Basics of CNC Engraving: Getting Started Guide

CNC engraving is milling with a very small cutter. A rotating tool, usually a V-bit, a ball nose cutter or a flat end mill under 3 mm, follows a toolpath generated from vector geometry. The tip contacts the surface and cuts a groove whose shape is set by the tool profile and the depth of cut. Nothing is stamped, burned or rolled. The mark is removed material, so it survives the same finishing operations the rest of the part goes through.

Because the tool is small, the forces are small. That is the main advantage. You can engrave a thin wall, a machined boss or a part already close to final size without deflecting it. The trade-off is time. A 0.5 mm cutter running at a conservative feed covers a short distance per minute, so a large engraved logo or a long serial number adds real cycle time.

The geometry that matters most is the included angle of the tool. A 60° V-bit cuts a narrow line at shallow depth and a wider line as you go deeper. A 90° V-bit widens twice as fast for the same depth. A ball nose cutter produces a rounded groove with a fixed width equal to the ball diameter. A flat end mill produces a groove with vertical walls and a width equal to the cutter diameter, which is what you want when the engraving has to hold a precise line width.

• 1
  V-bitLine width changes with depth; good for text and logos.
• 2
  Ball noseFixed round groove, diameter sets width; good for blending.
• 3
  Flat end millConstant width, vertical walls; use when width is toleranced.

Depth of cut is the single number that decides how the engraving looks. Too shallow and the mark disappears after anodizing, bead blasting or a light polish. Too deep and a V-bit produces a wide, ragged groove that no longer matches the drawing. For most metals we run 0.05–0.15 mm depth on a V-bit and adjust from there. Stainless and tool steel work-harden at the tip, so a deeper single pass is often better than several shallow ones that rub instead of cut.

Stepover controls the surface inside the groove. On a V-bit you normally cut a single centerline pass and let the geometry form the groove. On a flat or ball cutter you may need two or three overlapping passes to clear the full width, and the stepover has to stay under about 40 percent of the cutter diameter or you leave a ridge down the middle of the mark. That ridge is visible after anodizing even when it looks fine on the machine.

Spindle speed and feed are set by the tool tip, not the shank. A 0.5 mm tip needs high rpm and a light chip load. Run the numbers for the tip diameter and the material, not for the 3 mm shank the tip is ground into. On aluminium we commonly run 12,000–18,000 rpm; on stainless, lower surface speed and a feed that keeps the tip cutting rather than polishing. Air blast or a small amount of lubricant is usually enough to clear chips from a groove this narrow.

• 1
  Depth 0.05–0.15 mmTypical starting range for V-bit engraving in metal.
• 2
  Stepover < 40% of cutterPrevents a visible ridge inside wide grooves.
• 3
  Tip speed, not shank speedCalculate rpm and feed from the cutting tip diameter.

Choose CNC engraving when the mark has to be permanent metal, when it sits on a curved or stepped surface, or when the part will be anodized, plated or powder coated afterward. Because the material is removed, the mark stays visible through those processes. It also works when the engraved feature is functional rather than decorative: a shallow groove that locates a gasket, a witness line, a part number that has to be readable after 10 years in service.

Choose laser marking when the mark is small, the surface is flat, and the part cannot tolerate any cutter force. Laser marking on the finishes we offer has a minimum character height of 1.5 mm, and it changes the surface rather than removing material. That is fine on many parts, but on a hardcoat anodized surface the mark can be less legible than a cut groove. It also does not produce a tactile mark.

Do not engrave when the wall behind the mark is thinner than about three times the depth you need. A 0.1 mm groove in a 0.25 mm wall leaves the wall too weak and may push through. Do not engrave on a part that will be tumbled heavily afterward, because the groove edges round over and the text fills in. And do not specify engraving on a surface that is still going to be machined, because the second operation erases it.

• 1
  Good fitCurved surfaces, functional grooves, marks that survive finishing.
• 2
  Use laser insteadFlat surfaces, no cutter force allowed, marks under 1.5 mm.
• 3
  AvoidVery thin walls, heavy tumbling after engraving, later machining passes.

Engraving is a finishing operation, so the part is usually already at final size and often already finished. That changes the workholding plan. Soft jaws machined to the part profile, a vacuum plate on flat plate stock, or a low-profile clamp set outside the engraving zone all work. What you cannot do is clamp across the surface being engraved. A single clamp mark on a finished cosmetic face turns a good part into scrap, and re-machining the face to remove it costs more than the engraving did.

Tool wear shows up earlier on engraving than on most milling. The tip is the smallest part of the cutter and it does all the work. A worn V-bit produces a wider, duller groove with a burr on both edges. On a production run, change the tool on a count or on a measurement of the first-off groove width, not when it looks bad. Keep a first-off part next to the machine and compare under a loupe at each setup.

Inspection is straightforward but has to be defined on the drawing. State the line width and its tolerance, the depth, and whether the mark is decorative or functional. We check engraving at 100 percent before shipment along with the rest of the part. For a functional groove, we can supply a report with the measured width and depth. For decorative text, a visual check against the approved artwork is usually enough.

• 1
  Never clamp the engraved faceWorkholding marks on a cosmetic surface are not recoverable.
• 2
  Change tools on a countTip wear widens the groove before it looks dull.
• 3
  Define the mark on the drawingWidth, depth, and whether it is decorative or functional.

Send vector geometry, not a raster image. DXF, DWG, STEP or a clean SVG all work. A logo pulled from a website is usually a bitmap, and converting it to vectors introduces small nodes and open contours that a cutter will follow exactly. Those artifacts show up in the finished part. A redrawn vector with smooth curves and closed contours machines faster and looks better.

Text has its own rule. Engraved stroke width has to be wide enough for the cutter tip to pass through without rubbing. As a working minimum, keep the stroke at least 0.1 mm wider than the tip diameter you plan to use, and keep character height at 1.5 mm or more if the part also gets laser marking or you want to leave that option open. Very small serif fonts lose their thin strokes first.

Include the depth and the datum in the file or on the drawing. If the engraving is on a curved surface, say so, because we will need to project the toolpath onto the actual CAD surface rather than a flat plane. If the mark has to sit at a specific distance from an edge or a hole, dimension it from that feature. We review the file and return a DFM note with the quotation, usually within 12 hours, so the engraving callout can be corrected before the first cut.

• 1
  Vector onlyDXF, DWG, STEP or clean SVG; redraw logos before machining.
• 2
  Stroke ≥ tip Ø + 0.1 mmNarrow strokes cause rubbing and a ragged mark.
• 3
  Dimension from a real featureEdge, hole or datum on the part, not from the artwork frame.