Laser work with Laser.myWerkzeug.de

Laser.myWerkzeug.de and CNC.myWerkzeug.de are the same program in two modes. Drawing, text, import, templates, account and help are identical. Projects open in both: when loading, the app swaps milling tools and laser profiles and tells you.

What the laser does

Every layer and every shape gets a task. Choose it in the window at the object or in the Layers tab:

• Line: the beam runs exactly on the line. Engraving, lettering, scoring.
• Outside: the beam runs outside the outline and cuts the part free. It keeps its size because the app offsets by half the beam spot.
• Inside: the beam runs inside the outline: holes and openings.
• Fill: the area is filled with closely spaced lines (area engraving). Line spacing, angle and cross-hatch are set in the profile.
• Off: not lasered.

Laser profiles

A laser profile sums up how the laser works: speed in mm/min, power in percent, passes, beam spot, for areas line spacing and angle, an overscan at the line ends and the controller's highest S value (Grbl $30, usually 1000).

New projects come with "Engraving" and "Cutting". You create your own profiles in the Laser → Laser profiles … menu. Each layer picks one, a single shape may differ.

More settings in the profile:

• Bridges when cutting: with "Outside" the beam leaves pieces of the outline unburned at an even spacing (the bridge width). The part stays in the material and snaps out after lasering. Inside cuts and holes get no bridges.
• Air assist: turns the air on (M8) for this profile, off afterwards (M9).
• Scan offset: compensates the offset of the return lines in fast back-and-forth engraving. Tune with a test image, usually 0.1 to 0.5 mm.
• Beam spot Y: many diode lasers have an oval focal spot. Enter its width across the X axis here; the app then compensates the kerf separately in X and Y, and parts keep their size in both directions. 0 means: round, same as the beam spot.
• Z step per pass: in thick material the head lowers by this amount after every pass so the focus follows into the cut. After the last pass it returns to the focus height. 0 = off.

Order: the app orders the cuts itself. Engraving comes first, then cutting. Holes and parts that sit inside another part come before its outline, so nothing drops out or shifts before it is finished. Every outline starts where the head gets to fastest, and lines run backwards when that is shorter. The app then checks whether another order is shorter and swaps whole sections. This keeps travel moves short.

Thicker material needs more passes instead of more power: the laser traces the outline several times. The material library provides starting values for your material.

Kerf offset

When cutting outside, the beam centre runs beside the contour so the part keeps its size; inside it runs inward accordingly. Without your own value the app uses half the beam spot. It gets more precise with the measured value in the laser profile, field Kerf offset.

Measure kerf (menu Laser → Measure kerf …, also in the laser profile, after the test grid and in the command search) guides you in three steps:

1. Choose the profile you cut with. Power, speed and passes come from the profile.
2. Cut the test part: a square (default 20 mm) with a round hole (default Ø 10 mm), optionally with the sizes as a fine engraving. The laser cuts exactly on the line, without offset, first the hole, then the square. The origin is the bottom left corner.
3. Measure and enter: the square with the outside jaws, the hole with the inside jaws of the calipers, ideally on the underside. The square gets smaller by one kerf width, the hole larger by one kerf width. The app takes the mean of both (one value is enough too) and shows the kerf width and the offset (half of it).

Example: square 19.84 mm, hole 10.16 mm → kerf 0.16 mm, offset 0.08 mm. Apply to “profile” writes the offset into the profile; Undo in the window or Ctrl+Z restores the old value.

Oval laser spot: with Measure the square separately in X and Y you enter the outer size in both directions (then measure the hole across in X). If the kerf in Y differs, say 0.24 instead of 0.16 mm, applying also sets the profile's spot Y in the same ratio (here 1.5 times the spot), and the app compensates X and Y separately; equal kerfs set the spot to round.

The app checks the values: a square larger than drawn or a hole smaller than drawn cannot happen when cutting on the line; a kerf above 1.5 mm is not plausible. If square and hole differ by more than 0.06 mm (or 40 % of the kerf), it suggests measuring again: often the cut edge is slanted (focus) or the calipers are tilted. If you share your values in the material library, you can include the measured kerf; whoever applies them gets it in the new profile.

It also works by hand: cut a 20 mm square outside, measure it (for example 19.82 mm), the kerf is 20 − 19.82 = 0.18 mm, the offset half of it: 0.09 mm.

0 means automatic (half the beam spot). If the beam spot is oval (Beam spot Y), the offset in Y follows in the same ratio. Line and fill are not affected. The Laser tab shows the value next to the profile (“kerf 0.09 mm”). LightBurn projects and libraries bring the layer's “Kerf Offset” along (LightBurn).

Your laser machine

Under Machine → Set up machine you pick your laser from the list of common diode lasers (Sculpfun, Ortur, Atomstack, xTool, Creality, Longer, TwoTrees, Comgrow). The app takes over the work area, optical power, beam spot in X and Y and whether air assist is built in. If your model is missing, choose "Weitere Modelle" (other models) or "Diodenlaser (Grbl, generisch)" and enter the values yourself. The power is the optical output of the beam, not the electrical input that often appears in the model name.

The app builds on this: new laser profiles get the machine's beam spot and S range, cutting profiles from the material library switch the air on, and the material library calculates its starting values with your power. If an existing profile differs, Laser → Laser profiles … offers the Use machine values button.

CO₂ lasers with a Ruida controller, the K40 with an M2 Nano board and devices that only run through the maker's cloud do not speak Grbl and are therefore greyed out in the list.

G-code for GRBL, Marlin and LinuxCNC

The app itself always lasers with Grbl. Saved G-code files (Export and ZIP) are written for the controller chosen under View → Settings → Machine → G-code files, for example for a laser at another computer:

• Grbl / grblHAL / FluidNC: M4 (dynamic power, off during rapids), S 0 up to the S range of the laser profile ($30). The controller must run in laser mode $32=1.
• LinuxCNC: M4 with S 0–1000 as power, % at start and end, path mode G64, extension .ngc. LinuxCNC (analog M67): M3 enables the laser, M67 E0 Q0–100 sets the power synchronised with the next move, Q0 before every rapid; the analog output E0 is wired to the laser in HAL.
• Marlin (laser M3/M4 inline) for Marlin 2.x with the laser feature: M4 I switches inline mode on, S 0–255 applies per move, every rapid gets S0, M5 I at the end. Semicolon comments, no G94, no M30 (which deletes a file on the SD card in Marlin), extension .gcode.
• Marlin (laser on fan output M106) for older firmware without the laser feature: M106 S0–255 before every cut, M107 before every rapid and at the end.

The paths are the same everywhere; the preview shows a short example. Customise turns it into your own setting: switch on with M4 (dynamic) or M3 (constant), power as S, M106 or M67, inline mode, maximum power value (0 = S range of the laser profile) and the commands for air on/off (default M8/M9; for Marlin without coolant commands for example M106 P1 S255/M107 P1). Plus file extension, comments, line numbers, decimal point and program start and end with placeholders for laser profile, power value and project.

Duration and checking

The Laser tab shows all tasks by profile with the estimated duration. A click selects the shapes. Notes from the app (shapes too narrow, open lines when filling) appear below.

Then continue with the Laser button: Start lasering.