CNC Machining of Plastics
CNC (Computer Numerical Control) routing is the most versatile method for cutting, drilling, engraving, and shaping acrylic and engineering plastics. This article covers 3-axis vs 5-axis machines, cutting parameters for common materials, tool selection, achievable tolerances, chip evacuation strategies, and troubleshooting of common machining defects.
Table of contents
1. 3-Axis vs 5-Axis CNC Routing
3-Axis CNC
The cutting tool moves along three linear axes (X, Y, Z). The workpiece remains stationary on the vacuum table. This is the standard configuration for flatbed routing of sheet plastics — cutting profiles, pockets, drilled holes, and engraved text. Suitable for the vast majority of acrylic fabrication work: display cases, signage panels, protective covers, and custom shapes.
5-Axis CNC
Adds two rotational axes (typically A and B or A and C) to the three linear axes, allowing the cutter to approach the workpiece from virtually any angle. Essential for machining complex 3D shapes: contoured surfaces, undercuts, bevelled edges at non-standard angles, and multi-sided parts in a single setup. Used in PlexiSystem for precision components, moulds, and high-end architectural elements.
| Feature | 3-Axis CNC | 5-Axis CNC |
|---|---|---|
| Typical applications | Flat profiles, pockets, holes, engraving | 3D contours, undercuts, bevels, multi-face parts |
| Setup complexity | Low — vacuum hold-down | High — fixtures, probing |
| Programming | 2D CAM (DXF input) | 3D CAM (STEP/IGES input) |
| Edge finishing | Vertical edges only (90°) | Any angle, chamfers, complex profiles |
| Cost per part | Lower | Higher (more setup, longer cycle) |
| Typical tolerance | ±0.1 mm | ±0.05 mm |
When to choose 5-axis
If your part has any of these features, 5-axis machining is likely necessary: non-perpendicular edges, sculpted surfaces, multiple machined faces requiring sub-0.1 mm alignment, or complex pocket shapes that would require multiple setups on a 3-axis machine. Contact us with your STEP file and we will advise on the optimal approach.
2. Tool Selection
Choosing the correct cutter geometry is critical for plastics. Unlike metals, plastics are poor thermal conductors — heat generated during cutting stays in the cut zone, causing melting, discolouration, and poor edge quality. The key principles:
- Single-flute (O-flute): The workhorse for acrylic and most plastics. Large chip clearance prevents re-welding of chips to the edge. Produces the cleanest cuts in PMMA, PET-G, and polycarbonate.
- Two-flute spiral: Higher feed rates possible but generates more heat. Suitable for harder materials like HPL, or when surface finish is less critical.
- Compression cutter: Upcut on the bottom, downcut on top. Prevents chipping on both faces of the sheet. Ideal for laminated materials, PVC foam, and thin sheets.
- Diamond-coated (PCD): For abrasive materials like HPL, glass-filled nylon, and carbon fibre composites. Extremely long tool life but high initial cost.
- Ball-nose: Used on 5-axis machines for 3D contouring. Produces scalloped surface that may require finishing.
| Cutter type | Diameter | Best for | Avoid with |
|---|---|---|---|
| Single-flute O-flute | 3–8 mm | PMMA, PET-G, PC, ABS | HPL (too soft, dulls quickly) |
| Two-flute upcut spiral | 3–12 mm | HIPS, PVC, nylon, Delrin | Clear PMMA (may cause heat haze) |
| Compression cutter | 5–10 mm | PVC foam, laminates, thin sheet | Thick solid plastics (>10 mm) |
| PCD diamond | 3–8 mm | HPL, Corian, composites | Soft plastics (overkill) |
| Ball-nose end mill | 2–10 mm | 3D contouring (5-axis) | 2D profiles (use flat end mill) |
Tool sharpness matters
Dull tools are the single most common cause of poor edge quality in plastics machining. Unlike metals, where a slightly worn tool still cuts, plastics will melt and smear with a dull edge. Replace or resharpen cutters at the first sign of edge degradation — milky edges on clear acrylic, burr formation, or increased cutting noise. Track tool usage in metres of cut to establish replacement intervals.
3. Cutting Parameters by Material
The table below provides starting parameters for CNC routing of common plastics. These values assume a single-flute O-flute cutter of 6 mm diameter on a machine with at least 18,000 RPM spindle speed. Adjust based on your specific machine rigidity and material batch.
