Machining Parameters Guide
A complete machining reference: cutting speed (Vc) charts by material, feed rates, machining formulas and calculators, tool coatings, coolant selection, parameters by material and process, and a troubleshooting guide for common machining problems.
๐ง Cutting Speeds โ Vc (m/min) โ Starting Point
| Material | Turning HSS | Turning Carbide | Milling HSS | Milling Carbide | Drilling HSS | Notes |
|---|---|---|---|---|---|---|
| Mild Steel (S235) | 25-35 | 80-120 | 20-30 | 60-100 | 25-35 | Coolant recommended |
| Medium Steel (4140 Q&T) | 15-25 | 60-100 | 15-20 | 50-80 | 15-25 | Coolant mandatory |
| Stainless 304/316 | 8-12 | 40-70 | 5-10 | 30-50 | 8-12 | High pressure, flood coolant |
| Aluminum 6061 | 80-150 | 200-500 | 60-100 | 150-400 | 60-100 | Can run dry, very high Vc |
| Aluminum 7075 | 80-140 | 200-450 | 50-90 | 150-350 | 60-90 | โ |
| Titanium Ti-6Al-4V | 4-8 | 30-60 | 3-6 | 20-40 | 5-10 | Flood coolant mandatory, low Vc! |
| Gray Cast Iron | 20-30 | 80-150 | 15-25 | 60-120 | 25-35 | Can run dry |
| Tool Steel D2 | 8-12 | 40-70 | 5-8 | 30-50 | 8-12 | Machine before hardening |
| Inconel 718 | 2-4 | 15-30 | 1-3 | 10-20 | 3-5 | Carbide+TiAlN mandatory, flood coolant |
| Copper/Bronze | 50-80 | 150-300 | 40-60 | 120-250 | 50-80 | No coolant needed |
โ ๏ธ These values are a starting point only! They depend on tool diameter, depth of cut, machine condition, and tool coating. Always verify in practice and refine based on chip performance.
๐ Taylor's Tool Life Equation โ Tool Life vs. Speed
Vc ร Tโฟ = C โ n depends on the tool/material pair (HSSโ0.1-0.15, Carbideโ0.2-0.4, Ceramicโ0.5-0.7). The larger n is, the more the tool "forgives" a speed increase.
Rule of thumb: raising Vc by 20% shortens tool life by about 50% (for nโ0.25, typical for carbide). Before speeding up production โ check the real cost in tool wear!
โก๏ธ Feed per Tooth (fz) by Material and Tool Diameter โ Milling [mm/tooth]
| Material | โ6-10mm | โ12-20mm | โ25mm+ | Notes |
|---|---|---|---|---|
| Aluminum | 0.05-0.10 | 0.10-0.18 | 0.15-0.25 | Can be increased with Chip Thinning |
| Mild Steel | 0.04-0.08 | 0.08-0.15 | 0.12-0.20 | Coarser = more productive |
| Medium/Hardened Steel | 0.03-0.06 | 0.06-0.10 | 0.08-0.15 | Reduce for chatter |
| Stainless | 0.03-0.05 | 0.05-0.08 | 0.08-0.12 | Too fine = work hardening! |
| Titanium | 0.02-0.04 | 0.04-0.07 | 0.06-0.10 | Keep constant, don't reduce too much (heat) |
| Inconel/Superalloy | 0.02-0.03 | 0.03-0.05 | 0.05-0.08 | Hard on the tool โ Trochoidal preferred |
โ ๏ธ Minimum fz is critical! Below the minimum = rubbing (instead of cutting) โ heat โ work hardening โ premature tool failure.
โก๏ธ Feed per Revolution (fn) โ Turning [mm/rev]
| Operation Type | Typical fn | Expected Ra |
|---|---|---|
| Roughing | 0.2-0.5 | 3.2-6.3ฮผm |
| General | 0.1-0.3 | 1.6-3.2ฮผm |
| Finishing | 0.05-0.15 | 0.8-1.6ฮผm |
| Fine Finish + Wiper | 0.15-0.3 | 0.4-0.8ฮผm |
Formula: Ra โ fnยฒ/(8รRฮต)ร1000 [ฮผm], where Rฮต = tool nose radius (mm). A Wiper Insert allows double the fn at the same Ra!
๐ Chip Thinning โ Feed Compensation in Partial Side Milling
When ae (radial depth) is less than 50% of the tool diameter, the actual chip thickness is smaller than the nominal fz โ you can (and should!) increase fz to maintain proper tooth loading and prevent rubbing.
