The basic operations of any device can be categorized in one of two ways: Cut and Scan. These two options combined with variations in power and speed can achieve a variety of results.
Settings will vary from machine to machine and acrosss different materials. It is recommended to test your settings on a scrap piece of the same material as your final work piece before your final run.
Please Note: Cut speeds have been limited to 2000mm/s (or equivelant) This will prevent issues of entering too high of a speed which we are sure your machine will not like.
To the right of the cut window you will see 4 arrows. The up and down arrows allow you to change the order of the highlighted cut or scan layer, and the right and left arrows allow you to copy cut or scan settings into the cache, and write those cached settings into a cut or scan layer. Useful for copying settings from one layer to another.
Output is an on/off selection. By default this setting is on for a layer. This means that the laser will output the contents of the layer. Turning this setting off will skip creating instructions for the layer and the layer will be ignored. This is useful for alignment lines or other content that should not be in the end product.
This is also an on/off selection. If your machine is capable of turning air assist on or off automatically, set this to on to enable your air assist or off to keep it off. If your air assist is always on or manually controlled, this will have no effect.
Speed is the feed rate when the laser is firing. This does not affect the feed rate for rapid move (IE moves traversing between cuts). By default, speeds are shown in mm/sec, however if you are using a lower power diode laser, you can change this to mm/minute in the settings.
This is the maximum percentage of power that the laser will produce during the cut.
For DSP devices (not GCode based controllers) this is the minimum percentage of power that the laser will produce during the cut. On Ruida machines, this is power setting that will be used during a cut when the machine slows down to reverse direction, or make a sharp corner. You should normally set this number to just above the threshold where your laser fires. Setting it the same as Max Power means the laser will not change power output as the speed varies, which will result in a poorer quality cut, particularly on thinner materials.
Please note: Ruida controllers have a “Start Speed” value in the controller that is the point where they start ramping power from Min to max. Below that they just use min power. If you’re cutting slow, set min/max to the same value.*
This can be used to choose the operation for the layer. Cut, Scan, or Scan+Cut
Line will trace the laser along the vector path. Depending on the power and feed rate settings, this can be used to cut through a material in single or multiple passes, using high power, or to simply mark a line on the surface with lower power.
This setting is only available for Ruida and GRBL based machines. Enabling this setting will allow the laser to dwell in the same position after initially firing or before turning off based on the settings below, and is useful for piercing thick materials before the cut starts.
- Start pause time (ms): Number of milliseconds to fire the laser before moving
- End pause time (ms): Number of milliseconds to fire the laser at the end of a move
- Power (%): Percentage of laser power while paused
- Kerf offset: Allows you to shift the cut inward or outward from a closed shape to compensate for the diameter of the beam. This is useful when making parts like inlays or finger joins.
- Z Offset: Specifies an amount to offset the laser head (or bed) for this cut. Useful for defocusing, or pushing the focus point into deep materials for cutting.
- Number of Passes: The number of times the laser will trace the same path
- Z step per pass: Increase or decrease bed height for powered Z bed
Perforation mode allows cutting perforated or dotted lines (lines with gaps) without having to change the source artwork. You specify how long you want the cut, and how long you want the gap (skip), and LightBurn will alter the output when generating the cut.
This is most commonly used to create fold lines, but can also be used for living hinges or creating bridges or tabs in your designs. For example, setting a very long cut length, with a very short gap, will insert periodic gaps in the cut. The perforation mode is smart - if possible, it will make sure your shapes have at least one gap in them if the cut length is longer than the line to be cut. Perforation mode is also useful if cutting very delicate material. By setting short Cut and Skip values, you can reduce the amount of power the laser outputs to the material, much like dithering. This can reduce scorching on paper, or melting on thin plastics from overheating.
Dot Mode is similar to perforation mode, shown above, but the laser stops for each dot, fires for a set amount of time, and then continues.
The firing time is specified in milliseconds (thousandths of a second) and the spacing will be in whatever your distance units are set to (mm by default, or inches if you've changed it).
- Clicking on the Reset to Defaults button, will reset all cut settings to their default settings.
This option will fill the interior of a vector similar to engraving a raster image. When you select Fill from the Mode options, the settings below will become available.
This is an on/off value. With bi-directional scanning on, the laser sweeps back and forth, cutting from left to right, then right to left, and back again. With bi-directional scanning off, the laser fires only in a single direction, say left to right, then returns without firing, then fires again from left to right, and so on. The images below illustrate the difference - the black arrows show the direction of the laser firing, and the red lines show the path of the laser between firing moves (also called traversals). Bi-directional ON is usually preferred, because it is twice as fast.
