🚧 Under construction — VoTechWorks is being built. A free tech program — complimentary, as our commitment to get America working.
voTechWorksGrade 13 · a vocational technology learning center, by urbanicity
newSchoolWorks.com › VoTechWorks › Manufacturing & Marine › CNC Machining › G-Code Programming for CNC Mills and Lathes › Lesson 12
MFG-CNC14-04 · Lesson 12 · 20 clock hours · lab

Integrated G-Code Programming Project: Mill and Lathe Combination Part

Objective. Students independently write, simulate, prove out, and run complete G-code programs for both a milled feature and a turned feature on a single combination part, producing dimensions within blueprint tolerance.

⚠ Pending professional review

This lesson, its worked examples and its practice questions has not yet been verified by a licensed engineer or certified journey-level tradesperson or by a certification or approval body. It is a study draft and may contain errors. Do not use it as instructions for work on a job site or on live equipment. Always follow your instructor, your supervising professional, and current official references and regulations.

VoTechWorks program approval and accreditation are still in progress. Credentials are issued only by the certifying bodies named in each program, after their own exams.

Integrated G-Code Programming Project: Mill and Lathe Combination Part

This lab is the capstone of your G-code programming course. You will plan, write, simulate, prove out, and run complete programs for both a milled feature and a turned feature on a single combination part. Every earlier skill—coordinate math, canned cycles, tool offsets, feeds and speeds, and safe machine operation—must work together here.

Why a Combination Part?

Real manufacturing rarely involves only a mill or only a lathe. A shaft with a milled keyway, a flanged part with turned OD and drilled bolt holes, or a marine drive component with threaded ends and broached features all require both machine types. Employers expect a machinist to move a part between machines, maintain a common datum, and hold blueprint tolerances across every operation. This project simulates that workflow.

Phase 1: Planning Packet

Before you open a simulator or step onto the shop floor, you must complete a planning packet and receive instructor approval. This is not optional—machining without an approved plan is a safety and quality failure.

Your planning packet must include:

Phase 2: Simulation in CNCSimulator Pro

Once your packet is approved, load both programs into CNCSimulator Pro. Watch the full toolpath. Confirm:

Fix any errors in the program file, not by hand-editing at the control. Document every change on your planning packet.

Phase 3: Prove-Out Checklist on the Haas VF-2 and ST-10

Lockout/Tagout (LOTO) is required before loading or removing workholding, inserting tools, or touching any mechanism with power available. Follow your shop's written LOTO procedure. Your signed LOTO checklist must be on file with the instructor before the machine is powered for your setup.

PPE for this lab: safety glasses (ANSI Z87.1) at all times in the shop; hearing protection when the machine is running; no loose clothing, gloves near rotating spindles, or open-toed shoes.

Prove-out steps (complete every step in order; skipping one step requires a full restart):

1. Set work offsets (G54 on the mill; work shift or G54 on the lathe). Verify with a dial indicator.

2. Set tool-length offsets on the mill; set tool-nose radius compensation and X/Z geometry offsets on the lathe.

3. Load and run the program in single-block mode with the feed-rate override at 5–10 % for the first few moves.

4. Execute a supervised air-cut with the spindle on and the Z axis raised 2–3 inches above the part. Confirm X-Y (mill) or X-Z (lathe) motion matches the blueprint profile.

5. Lower to cutting depth only after the instructor observes and clears the air-cut.

6. Run the first cut, measure critical features with calipers and micrometer, adjust offsets as needed, then run finish passes.

Phase 4: Inspection and Root-Cause Analysis

After machining, measure every dimension called out on the blueprint. Record nominal, tolerance, and actual on the inspection report form. If any dimension is out of tolerance, you must:

1. Identify the specific feature and the magnitude of the error.

2. State whether the likely cause is a program coordinate error, a work-offset error, a tool-offset error, or a cutting-condition issue.

3. Propose a specific G-code or offset edit that would correct it.

The inspection report is part of your grade. A part that fails a dimension but has a complete, correct root-cause analysis demonstrates professional-level process thinking.

Grading Threshold

At least 80 % of blueprint dimensions must be within stated tolerance on the first article. Your planning packet must be approved before any machining begins, your LOTO checklist must be signed by the instructor, and the full prove-out sequence must be completed without skipped steps. The inspection report must be submitted and reviewed before the grade is recorded.

