MACHINING CENTERMachining Center

▦Types of Machining Centers

✓Exercises (Pass When the Part Is Cut on Size)

Your part is graded automatically against the drawing shape on stock left, gouges, and hole depth. If you get stuck, see the “sample answer”.

O0001
G21 G90 G17 G40 G49 G80
G54
T1 M06
S3000 M03
G00 X0. Y-5.
G43 H1 Z30.
M08
Z2.
G01 Z-5. F300
G41 D1 X10. Y0. F600
Y50.
X70.
Y10.
X5.
G40 X0. Y-5.
G00 Z30.
M09
M30

O0002
G21 G90 G17 G40 G49 G80
G54
T1 M06
S3000 M03
G00 X0. Y-5.
G43 H1 Z30.
M08
Z2.
G01 Z-4. F300
G41 D1 X10. Y0. F600
Y42.
G02 X18. Y50. R8.
G01 X62.
G02 X70. Y42. R8.
G01 Y18.
G02 X62. Y10. R8.
G01 X18.
G02 X10. Y18. R8.
G01 Y20.
G40 X0. Y25.
G00 Z30.
M09
M30

O0003
G21 G90 G17 G40 G49 G80
G54
T5 M06
S5000 M03
G00 X42. Y30.
G43 H5 Z30.
M08
Z1.
#1=0
WHILE [#1 GT -6] DO1
#1=#1-1.5
G03 X42. Y30. Z#1 I-2. J0. F300
END1
G03 X42. Y30. I-2. J0.
G01 X23. Y21. F500
X57.
Y25.
X23.
Y29.
X57.
Y33.
X23.
Y37.
X57.
Y39.
X23.
Y21.
X57.
Y39.
X23.
Y21.
G00 Z30.
M09
M30

O0004
G21 G90 G17 G40 G49 G80
G54
T2 M06
S2000 M03
G00 X15. Y15.
G43 H2 Z30.
M08
G99 G81 X15. Y15. Z-2. R2. F150
X65.
Y45.
G98 X15.
G80
T3 M06
S1800 M03
G00 X15. Y15.
G43 H3 Z30.
G99 G83 X15. Y15. Z-18. R2. Q3. F180
X65.
Y45.
G98 X15.
G80
T4 M06
S400 M03
G00 X15. Y15.
G43 H4 Z30.
G99 G84 X15. Y15. Z-14. R5. F500
X65.
Y45.
G98 X15.
G80
M09
M30

O0005
G21 G90 G17 G40 G49 G80
G54
T3 M06
S1800 M03
G00 X10. Y30.
G43 H3 Z30.
M08
#1=10
WHILE [#1 LE 70] DO1
G99 G81 X#1 Y30. Z-10. R2. F180
#1=#1+10
END1
G80
G00 Z30.
M09
M30

≡How to Read Specs

⌖Coordinate Systems and Tool Offsets

• X, Y, and Z form a right-handed Cartesian coordinate system. On a typical vertical machine, left-right is X, front-back is Y, and up-down is Z^{[1][14][15][16]}
• Z is the axis parallel to the spindle. Positive is toward the spindle (the direction in which the tool moves away from the workpiece)One source / reference^[16]
• Machine coordinate system: coordinates fixed to the machine. Machine coordinate 0 is machine zero. The reference point is a fixed point in machine coordinates that the axes return to with G28; it is used for the tool change position and the like^[1][15]
• Work coordinate system: the coordinates you write the program in. The work coordinate system offset is the position of work zero as seen in machine coordinates. Choose one of six with G54–G59; G54 is active at power-on^[1][15][19]
• G53 moves in machine coordinates for that block only (e.g., G53 G49 Z0 sends Z to machine zero)^[4][20][14]
• Tool length offset: each tool has a different length, so the offset for the H number is added to Z with G43, letting you command positions at the tool tip. Enter the offset values on the tool offset screen beforehand^[1][15][21]
• Cutter radius compensation: write the program to the part shape (drawing dimensions), and the tool is shifted left (G41) or right (G42) by the radius offset for the D number. Wear and finishing allowance can be adjusted through the offset value^[22][15][21]
• Write the program as if the tool moves relative to a stationary workpiece. Even on machines where the table moves, think in terms of the tool's motion as seen from the workpiece^[14][16]
• The rotary axes about X, Y, and Z are A, B, and C. Direction follows the right-hand rule (NIST: positive is counterclockwise when viewed from the positive side of the axis)^[15][14][16]
• The standard for coordinate systems and motion symbols is ISO 841:2001 (confirmed 2023), with the equivalent JIS B 6310:2003 (draft prepared by the Japanese Standards Association and JMTBA)^[17][18]

⚙Setup

• Workholding: vises, chucks, toe clamps (hold-downs), and so on. Incorrect clamping affects both safety and accuracyOne source / reference^[21]
• Finding work zero: pick up edges or corners with an edge finder, an electronic probe (touch probe), a pointer, etc., and enter that position in the work coordinate system offset (G54, etc.)One source / reference^[21]
• Touch probe (workpiece measuring probe): measures the shape, size, and position of the workpiece on the machine to automate setup. Combine it with automatic offset updatesOne source / reference^[23][21]
• Manual on-machine measurement: put the tool in the spindle, place a sheet of paper between it and the top of the workpiece, lower it to the point where the paper can still just move, and register that position as the tool length (H) (Haas procedure)One source / reference^[21]
• On-machine tool measurement (tool setter): contact type (the tool touches the measuring device; plunger and probe types) and non-contact type (finds tool length and diameter from the moment the tool interrupts a laser beam). Both can be used to detect tool breakageOne source / reference^[24]
• Tool presetter (off-machine measurement): measures tool length and diameter (and, on some models, edge angle and nose radius) outside the machine and sends the data to the NC. It reduces the time spent stopping the machine to measure, and prevents manual entry errors and collisions^[25][26]
• At every tool change, place a “safe startup line” (e.g., G00 G90 G17 G40 G49 G54) so that offsets and modes from the previous tool do not carry over^[4][27]

