Home / docs / Cnc plastic materials / Machining process / Plastic CNC Machining — Process & Technology Guide

Plastic CNC Machining — Process & Technology Guide

Cnc plastic materials
Last updated: May 23, 2026

Plastic CNC Machining — Process & Technology Guide

← Back to the Plastic Materials Handbook

Plastics do not machine like metals. Most engineering plastics have lower stiffness, lower thermal conductivity, higher thermal expansion, and softer cutting behavior than aluminum or steel. Heat stays near the cutting edge instead of flowing into the workpiece, so dull tools or rubbing quickly cause melting, gumming, burrs, dimensional drift, or surface damage. Many plastic stock shapes also contain residual stress from extrusion, casting, or molding; when material is removed, the part may warp unless the process includes proper tool geometry, heat control, stress relief, and careful workholding.

Rating legend — ★★★★★ best · ★☆☆☆☆ worst. For machinability/stability/heat resistance more stars = better; for cost, fewer stars = cheaper.

1. Tool Selection Guide

1.1 The #1 Rule: Keep Tools Sharp ⭐

For plastic CNC machining, sharp tooling is more important than high spindle speed or heavy coolant. A sharp tool shears the plastic cleanly and carries heat away in the chip. A dull tool rubs, compresses, melts, smears, and generates internal stress.

Tool Condition Cutting Result Typical Defects
✅ Sharp, polished tool Clean chip formation, low heat, good finish Minimal burrs, stable dimensions
⚠️ Slightly worn tool More rubbing, rising temperature Fuzzy edges, light burrs, poor repeatability
❌ Dull tool Heat buildup, plastic deformation instead of cutting Melting, gumming, cracking, oversized/undersized features

1.2 Tool Material Selection

Tool Material Suitability Best Use Notes
Carbide ★★★★★ General CNC milling, turning, drilling of engineering plastics Preferred default: rigid, wear-resistant, holds sharp edge well
PCD / diamond-coated / diamond tooling ★★★★★ Abrasive filled grades: glass-filled PEEK, carbon-filled PEEK, filled PI, filled PPS Higher cost but dramatically better edge life on abrasive materials
HSS ★★★☆☆ Soft commodity plastics, manual machining, low-volume drilling Can work well if extremely sharp; wears faster than carbide
Uncoated polished carbide ★★★★★ Acrylic, PC, POM, PA, PE, PP, PTFE Often better than rough coatings because chips slide out cleanly
TiAlN / hard-coated metal tools ★★☆☆☆ Limited use Some coatings increase friction or chip sticking; test before production

💡 Carbide is the standard choice for most plastic CNC work. Use PCD/diamond when machining abrasive glass-filled or carbon-filled high-performance plastics.

Geometry Item Recommendation Why It Matters
Cutting edge Very sharp, honed only lightly Reduces cutting force and heat generation
Rake angle Large positive rake, typically 10°~20° Slices material instead of pushing/deforming it
Flute finish Polished flutes Prevents chip welding, gumming, and recutting
Helix angle High helix for many milling operations Improves chip evacuation and surface finish
Number of flutes Fewer flutes; large chip gullets Creates space for bulky plastic chips
O-flute / single-flute Excellent for acrylic, PC, soft plastics, sheet machining Produces clean chips and low heat at high RPM
Corner radius Small radius for strength when needed Reduces chipping on brittle plastics but avoid excessive rubbing
Drill point Sharp point, polished flute, appropriate point angle Prevents grabbing, heat buildup, and exit cracking

1.4 Tool Recommendations by Plastic Family

Plastic Family Examples Tool Material Geometry Recommendation Key Operator Note
Soft / commodity plastics PE, HDPE, UHMW-PE, PP, PVC, PTFE Sharp carbide or sharp HSS Single-flute or 2-flute, large rake, large chip space Avoid rubbing; soft materials can smear and deflect
Transparent / brittle plastics PMMA/acrylic, PC, PS Polished carbide, O-flute, diamond for optical finish Single-flute O-flute, very sharp edge, high rake Prevent heat and stress cracking; support edges carefully
Engineering plastics POM, PA/nylon, PET, PBT, ABS Carbide 2-flute or 3-flute, positive rake, polished flutes Good balance of rigidity and machinability; watch moisture in PA
High-performance plastics PEEK, PEI, PSU, PPS, PI Carbide; PCD for filled grades Rigid setup, sharp positive geometry, controlled finishing passes Higher heat resistance but still needs heat control and stress relief
Filled / reinforced plastics Glass-filled PEEK, carbon-filled PEEK, GF PPS, GF nylon PCD/diamond preferred; carbide acceptable for short runs Wear-resistant tooling, rigid holder, conservative finishing allowance Abrasive fillers rapidly dull normal carbide tools
Flexible elastomer-like plastics TPU, soft PE, rubber-like plastics Razor-sharp carbide, special single-flute tools Very positive rake, low cutting pressure, strong support Difficult to hold; use freezing/support fixtures when needed