Approximate formula: fz_corrected = fz ร D/โ(Dรaeโaeยฒ). At ae=10%D, you can usually multiply fz by 1.5-2ร!
๐ Machining Formulas
| Parameter | Formula | Units |
|---|---|---|
| RPM | n = (Vc ร 1000) / (ฯ ร D) | rev/min |
| Table Feed Vf | Vf = fz ร z ร n | mm/min |
| MRR (Material Removal Rate) | MRR = ae ร ap ร Vf | mmยณ/min |
| Cutting Force Fc | Fc = kc ร ap ร fz ร z | N |
| Power P | P = Fc ร Vc / 60000 | kW |
| Turning Time Tm | Tm = L / (f ร n) | minutes |
fz=feed per tooth(mm) ยท z=number of teeth ยท ae=radial depth ยท ap=axial depth ยท kc=specific cutting force
๐งญ kc โ Specific Cutting Force by Material [N/mmยฒ]
| Material | kc |
|---|---|
| Aluminum | 500-900 |
| Mild Steel | 1800-2200 |
| Hardened Steel | 2500-3200 |
| Stainless | 2200-2800 |
| Titanium | 1800-2400 |
| Inconel | 2800-3500 |
kc directly determines the required force and power โ important to check against spindle power for roughing operations!
๐งฎ RPM / Feed / MRR Calculator
Live Calculation
โ
๐ฉ Tool Coatings and Their Applications
| Coating | Hardness HV | Tmax ยฐC | Best Application |
|---|---|---|---|
| TiN (Titanium Nitride) | 2300 | 500 | Steel turning, default choice |
| TiCN | 3000 | 400 | Hard steel, coolant |
| TiAlN | 3300 | 800 | High-speed milling, dry, SS |
| AlCrN | 3200 | 1100 | Hard alloys, Inconel |
| DLC | 3000-5000 | 300 | Al, Cu โ anti-adhesion |
| CVD AlโOโ | 2400 | 1200 | High-speed turning |
๐ Insert Geometry โ Quick Selection
Point Angle
80ยฐ (Diamond C) โ strong, universal
55ยฐ/35ยฐ (V) โ sharp, for profiles/corners
90ยฐ (S Square) โ perpendicular walls
55ยฐ/35ยฐ (V) โ sharp, for profiles/corners
90ยฐ (S Square) โ perpendicular walls
Chip Breaker
Roughing โ a deep channel, breaks thick chips
Finishing โ a shallow channel, low Ra
General โ a compromise in between
Finishing โ a shallow channel, low Ra
General โ a compromise in between
Nose Radius (Rฮต)
Small (0.2-0.4mm) โ small holes, low vibration
Large (0.8-1.6mm) โ good Ra, stability, but higher Fc
Large (0.8-1.6mm) โ good Ra, stability, but higher Fc
๐ฏ Insert ISO Coding โ Quick Decoding
Example: CNMG 120408 โ C(shape: 80ยฐ diamond) N(clearance: 0ยฐ) M(tolerance: ยฑ0.13) G(hole+chip breaker) 12(edge 12mm) 04(thickness 4.76mm) 08(radius 0.8mm)
Grade is selected separately: P (steel), M (stainless), K (cast iron), N (non-ferrous/Al), S (superalloy), H (hardened).
๐ง Coolant Selection by Process and Material
| Condition | Material | Recommendation |
|---|---|---|
| Aluminum Milling | Al | Emulsion 5-8% / dry |
| Stainless Turning | SS | High-concentration oil 10-15% |
| Deep Drilling | Any material | High-pressure cutting, oil |
| Titanium Milling | Ti | Flood emulsion 8-10% |
| Coated Carbide | โ | Dry is usually preferable |
| HSS Turning | โ | Emulsion always |
| Cast Iron | Cast | Dry preferred |
๐ฟ Coolant Delivery Methods
Flood
The most common. Cheap, reliable. Doesn't always reach the cutting zone in depth.
Through-Tool
20-70bar through holes in the tool. Mandatory for deep drilling (L/D>5). Extends tool life significantly.
MQL (Minimum Quantity Lubrication)
Oil mist 5-50ml/h. Green and economical. Excellent for aluminum, less so for deep drilling.
Dry Cutting
Requires TiAlN/AlCrN coating. Cast iron, high-speed steel milling. Saves 15% in operating costs.
