How do I install the Cuttingparams skill?

Run npx skillmds add tools-only/cuttingparams in your terminal (requires Node.js), paste this page's agent-chat prompt into Claude, Cursor, or any MCP-connected agent, or download the SKILL.md file and copy it into your agent's skills directory.

What does the Cuttingparams skill do?

Cutting parameter lookup and optimization for CNC machining. Covers feeds, speeds, depths of cut for common materials and operations. USE WHEN user asks 'feeds and speeds', 'cutting parameters', 'SFM for', 'what RPM', 'feed rate for', 'DOC for', or needs machining parameter guidance. It is listed under Coding & Dev Tools on SkillMD.

Is Cuttingparams safe to use?

This skill has not completed SkillMD's automated safety review yet. Capability flags: docs only. SkillMD never runs a skill's scripts for you; review the SKILL.md before installing.

Which AI agents work with Cuttingparams?

This skill is tagged as working with Claude Code, Claude.ai, OpenAI Codex. SKILL.md is an open format, so most agents that read a skills directory can load it too.

Is Cuttingparams free to use?

Yes. Installing skills from SkillMD is free, and the skill stays under its author's original license.

Who published Cuttingparams?

tools-only (@tools-only) published this skill. Their other Agent Skills are listed on their SkillMD profile.

Cuttingparams by tools-only — Agent Skill

Name: Cuttingparams
Rating: 4.2 (5 reviews)
Author: tools-only

CuttingParams - Machining Parameter Reference

Purpose: Quick lookup and calculation of cutting parameters. Starting points that work, with adjustment guidance.

When to Activate

"What's the SFM for 316 stainless?"
"Feeds and speeds for 7075 aluminium"
"What RPM for a 12mm endmill in steel?"
"Recommended DOC for titanium roughing"
"Help me optimize my cutting parameters"

Core Formulas

Spindle Speed (RPM)

RPM = (SFM × 3.82) / Diameter (inches)
RPM = (Vc × 1000) / (π × Diameter mm)
RPM = (Vc × 318.3) / Diameter (mm)

Where:
- SFM = Surface Feet per Minute
- Vc = Cutting Speed in m/min

Feed Rate

Turning:

Feed (mm/min) = Feed per Rev (mm/rev) × RPM

Milling:

Feed (mm/min) = Feed per Tooth (mm/tooth) × Number of Teeth × RPM

Metal Removal Rate (MRR)

Turning:

MRR (cm³/min) = DOC × Feed × Vc × 1000

Milling:

MRR (cm³/min) = WOC × DOC × Feed Rate / 1000

Material Parameters - Turning

Aluminium Alloys

Material	Vc Rough (m/min)	Vc Finish (m/min)	Feed Rough (mm/rev)	Feed Finish (mm/rev)	DOC Rough (mm)
6061-T6	300-500	400-600	0.2-0.4	0.08-0.15	2-5
7075-T6	250-400	350-500	0.15-0.35	0.08-0.12	2-4
2024-T3	250-400	350-500	0.15-0.35	0.08-0.12	2-4
Cast Aluminium	200-350	300-450	0.15-0.3	0.08-0.12	1.5-3

Tool: Uncoated carbide, polished rake face, sharp edge Coolant: Flood or mist, water-soluble OK

Carbon & Alloy Steels

Material	Hardness	Vc Rough (m/min)	Vc Finish (m/min)	Feed Rough (mm/rev)	Feed Finish (mm/rev)	DOC Rough (mm)
1018	130 HB	180-250	220-300	0.2-0.4	0.08-0.15	2-4
1045	180 HB	150-220	180-260	0.15-0.35	0.08-0.12	1.5-3.5
4140	200 HB	120-180	150-220	0.15-0.3	0.08-0.12	1.5-3
4140	300 HB	80-120	100-150	0.1-0.25	0.05-0.1	1-2.5
4340	280 HB	90-140	120-170	0.1-0.25	0.05-0.1	1-2.5

Tool: Coated carbide (CVD for roughing, PVD for finishing) Coolant: Flood, high-pressure preferred

Stainless Steels

Material	Vc Rough (m/min)	Vc Finish (m/min)	Feed Rough (mm/rev)	Feed Finish (mm/rev)	DOC Rough (mm)
303	120-180	150-220	0.15-0.3	0.08-0.12	1.5-3
304	100-150	120-180	0.12-0.25	0.06-0.1	1-2.5
316	80-130	100-160	0.1-0.22	0.05-0.1	1-2
316L	80-120	100-150	0.1-0.2	0.05-0.1	1-2
17-4PH (H1025)	70-110	90-140	0.1-0.2	0.05-0.08	0.8-1.8
17-4PH (H900)	50-80	70-100	0.08-0.15	0.04-0.08	0.5-1.5