📌 Practical rule: Use the fewest flutes that still provide stable cutting. Plastics make large, continuous chips; chip space is often more valuable than flute count.

2. Cutting Parameters

2.1 General Cutting Principles ⭐⭐ Core

Plastic machining parameters must create a real chip, not rubbing contact. The chip carries away most of the heat, so the process should be tuned for clean shearing + fast chip evacuation.

Principle Recommended Practice Avoid
Spindle speed Generally high RPM with sharp tools Excessive surface speed with dull tools
Feed rate Moderate to high enough to form chips Too low feed causing rubbing and melting
Toolpath Climb milling for better finish and lower burrs Dwelling in corners or pausing while cutting
Finishing Shallow final pass with sharp tool Heavy finishing pass that releases stress
Heat control Air blast, chip evacuation, correct chip load Recutting chips or packing slots
Accuracy Rough → rest → stress-relieve if needed → finish Chasing tight tolerance while the part is warm

⚠️ Reference only — the table below gives starting ranges, not universal settings. Always adjust to machine rigidity, tool diameter, tool geometry, holder runout, plastic grade, stock shape, and part geometry.

2.2 Consolidated Cutting Parameter Reference

Typical assumptions: sharp carbide tools, stable CNC machine, metric units, dry cutting or air blast, common tool diameters approximately 3~10mm for milling. For very small tools, reduce depth of cut and feed; for large tools, calculate chip load and surface speed carefully.

Material / Family Rough Milling RPM Rough Feed (mm/min) Finish Milling RPM Finish Feed (mm/min) Turning Speed / Feed Drilling RPM / Feed Machining Notes
POM / Acetal 5000~10000 1500~3000 8000~15000 800~1500 15003000 RPM; 0.100.30 mm/rev 10003000 RPM; 50200 mm/min Excellent machinability; stable chips; low burr tendency
PA / Nylon 4000~9000 1000~2500 6000~12000 600~1400 10002500 RPM; 0.100.25 mm/rev 8002500 RPM; 40180 mm/min Dry stock before precision machining; moisture changes size
PE / HDPE / UHMW-PE 5000~12000 1200~3500 8000~18000 800~2000 10002500 RPM; 0.100.35 mm/rev 8002500 RPM; 50200 mm/min Very soft; use high rake and support well to reduce deformation
PP 5000~12000 1000~3000 8000~16000 700~1800 10002500 RPM; 0.100.30 mm/rev 8002500 RPM; 50180 mm/min Soft and elastic; avoid clamping distortion
PMMA / Acrylic 8000~18000 800~2500 10000~24000 500~1500 15003500 RPM; 0.050.20 mm/rev 10003000 RPM; 30150 mm/min Use polished O-flute; avoid heat cracking and chipping
PC / Polycarbonate 6000~14000 800~2200 8000~18000 500~1400 12003000 RPM; 0.050.20 mm/rev 8002500 RPM; 30150 mm/min Tough but stress-crack sensitive; avoid solvent fluids
ABS 5000~12000 1000~2500 8000~16000 600~1600 12003000 RPM; 0.080.25 mm/rev 8002500 RPM; 40180 mm/min Easy to machine; moderate burrs; good chip evacuation needed
PVC 4000~10000 800~2200 6000~14000 500~1400 10002500 RPM; 0.080.25 mm/rev 8002200 RPM; 40160 mm/min Avoid overheating; decomposition can release HCl gas
PTFE 3000~8000 600~1800 5000~12000 400~1200 8002000 RPM; 0.080.25 mm/rev 5001800 RPM; 30120 mm/min Very soft, high expansion, creeps under clamp pressure
PEEK 4000~9000 700~2000 6000~12000 400~1200 10002500 RPM; 0.050.20 mm/rev 8002200 RPM; 30150 mm/min Use carbide; anneal precision parts; PCD for filled grades
PEI / Ultem 4000~9000 600~1800 6000~12000 400~1100 10002200 RPM; 0.050.18 mm/rev 7002000 RPM; 30120 mm/min Stress-sensitive; avoid aggressive coolants and heavy finishing cuts
PSU / PPSU 4000~9000 600~1800 6000~12000 400~1100 10002200 RPM; 0.050.18 mm/rev 7002000 RPM; 30120 mm/min Stress-relieve for tight tolerance; avoid solvent exposure
PPS 4000~9000 700~1800 6000~12000 400~1100 10002200 RPM; 0.050.18 mm/rev 7002000 RPM; 30120 mm/min Stable high-performance plastic; filled grades are abrasive
PI / Polyimide 3000~8000 400~1400 5000~10000 300~900 8002000 RPM; 0.030.15 mm/rev 5001800 RPM; 20100 mm/min Expensive; use conservative passes and excellent dust extraction
Glass-/carbon-filled grades 3000~8000 400~1600 5000~10000 300~1000 8002200 RPM; 0.030.18 mm/rev 5001800 RPM; 20120 mm/min Abrasive; PCD/diamond recommended; monitor tool wear closely

