilling sections
4
ID boring
Internal boring
5
ID threading
Internal threads
6
OD threading
External threads
7
9.2 mm drill
Drilling caps
8
8.2 mm drill
Drilling bodies
Figure 1. Annotated identification guide. Use the angled photograph for an additional view of the mounting.Figure 2. Angled view identifying all eight tools and their functions.
3 - Use the Offsets tab and assign tools
What the Offsets tab is used for
The Offsets tab is where you tell PathPilot which tools are installed, how their cutting points are oriented, and where each tool is located. You will use it first to assign the tool configurations, then to establish their X and Z references in the offset-setting steps later in this lesson.
Tormach references: 15L PathPilot Tools and Features, under Set Tool Geometry Offsets, covers tool selection and touch-off controls. 15L Programming, under Controlled Point, explains numbered cutting-point orientations.
Open the tab and select a tool
Go to the Offsets tab. Enter the tool number in the field in the upper-right corner and press Enter to confirm the selection. Always confirm the selected tool before changing its configuration or setting its offsets.
The numbered red boxes on the introductory unassigned-tool screenshot identify controls 1 through 4. RESET TOOL appears after a tool is configured and is explained separately below. The individual Tool 1 through Tool 8 screenshots are left unmarked so you can focus on their tool graphics and orientations. The callout numbers refer to controls, separately from tool numbers and orientation numbers.
Offsets tab: Open this tab to configure tools and set offsets.
Tool-number field: Enter the tool number and press Enter.
TOUCH X box: Enter the X reference value, then click TOUCH X.
TOUCH Z box: Enter the Z reference value, then click TOUCH Z.
Recognize an unassigned tool
If the selected tool has no assigned configuration, PathPilot displays the full gallery of tool graphics shown below. You may see this when setting up a new tool, selecting an unassigned tool number, or after using RESET TOOL.
Figure 3. Tool selection screen for an unassigned, new, or reset tool. References 1–4 identify the Offsets tab, tool-number field, TOUCH X box, and TOUCH Z box. RESET TOOL is not shown on this screen. This example shows T0; select the intended tool number for your setup.
Assign the tool graphic and orientation
Choose the graphic that matches the tool function, mounting side, and physical orientation. In Figure 4, positive X is on the rear-tool side above the spindle centerline, and negative X is on the front-tool side below it. Above and below describe the diagram, rather than tool center height. The orientation numbers in the right-hand diagram are separate from the assigned tool numbers.
Figure 4. X zero is the spindle centerline. Positive X is on the rear-tool side, shown above the line; negative X is on the front-tool side, shown below it. Diagram adapted from the Tormach video Setting Work and Tool Offsets.
Use the eight tool examples below to match this gang tooling arrangement. Their screenshots show the required configurations. The captured position values and inch-mode status are not setup entries to copy; the offset-setting examples in this lesson use millimeters.
Reset an existing tool configuration when needed
If the selected tool already has an incorrect configuration, click RESET TOOL to return to the tool-selection gallery. You can then choose its tool graphic and orientation again. This is especially useful when setting up a used machine with tool definitions left by the previous owner.
RESET TOOL also clears the selected tool geometry offsets. Use it before establishing the tool offsets. If you reset a tool that has already been referenced, establish its offsets again before machining.
To start over, select the tool number and press Enter, click RESET TOOL, choose the correct graphic and orientation, then follow the offset-setting procedure later in this lesson.
Select Tool 1 and the cutoff/grooving graphic with orientation 2. This tool works on the positive-X side and is mounted upside down in the instructor’s holder.
Figure 5. Tool 1 configuration.
Tool 2 OD turning and master tool
Select Tool 2 and the OD turning graphic shown under FRONT POST, with orientation 3.
Figure 6. Tool 2 configuration.
Tool 3 7 mm drill for sections
Select Tool 3 and the drill graphic with orientation 7. This is the 7 mm drill for sections.
Figure 7. Tool 3 configuration.
Tool 4 ID boring
Select Tool 4 and the ID boring graphic shown under FRONT POST, with orientation 2.
Figure 8. Tool 4 configuration.
Tool 5 ID threading
Select Tool 5 and the ID threading graphic shown under FRONT POST, with orientation 6.
Figure 9. Tool 5 configuration.
Tool 6 OD threading
Select Tool 6 and the OD threading graphic shown under FRONT POST, with orientation 8.
Figure 10. Tool 6 configuration.
Tool 7 9.2 mm drill for caps
Select Tool 7 and the drill graphic with orientation 7. This is the 9.2 mm drill for caps.
Figure 11. Tool 7 configuration.
Tool 8 8.2 mm drill for bodies
Select Tool 8 and the drill graphic with orientation 7. This is the 8.2 mm drill for bodies.
Figure 12. Tool 8 configuration.
4 - Understand the reference method
Tool offsets describe the positions of the tools so they can work on the same part. Tool 2 is the master tool. Its skim-cut diameter provides a known X reference; its finished stock face provides the common Z reference.
The instructor uses a floating Z zero. Machining zero is not a permanent Z position relative to the headstock. For each individual program, the instructor uses the program’s Z-zero function to establish Tool 2’s job reference; the remaining tools follow through their established offsets.
Course development notes: Add the exact controls or commands used to establish program Z zero. A fixed Z reference at a particular physical location is an alternative method; contributors who use it will provide that procedure later.
Choose the sign of the X touch-off value
Use Figure 4: spindle centerline is X = 0; the rear-tool side above the line is positive X; the front-tool side below it is negative X. The sign describes the reference contact position, not the jog direction.
The micrometer measures the tenon diameter. Apply the sign for the contact side when entering it in the TOUCH X box. For a 12.00 mm tenon, the entry is +12.00 on the rear side and -12.00 on the front side.
Tool
Signed TOUCH X entry for this setup
1 Cutoff and grooving
Positive measured diameter
2 OD turning and master tool
Negative measured diameter
4 ID boring
Positive measured diameter at the external tenon contact
5 ID threading
Positive measured diameter at the external tenon contact
6 OD threading
Negative measured diameter
3, 7, and 8 Drills
0 at spindle centerline during the final centering step
These signs describe the touch-off contacts, which can differ from the side used for cutting. Tools 4 and 5 both use a positive-X touch-off contact and a negative-X working position. Their TOUCH X entries are positive because they reference the positive-X surface of the tenon. The ID tools touch the outside of the reference tenon in this procedure. If the mounting side or reference contact changes, reassess the sign using Figure 4.