Tool: PVD coated carbide (TiAlN, AlTiN), positive rake Coolant: High-pressure flood essential, don't let it rub Warning: Work hardens - stay aggressive, don't dwell

Tool Steels

Material	Condition	Vc Rough (m/min)	Vc Finish (m/min)	Feed Rough (mm/rev)	Feed Finish (mm/rev)
D2	Annealed	60-100	80-120	0.1-0.2	0.05-0.1
D2	Hardened (58-62 HRC)	CBN/Ceramic only	80-150	0.05-0.12	0.03-0.08
H13	Annealed	80-120	100-150	0.12-0.22	0.06-0.1
H13	Hardened (48-52 HRC)	40-70	60-100	0.08-0.15	0.04-0.08
A2	Annealed	70-110	90-140	0.1-0.2	0.05-0.1
S7	Annealed	80-120	100-150	0.12-0.22	0.06-0.1

Tool: For hardened - CBN or ceramic inserts Coolant: Often dry for hardened (CBN), flood for annealed

Titanium Alloys

Material	Vc Rough (m/min)	Vc Finish (m/min)	Feed Rough (mm/rev)	Feed Finish (mm/rev)	DOC Rough (mm)
CP Grade 2	60-90	80-120	0.15-0.25	0.08-0.12	1-2.5
Ti-6Al-4V	40-70	55-90	0.1-0.2	0.06-0.1	0.8-2
Ti-6Al-4V (aged)	35-55	45-75	0.08-0.15	0.05-0.08	0.5-1.5

Tool: Uncoated or PVD carbide, sharp edge, positive rake Coolant: HIGH-PRESSURE flood (70+ bar), copious amounts Warning: Fire risk with chips, poor thermal conductivity

Superalloys

Material	Vc Rough (m/min)	Vc Finish (m/min)	Feed Rough (mm/rev)	Feed Finish (mm/rev)	DOC Rough (mm)
Inconel 718	25-45	35-60	0.1-0.18	0.05-0.1	0.5-1.5
Inconel 625	25-40	35-55	0.08-0.15	0.05-0.08	0.5-1.2
Hastelloy C-276	20-35	30-50	0.08-0.15	0.04-0.08	0.4-1
Waspaloy	20-40	30-55	0.08-0.15	0.05-0.08	0.5-1.2

Tool: Ceramic (roughing), CBN (finishing), or whisker-reinforced Coolant: High-pressure flood or dry with ceramic Warning: Extreme tool wear, work hardens badly

Plastics

Material	Vc (m/min)	Feed (mm/rev)	DOC (mm)	Notes
Delrin/Acetal	200-400	0.1-0.3	1-4	Sharp tools, watch heat
Nylon	150-300	0.1-0.25	1-3	Flexible, support well
PEEK	100-200	0.08-0.2	0.5-2	Expensive, careful
PTFE	150-300	0.1-0.25	1-3	Very flexible
Polycarbonate	150-300	0.1-0.2	0.5-2	Stress cracking risk

Tool: Sharp, polished, uncoated carbide or PCD Coolant: Air blast or mist (avoid flooding most plastics)

Brass & Bronze

Material	Vc Rough (m/min)	Vc Finish (m/min)	Feed Rough (mm/rev)	Feed Finish (mm/rev)
Free-cutting Brass	200-400	300-500	0.15-0.35	0.08-0.15
Naval Brass	150-250	200-350	0.12-0.28	0.06-0.12
Phosphor Bronze	100-180	150-250	0.1-0.22	0.05-0.1
Aluminium Bronze	80-140	120-200	0.1-0.2	0.05-0.1

Tool: Uncoated carbide, neutral or slightly negative rake for brass Coolant: Often dry, light mist for finish

Material Parameters - Milling

Aluminium Alloys

Material	Vc (m/min)	Fz Rough (mm/tooth)	Fz Finish (mm/tooth)	Ae Rough	Ap Rough
6061-T6	300-600	0.1-0.2	0.05-0.1	50-70%	1-2×D
7075-T6	250-500	0.08-0.18	0.04-0.08	50-70%	1-1.5×D

Tool: 2-3 flute, polished, high helix (45°), uncoated or ZrN

Steels

Material	Hardness	Vc (m/min)	Fz Rough (mm/tooth)	Fz Finish (mm/tooth)	Ae Rough	Ap Rough
1018	130 HB	150-250	0.08-0.15	0.04-0.08	40-60%	0.5-1×D
4140	200 HB	100-180	0.06-0.12	0.03-0.06	30-50%	0.5-1×D
4140	300 HB	60-100	0.04-0.1	0.02-0.05	25-40%	0.3-0.7×D