Cross hatch is an on/off value. By default this is off which means your laser will only burn in the direction you have chosen. By turning this setting on you will get a second operation that will burn lines at 90 degrees to the first set, creating a cross-hatch pattern as shown below. This is mostly useful at higher interval settings as a way to give the appearance of a filled shape, while taking less time.
When engraving, the head is scanning back and forth. Because the laser has to accelerate and decelerate the head at the beginning and end of each line, on machines with limited power control this can cause darker edges than expected.
Overscanning generates extra moves, past the ends of each line, switching the laser off before it fully stops, or even before it begins to decelerate, allowing the entirety of the engraving to happen at the desired head speed and then decelerating while the laser is not burning. The overscan number is a percentage of your cut speed - the default setting is 2.5%, meaning a cut at 100mm/sec will move an additional 2.5mm past the last cut with the laser off.
Note, Overscan is applied automatically by DSP hardware, like Ruida and Trocen controllers. This setting is only available for gcode based systems which do not do this automatically.
Line interval is the spacing between scan lines. The lower this value, the less space will be left between successive passes. Lowering this value can create a slight overlap causing the laser to slightly trace over the previous line. Setting a higher value will leave untouched material between passes leaving visible scan lines. This is roughly equivalent to stepover for a CNC.
This is simply a different way to represent the Line Interval value above - more lines per inch is a smaller interval, and vice versa. Lines per Inch is a more intuitive number for many.
Setting this value controls the length of the ramp, or slope, on the sides of an engraving. Zero is the default, meaning that engravings will have vertical walls. If you create stamps with fine details, using a non-zero value for the ramp length will produce a ramp (from Min Power to Max Power) as the engraving moves away from the edges of your design, producing sloped walls that can help stabilize the stamp when in use.
This image shows a preview of the difference between an engraving with ramp applied, on the left, vs an engraving with no ramping, on the right:
The default scan angle is 0. This will produce scan lines along the X path only. By introducing a scan angle, your laser head will track at the selected angle using both X and Y during operation. As you change this angle, the graphic will show you the expected result.
On Ruida hardware, scan angles that are multiples of 90 degrees are supported natively by the hardware and will automatically overscan for you. Other angles are scanned using standard cutting commands.
Note: By default, LightBurn scans shapes from bottom up, because most laser systems exhaust in the rear, and this prevents smoke from being pulled across the freshly cut region. If you wish to scan a shape from top to bottom, simply set the scan angle to 180 degrees.
These options behave identically to their counterparts in a standard cut.
This setting tells the scanner to group all shapes within a cut layer together and scan them all at once. In most cases this is faster than scanning individually, if your laser is fast.
This will scan each distinct shape in your layer one at a time. For users with slower moving lasers, this will occasionally be faster than scanning shapes together. For example, if you have two filled shapes on opposite sides of your work area, filling one, then the other is probably faster than continually scanning back and forth across the work area.
This setting will treat grouped objects as a single unit for the purpose of scanning, allowing you the flexibility to choose which shapes get scanned together. For example, if you had 10 small shapes on the left side of your work area, and 10 more on the right side, scanning all shapes together would be slow, but scanning each one individually would be slow as well. Grouping the left objects into a group, and the right objects into another group, then using "Scan Groups Together" allows you to scan the 10 left objects in a single pass, then scan the 10 right objects in another pass, without having to traverse the entire work area.
This option is intended for use with slower machines where traversing is more time consuming than reversing direction. It will prefer direction changes over long traversals, and will save scanning time if the machine has a slow rapid speed, or quick acceleration. This can be used with image scans as well, but the cost to compute the path can be very high - use sparingly, and only with very simple image modes like threshold. It is worth noting that Flood Fill is affected by the "Scan all at once", "Scan together", and "Scan groups" settings, and it can also produce paths that are quite erratic, seemingly skipping lines at random. It will eventually go back to fill them in, so don't panic if you see this happen. It is a good idea to use the preview (and move the slider) to get a feel for how a Flood Filled job will progress, because it can be unpredictable.
Note the flood fill option is not available for DSP controllers at this time because the paths generated confuse the hardware. We are investigating this to see if we can correct it.
Fill+Line, as the name suggests, combines the fill and line operations. In order of operations, the fill will happen first followed by the line. This can be used to cut out a part once the fill is complete or simply emphasize the outline of the part before moving on to the next operation.
When you enable Fill+Line you will get the additional settings below. See the Line section for a description of each setting.
