CNC Engraving Process: A Complete Guide
This guide is for engineers and buyers who need crisp, repeatable marks on metal and plastic parts. It covers the tools, the parameters, the fixture, and the inspection checks that decide whether the CNC engraving process works on your part.
Key takeaways
What the CNC engraving process actually removes
Engraving is a controlled scratch. A rotating cutter, usually a single-flute tool with a 30°, 60°, or 90° included angle, is driven along a toolpath a few hundredths of a millimeter below the surface. The tip does the cutting. The shank does nothing but transmit rotation.
That geometry matters because the tip has almost no stiffness. A 60° tool with a 0.1 mm tip leaves a V-shaped groove about 0.12 mm wide at 0.1 mm depth. The same tool pushed to 0.4 mm depth now cuts a groove 0.46 mm wide and loads the tip hard enough to snap it on a hard inclusion.
Most shops run engraving after the part is finished. The visible face is already at its final Ra 0.8–1.6 μm, so any burr raised along the groove edge is a defect you cannot polish away without changing the surface.
The process suits flat or gently curved faces, part numbers, logos, scale marks, and traceability codes. Deep decorative carving, sharp internal corners, and text below 1.5 mm character height are better handled by laser marking or by a different process entirely.
Tool selection for the CNC engraving process
A 60° single-flute carbide cutter covers most jobs. It gives a readable groove at 0.08–0.12 mm depth and survives 0.05 mm stepover passes in aluminium and brass. Use 90° when the customer wants a wide, shallow mark that survives light abrasion. Use 30° for fine text on small parts, and accept that the tip will chip if depth creeps past 0.1 mm.
Coating choice follows the material. Uncoated carbide works on aluminium, brass, and plastics. TiAlN helps on stainless and tool steel, where the tip otherwise wears round after a few hundred millimeters of travel. Diamond coating is worth it on carbon fibre and on long runs of abrasive composites.
Shank diameter should be 3.175 mm or 6 mm. A 6 mm shank in a shrink-fit or hydraulic holder runs truer than a 3.175 mm tool in a collet, and runout below 0.01 mm is the practical target. Measure it with a dial indicator on the shank, not on the tip.
Never use a broken-tip cutter to save a setup. The groove width changes, the depth reading drifts, and the second half of the run will not match the first. Replace the tool whenever the measured groove width moves more than 0.02 mm from nominal.
- 130° included angleFine text and small scale marks; fragile tip, keep depth under 0.1 mm.
- 260° included angleGeneral purpose; the default for part numbers and logos.
- 390° included angleWide shallow marks; better wear resistance on handling surfaces.
- 4Flat-bottom cutterOnly for pockets and filled marks, not for line engraving.
Speeds, feeds, and depth that hold up
Spindle speed sits high because the tool is small. On aluminium, 12,000–18,000 rpm is normal. On stainless, drop to 8,000–12,000 rpm and expect shorter tool life. On plastics such as POM and PMMA, 10,000–14,000 rpm with a sharp uncoated tool gives a clean edge; too much speed melts the chip back into the groove.
Feed per tooth is tiny. A practical range is 0.01–0.03 mm per tooth for a single-flute cutter, which at 15,000 rpm gives 150–450 mm/min. Start at the low end, listen for chatter, then step up. Chatter on an engraving pass shows as a rippled groove floor that no amount of polishing hides.
Depth per pass should not exceed half the tip width. For a 0.1 mm tip, take 0.05 mm per pass and make two passes to reach 0.1 mm. A single 0.2 mm plunge on stainless is the most common cause of tip breakage we see in incoming jobs.
Stepover for filled areas runs 40–60% of the groove width. At 0.1 mm groove width, that is 0.04–0.06 mm. Finer stepover looks better but multiplies cycle time linearly. On a 30 × 30 mm logo panel, going from 0.06 mm to 0.03 mm stepover can double the run from about 20 minutes to 40 minutes.
Workholding and the exit burr
An engraving cutter pushes material sideways and down. Where the groove runs off the edge of the part, the tip has nothing to cut against, and the edge tears. The fix is a sacrificial backing plate. Clamp a flat piece of aluminium or acrylic directly under the part, zero the tool to the part surface, and let the tip cut 0.05 mm into the backing.
For thin parts, vacuum chucks and double-sided tape work better than clamps. A 1 mm aluminium panel will bow under three-point clamping, and the engraved depth will vary across the face even though the machine is holding Z perfectly.