Tool: 4+ flute, AlTiN or TiAlN coated, variable helix

Stainless Steels

Material	Vc (m/min)	Fz Rough (mm/tooth)	Fz Finish (mm/tooth)	Ae Rough	Ap Rough
304	80-140	0.05-0.1	0.03-0.06	30-50%	0.3-0.8×D
316	60-120	0.04-0.09	0.02-0.05	25-45%	0.3-0.7×D
17-4PH	50-100	0.04-0.08	0.02-0.05	25-40%	0.3-0.6×D

Tool: 5+ flute, AlTiN coated, variable pitch, through-coolant Strategy: High-efficiency milling (HEM) / trochoidal preferred

Titanium

Material	Vc (m/min)	Fz (mm/tooth)	Ae	Ap	Notes
Ti-6Al-4V	40-70	0.05-0.1	10-20%	1-2×D	HEM essential

Tool: 5+ flute, variable helix, through-coolant, sharp Strategy: Light radial, deep axial, high-pressure coolant

Superalloys

Material	Vc (m/min)	Fz (mm/tooth)	Ae	Ap	Notes
Inconel 718	20-45	0.03-0.08	10-15%	0.5-1.5×D	Ceramic or CBN

Tool: Ceramic endmills for roughing, CBN for finishing Strategy: Light engagement, rigid setup essential

Drilling Parameters

Material	Vc (m/min)	Feed (mm/rev)	Peck Depth	Notes
Aluminium	80-150	0.15-0.3	3×D	Through-coolant preferred
Mild Steel	25-40	0.1-0.25	1-2×D	Flood coolant
Stainless	15-30	0.08-0.18	0.5-1×D	High-pressure, frequent peck
Titanium	12-25	0.06-0.12	0.3-0.5×D	Through-coolant essential
Inconel	8-15	0.04-0.1	0.2-0.3×D	Carbide or CBN

Peck Drilling Guide

Hole Depth	Peck Frequency	Retract
< 3×D	No peck needed	-
3-5×D	Every 1×D	Full retract
5-10×D	Every 0.5×D	Full retract
> 10×D	Gundrilling	-

Threading Parameters

Single-Point Threading (Turning)

Material	Vc (m/min)	Infeed Method	Passes
Aluminium	100-200	Flank/Modified	4-6
Steel	60-100	Modified flank	6-10
Stainless	40-80	Modified flank	8-12
Titanium	25-50	Radial	10-15

DOC per pass: Start at 0.2-0.3mm, reduce progressively

Thread Milling

Material	Vc (m/min)	Fz (mm/tooth)
Aluminium	150-300	0.05-0.1
Steel	80-150	0.03-0.08
Stainless	50-100	0.02-0.06
Titanium	30-60	0.02-0.05

Tapping

Material	Vc (m/min)	Notes
Aluminium	20-40	Spiral flute, flood
Steel	10-25	Spiral point, flood
Stainless	5-15	Form tap or spiral flute
Titanium	3-8	Spiral flute, high-pressure

Insert Selection Guide

Turning Insert Grades

Material	Roughing	Finishing
Aluminium	Uncoated, polished	PCD or uncoated polished
Steel (<300 HB)	CVD coated	PVD coated
Steel (>300 HB)	Ceramic/CBN	CBN
Stainless	PVD (TiAlN)	PVD (AlTiN)
Titanium	Uncoated or PVD	Uncoated sharp
Inconel	Ceramic	CBN or ceramic

Insert Geometry

Application	Nose Radius	Rake	Lead Angle
Heavy roughing	1.2-1.6mm	Negative	45°
Light roughing	0.8mm	Neutral	90°
Finishing	0.4mm	Positive	90°
Precision finish	0.2mm	Positive	90°
Interrupted cut	0.8-1.2mm	Negative	45°

Troubleshooting Parameters

Problem: Poor Surface Finish

Symptom	Likely Cause	Fix
Rough, torn	Speed too low	Increase Vc 20%
Feed marks visible	Feed too high	Reduce feed 20%
Chatter marks	Vibration	Reduce DOC, increase feed
Built-up edge	Wrong speed/material	Increase speed, change insert
Smearing	Rubbing	Sharper insert, increase feed

Problem: Rapid Tool Wear

Wear Type	Cause	Fix
Flank wear	Speed too high	Reduce Vc 15-20%
Crater wear	Heat/chemical	Better coating, reduce speed
Notch wear	Work hardening	Vary DOC, change lead angle
Chipping	Interrupted/shock	Tougher grade, reduce feed
Built-up edge	Speed too low	Increase Vc, better coating

