-
Factors affecting cutting temperature: cutting speed, feed rate, depth of cut.
Factors affecting cutting force: depth of cut, feed rate, cutting speed.
Factors affecting tool life: cutting speed, feed rate, depth of cut. - Doubling the depth of cut doubles the cutting force.
Doubling the feed rate increases cutting force by about 70%.
Doubling the cutting speed gradually reduces cutting force.
In other words, when using G99, increasing cutting speed will not significantly change the cutting force. - The shape and behavior of chips can be used to determine whether cutting force and temperature are within normal ranges.
- When the difference between the actual measured value X and the drawing diameter Y exceeds 0.8 mm in concave arc turning, using a 52° secondary cutting-edge angle (commonly a 35° insert with a 93° main cutting-edge angle) may cause tool rubbing at the arc’s starting point.
- Chip color as a temperature indicator:
- White: < 200 °C
- Yellow: 220–240 °C
- Dark blue: ~290 °C
- Blue: 320–350 °C
- Purple-black: > 500 °C
- Red: > 800 °C
- Default G-code settings in FANUC Oi MTC:
- G69: (uncertain)
- G21: Metric input
- G25: Spindle speed fluctuation detection OFF
- G80: Cancel canned cycle
- G54: Default work coordinate system
- G18: ZX plane selection
- G96 (G97): Constant surface speed control / Cancel
- G99: Feed per revolution
- G40: Cancel tool nose radius compensation (G41/G42)
- G22: Stroke limit detection ON
- G67: Cancel modal macro call
- G64: (uncertain)
- G13.1: Cancel polar coordinate interpolation
- External thread minor diameter ≈ 1.3 × pitch (P).
Internal thread minor diameter ≈ 1.08 × pitch (P). -
Thread spindle speed formula:
S = 1200 ÷ pitch × safety factor (typically 0.8). -
Manual tool nose R compensation for chamfering:
Bottom-up chamfer:
Z = R × [1 − tan(a/2)]
X = Z × tan(a)
Top-down chamfering: replace subtraction with addition. - For every 0.05 mm/rev increase in feed, reduce spindle speed by 50–80 rpm. This slows tool wear and compensates for the increased cutting force and temperature caused by higher feed.
- Cutting speed and cutting force have a major impact on tool life. Excessive cutting force is the main cause of tool breakage. Increasing cutting speed slightly reduces cutting force at constant feed, but accelerates tool wear, which in turn increases both force and temperature until the insert fails.
-
Important tips for CNC turning:
- Economy CNC lathes in China typically use standard three-phase asynchronous motors with variable frequency drives for stepless speed control. Without mechanical reduction, low-speed torque may be insufficient, causing stalling under heavy loads (gearbox-equipped machines solve this well).
- Choose tooling that can finish a part or an entire shift without replacement, especially for large finishing jobs.
- Use higher speeds when threading for better quality and efficiency.
- Use G96 constant surface speed whenever possible.
- High-speed machining relies on feed rates exceeding the speed of heat conduction, carrying heat away in the chips and keeping the workpiece cool. This requires high cutting speed, high feed rate, and small depth of cut.
- Always compensate for tool nose radius.
- Reference charts: machinability grading of materials (P79), common thread cutting passes & depth of cut (P587), geometric formulas (P42), inch–mm conversion (P27).
- Grooving often causes vibration and tool breakage due to high cutting forces and insufficient rigidity. Shorter overhang, smaller clearance angle, and larger insert contact area improve rigidity.
-
Grooving vibration causes:
- Excessive tool overhang reduces rigidity.
- Feed rate too slow increases unit cutting force, causing vibration. Formula: P = F / (depth of cut × feed), where P = unit cutting force, F = cutting force. High spindle speed can also cause vibration.
- Poor machine rigidity—tool can handle the force, but the machine cannot. Usually occurs in older or heavily worn machines.
- Dimensional drift over time may be caused by tool wear increasing cutting force, which shifts the workpiece in the chuck.
- In FANUC, G71 P/Q values must not exceed the total number of program blocks, or an alarm will occur.
-
FANUC subprogram formats:
- P0000000: first three digits = repetitions, last four = program number.
- P0000L000: first four = program number, L + last three = repetitions.
- If the arc start point is fixed but the Z end point shifts by “a” mm, the arc’s bottom diameter shifts by a/2.
- In deep-hole drilling, do not grind chip evacuation grooves if you want smoother chip flow.
- When using a fixture-mounted drill, slightly rotating the drill can change the hole diameter.
- For drilling stainless steel, use a smaller center drill. With cobalt drills, avoid grinding chip grooves to prevent annealing during drilling.
- Common blank cutting methods: single-piece cut, double-piece cut, full-bar cut.
- Elliptical threads may be caused by workpiece looseness—lightly recut several passes to correct.
- Systems supporting macros can replace subprogram loops with macros, saving program numbers and avoiding errors.
- If a drilled hole has large runout, use a flat-bottom drill instead of a twist drill, and keep the drill short to improve rigidity.
- Direct drilling on a drill press may produce size errors, but boring (e.g., enlarging a 10 mm hole) usually maintains ±0.03 mm accuracy.
- When turning small through-holes, aim for continuous chip curling and rear chip evacuation:
- Raise tool position slightly.
- Use proper rake angle, depth of cut, and feed rate.
- Avoid setting the tool too low.
- A larger secondary cutting-edge angle helps prevent chip jamming.
- The larger the toolholder cross-section inside the hole, the less vibration. Wrapping a strong rubber band around the toolholder can also help dampen vibration.
- When turning copper holes, a larger tool nose radius (R0.4–R0.8) is beneficial, especially for taper turning. This reduces chip jamming, which is more severe with copper than steel.