๐งช Coolant Concentration โ Testing and Maintenance
Emulsion concentration: 5-10% measured with a refractometer. Desired pH: 8.5-9.5. Bacteria = bad odor + skin conditions โ weekly testing!
Aluminum (6061/7075)
Vc: 200-500 (carbide)
fz: 0.10-0.25mm
Coolant: dry/light emulsion
Tip: BUE is the main issue at low Vc โ raise speed, sharp tool, DLC coating. Wide chip-clearance flutes.
fz: 0.10-0.25mm
Coolant: dry/light emulsion
Tip: BUE is the main issue at low Vc โ raise speed, sharp tool, DLC coating. Wide chip-clearance flutes.
Mild/Medium Steel
Vc: 60-120 (carbide)
fz: 0.08-0.20mm
Coolant: emulsion 8-10%
Tip: The default starting point. P-Grade insert, TiAlN. Moving to 4140 Q&T โ reduce Vc by 30-40%.
fz: 0.08-0.20mm
Coolant: emulsion 8-10%
Tip: The default starting point. P-Grade insert, TiAlN. Moving to 4140 Q&T โ reduce Vc by 30-40%.
Stainless (304/316)
Vc: 40-70 (carbide)
fz: 0.05-0.10mm
Coolant: flood, high concentration
Tip: Work hardening is enemy #1! Never rub (minimum fz!). M-Grade insert, always a sharp tool.
fz: 0.05-0.10mm
Coolant: flood, high concentration
Tip: Work hardening is enemy #1! Never rub (minimum fz!). M-Grade insert, always a sharp tool.
Titanium (Ti-6Al-4V)
Vc: 30-60 (carbide)
fz: 0.04-0.08mm
Coolant: flood mandatory!
Tip: Low thermal conductivity = heat stays in the tool. Low Vc, deep ap (not shallow!), Trochoidal recommended.
fz: 0.04-0.08mm
Coolant: flood mandatory!
Tip: Low thermal conductivity = heat stays in the tool. Low Vc, deep ap (not shallow!), Trochoidal recommended.
Inconel/Superalloy
Vc: 15-30 (carbide)
fz: 0.03-0.06mm
Coolant: high-pressure flood
Tip: Work hardening is worse than SS! Trochoidal is almost mandatory. AlCrN/ceramic. Steady load โ avoid rubbing.
fz: 0.03-0.06mm
Coolant: high-pressure flood
Tip: Work hardening is worse than SS! Trochoidal is almost mandatory. AlCrN/ceramic. Steady load โ avoid rubbing.
Gray Cast Iron
Vc: 80-150 (carbide)
fz: 0.10-0.20mm
Coolant: dry preferred!
Tip: Graphite self-lubricates โ coolant can cause thermal shock and cracking. Dust โ good extraction needed.
fz: 0.10-0.20mm
Coolant: dry preferred!
Tip: Graphite self-lubricates โ coolant can cause thermal shock and cracking. Dust โ good extraction needed.
Copper/Bronze/Brass
Vc: 150-300 (carbide)
fz: 0.10-0.20mm
Coolant: usually not needed
Tip: Pure copper is gummy โ sharp tool + high Vc. Free-machining brass (leaded) โ excellent machinability.
fz: 0.10-0.20mm
Coolant: usually not needed
Tip: Pure copper is gummy โ sharp tool + high Vc. Free-machining brass (leaded) โ excellent machinability.
Hardened Tool Steel (D2/H13)
Vc: 40-80 (carbide)/80-200 (CBN)
fz: 0.05-0.15mm
Coolant: process-dependent
Tip: Above HRC45 โ switch to Hard Turning with CBN instead of grinding. Small ap, machine rigidity is critical.
fz: 0.05-0.15mm
Coolant: process-dependent
Tip: Above HRC45 โ switch to Hard Turning with CBN instead of grinding. Small ap, machine rigidity is critical.
โ๏ธ Parameter Selection by Process
For a full explanation of how each process works (turning/milling/drilling/grinding) โ see the "Manufacturing Technologies" tab. Here: parameter selection only.
Turning
Roughing: ap=2-5mm, fn=0.2-0.4
Finishing: ap=0.2-0.5mm, fn=0.05-0.15
Tip: A Wiper Insert for finishing = double the feed at the same Ra. Minimum finish depth: above 0.1mm (below = rubbing).
Finishing: ap=0.2-0.5mm, fn=0.05-0.15
Tip: A Wiper Insert for finishing = double the feed at the same Ra. Minimum finish depth: above 0.1mm (below = rubbing).
