How to Engrave Using a CNC Machine

• 1
  Key takeaways
• 2
  What engraving does to the part
• 3
  Tooling, fixturing, and CAD prep for clean lettering
• 4
  Speeds and depths that work across common materials
• 5
  What goes wrong and how to fix it
• 6
  How to engrave using a CNC machine in 6 steps
• 7
  Choosing between CNC engraving, laser marking, and dot peen

Engraving is a controlled cut. The tool tip enters the surface, travels along a toolpath, and leaves a groove of known width and depth. That is different from dot peen or ink marking, where the surface stays largely intact. Because material is removed, the characters stay legible after anodizing, bead blasting, or years of handling.

The groove geometry follows the tool. A 90° V-bit cutting 0.1 mm deep produces a groove roughly 0.2 mm wide at the top. A 60° bit at the same depth gives about 0.12 mm. If your character stroke is 0.15 mm wide, the 60° tool is the safer choice because the tip fits the stroke instead of widening it.

Depth matters more than most people expect. Shallow marks disappear after a light polish. Marks over 0.3 mm deep on thin walls can distort the part or break through a 0.5 mm web. For serial numbers and logos on machined faces, 0.05–0.15 mm is the usual working range.

Engraving also changes the local surface finish. The cut face is typically rougher than the surrounding milled surface, often Ra 1.6–3.2 μm depending on feed and tool condition. If the part is later anodized, that roughness reads as a darker, matte character, which is usually what the customer wants.

• 1
  Cut, do not scratchA spring-loaded scribe gives a cosmetic line with no depth and no wear resistance.
• 2
  Match tip angle to stroke widthA 60° tip holds fine text; a 90° tip is faster for bold logos.
• 3
  Check wall thicknessKeep engraving depth under one third of the remaining wall.

Start with the file, not the machine. Use single-line fonts for engraving where the software supports them; they follow the character centerline and avoid the double pass a TrueType outline creates. If you must use a filled font, keep the smallest stroke above 0.2 mm so the V-bit can follow it without stepping over itself.

Tool holding is the next decision. A dedicated engraving spindle that runs 20,000–40,000 rpm gives a cleaner cut than a 12,000 rpm main spindle, mainly because the higher surface speed lets you feed faster with less built-up edge. On aluminium, 0.05 mm depth at 300–600 mm/min with a single-flute cutter is a reasonable starting point.

Fixturing should hold the part flat and rigid. Any lift or vibration shows up as a wavy line. For flat plates, a vacuum chuck or a set of low-profile clamps works well. For curved or already-machined parts, a soft jaw pocket cut to the part profile keeps the surface parallel to the tool axis.

Finally, define your zero. X and Y zero can sit at a corner or the part center, but Z zero must be the actual surface to be engraved. If the surface has a draft or a step, probe it or set zero on a known pad and compensate in the program.

• 1
  Single-line fontsOne pass per stroke, no fill, no double cutting.
• 2
  High-speed spindle20,000–40,000 rpm for aluminium and plastics.
• 3
  Rigid fixtureFlat contact over the whole engraving area.
• 4
  Z zero on the surfaceNot on the vise or the table.

Aluminium is the easiest metal to engrave. 6061 and 7075 both cut cleanly with a single-flute V-bit at 20,000–30,000 rpm and 300–600 mm/min. Keep depth per pass at 0.05–0.1 mm. A light air blast clears chips; coolant is rarely needed and can stain the surface if it sits.

Stainless 304 and 316 work-harden quickly. Use a fresh carbide bit, keep the spindle at 15,000–25,000 rpm, and feed at 150–300 mm/min. Do not dwell in the cut. A 0.05 mm pass is enough; a second pass adds depth without loading the tip. 17-4PH behaves similarly but wears tools faster.

Brass and copper C36000 and C110 cut with short chips and give a crisp edge. Run 18,000–28,000 rpm at 250–500 mm/min. Plastics are the opposite problem: ABS, POM, and PMMA melt if the feed is too slow. Use 20,000–35,000 rpm, 500–1,200 mm/min, and a sharp bit with a polished flute. PEEK and carbon fibre need carbide and a slower feed to avoid fraying.

Titanium Ti-6Al-4V and Inconel are not good candidates for deep engraving. They can be marked, but the tool wear and heat make fine text expensive. For these materials, laser marking is often the better process, especially when the character height is under 2 mm.

• 1
  Aluminium20,000–30,000 rpm, 300–600 mm/min, 0.05–0.1 mm per pass.
• 2
  Stainless15,000–25,000 rpm, 150–300 mm/min, 0.05 mm per pass.
• 3
  Brass and copper18,000–28,000 rpm, 250–500 mm/min.
• 4
  Plastics20,000–35,000 rpm, 500–1,200 mm/min, sharp polished bit.

The most frequent complaint is that the characters look shallow or inconsistent. That is almost always a Z zero problem. If the part is not flat, or the vise jaw was used as the zero point, the tool follows the error and the depth changes across the face. Probe the surface or set zero on a machined pad.

Burrs around the groove are the second issue. They come from a dull tip, a feed that is too slow, or a depth pass that is too deep. Replace the bit, raise the feed by 20–30%, and reduce the pass depth. On aluminium, a single pass at 0.05 mm with a sharp tool usually leaves a clean edge.

Wide or fuzzy strokes usually mean the tool is too large for the font. A 90° bit on 1.5 mm text will widen every stroke and close the counters in letters like e and a. Switch to a 60° bit or a 30° bit for very fine work. Also check that the CAM is using the centerline of the stroke, not an offset.

Finally, watch for tool breakage. V-bits snap when they plunge straight into the surface or when the depth pass exceeds 0.15 mm on metal. Use a ramp or a lead-in, keep the tip clear of chips, and never run a 0.1 mm tip at a feed rate meant for a 3 mm end mill.

• 1
  Shallow or uneven depthRecheck Z zero on the actual engraving surface.
• 2
  BurrsNew bit, higher feed, shallower pass.
• 3
  Fuzzy strokesSmaller tip angle, centerline toolpath.
• 4
  Broken tipAdd lead-in, cap depth at 0.15 mm per pass.