Plastic CNC Cutting Parameters — Quick Reference
Last updated: May 23, 2026
Plastic CNC Cutting Parameters — Quick Reference
← Back to the Plastic Materials Handbook
⚠️ Important disclaimer — STARTING POINTS ONLY
The parameters below are reference starting points, not fixed production settings. Actual values depend on machine rigidity, tool diameter, tool material, tool sharpness, flute geometry, part geometry, wall thickness, fixturing, coolant/air blast, stock stress, and required tolerance. Always test on scrap material first, inspect chip formation and surface finish, then adjust step by step.
1. How to Read This Table
This page is intended as a shop-floor quick reference for common plastic CNC machining jobs. It uses metric units throughout.
| Term | Meaning | Practical Note |
|---|---|---|
| RPM | Spindle speed in revolutions per minute | Higher RPM can improve finish, but too much heat causes melting, gumming, or stress cracking |
| Feed (mm/min) | Linear feed rate for milling and drilling | Feed must be high enough to make chips, not dust or melted plastic |
| Feed (mm/rev) | Feed per spindle revolution for turning | Common for lathes; increase gradually if chips are too fine or heat builds up |
| Depth of Cut (mm) | Radial/axial material removed per pass | Reduce depth for thin walls, weak fixturing, brittle materials, or tight tolerances |
| Surface Speed | Cutting speed at the tool/workpiece surface | Larger tools reach higher surface speed at the same RPM, so large cutters usually need lower RPM |
💡 General plastic rule: plastics usually tolerate high spindle speeds with moderate feeds, but the correct balance is chip evacuation and heat control. A sharp tool making continuous chips is normally better than a dull tool rubbing at high RPM.
📌 For small end mills, RPM may need to be near the upper end of the range. For large cutters, filled grades, thin-wall parts, or weak setups, start at the lower end.
2. Master Milling Parameters Table
Typical tools: sharp carbide end mills, 13 flutes, polished flutes, high rake angle, air blast or mist coolant when needed. Values assume common tool diameters around 310mm and stable workholding.
| Material | Rough Milling RPM | Finish Milling RPM | Feed (mm/min) | Depth of Cut rough (mm) | Notes/special |
|---|---|---|---|---|---|
| PMMA / Acrylic | 6000~12000 | 10000~18000 | 600~1800 | 0.5~2 | Brittle and crack-sensitive. Use very sharp single/2-flute tools, light finish passes, and avoid aggressive entry. Flame-polished edges may show stress if overheated. |
| ABS | 6000~12000 | 8000~16000 | 1000~2500 | 1~4 | Easy to machine but can burr or melt if rubbing. Good general-purpose starting range; use air blast for chip removal. |
| PP | 5000~10000 | 7000~14000 | 1200~3000 | 1~4 | Soft, ductile, and gummy. Use high rake, large chip space, sharp tools, and enough feed to form chips. Support thin parts well. |
| PE / HDPE / UHMW | 5000~10000 | 7000~14000 | 1200~3500 | 1~5 | Very slippery and ductile; UHMW tends to fuzz and burr. Use razor-sharp tools, climb milling, air blast, and generous chip evacuation. |
| PVC | 4000~9000 | 6000~12000 | 800~2200 | 1~3 | Machines cleanly but avoid overheating. ⚠️ Excessive heat can release corrosive/irritating fumes; use sharp tools and ventilation. |
| POM / Acetal | 5000~10000 | 8000~15000 | 1500~3000 | 1~4 | ⭐ Excellent machinability and dimensional stability. Produces clean chips and good surface finish; watch internal stress on precision parts. |
| PA / Nylon | 4000~9000 | 6000~12000 | 1000~2500 | 1~4 | Tough and elastic; may deflect or absorb moisture. Use sharp tools, firm support, and allow for dimensional change from humidity. |
| PC / Polycarbonate | 5000~10000 | 7000~14000 | 800~2200 | 0.5~3 | Tough but stress-sensitive. Use sharp tools, avoid overheating, and consider annealing for tight-tolerance or threaded parts. |
| PET / PET-P | 5000~10000 | 7000~14000 | 1000~2500 | 1~3 | Good dimensional stability and clean machining. Avoid excessive heat; use sharp tools to prevent whitening or edge chipping. |