Milling
Slotting: ae=100%D
Shoulder: ae=30-50%D
Trochoidal: ae=5-15%D, ap=1-3รD
Tip: Climb milling always on CNC. Trochoidal for SS/Ti/Inconel = 30-300% higher MRR.
Shoulder: ae=30-50%D
Trochoidal: ae=5-15%D, ap=1-3รD
Tip: Climb milling always on CNC. Trochoidal for SS/Ti/Inconel = 30-300% higher MRR.
Drilling
L/Dโค4: normal drilling
L/D 4-10: Peck Drilling (G83)
L/D>10: Gun Drill + internal coolant
Tip: A spot drill for accurate positioning before a long drill. Carbide+TSC drill = 3-5ร the speed of HSS.
L/D 4-10: Peck Drilling (G83)
L/D>10: Gun Drill + internal coolant
Tip: A spot drill for accurate positioning before a long drill. Carbide+TSC drill = 3-5ร the speed of HSS.
Grinding
Surface: 0.005-0.02mm/pass
Cylindrical: wheel Vc 25-35 m/s
Tip: Grinding burn = hidden damage! Frequent dressing, adequate coolant, not too aggressive an infeed.
Cylindrical: wheel Vc 25-35 m/s
Tip: Grinding burn = hidden damage! Frequent dressing, adequate coolant, not too aggressive an infeed.
Tapping
Rigid Tapping: n=const, F=Pรn
Form Tap: a larger drill (separate table)
Tip: 75% thread depth is almost always enough. Spiral Point for through holes, Spiral Flute for blind holes.
Form Tap: a larger drill (separate table)
Tip: 75% thread depth is almost always enough. Spiral Point for through holes, Spiral Flute for blind holes.
Thread Milling
Vc like regular milling, one tool for every diameter
Tip: Mandatory for hard materials and large holes. Diameter control via Offset โ corrects wear!
Tip: Mandatory for hard materials and large holes. Diameter control via Offset โ corrects wear!
๐ Machining Troubleshooting โ by Symptom
Visual identification of the problem is the core skill in machining diagnostics โ that's why visual reference links are included here.
Chip Not Breaking / Stringing
Cause: unsuitable chip breaker, fz too low, Vc not matched to material.
Solution: increase fz, check insert geometry, smaller Rฮต.
โถ YouTube
Solution: increase fz, check insert geometry, smaller Rฮต.
BUE โ Built-Up Edge
Cause: Vc too low, gummy material (Al/soft SS), insufficient coolant.
Solution: increase Vc, DLC/TiAlN coating, adequate coolant, a sharper tool.
โถ YouTube
Solution: increase Vc, DLC/TiAlN coating, adequate coolant, a sharper tool.
Chatter โ Vibration and Wavy Finish
Cause: natural frequency, large overhang, low holding rigidity.
Solution: change RPM (Stability Lobes!), reduce ap, a shorter tool, good clamping.
โถ YouTube
Solution: change RPM (Stability Lobes!), reduce ap, a shorter tool, good clamping.
Fast Tool Wear (large VB)
Cause: Vc too high, unsuitable coating, insufficient coolant.
Solution: reduce Vc per Taylor, upgrade coating, check coolant flow to the cutting zone.
โถ YouTube
Solution: reduce Vc per Taylor, upgrade coating, check coolant flow to the cutting zone.
Poor Surface Finish (high Ra)
Cause: fn/fz too high, small Rฮต, a worn tool, chatter.
Solution: reduce feed, a Wiper Insert, check tool wear, ensure holding rigidity.
Solution: reduce feed, a Wiper Insert, check tool wear, ensure holding rigidity.
Sudden Tool Breakage
Cause: overload, sudden entry (no ramping), inconsistent material/inclusions.
Solution: ramping/helical entry, check raw material, reduce ap/fz on first entry.
Solution: ramping/helical entry, check raw material, reduce ap/fz on first entry.
Overheating / Discoloration on the Part
Cause: coolant not reaching the zone, high Vc, low fz (rubbing).
Solution: through-tool coolant, check nozzle direction, increase fz to prevent rubbing.
Solution: through-tool coolant, check nozzle direction, increase fz to prevent rubbing.
Dimensional Drift
Cause: accumulated tool wear, machine/spindle heating, outdated tool offset.
Solution: frequent probing, wear compensation via offset, machine warm-up before precise work.
Solution: frequent probing, wear compensation via offset, machine warm-up before precise work.