Preparing DXF Files for a Clean CNC Cut
A DXF file is a contract between the designer and the machine. It says: here are the lines, here are their layers, here are the units. Everything else — toolpath, depth, feed rate, fixturing — happens on the CAM side, where the operator decides how to cut what the file describes.
Tervika's DXF export is designed to make that contract clean. The plate outline goes on one layer, the engraved text goes on another, alignment guides go on a third. The units are explicit. The polygons close. There are no stray nodes, no tiny segments left over from booleans, and no self-intersections. This article describes what's in the file you get, and what to do with it on the CAM side to turn it into a finished plate.
It is intentionally tool-agnostic. Whether you're using a hobby CNC with VCarve, a fibre laser with Lightburn, a Shopbot with Aspire, or a 5-axis mill with Fusion 360, the same principles apply.
What's actually in the file
Tervika exports to ASCII DXF (R2000 / AutoCAD 2000 format), which all CAM tools accept. Each export contains one or more entities organised into named layers:
PLATE_OUTLINE— the closed outline of the plate. One polyline per plate. This is what gets cut.PLATE_TEXT— the destination text and any decorative text, expressed as closed polygons (one per glyph). This is what gets engraved or pocketed.PLATE_HOLES— mounting holes, if you've added them. Closed circles.PLATE_GUIDES— alignment marks (origin crosshair, plate centerlines). Construction-only — do not cut these.
Units are real-world: millimeters or inches based on your Tervika settings. There's no scaling required when importing. A 600 mm plate exports as a 600 mm polyline.
A common operator surprise: the text is not text. It's outlines. A glyph like the lowercase "g" is exported as two closed polygons — the outer outline and the inner counter (the closed shape inside the loop). This is intentional. CAM tools that try to interpret DXF "TEXT" entities have to guess at the font, the kerning, and the glyph shapes; pre-converted outlines remove the guesswork. The downside is that you can't edit the text in the DXF — that has to happen back in Tervika.
Toolpath choices
Once you've imported the DXF, the next decision is what kind of toolpath to run on each layer.
For the plate outline
There are three main options:
Profile / cutout toolpath. A through-cut around the outside of the polyline. The router or laser follows the outline at full material depth, separating the plate from the stock. This is what you almost always want for the plate outline.
For routers, set the toolpath to cut on the outside of the polyline, with a tool diameter that matches the smallest inside corner radius in your design. A 3 mm bit can cut a 1.5 mm inside radius; a 6 mm bit can't go below 3 mm radius. If your design has sharper corners than your tool, the corners will be radiused to the tool's diameter. Tervika's plate shapes are designed with this in mind, but if you're using custom shapes, check the inside radii before exporting.
For lasers, the kerf (the width of the cut) is small enough that profile cuts are essentially "follow the line." Some operators offset the cutting line by half the kerf width to land at the exact specified dimensions; others don't bother for sign work, where 0.1 mm is invisible.
For the text
Three main options:
Pocket / engrave at fixed depth. The router clears out the inside of each glyph polygon to a fixed depth — 1 mm, 2 mm, whatever you specify. This produces flat-bottom letters that contrast cleanly with the surrounding surface. Use this when you'll fill the pockets with paint, resin, or a contrasting wood.
V-carve. The router follows the centerline of each glyph with a V-bit, varying the depth based on the local glyph width. Wider parts of the glyph cut deeper; narrower parts cut shallower. This produces letters with sharp ridges and natural typographic emphasis. The trade-off is that V-carve toolpaths are slower to compute and slower to cut, and the visual effect depends on the bit angle (60° and 90° are common; the choice affects the look significantly).
Through-cut text. The router or laser cuts all the way through the plate, leaving holes shaped like the glyphs. For metal plates with backlighting, this is the right answer. For wood, the inner counters of glyphs like "o" and "g" become small offcut "ghost" pieces that have to be removed, and the plate is structurally weakened.
For most fingerpost signs in wood, V-carve is the typographically richest choice; pocket-engrave is the most reliable.
For the holes
A standard drilling toolpath. Specify the through-depth (material thickness plus a small breakthrough — 1-2 mm extra is plenty) and the hole diameter from the import. If the holes are smaller than your smallest end mill, switch to a drill bit; if larger, a helical or pocket toolpath works fine.
Tool diameter vs. font weight
The single largest source of disappointment in CNC sign making is fonts that don't fit the tools.