2.3 Speeds, Feeds, and Chip Load

Parameter Practical Guidance
Surface speed Plastics can run fast, but the limit is usually heat, melting, chip evacuation, or part rigidity rather than spindle power
Chip load Do not feed too lightly. A real chip is needed to remove heat; rubbing creates more heat than cutting
Feed override Increase carefully if chips are powdery or the tool is rubbing; decrease if the part deflects or finish tears
Tool runout Runout causes one flute to rub and overheat; use good collets and short tool stick-out
Warm-up effects Measure critical dimensions after the part returns to room temperature, not immediately after hot cutting

2.4 Depth of Cut and Finishing Strategy

Operation Typical Strategy Notes
Rough milling Moderate radial engagement, controlled axial depth Remove material efficiently but avoid heating the whole part
Slotting Use air blast and chip clearance; reduce engagement when chips pack Slotting traps heat and chips more than side milling
Finishing pass Leave 0.1~0.5mm stock for final cut on many plastics Use a sharp tool and stable feed; avoid spring passes that only rub
Thin walls Machine in steps and leave support material as long as possible Final wall thickness should be reached late in the process
Precision parts Rough → anneal/rest → finish Reduces stress movement and dimensional drift

💡 For many plastic parts, one clean finishing pass is better than several rubbing spring passes.

2.5 Drilling Deep Holes

Deep drilling is one of the most common causes of melting and oversize holes in plastics because chips pack inside the flute and heat cannot escape.

Hole Type Recommended Method Key Tips
Shallow holes Standard sharp drill or carbide drill Use controlled feed; avoid dwelling at the bottom
Deep holes Peck drilling Retract often to clear chips and cool the drill
Small holes High RPM, light but positive feed Prevent drill wander; use spot drill if needed
Large holes Step drilling, boring, or interpolation Reduces heat and grabbing compared with forcing a large drill
Through holes Back up the exit side Prevents breakout, chipping, and burrs

Peck drilling reference: for holes deeper than 3×D, start with pecks around 0.5×D~1×D and adjust based on chip evacuation. For very soft plastics or sticky chips, peck more frequently.

2.6 Tapping and Threading Tips

Threading Method Best Use Recommendations
Cut taps General plastics, low to medium volume Use sharp taps, generous chip clearance, avoid bottom dwell
Form taps Tough ductile plastics such as nylon or POM in some cases Test first; forming increases stress and may distort thin walls
Thread milling Precision internal threads, expensive parts, difficult materials Lower cutting pressure and better size control
Single-point turning External/internal lathe threads Use sharp insert, support slender parts, avoid heat buildup
Thread inserts Repeated assembly, high load, soft plastics Consider metal threaded inserts, helicoils, or molded-in alternatives

⚠️ Threads in plastics are weaker than metal threads and can creep under load. Increase thread engagement, use inserts, or design larger thread forms when repeated assembly is required.

3. Cooling & Chip Evacuation

3.1 Why Heat Control Matters

Heat control is not only about surface finish. It affects part size, safety, dimensional stability, and material integrity.