Problem: Chatter/Vibration

Cause	Solution
Tool overhang	Reduce stickout, larger shank
Light cut	Increase feed or DOC
Wrong speed	Adjust RPM (try ±20%)
Part not rigid	Better workholding, steadies
Insert nose radius	Smaller radius

Problem: Chip Control

Issue	Material	Solution
Bird's nest	Stainless, aluminium	Chipbreaker, increase feed
Stringy chips	Ductile materials	Higher feed, chipbreaker
Long chips	Low carbon steel	Increase feed, DOC
Chip packing	Deep holes	Peck drilling, through-coolant
Welding to tool	Aluminium, stainless	Increase speed, better coating

Swiss Machine Parameters (CITIZEN)

Small Diameter Work (Ø3-10mm)

Material	Vc (m/min)	Feed (mm/rev)	DOC (mm)
303SS	80-120	0.02-0.06	0.2-0.8
316SS	60-100	0.02-0.05	0.15-0.6
Brass	150-250	0.03-0.08	0.3-1.0
Aluminium	200-350	0.03-0.08	0.3-1.2
Ti-6Al-4V	30-50	0.01-0.04	0.1-0.4

LFV Settings (CITIZEN LFV)

Material	Use LFV?	Frequency	Amplitude
316SS	Yes	10-20 Hz	0.05-0.15mm
304SS	Yes	10-20 Hz	0.05-0.15mm
Titanium	Yes	8-15 Hz	0.03-0.1mm
Aluminium	Rarely	-	-
Brass	No	-	-
Plastics	Sometimes	5-10 Hz	0.02-0.08mm

LFV Benefits: Breaks chips into small segments, eliminates bird-nesting, improves surface finish on gummy materials

Quick Reference Cards

Turning - Starting Points

ALUMINIUM:  Vc=400  Feed=0.2   DOC=3mm
STEEL:      Vc=180  Feed=0.2   DOC=2mm
STAINLESS:  Vc=100  Feed=0.15  DOC=1.5mm
TITANIUM:   Vc=50   Feed=0.12  DOC=1mm
INCONEL:    Vc=30   Feed=0.1   DOC=0.8mm

Milling - Starting Points

ALUMINIUM:  Vc=400  Fz=0.15  Ae=50%  Ap=1×D
STEEL:      Vc=150  Fz=0.08  Ae=40%  Ap=0.7×D
STAINLESS:  Vc=90   Fz=0.06  Ae=30%  Ap=0.5×D
TITANIUM:   Vc=50   Fz=0.06  Ae=15%  Ap=1.5×D (HEM)
INCONEL:    Vc=30   Fz=0.05  Ae=10%  Ap=1×D (HEM)

RPM Quick Calc (metric)

RPM = (Vc × 318) / Diameter(mm)

Examples @ Vc=100 m/min:
Ø6mm  = 5,300 RPM
Ø10mm = 3,180 RPM
Ø12mm = 2,650 RPM
Ø16mm = 1,990 RPM
Ø20mm = 1,590 RPM
Ø25mm = 1,270 RPM
Ø50mm = 636 RPM

Integration

CNCSetup: Auto-populate cutting parameters in setup sheets
TribalKnowledge: Store proven parameters that beat book values
QuoteEstimator: More accurate cycle times with real parameters
PlantCapability: Material-specific machine recommendations

Cuttingparams

File contents

CuttingParams - Machining Parameter Reference

When to Activate

Core Formulas

Spindle Speed (RPM)

Feed Rate

Metal Removal Rate (MRR)

Material Parameters - Turning

Aluminium Alloys

Carbon & Alloy Steels

Stainless Steels

Tool Steels

Titanium Alloys

Superalloys

Plastics

Brass & Bronze

Material Parameters - Milling

Aluminium Alloys

Steels

Stainless Steels

Titanium

Superalloys

Drilling Parameters

Peck Drilling Guide

Threading Parameters

Single-Point Threading (Turning)

Thread Milling

Tapping

Insert Selection Guide

Turning Insert Grades

Insert Geometry

Troubleshooting Parameters

Problem: Poor Surface Finish

Problem: Rapid Tool Wear

Problem: Chatter/Vibration

Problem: Chip Control

Swiss Machine Parameters (CITIZEN)

Small Diameter Work (Ø3-10mm)

LFV Settings (CITIZEN LFV)

Quick Reference Cards

Turning - Starting Points

Milling - Starting Points

RPM Quick Calc (metric)

Integration

Related skills

Frequently asked questions

How do I install the Cuttingparams skill?

What does the Cuttingparams skill do?

Is Cuttingparams safe to use?

Which AI agents work with Cuttingparams?

Is Cuttingparams free to use?

Who published Cuttingparams?