Application of the Laser Cut: What Engineers Should Check First

• 1
  What matters before you send a laser-cut part
• 2
  What the application of the laser cut actually covers
• 3
  Kerf, heat, and the edge you actually get
• 4
  Hole size, spacing, and features that survive the cut
• 5
  Cut the blank, machine the critical features
• 6
  How different metals behave under the beam
• 7
  Laser cutting vs CNC machining: which one for which feature

A laser cutter is a 2D machine. The beam follows a flat toolpath and cuts through the sheet in one pass. Anything you can draw as a closed profile on a flat plate is a candidate: brackets, gussets, mounting plates, cover panels, shims, and busbar stock. This is why the application of the laser cut dominates sheet metal work. Setup is fast, no hard tooling is needed, and design changes only require a new DXF file.

The process does not remove material in three dimensions. It cannot cut a pocket to a controlled depth, a countersink, a thread, or a tapered wall. If a print calls for a 10 mm deep cavity with a 2 mm corner radius, the laser is the wrong tool. The right move is to cut the flat blank and pass it to a CNC mill for the 3D features.

The economics are simple. Laser cutting wins on flat parts with complex outlines, short runs, and frequent design revisions. CNC milling wins once you add depth, tight bores, or a surface finish that has to be measured. Many parts use both. Cut the profile on the laser, then machine the critical features. That split keeps cost down and still holds tolerance.

A laser cuts by melting and vaporizing metal along a narrow path. The width of that path is the kerf, and it is not zero. On a fiber laser cutting 1 mm stainless, kerf typically runs 0.1 to 0.2 mm. On 12 mm mild steel it can reach 0.5 mm or more. If your DXF was drawn to a nominal outline, the finished part will be undersized by roughly half the kerf unless the CAM operator compensates for it. Good shops compensate by default. Ask.

Heat is the second issue. The cut edge sits in a heat-affected zone where grain structure changes. On mild steel this zone is soft and cuts clean. On martensitic stainless or high-carbon steel, the edge can harden and micro-crack. That is a real risk on parts that will be bent or cycled in service. For those materials, either stress-relieve after cutting or leave stock for a machining pass that removes the zone entirely.

The edge itself is a striated, slightly oxidized surface. It is fine for brackets and covers. It is not fine for a sealing face, a bearing bore, or a sliding surface. Typical laser-cut edge roughness lands around Ra 3.2 to 6.3 μm depending on material and gas. If the print calls for Ra 0.8–1.6 μm, plan a finishing cut.

Small holes are the most common design mistake. As a rough rule, the minimum hole diameter should be at least equal to the material thickness. Cutting a 1 mm hole in 6 mm steel is unreliable; the beam cannot clear the dross and the hole comes out tapered or plugged. If the print requires a small hole in thick plate, drill it after cutting instead.

Keep features spaced. Leave at least one material thickness between a hole and an edge, and between two adjacent holes. Tighter spacing leaves a thin web that can distort from heat or snap during handling. Sharp inside corners are another trap. A laser can cut a sharp corner, but the corner concentrates stress. Add a radius of at least half the material thickness wherever the part will see load.

Pierce points matter on thick plate. The beam punches through at the start of each contour, and that pierce leaves a small crater. On visible surfaces, place pierce points in scrap or on a non-cosmetic edge. On thin sheet under 2 mm, the pierce is small enough to ignore. Above 6 mm, it should be planned into the nesting.

The strongest use of laser cutting in a machine shop is as a blanking step. Cut the profile and the non-critical holes on the laser, then clamp the blank on a CNC and machine the bores, faces, and threads that carry the tolerance. This avoids roughing out the whole outline with an end mill, which wastes tool life and cycle time on a shape that a laser can produce in seconds.

The sequencing matters. Leave 0.3 to 0.5 mm of stock on any surface that will be machined. That stock absorbs the heat-affected zone and the kerf variation. For a bearing bore, leave more. For a cosmetic face, leave enough to take a single clean pass. If the blank is thin, plan a fixture or a vacuum plate so the part does not deflect during the finishing cut.

This approach holds ±0.005 mm on the machined features and keeps the flat profile cheap. It also shortens lead time. A laser can produce blanks in hours, and the CNC queue only carries the finishing operations. On a 500-part run of mounting plates with two precision bores, this split is usually the lowest-cost route.

Mild steel and stainless are the everyday materials. Mild steel cuts clean up to about 20 mm with a fiber laser, with a slightly oxidized edge. Stainless needs nitrogen assist gas to keep the edge bright and oxide-free, and it cuts well up to around 12 mm. Aluminum is trickier. It reflects the beam at low power, conducts heat away fast, and tends to leave dross on the underside. It cuts, but edge quality is rougher than steel at the same thickness.

Copper and brass are the hard cases. Both reflect infrared light strongly, so a standard fiber laser struggles below a certain thickness. A higher-power source with the right wavelength helps, but many shops still route copper parts to CNC or waterjet. If your design uses copper busbar, ask about the process before you assume laser is available.

Titanium cuts well with the right assist gas, but the edge must be protected from oxygen. Inconel and other nickel alloys cut slowly and leave a heavier heat-affected zone. For these, factor in a post-cut machining pass if the part sees fatigue load. The material list matters more than the machine spec when you are choosing a process.