CNC Engraving: How the Cut Works and Where It Stops

• 1
  Key takeaways
• 2
  What CNC Engraving Actually Does to the Part
• 3
  Depth, Width, and Character Height Limits
• 4
  How CNC Engraving Behaves in Common Materials
• 5
  When CNC Engraving Beats Laser Marking
• 6
  Specifying an Engraved Mark on a Drawing
• 7
  CNC Engraving vs Laser Marking: Fit by Requirement

CNC engraving is a controlled milling cut. A small-diameter cutter, usually a V-bit, a flat end mill, or a ball nose tool, follows a programmed toolpath and lifts material out of the surface. The result is a groove with measurable depth and a defined edge. That groove is what you read as text, a logo, a serial number, or a datum mark.

Because the mark is cut, it does not sit on top of the substrate. It becomes part of the part. That distinction matters in service. A machined groove will survive solvent wipe-down, abrasive handling, and most rework cycles that would destroy a printed label. The trade-off is that the mark is permanent in a way that can be inconvenient: a wrong serial number cannot be wiped off.

The cutting action also changes the local surface. Most engraved areas show Ra 1.6–3.2 μm as-machined, which is rougher than a finished face. If the surrounding surface is polished to Ra 0.2–0.8 μm, the contrast will be visible even without color fill. Some engineers want that contrast. Others want the mark to disappear into the background, and that requires planning at the drawing stage, not after the cut.

Depth tolerance is where drawings usually get vague. A callout of "engrave 0.2 mm deep" can be held to ±0.005 mm on flat aluminum with a sharp tool and a rigid setup, but not across a curved casting with interrupted cuts. On a five-axis machine, the tool axis stays normal to the surface, so depth stays uniform around a curved wall. On a three-axis machine, a curved wall changes the effective depth as the tool moves off-normal.

• 1
  Cut, not depositMaterial leaves the part. Thickness and mass change slightly, which rarely matters but does show up on thin-wall work.
• 2
  Edge quality follows the toolA worn cutter leaves a burr on the lip of the groove. Fresh carbide gives a cleaner edge.
• 3
  Contrast is a design choiceAnodize color fill, paint fill, or a bead-blasted background all change how visible the mark is.

Character height sets the practical floor for the whole operation. Below about 1.5 mm, the strokes of a letter become thinner than the radius of the smallest cutter you can reliably run, and the mark turns into a smear. Laser marking can go smaller because it has no tool radius, but a cut groove cannot. If the drawing calls for 0.8 mm text, the process choice is wrong, not the toolpath.

Groove width tracks the cutter geometry. A 60° V-bit cutting 0.2 mm deep produces a groove roughly 0.23 mm wide at the surface. A 90° V-bit at the same depth produces about 0.4 mm. Wider angles give a shallower, more open groove that reads well from an angle; sharper angles give a deeper, narrower mark that holds paint better. The angle also sets how the mark looks under raking light, which matters on dark anodized surfaces.

Depth tolerance tightens as the feature shrinks. On a flat face with a rigid setup, ±0.005 mm is achievable. On a thin plate that deflects under cutting force, or on a casting with hard spots, expect ±0.03 mm or looser. The cause is not the machine. It is the local stiffness of the part and the variation in material hardness across the cut.

Spacing between characters matters as much as stroke width. Leave at least one stroke width of uncut material between adjacent letters, or the marks will merge after finishing. Coatings add thickness. Anodizing builds roughly 5–15 μm per surface, and powder coating can add 60–100 μm. Mask the engraved area or account for the build-up in the depth callout.

• 1
  Minimum height1.5 mm for cut characters on metal. Smaller text needs laser marking instead.
• 2
  Typical depth0.10–0.30 mm covers most identification and branding marks.
• 3
  V-bit angle60° for narrow deep marks, 90° for wider shallow marks.
• 4
  Coating buildAdd 5–15 μm for anodize, 60–100 μm for powder coat.

Aluminum is the easy case. Alloys like 6061, 7075, and 6082 cut cleanly with a sharp V-bit, hold a crisp edge, and tolerate fast feed rates. The softness that makes aluminum easy to cut also makes it easy to damage: a dropped part can smear a shallow mark. If the mark is functional, such as a part number that must stay readable after field handling, cut deeper and consider a hardcoat anodize afterward.

Stainless steels behave differently. Grades 303 and 304 work-harden under the tool, so a cutter that rubs instead of cutting will dull quickly and burnish the groove rather than cut it. Feed per tooth has to stay high enough to bite under the hardened layer. Grade 316 is gummier and tends to build up on the tool edge. Engraving on stainless is slower and tool life is shorter, but the resulting mark is very durable.

Plastics split into two groups. ABS, POM, and PC cut cleanly with sharp tooling and air blast to clear chips. PMMA and other acrylics are brittle: the cutter can chip the edge of the groove or leave a frosty halo around it. PEEK cuts well but is expensive to scrap, so run a test coupon first. Carbon fiber is abrasive and wears carbide quickly, and the cut exposes fibers that may need sealing.

Copper and brass cut beautifully. Brass, in particular, gives a crisp edge with almost no burr, which is why it shows up in instrument panels, nameplates, and electrical identification. Beryllium copper is a different story: the dust is a health hazard, so it needs controlled coolant and extraction. Titanium and Inconel can be engraved, but tool wear and heat make it a low-speed operation. On these alloys, laser marking is often the more practical choice.

• 1
  Clean cuttersAluminum, brass, ABS, POM, PC, PEEK.
• 2
  Care neededStainless 303/304/316, titanium, Inconel, carbon fiber.
• 3
  Chip riskAcrylic and other brittle plastics can chip at the groove edge.

Laser marking is fast, flexible, and needs no tooling. It also produces no measurable depth, which is fine for a logo on a housing and not fine for a serial number that a customer expects to feel with a fingernail. The choice usually comes down to whether the mark must survive abrasion, and whether an inspector needs to verify depth.

Engraving wins where the mark is functional. Traceability codes on aerospace and medical parts, torque specs on a wrench, or a part number on a surface that gets handled daily all benefit from a cut groove. Engraving also lets you fill the groove with paint or anodize dye for high contrast on a dark background, which laser marking on anodized aluminum cannot match.

Laser marking wins on speed and on curved or hard-to-fixture geometry. A laser can mark a part in seconds with no workholding beyond a simple nest. Engraving needs the part located, clamped, and often probed, which adds setup time. On a one-off bracket, that setup can cost more than the cut. On a 500-piece run, the setup amortizes and engraving becomes competitive.

There is also a hybrid route. Laser-mark the fine text, engrave the logo and the functional data. That splits the work by what each process does best and avoids the tool-radius limit on small characters. It adds a second operation and a second setup, so it only pays off when the part already moves between machines.

One more factor is surface finish. Engraving leaves a visible textured groove. On a mirror-polished or bead-blasted cosmetic surface, that texture is a design statement, not a defect. If the customer wants an invisible mark, neither process delivers it. That requirement points to a different method, such as an embedded tag or a laser-etched micro-mark in a hidden area.

• 1
  Pick engraving whenDepth is specified, abrasion resistance matters, or the mark gets paint fill.
• 2
  Pick laser whenSpeed dominates, the surface is curved, or characters are under 1.5 mm.
• 3
  Pick both whenFine text and a deep logo sit on the same part.