Skip to content

Cut Settings - Line Mode

The image above shows the settings for 'Line' mode. In this mode, the laser follows the exact path of your design, tracing the lines with the beam enabled at the power you've chosen. If you move quickly, or with low power, you will likely just etch the surface (sometimes called vector marking). If you move slowly and with high power, especially with a CO2 laser, you will cut deeper, possibly through the material.

The only difference between surface marking and cutting is the power and speed. (In older versions of LightBurn this was displayed as 'Cut', but the term was changed to make it easier for new users, and the functionality is identical).

Number of Passes

How many times the laser will repeat the shapes on this layer. Sometimes, when cutting thick material, trying to engrave very deep, or using a lower power laser, more than one pass may be necessary.

Z Offset

If you have Z moves enabled, and your controller supports it, the Z Offset setting can be used to move the laser head closer to the material (inward) or farther away from it (outward). Focusing deeper into the material can sometimes help to cut thicker material, and lifting the laser away from the material can produce a thicker line.

Z step per pass

When doing more than a single pass over a shape, the Z step per pass setting allows you to tell LightBurn to raise or lower the laser with each pass by some amount. This is most often used for thick cutting or deep engraving, allowing you to shift the focus point deeper with each pass to help maintain efficient cutting.


If your system uses auto-focus, you may not be able to push the focus point lower, because most systems treat the auto-focus height as the lowest possible height (Z limit) to avoid crashing the laser head. Be careful in general using Z moves, as this does have the potential to physically damage your laser.

Kerf offset

Kerf is used to mean the thickness of the cut itself when using a cutting tool. If you use a table saw, and the blade is 2mm wide, it has a kerf of 2mm (or just slightly more). A laser burns material to cut, and although the cut is very thin, it does have width, and this width needs to be compensated for if you are trying to make parts that fit together, like a tabbed box, or an inlay. Kerf offset works exactly the same as the Offset tool in LightBurn, but it happens "on the fly" as the cut data is generated for your laser, so it does not alter the original design.

Using outward kerf moves the laser beam outward, away from the shape, and using inward kerf moves it inward, into the shape. LightBurn accounts for the fact that holes in a shape will need to be offset in the opposite direction, as shown here - the solid lines are the original shape, and the dashed lines are the result of shifting the kerf out or in:

Perforation Mode

The dotted lines above were generated using a different setting, called Perforation Mode. If you are trying to cut fold lines in card stock, stitch holes in leather, or just make dashed lines, perforation mode allows you to choose the distance to cut, followed by the distance to skip.

This can also be very useful when trying to cut delicate material with a powerful laser - Setting very low cut and skip values, like 0.1mm each, toggles the beam on and off very quickly, and gives you an effectively lower power output. Varying the ratio between the two lets you adjust that power - using 0.1mm for both cut and skip would give you the effect of 50% of your chosen output power, because it is spending exactly half of the time with the power on. Using 0.05mm and 0.15mm for cut and skip, respectively, would be 25% of your chosen power, because it is only cutting for 25% of the total distance of the shape.

Tabs / Bridges

As Tabs / Bridges is a much more complicated feature, you can find an in-depth walk through on the Tabs / Bridges page.

Advanced Settings

Under the Advanced tab you'll find a couple useful, but less frequently used options.

Start / End pause time

These options can be used to add a delay at the beginning of a cut, the end, or both. If you also enable the 'Cut Through' option, the beam will be turned on during this pause, which can be used to 'prime' the cut, for example when cutting very thick material. The 'Power %' value sets the power of the laser during this pause.

If used without the 'Cut Through' toggle enabled, it can be used to add a delay to let the gantry settle down after a rapid move, or allow time for an air assist solenoid to engage.


This option tells LightBurn to keep cutting closed loops for the specified distance, which can help when cutting through thick material, where the start of the cut sometimes doesn't make it all the way through.

Override PWM Frequency

If you have an RF Excited tube, this setting allows you to control the PWM frequency of the pulses sent to the laser, and can change the edge finish on certain materials.

Override PPI

Only available on Trocen controllers, the PPI setting (Pulses Per Inch) lets you tell the laser to send an exact number of pulses per inch of travel, instead of varying the beam power directly. This is useful for delicate materials like paper, and is similar to using Perforation Mode, but is handled by the hardware itself.

Lead In / Lead Out

Lead-in and Lead-out are optional lines or curves added to the start or end of a cut. When cutting thick material, particularly if using 'Cut Through' delays, or cutting metal, there is often a mark left at the start of the cut that is slightly thicker than the rest, and can leave an indent on an otherwise smooth edge. With this setting, you can add a small line to the start or end of a cut, so that mark happens off the cut line itself. The 'Angle' value controls the placement of the lead line - a positive number tells LightBurn to put the lead line outside the shape, and a negative number means to put it inside. You can choose to make the lead a straight line, or a short arc.

The shape above on the left is using an arc set to +45 degrees, so it starts outside the shape. The one on the right is a line set to -20 degrees, so it appears inside the shape.

Dot Mode

When enabled, the laser will pause and pulse at regular intervals along the path, instead of cutting continuously. The 'Time' value specifies the pause delay in milliseconds, and the spacing parameter sets how far apart the pulses are. This can be an effective way to do stitching holes, or cut very thin or delicate materials, but the constant pausing can shake the machine - using Perforation Mode is often preferable for this reason. This setting is not available on all lasers.