Keep the reference values distinct
Throughout the offset steps, measured tenon diameter means the diameter recorded with the micrometer, expressed in millimeters. Apply the X sign listed above when entering that measurement. The 12.00 mm diameter is an example only; use your actual measured diameter.
Reference face means the finished tenon face established as Z zero with Tool 2. For a feeler-gauge touch-off, enter the positive thickness of the gauge you actually use. The lesson uses a 0.05 mm gauge as an example, so its numeric TOUCH Z entry is +0.05. With a 0.10 mm gauge, the entry would be +0.10.
Tool 2 is set directly at the finished face with a TOUCH Z entry of 0. Tools 1, 3, 4, 7, and 8 use the feeler-gauge thickness. Tools 5 and 6 use visual cutting-tip alignment with a TOUCH Z entry of 0. All three drills receive a TOUCH X entry of 0 only in the final centering step.
For most jobs, the instructor uses approximately 2 inches or 50.8 mm of stock stickout from the workholding.
Set Z from the finished face
Go to the Offsets tab, select Tool 2, and press Enter.
Use the jog wheel to manually take a facing cut.
When the face is flat, do not move Z. Preserve the Z position used for the finished face.
Enter 0 in the TOUCH Z box in the upper-right corner, then click TOUCH Z to establish the Z-zero reference for the master tool.
Set X from the measured diameter
Take a skim cut on the outside diameter, producing the reference tenon.
Do not move X. Retract in Z to clear the stock.
Stop the spindle and measure the freshly cut diameter with a micrometer.
Enter the measured diameter in millimeters as a negative X value in the TOUCH X box. Tool 2 contacts the front side below X zero in Figure 4; for 12.00 mm, enter -12.00.
Click TOUCH X.
Tormach reference: 15L PathPilot Tools and Features, under Touch X, describes the skim cut, Z retraction without changing X, micrometer measurement, and TOUCH X entry.
Record and preserve the references
Record the measured tenon diameter, the signed TOUCH X entry used for Tool 2, and the reference-face Z value of 0. Keep these reference values distinct from the machine-position readings. You now have known references for the other tools: the tenon’s outside surface and its finished front face.
Do not remove or reposition the reference workpiece. Keep it clamped in the headstock workholding until every tool has completed its required reference against the tenon. For subsequent X entries, use the measured tenon diameter with the sign for the reference contact side in Figure 4.
6 - Set Tool 1 cutoff and grooving offsets
Go to the Offsets tab, enter 1, and press Enter.
Set X
Mark the reference tenon with a black Sharpie to make contact easier to see.
With the spindle stopped, manually jog Tool 1 toward the tenon in X.
Use the inner step wheel on the jog mouse for the final approach. Rotate the headstock spindle by hand while step jogging until the tool tip just contacts the tenon.
Enter the recorded tenon diameter as a positive X value in the TOUCH X box, then click TOUCH X. Tool 1 contacts the rear side above X zero in Figure 4; for 12.00 mm, enter +12.00.
Set Z with a feeler gauge
You can use any feeler-gauge thickness. 0.05 mm is only the example used here. Because the reference face is Z zero, enter the positive thickness of your chosen gauge in the TOUCH Z box.
With the spindle stopped, place a feeler gauge of your chosen thickness (0.05 mm in this example) against the tenon face used for Tool 2’s Z zero.
Step jog the cutoff tool until its reference cutting edge just contacts the gauge.
Enter the positive gauge thickness in millimeters (+0.05 in this example) in the TOUCH Z box and click TOUCH Z.
For the 0.05 mm example: reference face Z + gauge thickness = 0 + 0.05 = +0.05 mm.
Course development note: Add a close-up identifying which edge of the cutoff insert is used for Z touch-off.
Tormach reference: 15L PathPilot Tools and Features, under Touch Z, accounts for paper thickness in the Z entry. This lesson applies that thickness-accounting principle to a feeler gauge.
7 - Set Tool 3 7 mm drill Z only
Go to the Offsets tab, enter 3, and press Enter. With the spindle stopped, use a feeler gauge of your chosen thickness (0.05 mm in this example) against the reference face. Step jog until the drill tip just contacts it. Enter the positive gauge thickness in millimeters (+0.05 in this example) in the TOUCH Z box and click TOUCH Z.
Leave the drill’s X setup until the final centering stage.
8 - Set Tool 4 ID boring offsets
Go to the Offsets tab, enter 4, and press Enter. Use the same contact-finding method and positive X touch-off value as Tool 1. Tool 4 uses a positive-X touch-off contact on the outside of the reference tenon and a negative-X working position for boring. Enter the touch-off value for the contact side, as shown in Figure 4.
X: Mark the tenon with Sharpie. With the spindle stopped, approach in X, then rotate the spindle by hand while step jogging until the boring tool’s cutting tip just contacts the tenon. Enter the recorded tenon diameter as a positive X value in the TOUCH X box and click TOUCH X. Tool 4 makes this reference contact on the positive-X side above the centerline in Figure 4; for a 12.00 mm tenon, enter +12.00.
Z: With the spindle stopped, place a feeler gauge of your chosen thickness (0.05 mm in this example) against the reference face. Step jog the tool’s reference cutting point into contact with the gauge. Enter the positive gauge thickness in millimeters (+0.05 in this example) in the TOUCH Z box and click TOUCH Z.
9 - Set Tool 5 and Tool 6 offsets
Perform these steps separately for Tool 5, ID threading, and Tool 6, OD threading. Select the appropriate number in the Offsets tab and press Enter.
Set X using the tenon diameter
Use the same Sharpie and contact-finding method as Tool 1. With the spindle stopped, rotate the spindle by hand while making the final step-jog approach until the cutting tip just contacts the reference tenon. Enter the measured tenon diameter in the TOUCH X box with the sign for the reference contact of the selected tool:
Tool 5 ID threading: Use a positive-X touch-off contact on the outside of the reference tenon, shown above the centerline in Figure 4. The tool uses a negative-X working position for internal threading. Enter a positive diameter for this touch-off contact; for a 12.00 mm tenon, enter +12.00, then click TOUCH X.