→Machining Flow and Program Structure

• A program has three parts: preparation (work coordinates, tool selection, tool length offset, spindle and coolant, G90/G91) → cutting (toolpath and feed) → end (retract the tool, stop the spindle and coolant, move to a position where the workpiece can be removed)^[4][1]
• Example sequence: face the top (face mill) → rough steps and profiles → finish → slots. For each tool, start with T_ M06, G43 H_, S_ M03, M08, and end with M09, M05One source / reference^[27]
• Drilling order: to improve positioning accuracy, first spot with a center drill (starting drill) → tap drill → tap (or reamer)One source / reference^[28][29]
• Drill feed methods: straight to the hole bottom in one pass (like G81), peck feed that retracts out of the hole (like G83), peck feed that retracts only a little (like G73). Peck feed breaks chips short and prevents wrapping, but adds impact, wear, heat, and time, so avoid unnecessary pecks^[28][15][20]
• Guideline for when to start peck feed: OSG says one pass is fine up to 4–5× the diameter, while Haas recommends pecking when the hole depth exceeds 3× the diameterlow^[28][22]
• Choosing canned cycles: G81 for shallow holes and center drilling, G82 for counterboring, G73 (chip breaking) and G83 (chip clearing) for deep holes, G84 for right-hand tapping, G85 for reaming and boring, G86 to stop the spindle and pull out, G76 for fine boring (oriented spindle stop and shift away), and finally G80^[15][30][20]

Canned cycle list:Drilling Canned Cycles · Macros: Intro to Custom Macros

!Common Mistakes and Safety

• Mixed-up work zero: wrong work coordinate system number (G54 vs. G55, etc.) or a wrong offset entry. In the Haas procedure, pressing PART ZERO SET an extra time puts a value in the Z field, which can cause a crash or a Z-axis alarmOne source / reference^[21][1]
• Forgotten or wrong tool length offset: forgetting G43 H, or using an H number that doesn't match the tool, shifts the Z height by the tool length. Put G43 H_ at every tool change^[1][15][4]
• How to write G28: G90 G28 Z0 passes through Z0 of the work coordinates, so it can hit the workpiece or fixture. To return directly, use G91 G28 Z0; return Z first, then X and Y^[1][30]
• Rapid-move collisions: on some machines G00 moves each axis at its own rapid rate and does not follow a straight line (Siemens: if compensation is started with G00, each axis moves at a different speed). Raise Z to a safe height before moving X and YOne source / reference^[15][1]
• Leaving a canned cycle in G99 (return to R point) can hit clamps or steps when crossing over them. Use G98 (return to initial point) only for the holes that cross over. If you forget G80, the next move keeps drilling^[30][20][15]
• Cutter radius compensation failures: starting or canceling compensation inside an arc, a lead-in shorter than the tool radius, an inside corner radius smaller than the tool radius, three or more consecutive blocks with no move in the compensation plane^[22][15][20]
• Spindle state in canned cycles: Haas G81, G86, and G76 use the previous spindle command; if it is still M05, the machine moves without spinning (a cause of crashes)One source / reference^[30]
• Missing decimal point: some machines read X100 as 0.1 mm (treated as an integer count of the least input increment). Always put decimal points on coordinates and G65 arguments^[15][31]
• Chips: on vertical machines they pile up on the top face, and a tool that re-cuts chips can be damaged or break. For deep holes, use peck feed to prevent chip wrappingOne source / reference^[3][28]
• Coolant: turn it on with M08 and off with M09 at tool changes and at the end of machining. For safety and cleaning details, see the maintenance page (no air blast into the spindle taper, precautions for work inside the machine, etc.)^[4][27]
• Verify a program you are running for the first time with graphics (toolpath display). Sample programs also have not fixed the tools, offsets, material, or fixtures^[32][1]

↗Learning Path

1. Learn the machine layout and axis directionsTable, spindle, ATC, tool magazine; directions of X, Y, Z; machine coordinates and work coordinates
2. Read the shape of a programBlocks, words, addresses; modal vs. one-shot; the three-part structure of preparation, cutting, and end
3. Write paths with G00, G01, G02/G03Positioning, linear, and arc moves (R vs. I/J). Draw the toolpath in the simulator to check it
4. Set up coordinates and offsetsWork zero with G54, tool length offset with G43 H, return to reference point with G28
5. Try a setupClamping in a vise, finding work zero with an edge finder or probe, ways to measure tool length (on-machine, off-machine)
6. Drilling with canned cyclesG81, G83, G84, G98/G99, G80. Use the calculators for cutting conditions
7. Cut profiles with cutter radius compensationLeft/right with G41/G42, rules for lead-in and cancel, adjusting dimensions with the offset value
8. Subprograms, macros, and on to CAMRepeat the same shape with M98/M99 and G65, variables and WHILE. Use CAD/CAM for complex shapes

ƒHandy Formulas

⇄Related Pages