Laser cutter class
This page is the overview for the laser cutter class, a part of the Noiseschool project. The class is a project-based introduction to the software and hardware of the laser cutter, intended to teach participants in the class everything they need to know in order to use the laser cutter. We assume no prior knowledge of the software involved, only general knowledge of how to use a computer.
This class is broken into three main parts: part 1 deals with the design of the laser cut object using Inkscape, part 2 deals with the use of the laser cutter software, and part 3 deals with the operation of the machine itself.
- 1 Project Overview
- 2 Part 1: Design using Inkscape
- 3 Part 2: RDWorks/LaserWorks Laser Cutter Software
- 4 Part 3: Laser Cutter Machine Operation
- 4.1 Parts of the Laser cutter
- 4.2 Moving the Cut Head and Cut Bed
- 4.3 Preparing and Loading the Material
- 4.4 Focusing the Laser
- 4.5 Loading Files
- 4.6 Changing Layer Settings
- 4.7 Setting the Origin and Tracing a Bounding Box
- 4.8 Performing a Dry Run
- 4.9 Performing a Powered Run (ie Actual Cutting)
- 4.10 Cutting the Black Piece
- 4.11 Assembly
- 4.12 Cleaning the Catch Tray
In this project, we will create a laser cutter merit badge that employs many standard techniques in laser cutter design. This won't be a complete, in depth overview of the laser cutter and everything it can do. Instead, you'll learn a variety of standard techniques, along with the processes required to make use of them on the laser cutter, so that you become comfortable with the machine. These techniques include some basic design skills, preprocessing, vector cutting, vector engraving, press fit design, cut order optimization, and the general control of the machine. You will not learn laser safety: you must go through a separate training session for this. Please see the Laser Manual for more information about laser safety training.
This class has one suggested prerequisite, namely the class on design software, which will give you a more complete understanding of Inkscape than is provided here. While the prerequisite is not absolutely required, it's suggested because it helps you understand the software at a more general and fundamental level than we teach in this class.
Part 1: Design using Inkscape
In this part of the project, we will design the merit badge, both the physical aspects and its realization in software. There are therefore 2 main steps to perform here. The first step is to sketch out and decide on the overall design and dimensions, the second is to translate this into a precise sketch in Inkscape. This particular merit badge will be made of acrylic, but the steps described below work for pretty much any material you can cut on the laser cutter, provided it has sufficient thickness.
The merit badge we'll make will be based on the Noisebridge logo, as sketched below. We'll have an inset central Noisebridge logo out of black acrylic, and the rest out of blue acrylic. The outer portion of the logo will be engraved, as will the text.
Precise Sketch / Inkscape
We can get the Noisebridge logo in SVG format from the identity page. The direct link to the SVG file is https://noisebridge.net/wiki/File:Noisebridge_logo_not_by_idiots_for_cnc.svg. We'll open the logo in Inkscape and make some changes. Make sure to resize the canvas and save it as a new file. It's also useful to set up some grids. Millimeter units are generally the most useful.
Before we go any further, it'll be useful to resize the logo to be 60mm in both dimensions. This will make it easier to align things later. We'll select everything (control-A) and then set the size in the toolbar. Make sure the units are millimeters.
Now on to the real editing. First, let's get rid of the text, since we don't actually want that in the final logo. We can just select the text and delete it.
Next, we'll remove the negative space from the inner part of the logo, because we want the inner part of the logo to be solid black. To do this, we'll need to use the path editing tool in the toolbar on the left. We'll just select the nodes for the inner paths and delete them.
Now let's make the pill shape around the outside. We'll use the rectangle tool and round the corners. I'll make the height of the rectangle 10m more than the diameter of the logo (70mm), and the width will be three times the diameter plus 10mm (190mm). The corners will be rounded with a radius in both directions of half the height of the rectangle (35mm), to produce an actual semicircle instead of just a rounded rectangle. We'll also position the rectangle so that the logo is centered on the left end's semicircle. Again, make sure that all the units are in millimeters. Additionally, it's useful to make the fill of the pill shape partially transparent, or to use only a stroke, so that we can see the logo underneath it. You can also reorder the objects after you make the pill the right size.
Finally, let's add the text. We should leave some space on the right end so that we can optionally add a hole for putting the badge on a keychain or something like that. We'll adjust the size to be pretty big but not too big.