Tool 6 OD threading: Touch off on the negative-X side shown below the centerline in Figure 4. Enter a negative diameter; for a 12.00 mm tenon, enter -12.00, then click TOUCH X.
Set Z by visual alignment
With the spindle stopped, observe the threading tool’s cutting tip through a 10× jeweler’s loupe.
Carefully jog in Z until the cutting tip aligns with the tenon’s finished front face, established as Z zero with Tool 2.
Enter 0 in the TOUCH Z box and click TOUCH Z.
Use visual alignment for these threading tools. Their TOUCH Z entry is 0; no feeler-gauge thickness is added.
Course development note: Add close-up photographs identifying the exact cutting-tip alignment point on each threading tool. “Cutting tip” is the terminology used throughout this lesson.
10 - Set Tool 7 and Tool 8 Z only
Repeat the drill Z procedure from Section 7 separately for Tool 7, the 9.2 mm cap drill, and Tool 8, the 8.2 mm body drill.
Select the tool number in the Offsets tab and press Enter.
With the spindle stopped, place a feeler gauge of your chosen thickness (0.05 mm in this example) against the reference face.
Step jog the drill tip into contact with the gauge.
Enter the positive gauge thickness in millimeters (+0.05 in this example) in the TOUCH Z box and click TOUCH Z.
11 - Center the drills in X last
Supporting reference: Tormach drill touch-off methods. The pointed centering tool and loupe method below is the procedure taught in this lesson; perform it only after all tenon-based references are complete.
STOP AND CHECK: Tool 2 must be established; Tools 1, 4, 5, and 6 must have their X and Z references; Tools 3, 7, and 8 must have their Z references. Only then may you remove the reference workpiece and install the centering tool.
After all tenon-based references are complete, remove the reference workpiece and secure the centering tool in the headstock workholding.
Go to the Offsets tab, select Tool 3 and press Enter.
With the spindle stopped, jog the drill tip close to the centering-tool tip.
Observe the tips through the loupe. Carefully jog in X until the tips align and just touch.
Enter 0 in the TOUCH X box and click TOUCH X. At the spindle centerline in Figure 4, the drill X reference is zero.
Repeat for Tool 7 and Tool 8.
Each drill now has an X reference at the spindle centerline. Preserve the Z offsets already established against the reference face.
12 - Review before machining
Tormach reference: Tool Alignment and Crash Avoidance in the 15L Gen 2 Turret Installation Manual explicitly includes gang-mounted tools and recommends clearance planning and reduced-feed air cuts.
All eight tool numbers and graphics match the demonstrated arrangement.
Tool 2 is established as the master tool and its reference values are recorded.
Tools 1, 4, 5, and 6 have their X and Z references.
Tools 3, 7, and 8 have their Z references and have been centered at X zero.
For tenon-based TOUCH X entries, use the actual measured diameter: positive for Tools 1, 4, and 5; negative for Tools 2 and 6. The centered drills, Tools 3, 7, and 8, use 0.
Feeler-gauge TOUCH Z entries match the actual positive gauge thickness; direct-face and visual-alignment entries are zero.
PathPilot is in metric mode for all offset-setting steps.
Clearances have been checked for the whole gang arrangement.
Verify each tool cautiously before cutting, using controlled movements and suitable test cuts and measurements. Program-specific Z-zero setup and program prove-out will be developed in later instruction.
Turret references for a future lesson
Retain these official references for the coauthor developing the turret setup lesson. That lesson will cover the actual turret fitted to the machine; its alignment procedure will be separate from this gang-tooling workflow.
Gen 2 Turret Installation Manual: X and Y alignment, shimming, radial alignment, tool mounting, projection, and crash avoidance.
Gen 1 Turret Installation Manual: alignment and height checks for the earlier turret, including a facing-test pip measurement. Use the manual matching the installed turret generation.
15L operation guide: tooling arrangements and front and rear tool-post positions.
Coauthor development note: Identify the turret generation and machine model, then document installation checks, alignment, tool assignment, offsets, indexing clearance, and prove-out with photographs of that setup.
Remaining lesson development
Demonstrate the program Z-zero function.
Add detailed center-height, drill-alignment, mounting, projection, and moving-clearance instructions.
Add touch-off photos for the skim-cut measurement, Sharpie contact, feeler gauge, threading-tip alignment, and drill centering.
Add contributor guidance for an alternative fixed Z reference.
This lesson builds on the gang tooling setup and offsets established in Lesson 1. Start by organizing your pen programs. Then locate the workpiece face with Tool 2, the OD turning tool and master tool, to establish floating Z zero. The Conversational program setup will follow.
1 - Organize the pen programs
Before creating programs, make a main folder named pens, with an internals subfolder for internal machining programs and an externals subfolder for external machining programs.
pens/
internals/
externals/
Create the main folder
Click the File tab (1).
In the controller file area on the left, navigate to the location where you want the main folder.
Click the NEW folder button (2), labeled NEW with a yellow folder icon.
The Name dialog opens. Click the Name field (3) and type pens.
Click OK (4) to create the folder.
Figure 1. Folder creation: 1 File tab → 2 NEW folder → 3 enter the name → 4 OK. The Name dialog is the popup opened by clicking NEW. The existing folder tree on the right shows an example arrangement.
Create the two subfolders
Open pens in the controller file area.
Click NEW (2), enter internals in the Name field (3), and click OK (4).
With pens as the current parent folder, repeat to create externals.
Confirm both folders are directly inside pens, alongside each other. Neither should be inside the other.
The screenshot shows an existing main folder named 1.pens. This example uses pens; use your chosen main-folder name consistently.
2 - Establish the floating Z zero
Load the workpiece. Secure it in the chuck with approximately 2 inches (50.8 mm) of stickout.
Select the master tool. On the Main tab, type T2 in the MDI line and press Enter to select Tool 2. Confirm the active tool display shows T: 02.
Locate the workpiece face. With the spindle stopped, carefully jog the cutting tip of the OD turning tool to the front face of the workpiece.
