How to Get Script Fonts to Cut on CNC Machine

• 1
  Key takeaways
• 2
  Why script fonts behave differently from block lettering
• 3
  Prepare the font file before it reaches CAM
• 4
  Match script stroke, material and depth
• 5
  Pick the cutter and the toolpath strategy
• 6
  Set up the machine and verify before cutting
• 7
  Step by step: get script fonts to cut on CNC machine
• 8
  Which method fits your script lettering

Block letters are mostly straight walls and constant stroke width. A script typeface is the opposite: stroke width changes along every curve, counters close up, and the letterform depends on a thin connector that carries the eye from one glyph to the next. When you ask a cutter to reproduce that, the thinnest part of the letter governs the whole job. One 0.4 mm hairline at the top of a lowercase e can force a tool so small that the rest of the engraving takes hours.

The second difference is curvature. A script curve often has a radius below 1 mm at the entry and exit points. A cutter of radius R cannot reproduce an inside corner tighter than R, so it leaves an unmachined sliver. On a flat plaque this looks like a rounded, muddy join. On a raised letter it can leave a burr that survives deburring and shows up after anodizing.

The third difference is stroke intersection. Script glyphs share strokes, and the same physical groove may be traced by two or three separate segments in the vector file. If the CAM software treats each as a closed contour, the tool plunges, cuts, retracts, and plunges again at the same spot. That is where you get witness marks, chatter, and broken 1 mm tools.

So the real question is not how to engrave text. It is how to decide, before you cut, whether a given script face can be machined in the chosen material with the tools you own. That decision is made in the vector file and in the tool table, not on the machine.

Start with a script face that was drawn for signage, not for a wedding invitation. Faces with a monotone stroke and generous x-height machine well. Faces with extreme contrast between thick and thin strokes will force a compromise you cannot win. If the client insists on a high-contrast face, raise the minimum stroke width in the artwork and let the thin strokes grow. Nobody notices a 0.2 mm change in a plaque at arm's length.

Convert text to curves before export. Live text depends on the font being installed on the CAM workstation, and hinting or kerning differences change stroke positions. Outlines are fixed geometry. After converting, run a simplify or fit-curve pass with a tolerance around 0.005–0.01 mm. Raw font outlines often carry thousands of redundant nodes per glyph, and a node-dense curve makes the toolpath stutter and leaves faceting on the wall.

Weld overlapping strokes. Script glyphs touch, and outlines that merely cross rather than merge create open contours. Open contours are the single most common reason a CAM job refuses to generate a clean toolpath. Use a boolean union, then check for self-intersections. If the software has a contour-check tool, run it and fix everything it flags before you think about tools.

Scale the artwork to the final size and set the depth in the same file. Mixing a 1:1 drawing with a scaled toolpath is a common source of wrong-depth engraving. Decide now whether the script is engraved (material removed) or raised (background removed). The two paths need different tools and different stepover values.

• 1
  Minimum stroke width0.8 mm for engraving in aluminium and brass; 1.2 mm for steel.
• 2
  Minimum inside radiusKeep at or above half the cutter diameter plus 0.1 mm.
• 3
  Node toleranceSimplify to 0.005–0.01 mm before toolpath generation.
• 4
  Contour checkWeld every crossing stroke; open contours must be zero.

Aluminium is the friendliest material for fine script. 6061 and 6061-T6 cut cleanly with a two-flute carbide cutter and leave a sharp edge at 0.8 mm stroke width. Brass C36000 is even better for sharp detail because it chips cleanly and holds a crisp corner, which is why plaques and instrument bezels often use it. Plastics such as PMMA and POM also machine fine script well, but they are sensitive to heat: a 1 mm cutter at 18,000 rpm with no air blast will weld chips back into the groove.