| PEEK | 3000~8000 | 5000~12000 | 500~1800 | 0.5~2.5 | High-performance plastic; stronger and more heat resistant. Filled grades are abrasive — reduce RPM, use carbide/PCD where needed. |
| PTFE / Teflon | 3000~8000 | 5000~10000 | 800~2000 | 0.5~3 | Very soft, slippery, and deformation-prone. Use sharp tools, light clamping, support the part, and expect high thermal expansion. |
| PEI / Ultem | 3000~7000 | 5000~10000 | 500~1600 | 0.5~2 | High-temperature amorphous plastic; stress-sensitive. Use sharp carbide, light finish passes, and consider annealing for precision parts. |
| PI / Polyimide | 2500~6000 | 4000~9000 | 300~1200 | 0.3~1.5 | Very high-performance and expensive. Often brittle in thin sections; use conservative feeds, small depths, and excellent dust extraction. |
| PSU / PPSU | 3000~7000 | 5000~10000 | 500~1600 | 0.5~2.5 | Tough but heat/stress sensitive. Keep tools sharp, avoid rubbing, and use annealing for critical tolerance or threaded parts. |
| PPS | 2500~7000 | 4000~9000 | 400~1400 | 0.5~2 | Can be brittle; glass/mineral-filled grades are abrasive. Use carbide/PCD, lower RPM, light passes, and avoid edge chipping. |
⚠️ Filled materials need slower cutting. Glass-filled, carbon-filled, mineral-filled, or bearing-filled grades are more abrasive and often need 20~50% lower RPM, carbide or PCD tooling, and more frequent tool inspection.
3. Turning Parameters Table
Values below are starting points for CNC turning with sharp carbide inserts or polished high-rake tools. For small diameters, RPM may be used directly; for larger diameters, calculate from surface speed and respect chuck/workholding limits.
| Material | Speed (RPM or m/min) | Feed (mm/rev) | Depth of Cut (mm) | Notes |
|---|---|---|---|---|
| PMMA / Acrylic | 80 |
0.05~0.20 | 0.2~1.5 | Brittle; use sharp positive-rake tools and avoid interrupted cuts. Light finishing cuts reduce cracking and edge chipping. |
| ABS | 100 |
0.08~0.30 | 0.5~3 | Easy turning. Use enough feed to avoid rubbing; deburr edges after cutoff. |
| PP | 80 |
0.10~0.35 | 0.5~3 | Soft and stringy. Use chip control geometry, sharp tools, and avoid excessive clamping pressure. |
| PE / HDPE / UHMW | 80 |
0.10~0.40 | 0.5~4 | Long continuous chips are common. Use sharp tools, large rake, and safe chip management. UHMW may need very sharp cutoff tools. |
| PVC | 70 |
0.08~0.25 | 0.5~2.5 | Avoid heat buildup and fumes. Keep tools sharp and use ventilation/air blast. |
| POM / Acetal | 100 |
0.10~0.30 | 0.5~2 | ⭐ Excellent turning material. Produces stable chips and fine finish; use light finishing cuts for tight tolerances. |
| PA / Nylon | 80 |
0.10~0.35 | 0.5~3 | Elastic and moisture-sensitive. Support slender parts and account for spring-back. |
| PC / Polycarbonate | 80 |
0.08~0.25 | 0.3~2 | Tough but may develop stress whitening. Use sharp tools, moderate speed, and avoid heat. |
| PET / PET-P | 90 |
0.08~0.25 | 0.5~2.5 | Good dimensional stability. Avoid dull inserts that generate heat and smear the surface. |
| PEEK | 60 |
0.05~0.20 | 0.3~2 | High strength; use carbide and stable workholding. Filled grades require lower speed due to abrasion. |
| PTFE / Teflon | 50 |
0.08~0.30 | 0.3~2.5 | Very soft and flexible. Use minimal clamping pressure, sharp tools, and allow for thermal expansion. |
| PEI / Ultem | 50 |
0.05~0.18 | 0.3~1.5 | Stress-sensitive high-temperature plastic. Light finishing cuts and annealing improve stability. |
| PI / Polyimide | 30 |
0.03~0.15 | 0.2~1 | Expensive and often brittle. Use conservative cuts, dust extraction, and avoid chatter. |
| PSU / PPSU | 50 |
0.05~0.20 | 0.3~2 | Tough amorphous materials. Avoid heat and use sharp positive-rake tools. |
| PPS | 40 |
0.04~0.18 | 0.2~1.5 | Brittle and often filled. Lower speeds, carbide tools, and rigid setup are recommended. |
💡 Turning finish tip: for plastics, a very small final pass with a sharp tool often improves surface finish more than increasing RPM. If the tool rubs instead of cuts, increase feed slightly or use a sharper insert.