Set the job Z zero. Without changing that Z position, click Z ZERO, immediately to the left of the Z position readout on the Main tab. The work-coordinate Z readout should show zero; a display of -0.0000, as in the screenshot, is zero at the displayed precision.
Figure 2. Main tab after establishing floating Z zero with Tool 2. Numbered red boxes identify the controls and display described below. The loaded file, plotted dimensions, and other displayed values are captured screen content, not settings to copy.
Active-tool display: Immediately to the left of SET G30. It shows T: 02 when Tool 2 is selected.
MDI line: Below the G-code panel at the upper left. Type T2 here and press Enter to select Tool 2.
Z ZERO button: Immediately to the left of the Z position readout. Click it with Tool 2 at the workpiece face to establish the job Z zero.
Job zero and tool offsets: Use Z ZERO on the Main tab for this step, rather than TOUCH Z on the Offsets tab. You are locating the workpiece for this job using the already referenced master tool. The other tools use their established offsets to follow this Z reference.
This is the floating-zero approach: Z zero follows the face chosen for the current workpiece rather than a permanent position relative to the headstock.
G54 and floating zero: G54 locates the workpiece; tool offsets locate each tool. With G54 active, setting Z ZERO with Tool 2 makes the original face Z 0. After facing, the clean face is Z -1. Read Tormach guidance under Set Work Offsets.
3 - Begin the internals program in Conversational
On the File tab, navigate to your main pens folder.
Select and open the internals folder (1) in the controller file area on the left.
Click CONV EDIT (2), the Conversational Edit button at the top of the screen, to continue with the program-setup workflow demonstrated in this lesson.
Figure 3. 1 Select and open internals in the left controller file area, then 2 click CONV EDIT. The screenshot shows the folder selected within the main pens folder, before opening it.
4 - Insert the first program step
The Conversational job editor opens with the job-step list on the left and the tool-path display on the right. In this example, the job header shows Job: <None> and the step list is empty.
Click INSERT STEP (1) in the middle column to begin adding the first machining operation.
Figure 4. Click 1 INSERT STEP to begin defining an operation. The tool-path display is captured screen content, not a program or dimensions to copy.
5 - Body internals program overview
The job m13 bodyinternals contains the sequence shown below. It also includes external turning, chamfering, and cap-thread operations. Load the saved program and press CYCLE START once to run the operations in the order shown.
Figure 5. Complete operation list for the example body program. OD Turn 15.4mm is selected, so the Preview panel on the right describes that operation rather than the facing operation.
Order
Operation
1
facing
2
Drill converter hole (Tool 8, 8.2 mm)
3
id body 9.3 tenon relief
4
id body tenon relief
5
id thread m10x1
6
OD Turn 15.4mm
7
OD Turn 12.8mm tenon
8
chamfer tenon m13
9
OD Thread m13x2.4 pass 1
10
OD Thread m13x2.4 pass 2
11
OD Thread m13x2.4 pass 3
12
home
Names and settings: The list identifies the operations; the tenon-turning name is updated here to 12.8 mm. The overview screenshot retains its older 12.9mm title. The drilling screenshot retains its older 8mm title; Step 7 uses the 8.2 mm body drill in Tool 8. The three external-thread operations will be explained individually with their threading settings and start positions.
Keep the program Z convention throughout: face from Z 0 to Z -1, then reference subsequent machining depths and lengths from the clean face at Z -1.
6 - Set up the first operation facing
This example program machines the body internals for a pen with a 12.8 mm tenon prepared for nominal M13 cap threads, M13 × 0.8 triple-start cap threads, and M10 × 1 internal threads for the section. The cap-thread specification describes the mating design; this step is the facing operation.
Begin with a Face operation using Tool 2, the OD turning tool and master tool.
Figure 6. Facing operation in metric mode (G21), using Tool 2. Numbered red boxes match the quick-reference tables below. Dimensions and depths are in millimeters, surface speeds in meters per minute (MPM), and feeds in millimeters per revolution (mm/rev).
Explore the facing controls: Hover over a red number or highlighted field to open its value and explanation. Move into the popup to keep reading; move away to close it. Click or tap also works. Close with × or Escape.
View all facing settings as tables
Facing screen quick reference
The numbers match the controls in Figure 6.
All dimensions and depths below are in millimeters. MPM means meters per minute, mm/rev means millimeters per spindle revolution, and DOC means depth of cut.
Your OD turning tool and master tool, using its established offsets.
Cutting speeds and feeds
Field
This example
What it controls
4 · Roughing MPM
200 m/min
Target cutting surface speed for roughing.
5 · Finishing MPM
200 m/min
Target cutting surface speed for finishing.
6 · Max Spindle RPM
2000 rpm
Upper spindle-speed limit. As the tool moves toward center, constant surface speed increases RPM until this limit is reached.
7 · Roughing mm/rev
0.2000 mm/rev
Tool travel per spindle revolution during roughing.
8 · Finishing mm/rev
0.0800 mm/rev
Tool travel per spindle revolution during finishing.
Facing geometry and passes
Field
This example
What it controls
9 · Initial X
-20.5000
Starting stock diameter. The negative sign places Tool 2 on its negative-X working side.
10 · Final X
0.0000
Faces to spindle centerline. Tool clearance extends the tool path beyond this endpoint to clean up the center.
11 · Z Start
0.0000
The original stock face where you established floating Z zero.
12 · Z End
-1.0000
The clean finished face, 1 mm toward the headstock from the original face. Following steps reference this face at Z -1.
13 · Tool Clearance
1.0000
Clearance used by the routine for approach and retract moves and to extend the facing path past the final X endpoint.
14 · Roughing DOC
0.2000
Depth of each roughing pass in Z, with the finishing allowance retained.
15 · Finish DOC
0.0800
Axial material left for the single finishing pass at Z End.
Buttons and diagram
Control
Purpose
16 · Coolant faucet
Enables or disables coolant for the operation. The screenshot shows a green indicator.
17 · FINISH
Accepts the operation definition and returns to the job editor. It does not start machining.
18 · CANCEL
Leaves the operation editor without accepting the current changes.
Facing diagram
Shows the X and Z references, clearance, and roughing and finishing passes. The facing routine does not use tool-radius compensation.
