What Can a CNC Router Do?

• 1
  Key takeaways
• 2
  What a CNC Router Does: The Basics
• 3
  Profiling and Through Cutting
• 4
  Engraving, Marking, and Surface Detail
• 5
  3D Carving and Relief Work
• 6
  Drilling, Grooving, and Joinery
• 7
  Router or Milling Center: Which Job Goes Where

A router holds the workpiece flat on a table and moves a spinning cutter over it in three axes. The gantry carries the spindle across X and Y, and the Z axis sets depth. That is the whole mechanism. Everything else follows from how stiff that frame is.

Because the part sits flat and the tool comes down from above, the machine is built for sheet and plate. Cut a profile through 12 mm plywood, pocket a recess into an ABS panel, or trace a groove into a composite skin. Those are all the same motion at different depths.

The control reads G-code. Your CAD file becomes toolpaths: which tool, what feed, what speed, how deep each pass goes. A 6 mm cutter taking a 2 mm depth of cut behaves very differently from the same cutter buried 15 mm into the material.

That is the boundary most people miss. A router is not weak. It is shallow. Give it plate and it is fast and accurate. Ask it to carve a deep three-dimensional cavity out of a solid block and the tool hangs out of the collet, deflects, and leaves chatter marks.

Profiling is the bread-and-butter job. The cutter follows a closed path and drops the part out of the sheet. On a well-tuned machine with a sharp cutter, a 2D profile in aluminium plate holds about ±0.1 mm. That is enough for brackets, panels, and mounting plates.

Through cutting needs tabs or a sacrificial bed. If you cut all the way through, the part shifts on the last pass. Leave 0.3–0.5 mm tabs every 100–150 mm and snap them off by hand, or hold the sheet down with vacuum. Small parts that free themselves mid-cut are the most common cause of scrapped plate.

Feed and speed matter more than spindle power here. In 6061 aluminium, a 6 mm two-flute carbide cutter runs around 12,000–18,000 rpm with a feed near 1,500–2,500 mm/min, and single-pass depth stays under 3 mm. Push deeper and the cutter rubs, heats, and welds chips to the edge.

Success in profiling is usually about workholding, not the machine. If the sheet lifts, the cut drifts. Vacuum tables, double-sided tape, and low-tack fixturing are normal practice for thin plate.

Engraving uses a sharp V-bit or a small ball nose to cut shallow detail into the surface. A 60° or 90° V-bit gives crisp lettering and thin decorative lines. Depth is usually 0.2–1.0 mm, so cutting forces stay low and the machine runs fast.

This is where a router beats most other processes on cost. Serial numbers, alignment marks, control-panel legends, and calibration scales can all be cut directly into the part. No label, no adhesive, no separate operation. Laser marking is an alternative when the character height goes below about 1.5 mm or the surface cannot take tool marks.

The catch is resolution. A V-bit cuts a wider groove the deeper it goes, so strokes widen as depth increases. Keep engraving shallow and consistent. If the drawing mixes 0.3 mm and 0.8 mm depths on the same line, the line will not look uniform.

For decorative work on wood and MDF, a 30° V-bit with a stepover near 0.1 mm produces a clean carved effect. The same settings on aluminium will snap the tip. Tool geometry is matched to material, not to the picture.

Three-axis simultaneous motion lets the router sculpt curved surfaces. A ball-nose cutter sweeps back and forth with a small stepover, and the overlapping passes leave a smooth form. Stepover of 0.5–1.0 mm on a 6 mm ball nose gives a finish most people accept without hand sanding.

Relief carving works the same way. The toolpath follows a height map, so the tool climbs and drops with the surface. Shallow relief up to about 20 mm of total height difference is comfortable. Beyond that, the tool sticks out further and rigidity falls away.

The real limit is the ratio of depth to tool diameter. A cutter that extends more than four times its diameter past the collet will deflect under load. That deflection shows up as a tapered wall or a stepped floor, not as an obvious crash.

For deep 3D forms, the honest answer is a different machine. A 5-axis machining center or a mill-turn cell cuts the same geometry as a solid block and holds tolerance on the walls. Routing is the cheaper path when the form is shallow and the material is soft.

A router can drill. Plunge with an end mill or a drill bit and you get a hole. It is not a drill press, though. The tool enters straight down, so hole depth is limited by flute length and chip evacuation gets poor past about two diameters deep.

Peck drilling helps. Retract every 1–2 mm so chips clear the flutes. Without that, aluminium chips pack the hole and the cutter rubs instead of cutting. For holes deeper than about 3× diameter, drill on a mill or bore it after routing.

Grooving and channeling are natural fits. A cutter the width of the groove runs one pass and leaves a clean channel. This is common in panel work, cable channels, and gasket seats. Groove width tolerance follows the cutter, so pick a nominal size and hold it.

Joinery is where the process shines on wood and composites. Dados, rabbets, mortises, and finger joints all come off the same setup. Because the part never leaves the table, the joint lines stay aligned. That is a fixturing advantage more than a cutting one.