| Material | Spindle speed (RPM) | Feed rate (mm/min) | Depth of cut (mm) | Notes |
|---|---|---|---|---|
| PMMA (cast) | 18,000–24,000 | 2,000–4,000 | Full thickness (up to 15 mm) | Use compressed air. Produces clear chips. |
| PMMA (extruded) | 18,000–22,000 | 2,500–4,500 | Full thickness (up to 10 mm) | More prone to melting than cast. Faster feed helps. |
| PET-G | 16,000–20,000 | 1,500–3,000 | Full thickness (up to 8 mm) | Gummy chips. Compressed air essential. |
| Polycarbonate | 18,000–24,000 | 2,000–4,000 | Full thickness (up to 12 mm) | Long stringy chips. Good vacuum extraction needed. |
| HIPS | 18,000–24,000 | 3,000–5,000 | Full thickness (up to 6 mm) | Easy to cut. Low melting point — keep feed high. |
| PVC foam (Forex) | 18,000–24,000 | 3,000–6,000 | Full thickness (up to 19 mm) | Use compression cutter. Fine dust — good extraction. |
| HPL | 18,000–24,000 | 1,500–3,000 | Full thickness (up to 12 mm) | Very abrasive. PCD or carbide tools only. |
| POM (Delrin) | 18,000–22,000 | 2,500–4,000 | Up to 10 mm | Machines beautifully. Clean chip formation. |
Chip load formula
Chip load = Feed rate / (RPM × number of flutes). For single-flute cutters in acrylic, target a chip load of 0.10–0.20 mm/tooth. Too low (dust instead of chips) means the tool is rubbing, generating heat. Too high means risk of chipping or tool breakage. The optimal chip load produces clean, curly chips with no discolouration.
4. Achievable Tolerances
CNC routing of plastics can achieve excellent dimensional accuracy, but tolerances depend on machine calibration, material properties (thermal expansion, internal stresses), and cutting strategy.
| Tolerance class | Linear (mm) | Hole diameter (mm) | Requirements |
|---|---|---|---|
| Standard production | ±0.15 | ±0.10 | Standard CNC setup, vacuum hold-down |
| Precision | ±0.10 | ±0.05 | Calibrated machine, climate control, stress-relieved material |
| High precision (5-axis) | ±0.05 | ±0.03 | Precision fixtures, probing, temperature-stable environment |
Thermal expansion
Plastics have a coefficient of thermal expansion 5–10 times greater than metals. A 1-metre PMMA sheet changes length by approximately 0.07 mm per 1 °C temperature change. If your workshop temperature fluctuates by 10 °C during the day, that is a 0.7 mm variation on a 1-metre part. For precision work, condition the material in the machining environment for at least 24 hours before cutting.
5. Chip Evacuation & Cooling
Compressed air
The most common cooling method for plastics. Directed at the cutting zone, it removes chips and provides some cooling without introducing liquids that could stain or stress-crack the material. Essential for PMMA and PET-G.
Vacuum extraction
Integrated dust collection is critical for PVC foam (fine dust), HPL (abrasive dust hazardous to the respiratory system), and any high-volume production. A well-designed extraction system improves both cut quality and workshop air quality.
Mist cooling
Oil mist or water mist can be used for polycarbonate and nylon to improve surface finish in deep pocketing operations. However, mist can cause stress cracking in cast PMMA — never use on acrylic unless specifically tested and approved.
6. Common Errors & Troubleshooting
| Symptom | Likely cause | Solution |
|---|---|---|
| Melted or welded edges | Feed rate too low, dull tool, too many flutes | Increase feed, sharpen/replace tool, switch to single-flute |
| Chipped edges | Feed rate too high, wrong cutter direction, brittle material | Reduce feed, use climb milling, check material grade |
| Milky/frosted edge on clear PMMA | Micro-cracks from vibration or dull tool | Reduce vibration, replace tool, add finishing pass at light depth |
| Stringy chips wrapping around tool | Material too soft (PET-G, nylon), poor extraction | Increase compressed air, reduce depth of cut per pass |
| Dimensional inaccuracy | Material not flat, thermal expansion, worn tool | Flatten material, temperature-condition, measure tool diameter |
| Burn marks on edge | RPM too high for feed rate, chip re-cutting | Increase feed or reduce RPM, improve chip evacuation |
| Surface scratches | Chips dragging across surface, poor hold-down | Leave protective film on, improve vacuum hold-down, clean table |
7. Surface Finish Quality
CNC-routed edges in plastics range from functional (suitable for bonding or hidden edges) to near-optical quality, depending on the cutter, parameters, and material. For the best possible edge finish directly from the machine:
- Use a sharp single-flute O-flute cutter with polished flute
- Run a roughing pass leaving 0.3–0.5 mm stock, then a finishing pass at full depth with high feed
- Use climb milling (cutter rotation matches feed direction) for the finishing pass
- Ensure rigid workholding — no vibration
- Keep compressed air directed at the cut zone
If the CNC-routed edge is not sufficient for visible applications, post-process with flame polishing or diamond buffing to achieve full optical clarity.
PlexiSystem CNC capabilities
Our production floor includes 3-axis flatbed CNC routers with 2000×3000 mm working area and 24,000 RPM spindles. We process sheets up to 20 mm thick in a single pass for most materials. For complex 3D parts, we offer 5-axis machining with ±0.05 mm tolerance. See our machinery page for specifications.
Related articles
- Material Guide — properties and machinability of each plastic
- Laser Cutting — alternative cutting method, when to choose laser vs CNC
- Surface Finishing — post-machining edge polishing and treatment
- Designer’s Guide — DXF file preparation and design rules for CNC
- Joining Techniques — edge preparation requirements for bonding