Read this example as: Use Tool 2 to face a 20.5 mm diameter blank from Z 0 to Z -1, working from the negative-X side toward center. Keep Z zero at the original location; the next operation starts from the clean face at Z -1.
Reference: Tormach 15L PathPilot Tools and Features, under Create a Face on a Part and About Facing. The numbers shown are the settings for this example, rather than recommendations for every material.
Use the faced surface for all following Z dimensions
Every program in this workflow starts by facing from Z 0 to Z -1.000 mm to produce a clean reference face.
The clean face is now at Z -1.000 mm. Use Z -1.000 mm as the face reference for subsequent machining dimensions. Operations beginning at the face use Z Start -1; the phase-shifted cap-thread starts and final Tool 2 selection move intentionally use different Z Start values. Account for this 1 mm facing allowance in all following Z locations and overall axial dimensions.
For a feature extending a distance L into the part from the clean face, its endpoint is Z = -1.000 - L. For example, a hole 20 mm deep from the faced surface ends at Z -21.000 mm. Approach and retract positions still include the clearance required by the operation.
Program convention: Original stock face = Z 0. Clean faced surface = Z -1.000 mm. Subsequent feature dimensions are measured from Z -1.000 mm, while their program coordinates remain relative to the original Z zero. Cap-thread phasing and the final Tool 2 selection move have their own stated start positions.
7 - Drill the converter hole in the body
Use Tool 8, the 8.2 mm body drill, to drill the converter hole in the body, following the tooling arrangement in Lesson 1. We will focus on the drilling-specific controls rather than repeat the fields already explained for facing.
Figure 7. Converter-hole drilling setup illustration with Tool 8, the 8.2 mm body drill. Hover labels D1–D4 cover only the new drilling controls. The DRILL/TAP selector has been added to show the new-operation interface, with DRILL selected. The displayed title drill body 8mm is the operation name.
Tool assignment: Tool 8 is the 8.2 mm body drill; Tool 7 is the 9.2 mm cap drill. The Tool 8 selection shown is correct. The title drill body 8mm is an operation label; the actual body drill is 8.2 mm.
Choose drilling mode
Use the DRILL/TAP selector in the upper-right corner and confirm that DRILL has the green indicator for this operation.
Explore the new drilling controls: Hover over D1–D4 for explanations. Click or tap also works. Familiar fields are left unmarked.
View drilling-specific values as a table
Drilling-specific fields
Field
Displayed value
Meaning
D1 · DRILL/TAP
DRILL
Select drilling for the converter hole.
D2 · Peck Depth
5.0000 mm
Advance per peck, with retraction to help clear chips.
D3 · Spindle RPM
1200.0 rpm
Fixed spindle speed during drilling.
D4 · Dwell at Bottom
0.50 seconds
Pause at the final drilling depth before retracting.
Apply the established Z reference
Z Start = -1.0000 references the clean face left by the facing operation. Z End = -77.0000 places the drilling endpoint 76 mm into the part from that face. Tool Clearance is 3.0000 mm, and the active roughing feed shown is 0.1250 mm/rev. These are the displayed values for this converter-hole example.
8 - Bore the relief for the section threads
Use Tool 4, the ID boring tool, to enlarge the drilled 8.2 mm bore to 9.3 mm for 6.55 mm from the clean face. This first ID-turning operation creates the relief that accommodates the threaded portion of the section. It prepares the bore for the later internal-threading operation; it does not cut the threads.
Figure 8. Tool 4 bores the relief for the threaded portion of the section, with BASIC selected on the BASIC/EXTENDED selector. Both X entries are negative because this operation cuts on the negative-X side; Tool 4 was touched off using a positive X reference in Lesson 1.
Hover over I1–I4 to explore the new ID-turning settings. Click or tap also works.
View ID relief settings and explanations
Field
Displayed value
I1 · BASIC/EXTENDED
BASIC
Tool
4
I2 · Initial X
-8.2000 mm
I3 · Final X
-9.3000 mm
Z Start
-1.0000 mm
Z End
-7.5500 mm
Tool Clearance
1.0000 mm
I4 · ID Rough DOC
0.3800 mm
Finish DOC
0.1900 mm
Roughing / Finishing MPM
55 / 50 m/min
Max Spindle RPM
1000 rpm
Roughing / Finishing feed
0.2500 / 0.0700 mm/rev
Hover over I1–I4 for the new ID-turning settings. Click or tap also works. Familiar controls are left unmarked.
I1 · BASIC/EXTENDED
This example: BASIC.
Selects the basic or extended ID-turning interface. Use BASIC for the operation shown. Extended-mode settings will be covered if used in a later example.
I2 · Initial X for ID turning
This example: -8.2000 mm.
The starting bore diameter for the operation. The negative sign identifies the working side; it does not mean a negative physical hole size. Tool 4 uses a positive touch-off reference but cuts here on the negative-X side.
I3 · Final X for ID turning
This example: -9.3000 mm.
The target internal diameter is 9.3 mm. Increasing the bore diameter makes this negative-X coordinate more negative, from -8.2 to -9.3.
I4 · ID Rough DOC
This example: 0.3800 mm.
Controls the roughing depth for the ID-turning passes. This is a positive cutting-depth entry, distinct from the signed X diameters. Use the displayed value for this example; it is separate from the signed bore diameters.
The relief runs from Z -1 to Z -7.55, a length of 6.55 mm from the faced surface. Initial X is -8.2 and Final X is -9.3; both are signed diameter values.
9 - Bore the secondary relief for section seating
Continue with Tool 4 using the same ID-turning controls explained in Section 8. This secondary relief enlarges the entrance from 9.3 mm to 10.1 mm for 2 mm from the clean face, providing clearance so the section seats fully without obstruction.
Figure 9. Secondary relief provides clearance for full section seating. The field meanings are the same as in Section 8; the changed X diameters and Z endpoint define this shorter, wider relief.View the changed dimensions for the second relief
Field
Value
Initial X
-9.3000 mm
Final X
-10.1000 mm
Z Start
-1.0000 mm
Z End
-3.0000 mm
Tool 4, speeds, feeds, depths of cut, and clearance remain as shown in Section 8.
