Basic knowledge of glass CNC processing

• 1
  How glass behaves under a rotating tool
• 2
  Which glass grades actually machine well
• 3
  Coolant, tooling and the parameters that matter
• 4
  Edge chipping, surface finish and inspection
• 5
  Design rules and where CNC stops making sense
• 6
  Glass grade and process selection

Glass does not cut the way aluminum does. There is no chip that curls away from the edge. The tool creates a controlled network of micro-cracks, and the material leaves as fine powder and small flakes. That single fact drives every parameter choice downstream: tool type, feed, depth of cut, and coolant.

The crack network is the whole game. Push the tool too hard and the cracks join up into a fracture that runs past the edge you wanted. Cut too light and the tool rubs, heats the surface, and leaves a haze that has to be polished out later. Glass CNC processing sits in a narrow band between those two failures.

Hardness matters less than you might expect. Fused silica runs around 1,100 HV and soda-lime sits near 550 HV, but both are brittle. What changes between grades is thermal shock resistance and how far the crack network spreads before it stops. Borosilicate tolerates a wider thermal window than soda-lime. Fused silica is the most forgiving of the three in a wet cut.

Internal stress decides the rest. Annealed blanks machine predictably. Tempered glass holds a locked stress field that releases the moment you break the surface, so it usually cannot be drilled or milled at all. If a drawing calls for tempered glass with holes, the part should be cut in the annealed state and tempered afterward.

Borosilicate is the default for most machined parts. It handles thermal cycling, resists most laboratory chemicals, and delivers good optical clarity after polishing. Wall thickness down to 1 mm is routine. If the part touches hot liquid or goes through an autoclave cycle, start here.

Fused silica is the choice when transmission matters across a wide spectrum, from deep UV into the infrared. It also carries the lowest thermal expansion of the common grades, which keeps a 300 mm optical window stable through a temperature swing. It costs more and grinds slower. Use it when the optical requirement is real.

Soda-lime float glass is cheap and available in large sheets, which makes it useful for windows, cover plates and decorative panels where optical grade is not required. It chips more easily and has a higher expansion coefficient, so it is a poor fit for parts that see heat cycling.

Some materials get grouped with glass but behave differently. Sapphire is far harder and must be machined with diamond tooling at very light depths. PMMA and polycarbonate are polymers, not glass, and machine with standard carbide. Keep those in separate process plans, because the coolant, tool and feed rules do not transfer.

Coolant does three jobs at once. It carries heat out of the cut zone, flushes abrasive glass powder away from the tool path, and keeps the local temperature stable so the crack network stays shallow. A dry cut on glass is a short cut. The powder re-circulates, the tool rubs, and the edge spalls.

Flood coolant with a filtered loop is the standard approach. Water-based coolant with additives keeps the pH in a range that protects both the machine and the operator. For deep pockets or fine features, a mist of compressed air and carbon dioxide can help, because it cools sharply and leaves no liquid pooling in the cut.

Tooling is almost always diamond. Electroplated diamond tools remove material fast and cost less, but they wear and change diameter over a long run. Sintered or brazed diamond tools hold size better, which matters when you are holding ±0.005 mm across thousands of parts. Standard carbide will scratch glass and dull within minutes.

Feed and speed follow the tool, not a chart. A typical starting point for a 6 mm electroplated diamond burr is 8,000 to 15,000 rpm with a feed of 100 to 300 mm/min, and a depth of cut around 0.1 to 0.3 mm per pass. Increase depth before you increase feed. Feed too high is what chips edges.

Chipping shows up at the exit side of a hole and along the edge where the tool leaves the material. The cause is normally one of three things: feed too high, no backing support at the exit, or a dull tool. Supporting the exit face with a sacrificial plate removes most exit chips, and it is the cheapest fix on the list.

Surface finish depends on grit progression. A ground surface from a coarse diamond tool lands around Ra 1.6–3.2 μm. Stepping through finer grits gets you to Ra 0.8–1.6 μm. Optical faces that need Ra 0.2–0.8 μm go through a polishing step after machining, often with a cerium oxide slurry on a lap.

Micro-cracks are the hidden defect. A part can measure in tolerance and still fail later because a crack propagates under thermal load. Inspecting edges at 10× to 30× magnification catches most of them. For optical or vacuum parts, a dye penetrant check on the machined edges is worth the extra step.

Every glass part we ship is inspected before it leaves. That covers raw material check, in-process monitoring during the cut, and a final dimensional and visual inspection, with reports available on request. Dimensional inspection on glass uses non-contact methods where possible, because a touch probe can mark a polished face.

Holes should be at least one times the glass thickness away from any edge, and ideally two times. A hole drilled 0.5 mm from an edge will chip no matter how careful the setup is, because there is not enough material to resist the crack network reaching the boundary. Move the hole or thicken the wall.

Inside corners need a radius. A sharp internal corner concentrates stress, and glass will not hold it. Give every pocket a corner radius of at least half the tool diameter. If the drawing shows a 90° corner, the answer is a smaller tool and a bigger radius, not a sharper cutter.

Deep narrow slots are difficult. As depth-to-width passes about 3:1, the tool deflects and the powder is hard to flush. Consider whether the slot can be made wider, or whether the feature can be assembled from two thinner plates instead of cut into one block.

CNC is not always the right process. Long straight cuts in flat sheet are faster on a waterjet or a laser. High-volume simple discs are faster on a core drill. CNC earns its place when the geometry is complex, the tolerance is tight, the surface needs a controlled finish, or the part count is low enough that tooling cost rules out the alternatives.