Key Safety Reminders

Key terms10

Combination partA workpiece that requires both milling and turning operations to complete all features called out on the blueprint, typically referencing a common datum across both machine setups.
Planning packetA pre-machining document that records the operation sequence, calculated coordinates, speeds and feeds, canned-cycle parameters, and the full G-code listing for instructor review and approval before simulation or machining begins.
Air-cut (dry run)A supervised prove-out step in which the program runs at full speed with the tool path offset well above the workpiece so motion can be verified without cutting material.
Work offset (G54–G59)A stored coordinate value that tells the CNC control where the workpiece origin is located relative to the machine home position; must be set and verified before any cutting pass.
Canned cycleA pre-programmed machine routine (such as G81 for drilling or G71 for rough turning) that performs a repetitive operation with a single block of G-code by specifying key parameters like depth, retract height, and feed.
Tool-nose radius compensation (TNRC)A lathe control feature (G41/G42) that automatically offsets the programmed path to account for the physical radius of a turning insert tip, ensuring accurate part geometry on angled and curved surfaces.
Single-block modeA machine control setting that causes the program to execute only one block at a time, requiring the operator to press Cycle Start for each block; used during prove-out to catch errors before they cause a crash.
First article inspectionThe systematic measurement of every blueprint dimension on the first completed part from a new setup, used to verify that the program, offsets, and tooling produce parts within tolerance before running additional pieces.
Root-cause analysisA structured process of identifying the specific program, offset, or process error that caused an out-of-tolerance dimension, followed by proposing a corrective edit or adjustment.
Feed-rate overrideA manual control knob or percentage setting on the CNC control panel that scales the programmed feed rate up or down during a run, used at reduced percentages during initial prove-out for added safety.

Worked examples4

1. Calculate the spindle RPM for a 1/2-inch (0.500 in.) diameter two-flute end mill cutting 6061 aluminum at a recommended cutting speed of 600 SFM.
  1. Identify the formula: RPM = (CS × 3.82) ÷ D, where CS = cutting speed in SFM and D = cutter diameter in inches.
  2. Substitute values: RPM = (600 × 3.82) ÷ 0.500.
  3. Multiply numerator: 600 × 3.82 = 2292.
  4. Divide: 2292 ÷ 0.500 = 4584.
  5. Round to the nearest practical value: set the spindle to 4584 RPM (or the nearest setting the control accepts).
Answer: Spindle RPM ≈ 4584 RPM
2. Calculate the table feed rate (IPM) for that same end mill if the chip load per tooth is 0.003 inch per tooth.
  1. Identify the formula: Feed Rate (IPM) = RPM × number of flutes × chip load per tooth.
  2. Substitute values: Feed Rate = 4584 × 2 × 0.003.
  3. Multiply: 4584 × 2 = 9168; then 9168 × 0.003 = 27.504.
  4. Round to a practical value: program F27.5 (or F28).
Answer: Feed rate ≈ 27.5 IPM
3. A lathe program uses G83 (peck drilling) to drill a 0.250-inch diameter through-hole in 1018 steel. The part face is at Z0.0, the hole is 1.500 inches deep, the retract plane is at R0.100, and the peck increment is 0.150 inches. Write the G83 block.
  1. Identify required addresses: Z (full depth), R (retract plane), Q (peck increment in most Haas controls, expressed as a positive value in inches), and F (feed rate).
  2. Calculate RPM first (separate calculation): at 80 SFM for 1018 steel and 0.250 in. drill: RPM = (80 × 3.82) ÷ 0.250 = 305.6 ÷ 0.250 = 1222 RPM. Set S1222.
  3. Full Z depth is 1.500 below face, so Z = -1.500. Retract plane R = 0.100. Peck Q = 0.1500 (Haas uses decimal inches for Q in some controls; verify the specific control's format—some use Q150 meaning 0.150 in.).
  4. Assume a feed rate of 0.004 IPR × 1222 RPM ≈ 4.9 IPM, program F4.9.
  5. Write the block: G83 Z-1.500 R0.100 Q0.1500 F4.9 (preceded by a line positioning X and Y over the hole center and a G00 move to R plane).
Answer: G83 Z-1.500 R0.100 Q0.1500 F4.9 (with S1222 set on a preceding line)
4. After machining, a turned OD measures 1.253 inches. The blueprint calls for 1.250 ± 0.002 inches. Determine if the part is in tolerance, and calculate the offset correction needed if it is not.
  1. Determine the tolerance band: nominal 1.250 in., lower limit = 1.250 − 0.002 = 1.248 in., upper limit = 1.250 + 0.002 = 1.252 in.
  2. Compare the actual measurement: 1.253 in. is above the upper limit of 1.252 in. The part is OUT of tolerance (0.001 in. oversize).
  3. On a lathe, an oversize OD means the tool did not cut deep enough in the X axis. The diameter is 0.003 in. too large (1.253 − 1.250 = 0.003 in.).
  4. Because diameter is affected, the X offset must move the tool 0.003 in. deeper into the part. On a Haas lathe using geometry or wear offset, subtract 0.003 from the current X wear offset value (enter −0.003 in the wear column for that tool).
  5. Verify: re-run the finish pass with the corrected offset and re-measure before accepting the part.
Answer: Part is out of tolerance (oversize by 0.001 in.). Apply −0.003 in. to the X wear offset for that turning tool and re-run the finish pass.