10 - Cut the M10 x 1 internal section threads
Use Tool 5, the ID threading tool, to cut the threads that accept the section. Select INTERNAL and RH.
Figure 10. M10 x 1 internal threading illustration with INTERNAL and RH selected. Use the entered operation fields; the unrelated thread-preset dropdown is not part of this example.
Hover over T1–T11 for the new threading controls and displays. T7 and T8 are system-calculated values, not manual entries. Click or tap also works. Familiar settings are left unmarked.
View new threading settings and explanations
Control
Example
Meaning
T1 · External / Internal
INTERNAL
Chooses inside or outside threading. Select INTERNAL for the section threads inside the body.
T2 · RH / LH
RH
Chooses thread hand. RH makes the right-hand thread used here.
T3 · Taper
0.0000 mm
Sets thread taper. Zero produces a straight thread.
T4 · Lead Length
3.0 mm
Provides travel for spindle-synchronized Z motion to stabilize before cutting. This is not thread pitch or finished thread length.
T5 · X Start for threading
-9.3000 mm
The starting bore diameter for internal threading. Tool 5 works on the negative-X side, although its touch-off reference in Lesson 1 is positive.
T6 · X End for threading
-9.9500 mm
The final cutting diameter for this internal thread. This is the instructor example diameter, not a universal value for every M10 thread.
T7 · Threading Depth of Cut — calculated
0.2910 mm (calculated)
System-calculated threading infeed value; not a user-entered setting. Later cut depths decrease through constant-area degression.
T8 · Threads per mm — calculated
1.00 (calculated)
System-calculated from pitch; not a user-entered setting. A 1 mm pitch gives one thread per millimeter.
T9 · Pitch
1.0000 mm
Axial spacing between thread crests. This M10 x 1 section thread uses 1 mm pitch; it is separate from the triple-start cap thread.
T10 · Passes
5
Number of cutting passes used to reach the thread depth.
T11 · Spring Passes
2
Extra passes at full thread depth to clean up the thread and account for deflection.
Established settings: Tool 5; Z Start -1.0000; Z End -7.0000; Tool Clearance 1.0 mm; fixed spindle speed 500 rpm. The programmed Z span is 6 mm from the faced surface. Thread lead-in travel is additional to that span.
Use Tool 2, the OD turning tool, to reduce the top portion of the body close to its final outside diameter. This preparation helps prevent chip-out during later OD turning and profiling of the body.
Figure 11. Preliminary OD turning of the top portion of the body. Hover over O1–O3 for the OD-specific geometry and fillet setting.
Hover over O1–O3 for new explanations. Click or tap also works. Familiar speed, feed, Z, and clearance fields are left unmarked.
View new OD-turning settings and explanations
Control
Example
Meaning
O1 · Initial X for OD turning
-20.5000 mm
Starting outside diameter: 20.5 mm. Tool 2 cuts on the negative-X side. Unlike boring, this operation removes material from the outside.
O2 · Final X for OD turning
-15.4000 mm
Target outside diameter: 15.4 mm. Reducing the outside diameter moves the signed value toward zero, from -20.5 to -15.4.
O3 · Fillet Radius
0.0000 mm
Specifies a rounded transition at the shoulder. Zero requests no added fillet; the physical tool nose still has its own radius.
Z extent: Start at the clean face, Z -1.0000, and end at Z -12.5000. This turns 11.5 mm of body length from the faced surface.
View the familiar settings used in this example
Field
Value
Tool
2
Roughing / Finishing MPM
200 / 200 m/min
Max Spindle RPM
2500 rpm
Roughing / Finishing feed
0.2000 / 0.0800 mm/rev
Tool Clearance
1.0000 mm
Roughing DOC / Finish DOC
0.2000 / 0.0500 mm
12 - Turn the 12.8 mm tenon for the M13 cap threads
Use Tool 2 to turn the external tenon to 12.8 mm diameter before cutting the M13 cap threads. This follows the preliminary 15.4 mm OD turning operation. The controls are the same as in Step 11, so no new hover explanations are needed.
Figure 12. OD turning prepares a 12.8 mm tenon for subsequent external threading. The screenshot retains the old 12.9mm title; Final X -12.8000 is the correct setting. This operation does not cut the threads.
The tenon extends from Z -1.0000 to Z -7.5000, giving a 6.5 mm length measured from the clean faced surface. Tool 2 works on the negative-X side, so both diameter entries are negative.
View the tenon-turning settings
Field
Displayed value
Tool
2
Initial X
-15.4000 mm
Final X
-12.8000 mm
Z Start / Z End
-1.0000 / -7.5000 mm
Fillet Radius
0.0000 mm
Roughing / Finishing MPM
200 / 200 m/min
Max Spindle RPM
2500 rpm
Roughing / Finishing feed
0.1500 / 0.0600 mm/rev
Tool Clearance
1.0000 mm
Roughing DOC / Finish DOC
0.2000 / 0.0500 mm
Refer to Step 11 for the OD-turning field explanations.
13 - Chamfer the M13 tenon
Select CHAMFER and OD. Use Tool 2 to chamfer the front edge of the 12.8 mm tenon before cutting the cap threads. The chamfer provides a lead-in for smooth cap engagement and helps reduce the chance of cross-threading.
Figure 13. Chamfer the cap-thread tenon with Tool 2. Hover over C1–C7 for the chamfer-specific controls and behavior.
Hover over C1–C7 for the new chamfer details. Click or tap also works. Familiar fields are left unmarked.
View new chamfer settings and explanations
Control
Example
Meaning
C1 · Chamfer Angle
45 degrees
Sets the angle of the bevel at the end of the tenon. This example uses a 45-degree chamfer.
C2 · Chamfer X reference
-12.8000 mm
The outside diameter at the original tenon corner. Tool 2 works on the negative-X side, so the 12.8 mm diameter is entered as -12.8.
C3 · Chamfer Z extent
Z Start -1.0000; Z End -1.4500 mm
The bevel runs 0.45 mm back from the faced surface at Z -1. At 45 degrees this gives a 0.45 mm radial change across the bevel, corresponding to 0.90 mm in diameter.
