Machining
Chipping is a cutting-parameter problem. Cracking is a stress problem. They appear at the same moment and need different fixes, which is why changing only the feed rate rarely solves both.
A part comes off the router with a chipped edge, or it looks fine and cracks a week later at a hole. Both get blamed on “bad material” and both are actually process problems with different mechanisms.
Chipping happens during the cut. The tool exits the material and takes a fragment of the edge with it. It is a function of feed rate, spindle speed, tool geometry and how well the part is held.
Cracking happens after the cut, or weeks later. It is a function of residual stress — from the sheet, from machining, or from the cut itself — concentrated at a feature like a hole or a sharp internal corner.
Fixing the feed rate addresses the first and does nothing for the second. That is why the same part can come back twice with different complaints.
Feed rate. Too fast and the tool grabs rather than cuts, and the exit edge breaks away. Too slow and the material melts onto the tool, which then drags and chips worse on the next pass.
Spindle speed. Acrylic softens with heat. High spindle speed with a slow feed generates heat faster than the chip can carry it away, and the material welds to the cutting edge.
Tool geometry. Single-flute “O-flute” tools designed for plastics cut cleaner than general-purpose wood or metal router bits, because the single flute gives a large chip clearance and less rubbing. A two-flute tool in acrylic usually runs hotter and chips more.
Workholding. A part that vibrates will chip no matter what the parameters are. Vacuum tables and sacrificial backing boards both help, and for thin sheet the backing matters as much as the tool.
| Symptom | Most likely cause | First thing to change |
|---|---|---|
| Chipping on the exit edge | Feed too fast, or no backing support | Slow feed 20%, add sacrificial backing |
| Material welded to the tool | Spindle too fast or feed too slow — heat build-up | Reduce spindle speed, increase feed |
| Melted, stringy chips | Excessive heat; blunt tool | New tool, lower rpm, higher feed |
| Chipping on both edges of a slot | Tool deflection, too small a diameter for the depth | Larger tool or multiple shallower passes |
| Clean cut but cracked later | Residual stress — not a cutting problem | Anneal, change hole placement |
Laser cutting produces a different edge character than routing, and which one is better depends on the application.
| CNC routed | Laser cut | |
|---|---|---|
| Edge finish | Matte, machined, can be polished to clear | Glossy, slightly rounded, flame-polished look |
| Edge clarity | Opaque until polished | Semi-clear, never fully clear |
| Internal stress | Moderate | Higher locally at the cut |
| Thickness range | 2–50 mm | Up to about 20 mm practically |
| Tolerance | ±0.1 mm achievable | ±0.1 mm on thin sheet, wider on thick |
| Best for | Thick parts, tight tolerance, polishable edge | Thin sheet, intricate profiles, fast turnaround |
A common mistake is specifying a laser-cut edge where a polished clear edge is needed. Laser edges cannot be polished to full optical clarity because the cut zone has a different material structure. If the edge will be visible at close range on clear sheet, routing plus diamond polishing is the right route.
Holes are where stress concentrates, and three things make it worse.
Hole too close to the edge. The remaining ligament is too thin to carry the load, and the crack runs from the hole to the edge. Keep at least 1.5× the hole diameter of material between the hole edge and the part edge — 2× on anything load-bearing.
Sharp internal corners. A square-cornered pocket or slot has a stress concentration factor several times that of a radiused one. Internal radii should be at least half the tool diameter, ideally the full diameter.