The math in this lesson2

Learners compare a 1.253-inch OD to 1.250 ± 0.002 and compute the wear offset.
N-Q.3A-CED.4
Brush up in the math halls at newSchoolWorks.com:
In class: From a multi-view blueprint with both mill and lathe operations, students plan the operation sequence, calculate all coordinates, speeds, feeds, and canned-cycle parameters, then write the full G-code programs before touching any machine or simulator—planning packet submitted for pre-approval. · After instructor approval of the planning packet, students simulate both programs in CNCSimulator Pro, run through the full prove-out checklist on the Haas VF-2 mill and Haas ST-10 lathe, execute supervised air-cuts, then machine the actual aluminum or low-carbon steel part. · Inspect the finished part using calipers and a micrometer; record each measured dimension against the nominal and tolerance on an inspection report; identify any out-of-tolerance feature, diagnose the likely G-code or offset cause, and propose a corrective program edit.
Materials: Haas VF-2 CNC mill; Haas ST-10 CNC lathe; CNCSimulator Pro; aluminum 6061 or 1018 steel stock; combination-part blueprint; LOTO kit; cutting tools (end mill set, drill set, boring bar, turning insert, threading insert); 0–1 in. micrometer; 6 in. digital caliper; inspection report form
Check: ≥80% of blueprint dimensions within stated tolerance on first article; planning packet approved before machining; LOTO checklist signed by instructor; prove-out sequence completed without skipped steps—any step skipped requires full restart. Inspection report submitted and reviewed.

Practice check8

Answer each question, then check it. Nothing is recorded; this is your own practice.

CNC Setup and Operation
1. Before beginning to machine a combination part on the Haas VF-2, which action is required first according to the prove-out checklist?
Workplace Safety
2. A machinist is setting up a new job and must change the workholding on the Haas ST-10 lathe. Which safety procedure is mandatory before reaching into the machine work zone?
Process Planning and Calculation
3. Using the formula RPM = (CS × 3.82) ÷ D, what spindle speed should be programmed for a 0.750-inch end mill cutting 6061 aluminum at 500 SFM? (Round to the nearest whole number.)
G-Code Programming
4. During simulation in CNCSimulator Pro, a student notices a G00 rapid move that descends directly to Z-0.500 while cutter compensation G41 is still active. What is the most likely consequence if this error is not corrected before machining?
CNC Setup and Operation
5. A turned diameter measures 0.006 inch undersize after the finish pass. The machinist wants to correct this on the next part. Which action is most appropriate?
G-Code Programming
6. Which G-code block correctly programs a G83 peck-drilling canned cycle to a depth of 2.000 inches below the part face, with a retract plane at R0.100 and a peck increment of 0.200 inches?
Metrology and Inspection
7. A blueprint dimension reads 2.375 ± 0.005 inches. After inspection, the measured value is 2.369 inches. What is the correct determination?
Process Planning and CNC Setup
8. When transitioning a combination part from the CNC mill to the CNC lathe, why is it critical to re-establish the datum reference before running the lathe program?
Record this lesson on my transcript. Sign in with your key and enrollment email to record lessons (enroll free if you have no key). This page stays open to read and practise.
← Previous lessonProgram plan