Stainless and steel change the rules. A 0.8 mm stroke in 304 or 316 is possible but slow, and the cutter wears fast. Expect to double the minimum stroke width to about 1.2 mm and to use a coated cutter. Titanium and Inconel are worse; for those, treat fine script as a specialty job and expect to scrap the first attempt while dialing in the parameters.

Depth is a design decision with a machining cost. Engraving 0.2–0.3 mm deep reads well on a bead-blasted or anodized surface and keeps the tool load low. Going 0.5 mm deep on a 0.8 mm stroke increases the chance of tool breakage and does not look better. For raised script, the background depth is usually 0.8–1.5 mm, and the letter wall becomes the visible feature. A wall that thin needs a finishing pass with a small stepover, typically 5–8 percent of the cutter diameter.

Consider the surface finish you are engraving into. Anodized and powder-coated surfaces are brittle. A sharp cutter with a light finishing pass leaves a clean line. A dull cutter or too high a feed tears the coating and leaves a white halo around the letters. On polished or brushed metal, any witness mark from a plunge is permanent, so minimize Z retracts.

A two-flute carbide micro end mill or a single-flute engraving cutter is the standard choice. For 0.8–1.5 mm strokes, use a Ø1–2 mm cutter with a 0.1–0.2 mm corner radius if the geometry allows. A sharp-corner cutter leaves a cleaner intersection but is more fragile. A corner radius trades a tiny amount of definition for much better tool life. On aluminium, uncoated or DLC-coated carbide works well; on stainless, use AlTiN or similar.

Engrave toolpaths are usually generated as centerline passes. For script, that is the right approach: trace the medial axis of the stroke rather than offsetting the outline. Centerline cutting keeps the tool engaged along the whole stroke and avoids the slivers that outline offsetting produces in tight curves. Set the stepover for the finishing pass at 5–8 percent of the cutter diameter, and use a spring pass or a second finishing pass at the same depth to clean the wall.

Sequence the toolpath so the cutter stays down. Most CAM packages have a linking or stay-down option. Enable it, and order the strokes so connected glyphs are cut in one continuous move. This reduces Z retracts, which in turn reduces witness marks and cycle time. On a piece with 20 characters, stay-down linking can cut the cycle by a third.

Use climb milling on the finishing pass. Climb milling pushes the chip behind the cutter and gives a better wall on aluminium and brass. Conventional milling is occasionally useful on a very thin wall to avoid pulling the material, but it leaves a rougher surface. Test both on a scrap piece before committing to the production run.

• 1
  Engraving cutterØ1–2 mm, two-flute carbide, 0.1–0.2 mm corner radius.
• 2
  Centerline strategyTrace the medial axis instead of offsetting the outline.
• 3
  Finishing stepover5–8 percent of cutter diameter; add a spring pass.
• 4
  LinkingEnable stay-down moves between connected strokes.

Zero the Z axis on the actual workpiece surface, not on the vise or a gauge block. Script engraving is shallow, so a 0.05 mm error in Z changes the line width noticeably. Touch off on a scrap area of the same material, then confirm with a test cut. If the machine has a tool presetter, use it and then verify on the part.

Run a dry pass with the Z offset raised 5 mm. Watch the toolpath on the machine, not just on the screen. This catches the retract and linking moves that look fine in simulation but travel across a finished face. On a small part, a single unnecessary rapid across the engraving area can leave a scratch that ruins the piece.

Check runout on the cutter. A 1 mm cutter with 0.02 mm of runout cuts like a 1.04 mm cutter on one side and a 0.96 mm cutter on the other. That asymmetry shows up immediately in thin script as a wider, ragged stroke. Measure runout at the flutes, not at the shank, and re-seat the collet if it exceeds 0.01 mm.

Confirm coolant or air blast before you start. For aluminium and brass, a strong air blast clears chips from the narrow groove. Flood coolant works but can hide the cut and makes it harder to see a problem developing. For plastics, air only. For steel, flood or high-pressure coolant is usually necessary to control heat at the tip of a small cutter.