4. Drilling Parameters Table
Use sharp drills with polished flutes. For production holes, plastic-specific drills or modified drills with reduced grabbing tendency are recommended. For deep holes, chip evacuation is usually more important than pure RPM.
| Material | RPM | Feed | Peck drilling needed? | Notes |
|---|---|---|---|---|
| PMMA / Acrylic | 800~2500 | 30~150 mm/min | ✅ Yes for deep holes | Brittle and crack-prone. Use sharp drills, slow entry/exit, backup support, and avoid grabbing at breakthrough. |
| ABS | 1000~3500 | 50~250 mm/min | ⚠️ For deep holes | Easy drilling. Use air blast to clear chips and avoid melting in blind holes. |
| PP | 800~2500 | 80~300 mm/min | ✅ Usually | Soft and gummy. Peck frequently to clear long chips and prevent heat buildup. |
| PE / HDPE / UHMW | 800~2500 | 80~350 mm/min | ✅ Usually | Chips can pack in the flute. Use frequent pecking, sharp drills, and avoid excessive heat. |
| PVC | 800~2500 | 50~220 mm/min | ⚠️ For deep holes | Avoid overheating and fumes. Use sharp drills, chip evacuation, and good ventilation. |
| POM / Acetal | 1000~3000 | 50~200 mm/min | ⚠️ For deep holes | Drills cleanly. Peck for holes deeper than about 3×D and use air blast. |
| PA / Nylon | 800~2500 | 50~250 mm/min | ✅ For deep holes | Elastic material may close slightly after drilling. Ream critical holes after rough drilling. |
| PC / Polycarbonate | 800~2500 | 40~180 mm/min | ✅ Yes for deep holes | Tough but stress-sensitive. Avoid excessive heat; anneal before/after drilling for critical parts if needed. |
| PET / PET-P | 800~2500 | 50~220 mm/min | ⚠️ For deep holes | Generally clean drilling. Avoid dull drills that cause whitening or smeared holes. |
| PEEK | 600~2000 | 30~150 mm/min | ✅ Yes | Strong, heat-resistant material. Use carbide for filled grades and peck to control heat. |
| PTFE / Teflon | 500~1800 | 50~220 mm/min | ✅ Usually | Soft and deformable. Clamp lightly, support well, and expect some hole recovery/spring-back. |
| PEI / Ultem | 500~1800 | 30~120 mm/min | ✅ Yes | Stress-sensitive. Use sharp drills, conservative feed, and pecking to avoid heat cracking. |
| PI / Polyimide | 400~1500 | 20~100 mm/min | ✅ Yes | Can chip at entry/exit. Use backing material, sharp carbide drills, and dust extraction. |
| PSU / PPSU | 500~1800 | 30~130 mm/min | ✅ Yes | Tough but heat-sensitive. Peck deep holes and avoid rubbing. |
| PPS | 400~1500 | 20~120 mm/min | ✅ Yes | Brittle, especially filled grades. Use backing support, sharp carbide drills, and slow breakthrough. |
📌 Deep-hole rule: for holes deeper than 3× drill diameter, use peck drilling or high-pressure air/coolant to clear chips. Packed chips create heat quickly and can melt, seize, crack, or oversize the hole.