Heat-Related Problem What Happens Typical Cause
Melting / smearing Material sticks to tool or surface becomes glossy and deformed Dull tool, low feed, poor chip evacuation
Gumming Chips weld to the tool and are recut Soft plastics, unpolished flute, too much heat
Thermal expansion Part measures differently hot vs cold Long cycle time, heavy cutting, no rest before inspection
Warping Stock stress releases unevenly as material is removed Aggressive roughing, asymmetric material removal
Cracking / crazing Fine cracks appear after machining or cleaning Residual stress plus incompatible coolant/solvent
Decomposition fumes Material chemically breaks down Severe overheating; e.g., PVC may release HCl, PTFE fumes can be hazardous

⚠️ Never allow plastic to burn, smoke, or smolder in the cut. Stop machining, inspect the tool, improve chip evacuation, and increase ventilation.

3.2 Air Blast — The Default Choice ✅

For most plastic CNC machining, compressed air blast is the first choice.

Benefit Explanation
Chip evacuation Removes chips before they are recut
Heat removal Carries heat away with chips and airflow
Clean process Avoids coolant absorption, staining, and chemical compatibility problems
Visual control Operator can easily see chip formation and surface quality

📌 Use enough air to clear chips, but avoid blowing thin sheets or small parts out of position.

3.3 Coolant and Cutting Fluid Cautions

Water-soluble coolant may be useful for drilling, tight-tolerance work, or heat-sensitive operations, but plastics require compatibility checks.

Coolant Issue Materials of Concern Risk
Moisture absorption PA/nylon, some PET/PBT grades Dimensional growth, reduced stiffness, post-machining size change
Stress cracking / crazing PC, PMMA, PSU, PEI, some transparent plastics Cracks may appear after machining or cleaning
Chemical attack PS, ABS, PC, PMMA, PSU/PEI depending on fluid chemistry Surface whitening, cracking, embrittlement
Residue contamination Medical, food, optical, semiconductor parts Cleaning difficulty and inspection problems
Solvent-based fluids Most plastics Swelling, softening, stress cracking, safety risk

❌ Avoid aggressive solvent-based cutting fluids unless the material supplier explicitly approves them.

3.4 Coolant Recommendations by Material

Material Preferred Cooling Water-Soluble Coolant Special Notes
POM / Acetal Air blast ✅ Usually acceptable Avoid strong solvents; keep heat low to prevent fumes from overheating
PA / Nylon Air blast for precision; dry machining preferred ⚠️ Use cautiously Hygroscopic; dry stock and account for moisture growth
PE / PP / UHMW-PE Air blast ✅ Usually acceptable Soft chips can wrap; prioritize chip evacuation
PMMA / Acrylic Air blast or approved acrylic coolant ⚠️ Test first Stress-crack sensitive; avoid alcohol/solvent cleaners
PC / Polycarbonate Air blast ⚠️ Test carefully Very sensitive to stress cracking with incompatible fluids
ABS Air blast ⚠️ Usually possible, test first Some fluids can affect surface appearance
PVC Air blast ✅ Possible Avoid overheating; provide ventilation for HCl risk if overheated
PTFE Air blast and extraction ⚠️ Limited benefit Avoid overheating; fumes from thermal decomposition are hazardous
PEEK Air blast; coolant for drilling if approved ✅ Often acceptable Dry and stable; filled grades need strong chip extraction
PEI / PSU / PPSU Air blast ⚠️ Test first Stress-sensitive amorphous plastics; avoid solvent chemistry
PPS Air blast ✅ Often acceptable Filled grades are abrasive; extraction helps remove dust
PI Air blast + dust extraction ⚠️ Usually dry preferred Fine dust control is important; expensive material, test first

3.5 Vacuum and Chip Extraction

Situation Recommended Extraction
Routing sheet plastic Vacuum table plus chip/dust extraction hood
Filled high-performance plastics Local extraction to capture abrasive dust and fibers
PTFE, PVC, POM overheating risk Strong ventilation; stop immediately if odor/smoke appears
Optical plastics Clean air blast and vacuum to prevent chip scratching
Manual deburring / sanding Dust extraction and respiratory protection

💡 Good chip evacuation is often more effective than simply adding coolant. If chips stay in the cut, heat stays in the cut.

4. Annealing & Stress Relief

4.1 Why Annealing Matters ⭐

Plastic rods, plates, and tubes often contain internal stress from extrusion, casting, compression molding, or cooling. CNC machining then removes material unevenly and adds machining-induced stress. Without stress relief, precision plastic parts may move after machining.