C4 · Chamfer depth of cut
Roughing 0.1500; Finish 0.0500 mm
For chamfering, roughing depth is applied perpendicular to the chamfer, rather than as a facing depth in Z. The finishing pass removes the reserved allowance.
C5 · Tool radius compensation
Used
Unlike the earlier facing and basic turning screens, this routine uses tool-radius compensation. The tool nose radius must be correctly defined for Tool 2.
C6 · CHAMFER/RADIUS
CHAMFER
Choose a straight bevel rather than a rounded radius.
C7 · OD/ID
OD
Chamfer the outside edge of the tenon.
This chamfer starts at the clean face at Z -1 and extends to Z -1.45.
Before programming the three Tool 6 threading operations, distinguish pitch, lead, and starts. These are separate quantities, even when a control uses the word pitch for its distance-per-revolution entry.
Pitch: Axial spacing between adjacent thread crests.
Lead: Axial travel in one full revolution of the cap, following one continuous thread helix.
Starts: The number of separate, interleaved helices. Each start is its own groove.
Lead = pitch × number of starts.
Example with 0.8 mm pitch
Starts
Lead per revolution
Angular spacing
Single start
1
0.8 mm
360°
Triple start
3
2.4 mm
120°
Quad start
4
3.2 mm
90°
For this course, M13 × 0.8 triple start means nominal 13 mm threads with 0.8 mm pitch and 2.4 mm lead. Each individual groove advances 2.4 mm per revolution. A quad-start version with the same 0.8 mm pitch would advance 3.2 mm per revolution. More starts give more axial travel per turn; matching cap and body threads must share the pitch, lead, start count, hand, and compatible dimensions.
Three operations make three starts
The instructor uses three separate Conversational threading operations with Tool 6: one for each start. Each operation makes multiple cutting passes to form its groove. The Passes field and spring passes do not create additional starts.
All three operations use the same lead and thread dimensions, but must be phased differently so their grooves interleave. Three copies with identical phase would recut the same groove. Conceptually, the triple-start grooves are separated by 120°, equivalent to an axial phase spacing of 0.8 mm within a 2.4 mm lead. For four starts, the spacing is 90°, equivalent to 0.8 mm within a 3.2 mm lead.
How the PathPilot pitch field relates to lead
Tormach defines the G76 threading-cycle P value as distance per spindle revolution. For a multi-start thread, that motion must follow the lead of one helix: 2.4 mm/rev in this triple-start example. The earlier job titles OD Thread m13x2.4 pass 1, 2, and 3 are consistent with that lead; they are three start operations, not three ordinary depth passes.
Keep these three ideas separate: Finished thread pitch = 0.8 mm. Lead of each groove = 2.4 mm/rev. Lead Length in the UI is the approach distance for synchronization; it is not the thread lead. The worked example below shows the supplied Z Start phase changes for all three operations.
Do not use the larger lead as a reason to cut a deeper thread profile. Thread form, diameters, insert geometry, and clearance must suit the intended 0.8 mm-pitch multi-start thread. The worked example uses the supplied Tool 6 screens; thread-fit adjustments will be explained with the individual operations.
The three supplied screens use the same 2.4000 mm UI Pitch, 7.2 mm Lead Length, and Z End -5.5000. Only Z Start changes among these four fields.
Start operation
Z Start
Z End
UI Pitch
Lead Length
1
-1.0000
-5.5000
2.4000 mm/rev
7.2 mm
2
-0.2000
-5.5000
2.4000 mm/rev
7.2 mm
3
+0.6000
-5.5000
2.4000 mm/rev
7.2 mm
The Z Start difference is +0.8 mm each time: -1.0 → -0.2 → +0.6. Relative to a 2.4 mm lead, that is 0.8 ÷ 2.4 × 360° = 120° between starts. The three grooves interleave at the required 0.8 mm finished pitch.
Figure 14. Schematic of the three-start example, not to scale. Colored lines identify the separate starts. The shaded interval is the nominal axial thread region; the front chamfer changes where the full thread profile begins.
Why the later starts are in front of the workpiece
The clean faced surface stays at Z -1. Start 2 at Z -0.2 is 0.8 mm in front of the face; Start 3 at Z +0.6 is 1.6 mm in front of the face. Those extra portions are in air. They shift the helix phase rather than extend the physical tenon. All three operations finish at Z -5.5, preserving a common thread endpoint.
The nominal axial region from the faced surface at Z -1 to Z -5.5 is 4.5 mm. The previously cut tenon reaches Z -7.5, so these coordinates leave 2 mm between the programmed thread endpoint and the tenon shoulder.
What the 7.2 mm Lead Length means
7.2 = 3 × 2.4 mm. Here, the synchronization approach allows the equivalent of three revolutions at the programmed helix lead. It stays the same for all three operations. It is neither the finished thread pitch of 0.8 mm nor the lead of 2.4 mm per revolution. In this example, the phase change comes from Z Start, not from changing Lead Length.
At the displayed 500 rpm, the synchronized threading travel is 500 × 2.4 = 1200 mm/min. This illustrates why thread lead, spindle speed, and approach clearance must be considered together.
View M13 x 0.8 quad-start example and illustration
Quad-start comparison
For a hypothetical four-start version at the same 0.8 mm finished pitch, each helix would use a 3.2 mm lead. Four phase positions spaced by 0.8 mm correspond to 90° each. Starting from the same Z -1 datum, the conceptual sequence is -1.0, -0.2, +0.6, +1.4. This is a comparison, not a tested quad-start program; its approach distance, tool geometry, speeds, and clearance would need their own setup.
M13 x 0.8 quad-start calculation
Quantity
Calculation
Example value
Finished thread pitch
Specified by M13 x 0.8
0.8 mm
Starts
Quad start
4
Thread lead / UI Pitch
0.8 × 4
3.2 mm/rev
Lead Length using the three-revolution convention
3 × 3.2
9.6 mm
Axial phase increment
3.2 ÷ 4
0.8 mm
Angular phase increment
360° ÷ 4
90°
For this quad-start example, each of the four operations would use UI Pitch = 3.2000 and, following the same approach convention as the triple-start example, Lead Length = 9.6 mm. The finished thread pitch remains 0.8 mm.