5. Tapping & Threading Notes
Threading plastics is not difficult, but reliable threads require sharp tools, correct hole sizing, and control of stress and heat.
| Topic | Recommendation |
|---|---|
| Tap type | Use sharp taps with good chip clearance. Spiral-flute taps are useful for blind holes; spiral-point taps are useful for through holes. |
| Thread percentage | Avoid excessive thread engagement. 60~75% thread is often stronger and safer than forcing a near-100% thread in plastic. |
| Lubrication | Use air blast, water-soluble coolant, or plastic-compatible lubricant. Avoid solvent-based fluids that attack PC, PMMA, ABS, or PSU/PPSU. |
| Single-point threading | ✅ Recommended for precision threads, large diameters, high-value materials, or stress-sensitive plastics. It gives better control than tapping. |
| Thread milling | ✅ Good option for CNC machining because cutting load is lower and chip evacuation is better than conventional tapping. |
| Annealing | ⭐ For PMMA, PC, PEI, PSU/PPSU, and other amorphous stress-sensitive plastics, anneal before threading when cracks or tight tolerances are a concern. |
| Insert threads | For repeated assembly, use metal threaded inserts, helical inserts, or molded/pressed inserts where suitable. |
Practical threading tips:
- Use sharp taps only — dull taps generate heat and radial stress.
- Use proper tapping drill size; a hole that is too small can split brittle plastics.
- Do not bottom out the tap in blind holes; leave chip space.
- For PMMA and PC, avoid alcohols and aggressive solvents after threading because they may trigger stress cracking.
- For PTFE, PE, PP, and UHMW, threads may deform under load; use longer engagement or inserts.
- For PEEK, PPS, PI, and filled grades, inspect tools frequently because abrasive fillers quickly dull cutting edges.
⚠️ Stress-cracking warning: PMMA, PC, PEI, PSU, and PPSU can crack after machining if high residual stress combines with solvents, tight threads, or press-fit inserts. Use annealing, generous radii, correct hole size, and compatible cleaning fluids.
6. Quick Adjustment Rules
Use these rules when the first test cut does not look right.
| Symptom | Likely Cause | Quick Adjustment |
|---|---|---|
| Melting / gumming | RPM too high, feed too low, dull tool, poor chip evacuation | ✅ Reduce RPM, increase feed slightly, use air blast/coolant, check tool sharpness |
| Fine powder instead of chips | Tool rubbing instead of cutting | ✅ Increase feed per tooth, use sharper tool, reduce flute count, improve chip load |
| Chipping / cracking | Feed too high, tool too aggressive, brittle material, poor support | ✅ Reduce feed, use sharper tool, reduce depth of cut, support the exit side |
| Heavy burrs / fuzzy edges | Dull tool, soft ductile plastic, conventional milling, insufficient chip load | ✅ Use sharper tool, climb milling, increase chip load slightly, add light finishing pass |
| Poor surface finish | Tool marks, chatter, heat, wrong finishing strategy | ✅ Use higher RPM with lighter finish pass, reduce depth of cut, improve fixturing, use polished sharp tools |
| Dimensional drift after machining | Internal stress release, thermal expansion, moisture absorption, asymmetric material removal | ✅ Stress-relieve/anneal, rough-machine then finish-machine, allow cooling time, compensate thermal expansion |
| Hole oversize or melted hole wall | Chips packed in drill flutes, drill rubbing, too much heat | ✅ Peck drill, reduce RPM, use sharper drill, add air blast, clear chips frequently |
| Thread cracking | Tap hole too small, dull tap, brittle/stress-sensitive material | ✅ Enlarge tap drill slightly, use sharp tap/thread mill, anneal PC/PMMA/PEI, avoid solvent exposure |
Fast shop-floor checklist:
- ✅ Melting or gumming → reduce RPM, increase feed slightly, improve cooling/chip evacuation.
- ✅ Chipping or cracking on brittle plastics → reduce feed, use a sharper tool, reduce depth of cut, support the workpiece.
- ✅ Burring or fuzzy edges → use a sharper tool, climb milling, suitable chip load, and a light finishing pass.
- ✅ Poor finish → use higher RPM only if heat is controlled; take a lighter finishing pass with a polished sharp cutter.
- ✅ Dimensional drift → use stress relief, rough/finish sequencing, symmetric stock removal, and thermal expansion compensation.
- ✅ Filled material wears tools quickly → lower RPM, use carbide/PCD, inspect edges often, and replace tools before finish deteriorates.