Stress Problem Result on Finished Part
Residual stress in stock Warping after roughing or after unclamping
Machining-induced heat stress Dimensional drift after cooling
High clamping stress Part springs back after release
Solvent/coolant exposure on stressed parts Crazing, cracking, whitening
Thin-wall machining Bowing, twisting, and tolerance loss

Annealing helps prevent:

  • Warping after rough machining
  • Cracking or crazing during use
  • Dimensional drift after inspection
  • Flatness loss in plates and thin walls
  • Unexpected movement after pockets or slots are opened

4.2 Recommended Workflow: Rough → Anneal → Finish

1. Inspect and condition stock
2. Rough machine, leaving finishing allowance
3. Deburr sharp stress risers lightly
4. Anneal / stress-relieve according to material supplier schedule
5. Slow cool to room temperature
6. Allow part to stabilize
7. Finish machine critical faces, bores, and datums
8. Inspect after the part returns to room temperature
Workflow Stage Purpose Practical Note
Roughing Remove most material and release bulk stress Leave stock on all precision surfaces
Annealing Relax internal stress before final sizing Use slow heating and slow cooling
Stabilization Allow temperature equalization Do not inspect precision dimensions while warm
Finishing Achieve final tolerance and surface finish Use light, sharp, low-stress cuts

💡 For tight-tolerance plastic parts, finishing without prior stress relief often means chasing a moving target.

4.3 Reference Annealing Temperatures by Material Family

⚠️ Always follow the raw material supplier’s specific annealing schedule. Exact temperature, holding time, and cooling rate depend on grade, stock shape, thickness, crystallinity, filler content, and prior processing history.

Material Reference Annealing / Stress-Relief Approach Typical Notes
POM / Acetal 140~160 ℃ Common stress-relief range; slow furnace cooling; useful before finish machining precision gears, plates, and bushings
PA / Nylon Approx. 80~120 ℃, depending on grade Dry before machining if required; moisture conditioning may be needed after machining for final service dimensions
PC / Polycarbonate Approx. 120~125 ℃ Stress-crack sensitive; use controlled heating and avoid incompatible fluids after machining
PMMA / Acrylic Approx. 70~90 ℃; commonly around 80 ℃ Helps reduce crazing/cracking; slow cooling is critical for optical parts
ABS Approx. 70~90 ℃ Use for improved dimensional stability on larger parts; avoid overheating near softening range
PVC Approx. 55~70 ℃ Keep well below heat distortion risk; ventilate and avoid overheating
PTFE Supplier-specific; often requires controlled thermal cycling Very high expansion and creep; stress relief must be matched to grade and part geometry
PEEK Multi-step stress relief, e.g. 150 ℃ → 200 ℃ stages High-performance parts often benefit from rough → anneal → finish; filled grades need grade-specific schedules
PEI / Ultem Approx. 160~180 ℃ Amorphous and stress-sensitive; slow heating/cooling helps prevent cracking
PSU / PPSU Approx. 150~170 ℃ Use for tight-tolerance parts and to reduce stress cracking risk
PPS Approx. 130~160 ℃ Filled grades may need controlled schedules to reduce movement
PI / Polyimide Supplier-specific high-temperature schedule Expensive material; always use certified stock and supplier process data

4.4 Heating, Holding, and Cooling Rules

Rule Recommendation
Heat slowly Avoid steep temperature gradients between surface and core
Hold by thickness A common starting point is 30~60 min per 25mm wall thickness, but supplier schedules override this
Support the part Lay parts flat or fixture gently to prevent sagging during heating
Cool slowly Furnace cooling or controlled cooling reduces new stress
Avoid quenching Rapid cooling can lock in new stress or warp the part
Record process Track temperature, time, material lot, and dimensional change for repeat jobs

📌 Annealing improves stability, but it cannot correct poor machining strategy, overclamping, or overheated cutting.

5. Workholding & Fixturing

5.1 Why Plastic Workholding Is Different

Plastic parts often fail tolerance not because the toolpath is wrong, but because the part moved, flexed, warmed up, or relaxed after unclamping.

Challenge Cause Result
Clamp deformation Soft material compressed by vise or clamps Part springs back after release; dimensions change
Thin-wall chatter Low stiffness and poor support Poor finish, tapered walls, cracked corners
Slender part deflection Cutting force bends the workpiece Oversize/undersize features, oval turned parts
Vacuum leakage Porous spoilboard, small contact area, warped sheet Part shift or vibration
Thermal movement High coefficient of thermal expansion Size changes during cycle and inspection
Stress imbalance Heavy material removal on one side Bowing or twisting after roughing

5.2 Mechanical Clamping Best Practices

Practice Why It Works
Distribute clamping force Prevents local dents, creep, and distortion
Use soft jaws Matches part profile and increases contact area
Use parallels and full support Prevents bending during cutting
Clamp on sacrificial stock when possible Keeps precision surfaces free from clamp marks
Use torque control Improves repeatability from part to part
Avoid overhanging stock Reduces vibration and dimensional error

⚠️ If a plastic part measures correctly in the vise but incorrectly after release, suspect clamping deformation first.