9.6 mm is a chosen synchronization approach length, not a dimension fixed by the thread specification. It follows the three-revolution convention used in the supplied triple-start setup. Confirm acceleration and clearance for the actual machine and speed. At 500 rpm, the quad-start threading travel would be 500 × 3.2 = 1600 mm/min, compared with 1200 mm/min for the triple start.
Figure 15. Quad-start comparison using four Z start positions at 0.8 mm spacing, equivalent to 90-degree phasing. UI Pitch is 3.2 mm/rev; the example 9.6 mm Lead Length follows the three-revolution approach convention. The common Z End of -5.5 is retained for comparison. Conceptual illustration, not a tested machining program.
Starts versus passes: Each supplied screen shows 5 cutting passes and 2 spring passes for its own helix. Three separate operations create the three starts. The operation names containing pass 1, pass 2, and pass 3 refer to the three starts in this job.
15 - Cut cap-thread start 1
Use Tool 6, EXTERNAL, and RH. Set the first Z Start to -1.0000, at the clean faced surface.
Figure 16. Cap-thread start 1. EXTERNAL/RH selectors are included in this setup illustration. The unrelated preset dropdown is not used for this example.
Hover over S1 for this start phase and S4–S7 for the shared mode, pitch, and approach settings. Click or tap also works.
View start 1 settings
Setting
Value
S1 · Z Start
-1.0000 mm
Z shift relative to start 1
0 mm
Phase relative to start 1
0 degrees
Z End
-5.5000 mm
S6 · UI Pitch / S7 · Lead Length
2.4000 mm/rev / 7.2 mm
Tool
6
S4 · EXTERNAL / INTERNAL
EXTERNAL
S5 · RH / LH
RH
X Start / X End
-12.8000 / -11.8500 mm
Spindle RPM
500 rpm
Tool Clearance / Taper
1.0 / 0.0000 mm
Cutting passes / Spring passes
5 / 2 per start operation
Calculated Depth of Cut / Threads per mm display
0.4250 mm / 0.42 (rounded); system-calculated, not manual entries
These are the shared settings for all three starts. The X values are signed diameters; use the instructor example fit values rather than the unrelated preset.
16 - Cut cap-thread start 2
Use Tool 6, EXTERNAL, and RH. Keep the first operation settings and change Z Start to -0.2000, a +0.8 mm shift.
Figure 17. Cap-thread start 2. EXTERNAL/RH selectors are included in this setup illustration. The unrelated preset dropdown is not used for this example.
Hover over S2 for this start phase. Shared controls are explained in Step 15. Click or tap also works.
View start 2 settings and what changes
Setting
Value
S2 · Z Start
-0.2000 mm
Z shift relative to start 1
+0.8 mm
Phase relative to start 1
120 degrees
Z End
-5.5000 mm
UI Pitch / Lead Length
2.4000 mm/rev / 7.2 mm
All other settings remain as in Step 15. Only Z Start changes between these operations.
17 - Cut cap-thread start 3
Use Tool 6, EXTERNAL, and RH. Keep the shared settings and change Z Start to +0.6000, another +0.8 mm shift.
Figure 18. Cap-thread start 3. EXTERNAL/RH selectors are included in this setup illustration. The unrelated preset dropdown is not used for this example.
Hover over S3 for this start phase. Shared controls are explained in Step 15. Click or tap also works.
View start 3 settings and what changes
Setting
Value
S3 · Z Start
+0.6000 mm
Z shift relative to start 1
+1.6 mm
Phase relative to start 1
240 degrees
Z End
-5.5000 mm
UI Pitch / Lead Length
2.4000 mm/rev / 7.2 mm
All other settings remain as in Step 15. Only Z Start changes between these operations.
After all three starts: The combined thread has 0.8 mm finished pitch and 2.4 mm lead. Each start received its own 5 cutting passes and 2 spring passes.
18 - Finish with Tool 2 selected
The final operation, named home, is the instructor workaround for selecting Tool 2 at the end of the job. The Conversational workflow used here has no dedicated step for simply reselecting the master tool, so this uses an OD Turn operation positioned away from the stock.
Leaving Tool 2 active saves entering T2 in MDI each time you need to establish its floating Z zero between jobs. You still locate the next workpiece face and click Z ZERO yourself.
Figure 19. Final Tool 2 selection operation, with Z Start +111.0000 mm and Z End +110.0000 mm.
Hover over H1–H3 for the purpose and current values. Click or tap also works.
View final Tool 2 operation settings and purpose
Field
Use
Title / Operation
home / OD Turn
H1 · Tool
2
H2 · Z Start
+111.0000 mm
H3 · Z End
+110.0000 mm
Initial X / Final X shown
-20.5000 / -20.4000 mm
Tool Clearance shown
1.0000 mm
Coolant shown
Off
The Z entries match the updated illustration. Other visible fields are part of the OD Turn routine, not a dedicated tool-selection command.
What home means here: This is an operation name, not machine referencing, a G30 command, or RESET TOOL. It runs a motion-generating OD Turn routine and selects Tool 2.
Check the generated approach, cutting, retract, and tool-change moves against actual travel and clearance for the whole gang plate. Positive Z positions are relative to the current floating zero; +111 and +110 are instructor setup values, not universally clear machine positions.
19 - Save, load, and run the complete job
Save the program in internals
In the Conversational job editor, confirm the 12 operations are in the order shown in Step 5, from facing through home.
Click SAVE AS. In the save dialog, open the controller folder pens → internals. If you named your main folder 1.pens, open that folder first.
Name the file m13 bodyinternals.nc and save it. Use the job editor’s SAVE AS button to save the complete operation list in one file.
Load the saved program
Close the job editor and open the File tab.
In the controller file area, open pens → internals and select m13 bodyinternals.nc.
Click LOAD. On the Main tab, confirm the filename and check the tool-path preview.
Run the whole job
Confirm the workpiece is secure, its Z zero is set as in Step 2, and the programmed moves have clearance, including the final home move. Verify clearance before the first cut on a new setup.
With the program ready to run from its beginning and the enclosure closed, press CYCLE START once on the Main tab. PathPilot runs the saved operations in order, from facing through the three cap-thread starts and the final Tool 2 selection.
When the program completes, T: 02 shows that the master tool is selected for the next workpiece.