A 1.5 mm end mill can resolve glyphs with internal features as fine as ~1.5 mm. A 3 mm end mill can do ~3 mm. If your font has fine serifs, narrow strokes inside characters like "e" and "a", or thin counters, those features will be averaged away by the bit and the result will look smudged.
Two practical responses:
- Pick fonts with strokes proportional to your tool. Bold, geometric, sans-serif fonts engrave reliably with any common bit. Light or condensed fonts need fine bits and patient feeds.
- Cap-height matters more than font choice. A 30 mm cap-height "Open Sans Light" engraves cleaner than a 12 mm cap-height "Open Sans Bold," because the absolute size of the strokes is what determines whether the bit can resolve them.
Tervika lets you set cap-height directly (in mm or inches) rather than as a typographic font size, which avoids the most common mismatch.
Material allowances
Three numbers separate "the file" from "the finished plate."
Kerf. The width the cutter removes from the material. For a router, kerf equals tool diameter. For a laser, kerf is the heat-affected width of the cut, typically 0.1-0.3 mm. For waterjet and plasma it's larger. For a clean-fitting plate, you want the cut path offset by half the kerf so that the plate, not the line, ends up at the specified dimensions. Most CAM tools handle this automatically once you tell them the tool diameter and which side of the line to cut on.
Tabs / onion-skin / leave-skin. When you cut a plate fully through, the plate falls free of the stock. Small plates get sucked into the dust collector. Sharp arrow tips dive into the spoilboard. The fix is either to leave tabs (small uncut bridges, 5-10 mm wide, holding the plate to the stock) that you cut by hand after the toolpath, or to use an onion-skin technique that leaves the last 0.5-1 mm of material connecting the plate, which you snap or sand through afterwards. Tabs are more reliable; onion-skinning is faster.
Fixturing. A plate held to the spoilboard with double-sided tape works fine for one-offs. For production, vacuum holds are faster and more reliable. For thin plates (under 6 mm), use a sacrificial backer board to prevent the plate from flexing under tool pressure. For metal plates, clamps are usually safer than tape.
A pre-flight checklist
Before pressing "go" on the CAM side, run through:
- Units in CAM match the DXF. If Tervika exported in millimeters and your CAM is set to inches, your plate will be 25.4× too large. This catches more people than you'd expect.
- Tool list is selected. A common bug is that the toolpath references a tool number that doesn't exist in the tool library, and the machine cuts with whatever's in the spindle. Verify the tool before run.
- Origin / zero is set on the actual stock. If your DXF has its origin at the plate centerline but you've zeroed your machine at the stock corner, the plate cuts off the edge of the material.
- Toolpath simulation runs cleanly. Most CAM tools have a simulation step. Use it. It catches "the bit plunges through a clamp" before the bit plunges through a clamp.
- First cut is a "dry run" at full speed, no spindle. The machine moves through the program with the spindle off, so you can see whether the path is where you expect. This catches origin errors and is fast.
- Cut a test in scrap first, especially for engraving depth. A 0.5 mm depth difference looks fine in simulation and looks shallow on the actual material. One test cut saves a sign.
When the file looks wrong
If you import the DXF and it doesn't look right, the problem is usually one of:
- Self-intersecting polygons. Tervika's exports are clean, but if you've edited the DXF in another tool, you may have introduced overlaps. Most CAM tools highlight these.
- Missing layers. If the import shows only the outline and no text, check the layer-on/layer-off filter in the import. Tervika's text is on a separate layer that some imports default to "off."
- Tiny segments. Some CAM tools complain about polylines containing very short segments (under the tool's resolution). Tervika's exports should not produce these, but if you've run a simplification step that introduced them, run a "remove duplicate points" or "tolerance simplification" pass.
- Open polygons. Cut profiles need closed polylines. If the import shows the plate outline as a series of open arcs, run a "join" or "stitch" pass with a tight tolerance.
The general rule: if the DXF looks broken in CAM, re-export from Tervika rather than try to fix it downstream. The export is deterministic, and a fresh export takes a few seconds.
What good looks like
A well-prepared CNC sign comes off the machine looking almost finished. The text is readable from across the workshop. The edges are clean. The holes line up with the post hardware. The only remaining work is light sanding, finish, and assembly.
That outcome isn't about a fancier machine or a more expensive bit. It's about the file describing what you actually want, the CAM matching what the file says, and the operator picking toolpaths that suit the material. Tervika does the first part of that. The rest is craft.