5.3 Vacuum Tables and Sheet Fixturing

Fixturing Method Best For Advantages Cautions
Vacuum table Sheet, plate, nested routing Even holding force, fast loading Needs enough surface area; leaks reduce holding force
Fixture plate with screws Repeatable production parts Positive location, strong holding Screw pressure can distort soft plastics
Double-sided tape Thin sheet, prototypes, light finishing Good support, no clamp obstruction Adhesive cleanup; heat may soften tape
CA glue + tape method Small thin parts Strong temporary bond Test chemical compatibility; avoid brittle/stressed transparent plastics
Sacrificial tabs Profile cutting Prevents part movement at breakthrough Requires deburring and tab removal
Potting / support wax Flexible or delicate parts Supports thin walls and irregular shapes Extra process time; temperature compatibility needed

5.4 Thin Walls, Slender Parts, and Precision Features

Feature Type Recommended Strategy
Thin walls Leave walls thick during roughing; finish both sides progressively; support with sacrificial material
Deep pockets Rough in layers; clear chips; leave uniform finishing stock
Long slots Machine symmetrically where possible; avoid releasing one side completely early
Slender turned shafts Use tailstock, steady rest, sharp tools, light cuts, and multiple passes
Flat plates Face both sides in balanced steps; rest or anneal before final thickness
Precision bores Drill undersize, then bore/ream after stress relief if tolerance is tight

5.5 Balance Stress During Machining ⭐

Good Practice Poor Practice
✅ Remove material symmetrically from both sides ❌ Hog out one side completely, then flip
✅ Leave material for a final stress-relieved pass ❌ Finish critical surfaces before roughing nearby pockets
✅ Let warm parts cool before final inspection ❌ Inspect immediately after heavy cutting
✅ Use rough → anneal → finish for precision parts ❌ Expect extruded stock to remain flat after heavy machining
✅ Support thin walls until the final operation ❌ Cut delicate features early and expose them to later forces

💡 For high-precision plastic machining, the fixture, sequence, and stress strategy are as important as the cutting parameters.

6. General Best-Practice Checklist

Use this checklist before starting a plastic CNC job, especially for tight-tolerance, thin-wall, transparent, or high-value materials.

Check Item Requirement
✅ Sharp tools installed Use dedicated sharp plastic tools when possible; inspect for edge wear
✅ Correct geometry selected Positive rake, polished flutes, sufficient chip gullets, correct flute count
✅ Heat is managed Use air blast, proper feed, no dwell, no chip recutting
✅ Part is supported Use soft jaws, vacuum, fixture plates, or backing support for thin areas
✅ Clamping force is controlled Avoid crushing, bowing, or distorting soft plastics
✅ Stress-relief plan exists Rough → anneal → finish for precision parts or stress-sensitive materials
✅ Hygroscopic materials are dried Dry PA/nylon and other moisture-sensitive grades when required
✅ Moisture growth is considered Account for post-machining dimensional change in nylon and similar materials
✅ Thermal expansion is considered Inspect at stable room temperature; avoid chasing hot dimensions
✅ Parameters are tested on scrap Validate chip shape, finish, burrs, and size before cutting production parts
✅ Coolant compatibility is verified Avoid stress cracking, swelling, or residue problems
✅ Ventilation/extraction is active Especially for PVC, PTFE, POM overheating risk, and filled/dusty materials
✅ Deburring method is defined Prevent scraping, whitening, or rounding precision edges excessively
✅ Inspection timing is controlled Let parts cool and stabilize before final measurement

Quick Operator Rules

Rule Reason
Cut, do not rub Rubbing creates heat and poor finish
Make chips, then remove chips Chips carry heat away; recutting chips damages the surface
Clamp gently but securely Plastics deform under pressure but can still move if underclamped
Finish after stress is released Precision surfaces should be cut after roughing movement has occurred
Stop if you smell decomposition fumes Odor/smoke means unsafe overheating or material breakdown

🔗 Related Pages