From download to cut

A DXF file is a plain drawing file that every cutting program understands. The file contains only closed outlines — no text objects, no fills, no colours — which is exactly what a cutting controller wants.

Curves are written as many short straight segments rather than splines. Splines are the usual reason imported letters look lumpy or fail to generate a cut path.

If you turned on a backing plate, the plate outline and the letter holes are all in the file as separate closed contours. If you turned on stencil bridges, the bridge tabs are already cut into the letter geometry. RayTools does not need a special setting for either — it just cuts the shapes.

Tip You can verify the shapes by downloading the SVG and opening it in any browser — what you see is exactly what gets cut.

In RayTools, click File → Open (or the Open button) and select the .dxf file. The drawing arrives already in millimetres, so no scaling step is needed.

After import, RayTools can auto-optimise the graphic — let it. It will merge duplicate lines, join segments, and delete invisible micro-fragments.

Check the reported part size on screen against the width and height shown on the generator page before cutting.

A laser beam has a physical width (the kerf), typically 0.1–0.3 mm depending on material and thickness. Without compensation the cut parts come out slightly the wrong size — outer edges shrink and inner holes grow.

Select all the graphics, then click Compensate in the Home sub-page. In the compensation library, pick your material and thickness — RayTools loads the correct Extended Distance and Inside Shrink Distance automatically.

Set Compensation Way to "Expand and contract": outer contours (the plate outline) expand outwards, and inner contours (the letter holes) shrink inwards. This keeps both the plate and the letter cutouts at the right size.

Tip If you don't have a compensation library set up, enter the kerf value manually. For 3 mm mild steel with a 2 kW fiber laser, a typical kerf is 0.15–0.2 mm. Ask your laser supplier for the exact value for your machine and material.

Leadlines let the laser pierce outside the cut path and glide in smoothly, avoiding a burn mark at the start point. RayTools auto-detects inner and outer contours — the plate outline is the outer contour, and the letter holes are inner contours.

Select the letter-hole contours and click Inner Cut — this puts the leadline inside the hole so the pierce mark is hidden in the waste material.

Select the plate outline and click Outer Cut — this puts the leadline outside the plate so the pierce happens in the scrap around the sign.

Click Sort in the Home sub-page to auto-sort the cutting sequence. RayTools will typically cut all inner contours (letter holes) first and the outer contour (plate outline) last.

This matters: if the outer plate is cut first, the piece can shift on the bed before the letters are cut, and they end up in the wrong place. Inner-first keeps the plate rigid while the holes are cut.

Use Simulate (Simu button in the CNC sub-page) to verify the order before cutting. You should see all the letters cut first, then the plate outline traced last.

If you want the finished plate to stay attached to the surrounding sheet after the outer outline is cut (so it doesn't fall through the slats), add a MicroJoint. Click MicroJoint in the Home sub-page and click on the outer contour — RayTools leaves a tiny uncut tab that holds the piece in place.

After cutting, snap the sign free and file the tab flat. This is purely optional — if you have a clean bed or support bars, you can skip it.

Tip RayTools also has its own Bridge feature, but if you already turned on stencil bridges in this tool, do not also add RayTools bridges — you'll get double tabs.

Click Process and select your sheet material and thickness. RayTools loads matching power, speed, frequency, and gas pressure settings from its parameter library.

If you don't have a parameter library set up, enter the values your laser supplier recommends for the material and thickness you're cutting.

Run Simulate one more time to confirm everything looks right, then start the cut.

Thin strokes are the main failure point. As a rule of thumb keep the narrowest part of a letter at least twice the material thickness — in 3 mm steel, aim for 6 mm minimum stroke width. Increase the letter height or pick a heavier font if the preview looks spindly.

Serif fonts with hairline strokes need more height than a heavy sans to survive cutting and handling.

This tool never talks to the laser. The controller has no public interface, and driving a multi-kilowatt fiber laser around its own safety-checked software is not something to attempt. The DXF handoff is how the whole industry works.