Laser CNC Metal Cutting Guide

• 1
  How laser CNC metal cutting removes material
• 2
  Fiber, CO₂, and which one cuts your alloy
• 3
  Thickness, tolerance, and edge quality limits
• 4
  Design rules that keep laser parts cheap
• 5
  From CAD file to finished blank
• 6
  Step by step: from drawing to cut part
• 7
  Laser cutting versus milling versus waterjet

A laser CNC metal cutting machine focuses a beam onto a spot a few tenths of a millimeter wide. Power density at that spot climbs high enough to melt or vaporize the alloy, and the CNC moves the head along a toolpath taken from a CAD file. There is no cutter touching the work, so there is no tool wear and no clamping force pushing the sheet around.

An assist gas does half the work. It blows molten metal out of the kerf so the beam keeps reaching fresh material. Nitrogen gives a clean, oxide-free edge on stainless and aluminum. Oxygen adds an exothermic reaction that helps on mild steel, but it leaves a thin oxide layer you usually have to remove before painting or welding.

The kerf is not vertical. It tapers slightly, wider at the top than the bottom, and the taper grows with thickness. On 1 mm sheet the taper is small enough to ignore. Past 6 mm it can matter on a mating edge, so check the drawing if the part registers against another cut face.

Heat travels a short distance from the cut. A heat-affected zone a few hundredths of a millimeter deep is normal. On most brackets and panels that zone is harmless. On a hardened tool steel or a fatigue-critical aerospace part, it is a crack initiation site, and you should plan a light machining pass afterward.

• 1
  Kerf widthTypically 0.1–0.5 mm depending on thickness and nozzle.
• 2
  Heat-affected zoneTens of micrometers on thin sheet; grows with thickness.
• 3
  No contact forceThin sheet stays flat without heavy fixturing.

Fiber lasers dominate metal cutting today. A 1 μm wavelength is absorbed well by steel, stainless, aluminum, and copper alloys, and the beam can be delivered by a flexible fiber rather than mirrors. Diode-pumped designs run at roughly 30% wall-plug efficiency, so power draw and cooling load are lower than an equivalent CO₂ machine.

CO₂ lasers emit at 10.6 μm. They cut mild steel and stainless well, and they still handle some non-metals. The downside is optical alignment, mirror maintenance, and higher power consumption for the same cut. For job shops cutting mostly metal, fiber has largely replaced them.

Reflective alloys need attention. Copper, brass, and bare aluminum reflect a large share of the beam at room temperature. The cut usually starts once the surface heats and absorption rises, but a poorly tuned setup can send reflected light back into the optics. Use the machine maker's reflective-material recipe and inspect the protective window on schedule.

Magnesium is a different problem. Fine magnesium dust and chips ignite easily. Many shops decline magnesium on a laser and route it to milling instead. Titanium cuts acceptably with inert gas, but you must exclude oxygen and manage the dust, so it is a controlled process rather than a default one.

• 1
  Fiber 1 μmSteel, stainless, aluminum, copper, titanium with inert gas.
• 2
  CO₂ 10.6 μmMild steel, stainless, some plastics and organics.
• 3
  Avoid on laserMagnesium, and thick reflective copper without a proven recipe.

Cutting speed falls steeply with thickness. A 2 kW fiber source that runs 1 mm mild steel at several meters per minute will slow to a crawl at 12 mm, and the edge quality drops at the same time. For most job-shop work, 0.5–6 mm is the sweet spot where laser is fast and clean. Above 12 mm, plasma or waterjet often wins on cost per part.

Tolerance is not the same as precision machining. A laser holds roughly ±0.1 mm on thin sheet, and the achievable figure widens with thickness because the kerf tapers and heat distortion grows. If your print calls for ±0.005 mm, the laser cuts the blank and a CNC mill finishes the critical faces.

Edge condition depends on gas and speed. Nitrogen on stainless gives a bright, near-machined edge, often Ra 1.6–3.2 μm, ready for welding. Oxygen on mild steel is faster and cheaper but leaves a gray oxide that needs pickling or blasting. Too much power or too slow a feed produces dross on the underside; too fast leaves a rough, striated edge.

Small features have their own floor. A hole smaller than about the sheet thickness is hard to cut cleanly, and the diameter-to-thickness ratio matters more than the absolute number. Keep hole diameter at least 1× thickness, and 1.5× if you need a clean bore. Slots narrower than 1 mm in 3 mm plate tend to taper badly.

• 1
  Typical sheet range0.5–6 mm for clean, fast production.
• 2
  Practical toleranceAround ±0.1 mm; tighter needs a machining pass.
• 3
  Minimum holeAbout 1× material thickness, 1.5× for a clean bore.

Keep the part a constant thickness. A flat blank from one sheet needs no extra setup. The moment you add a bend, a counterbore, or a tapped hole, the part leaves the laser and enters a press brake or a mill, and the cost jumps. Design the flat profile first, then add secondary features only where they earn their place.

Give the beam room to enter. Every cut path needs a lead-in, usually a small pierce hole just off the profile. If a feature sits within 1 mm of the edge, the pierce can blow out the edge or leave a witness mark. Leave at least one material thickness between the cut and any finished edge.

Corner radius matters on thick stock. A sharp internal corner concentrates heat and often cuts with a small radius anyway. Specify an inside radius of at least half the sheet thickness so the corner cuts predictably and the drawing matches the part.

Watch the overall envelope. Large thin panels distort as heat builds. If the part is bigger than roughly 1 m on a side in thin sheet, expect some bowing and plan a stress-relief or a machining skim on any face that must sit flat. Nesting also matters: tight spacing between parts saves metal but leaves less room for the kerf and heat to spread.

• 1
  Constant thicknessOne sheet, one setup, lowest cost.
• 2
  Edge clearanceKeep pierce points at least one thickness from finished edges.
• 3
  Inside corner radiusAt least half the sheet thickness on thick stock.

The workflow starts with a 2D DXF or a 3D STEP file. The nesting software arranges parts on the sheet to reduce scrap, then assigns a lead-in, a pierce point, and a cut sequence that keeps the part from shifting as the skeleton weakens. On a good nest, scrap drops several percentage points compared with a hand layout.

Piercing is slow on thick material. The machine may pierce at low power for a few tenths of a second before switching to full cutting power. On 10 mm steel, pierce time can exceed the cut time for a small hole, which is one reason laser cost per part climbs quickly with thickness.

After cutting, parts go to deburring. Laser edges on thin sheet are often ready to use, but dross and a sharp top edge are common. Tumbling, brushing, or a light bead blast removes them. If the part will be anodized, the cut edge anodizes slightly differently from the rolled surface, so plan for a visible line on cosmetic parts.

For parts that need tight bores or flat mating faces, the laser produces the blank and a CNC mill finishes the rest. GreatLight runs this combination in one shop: laser or waterjet for the profile, then 3-, 4-, or 5-axis machining to ±0.005 mm and finishes from Ra 0.2–0.8 μm where the drawing requires it.

• 1
  Input file2D DXF for profiles, 3D STEP when features matter.
• 2
  Pierce timeDominates cycle time on steel above 8–10 mm.
• 3
  Post-cutDeburr, then machine critical faces if needed.