Curved surfaces need either a 4-axis setup or a contoured fixture. On a Ø400 mm rotary table, a cylindrical part can be indexed so the engraving stays near the top of the arc. Keep the mark within ±15° of top dead center; beyond that, the effective depth changes with the surface angle.
Clean the face before the run. A single chip under the part lifts it locally, and the mark on that area cuts deeper. Wipe with IPA and blow dry, then re-zero.
Step by step: setting up a CNC engraving job
- 11. Confirm the mark is engraving, not markingCheck the drawing for depth callout. If no depth is given, propose 0.08 mm for metal and 0.15 mm for plastic, and get it approved in writing before the run.
- 22. Pick the cutter and measure runout60° single flute for general work. Mount in a 6 mm hydraulic or shrink-fit holder, indicate the shank, and reject anything above 0.01 mm TIR.
- 33. Set the work offset on the finished faceTouch off on the actual engraved surface, not on the raw stock. If the part was faced after the first setup, the two surfaces differ by the facing allowance.
- 44. Add the sacrificial backingPlace a flat plate under the part, clamp lightly, and set Z so the tip cuts 0.05 mm into the backing at the end of each stroke.
- 55. Run a single-character testEngrave one character, then measure groove width and depth with an optical comparator or depth mic. Adjust feed before running the full text.
- 66. Cut the full mark in two passes0.05 mm rough and 0.03–0.05 mm finish. Keep spindle speed constant between passes so the groove floor stays uniform.
- 77. Deburr and inspectRemove the rolled edge with a fine ceramic fiber stick or a light bead blast. Check depth at three points and confirm character height is at least 1.5 mm.
- 88. Record the parametersLog tool angle, rpm, feed, depth, and stepover against the part number. The next run should not need a new test cut.
CNC engraving compared with laser marking
Both produce permanent marks. The choice depends on surface, depth requirement, and run size.
| Factor | CNC engraving | Laser marking |
|---|---|---|
| Depth control | 0.05–0.2 mm, measurable | Surface level, no measurable depth |
| Minimum character height | 1.5 mm practical | 1.5 mm at our shop |
| Best surface | Flat or indexed curved faces | Flat, painted, anodized |
| Tool wear | Tip wear on hard alloys | No contact, lens stays clean |
| Burr risk | Yes, needs deburring | None |
| Run size | Prototype to 10,000+ parts | Better above a few hundred parts |
| Setup time | Longer, needs test cut | Short, direct from file |
The short version
Engraving pays off when you need a measurable depth and full control over the mark. If the surface is coated, flat, and the text is small, laser marking is the cheaper answer. Send the drawing and we will tell you which one fits.
Questions engineers ask before quoting
How small can engraved text be?
Character height of at least 1.5 mm is the practical limit for a clean, readable mark. Below that, the groove width approaches the tool tip diameter and the strokes merge.
If your drawing calls for 1 mm text, laser marking gives a cleaner result on anodized or painted surfaces.
Can the CNC engraving process cut into hardened steel?
Yes, with coated carbide and reduced speed. Above about 45 HRC the tip wears quickly, and the groove width grows through the run.
For hardened tool steel, engrave before heat treatment whenever the drawing allows it. The mark stays legible and the tool cost drops.
Will engraving break the anodized layer?
It does. The cutter removes the coating and exposes bare aluminium, which shows as a bright or darker line depending on the alloy.
If the mark must stay within the coating, laser marking is usually the better route because it can work through the anodized layer without cutting a groove.
What depth should I specify on the drawing?
0.08 mm is a safe default for aluminium and brass. Use 0.10–0.15 mm on stainless and steel, and 0.15–0.20 mm on plastics where the material springs back slightly.
State the depth as a range with a tolerance, for example 0.08 ±0.02 mm, so the shop has room to adjust the test cut.
How long does engraving add to the cycle?
A short part number of 10 to 15 characters takes under a minute at 300 mm/min. A filled logo panel depends on area and stepover, and can run from several minutes to about 40 minutes.
Send the vector file with the quote request and we can estimate the engraving time before the job is scheduled.
Do you engrave on curved parts?
Yes, on a 4-axis setup with a Ø400 mm rotary table. The mark is kept within ±15° of top dead center so the effective depth stays even.
For full wrap-around marks or text over a compound curve, send the model and we will confirm whether engraving or laser marking gives the better result.
Send us your engraving drawing
Upload the part file and the marking detail. You get a quotation and a free DFM analysis within 12 hours, including a note on whether engraving or laser marking suits the surface.
12-hour quote100% inspectionNDA on request
More from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