Fastener bearing directly on acrylic. A bolt tightened onto acrylic concentrates load at the hole edge and, combined with vibration, cracks it. Compliant washers, bushings or a metal insert all help. Threads should never be cut directly into acrylic for anything load-bearing.
| Feature | Minimum | Recommended |
|---|---|---|
| Hole edge to part edge | 1.5 × diameter | 2 × diameter |
| Hole to hole | 2 × diameter | 3 × diameter |
| Internal corner radius | 0.5 × tool diameter | 1 × tool diameter |
| Thread in acrylic | Not recommended | Use insert or through-bolt |
| Slot width | 1.2 × tool diameter | 1.5 × tool diameter |
Starting points for single-flute carbide in cast acrylic. Real values depend on the machine, the tool and the geometry — these are where we start, not where we finish.
| Thickness | Tool diameter | Spindle (rpm) | Feed (mm/min) | Depth per pass |
|---|---|---|---|---|
| 3 mm | 3 mm | 18,000 | 2,500 | 1.5 mm |
| 5 mm | 4 mm | 16,000 | 2,200 | 2.5 mm |
| 8 mm | 6 mm | 14,000 | 2,000 | 3 mm |
| 10 mm | 6 mm | 12,000 | 1,800 | 3.5 mm |
| 15 mm | 8 mm | 10,000 | 1,600 | 4 mm |
| 20 mm | 10 mm | 9,000 | 1,400 | 5 mm |
The patterns worth remembering: spindle speed goes down as thickness goes up, and depth per pass should not exceed about half the tool diameter. Violating either produces heat, and heat produces both chipping and weld.
Chipping is sometimes repairable, depending on depth.
Light chips, under 0.2 mm. Sand progressively — 400, 800, 1200 grit — then polish with a compound. On a straight edge this can restore a fully clear finish.
Moderate chips, 0.2–0.5 mm. The edge will need to be re-machined or sanded back, which changes the dimension. Acceptable on a non-critical edge, not on a fit face.
Deep chips or cracks. Not repairable. A crack in acrylic propagates, and a part with a visible crack will fail in service.
Where a chipped edge is on a visible face and the dimension cannot change, the part is scrap. This is why the parameters matter more than the polishing skill — polishing recovers cosmetics, not geometry.
Instrument panel, 5 mm, 200 holes. Chipping on the exit side of every hole. Cause: drill bit with too aggressive a point angle and no backing. Fixed with a plastic-specific drill geometry, a backing board, and peck drilling.
Machine guard, 15 mm, large cut-outs. Clean cuts, cracks appearing at the corner radii two weeks later. Cause: internal radius smaller than the tool, plus no annealing. Fixed by increasing the radius and annealing after machining.
Display shelf, 6 mm, polished edges. Chipping along the top edge only. Cause: the sheet was not supported at the exit and the top edge was the last to be cut. Fixed with a sacrificial backing board.
Bonded housing, 10 mm. No chipping, but solvent-bonded joints failing. Cause: the machined faces had micro-chips creating a poor bond line, which is chipping measured at the wrong scale.
What to check on a machined acrylic part:
Edge. Inspect under grazing light. Chips larger than 0.2 mm on a visible edge are a defect; on a hidden edge, agree a limit in advance.
Holes. Check for cracks radiating from the hole, especially on the exit side. A crack may not be visible head-on — inspect at an angle.
Dimensions. On the critical features, at the agreed reference temperature.
Stress. For anything that will see solvent or load, ask whether it was annealed. If the answer is no and the part is thick or heavily machined, ask why.
The bottom is usually the exit side, where the tool pushes material out without support. A sacrificial backing board underneath — MDF or a dedicated spoil board — solves most of it. Reducing feed by 20% also helps but the backing is the bigger lever.
It works but chips more. A drill ground for plastics has a shallower point angle and less rake, which reduces the grabbing that causes exit chipping. Backing the exit side and pecking to clear chips matters as much as the drill geometry.
Residual stress releasing. Machining unbalances the stress in the sheet, and the part moves toward a new equilibrium, concentrating stress at holes and sharp corners. Annealing after machining releases it before it can crack.
Laser for thin sheet, intricate outlines and fast turnaround. CNC for thick parts, tight tolerance, and any edge that has to be polished clear. If the edge will be visible at close range on clear sheet, CNC plus diamond polishing is the only route to a truly clear edge.
Whether an edge will be polished, bonded or left as-machined changes the process. Tell us which, and we will quote the route that gets there without rework.