Looking at the overall size, it's a little large. Let's make it smaller. Select everything and scale it proportionally, so that the height is 30mm. Make sure that the proportional resizing lock is enabled so that the width is scaled automatically in proportion to the height.
The design is now done, and we can save the file.
Part 2: RDWorks/LaserWorks Laser Cutter Software
In this part, we'll go over how to import files into RDWorks and prepare them to be laser cut. We'll need to perform a number of steps, including a pre-processing conversion of the file into a usable format, an assignment of cutting properties appropriate for the material and process type, and an optimization of the cut order.
Converting to DXF and importing to RDWorks
The laser program RDWorks can accept a number of file types, but unfortunately SVG isn't one of them. What we'll do, then, is convert our SVG badge into a DXF file, which RDWorks can use. Before we do this, however, we'll need to perform some preprocessing steps. If we just save a DXF directly, without performing these steps , RDWorks will interpret the file incorrectly, like so:
As you can see, there are lots of extraneous lines, missing curves, no text. If we left the file as is, the laser cutter would cut precisely this, producing an incorrect piece. To fix this, we need to eliminate all the bezier curves in the image.
With the image loaded up in Inkscape, select everything and convert all of the objects to paths (Path > Object to Path). Next, ungroup all of the objects (Object > Ungroup>. This is especially important because we have text, where the whole text object is a group composed of multiple smaller objects for each letter.
Finally, we'll flatten out all of the bezier paths (Extensions > Modify Path > Flatten Beziers). We'll pick the flatness to be 0.1, which is the smallest we can produce with this tool. If we need a smaller size, we can always scale up the objects first, then apply the tool, then scale it back down.
Now we can save a DXF. In the save dialog window, select Desktop Cutting Plotter (AutoCAD DXF R14) (*.dxf) from the format dropdown menu. It's the longest entry in the list, which is useful to know if you plan on doing a lot of laser cutting. Make sure that the DXF's base units are set to millimeters so that when we import into the laser cutter software, everything will be sized correctly.
We can now import the file into RDWorks. In a new document, import the DXF file just created (File > Import). Be sure to use import, not open, as the open dialog window only supports RDWorks' own RLD format.
We can now see that the imported image has none of the extra lines that we had earlier.
Assigning Paths to Layers, Setting Layer Parameters (Blue Acrylic)
Because we're going to be using two different kinds of acrylic, and doing two different kinds of lasering, we need to assign the paths to different layers so that we can use different properties for each. We'll also need to have two separate patterns to send to the machine, one for the blue acrylic, and one for the black acrylic. We'll go through the process for the blue acrylic first.
Notice first that all of the paths are currently black. This means that they're assigned to the black layer. Layers are identified by color alone. Select the outer rings of the Noisebridge logo, and the text, by clicking the paths and/or click-dragging a marquee. Now assign them to the blue layer by clicking the blue square at the bottom left of the work area.
Now select the inner part of the Noisebridge logo and assign it to the red layer.
We've assigned three different layers because each will have distinct properties. The black layer will be a simple cut. We don't need it to be precisely sized because its just the external edge of the badge, and doesn't have to interlock with anything. The blue layer will be engraved, not cut. And finally, the red layer will be cut, but needs to have its size tightly controlled to adjust for the fact that when you cut material, the cut has a thickness, and the resulting piece is not precisely the size you've specified in software.
We'll now modify each layer to specify its different properties. Double click the black layer in layers tab at the top right of the work area. This brings up the layer properties pane for the black layer.
Since we want to cut this layer, we'll set the processing mode to Cut.
We also need to specify the speed and power for this layer. The blue acrylic I'm using is 3mm, so we look this up in the laser manual's section on known materials, so the speed is 20mm/s and the power is 55%, but the acrylic you use may have different settings. We'll enter these into the speed and power fields of the layer parameters pane. Make sure to set both the min power and max power to the same value.
Next, we need to make sure no special size adjustments are being made, so click the advanced button as shown below and make sure none of the boxes are checked. We'll see these again for the red layer.
That completes our settings for the black layer. We can now move on to the blue layer, which is for engraving. Click the blue swatch of color on the left side of the layer parameters pane.
As with the black layer, we need to set the processing mode, but this time it should be set to Scan, which tells the laser cutter that it should raster scan inside the paths rather than cut along them.
We'll also look up the speed and power settings for engraving and enter those as before. Acrylic engraves at 400mm/s and 5% power regardless of thickness.
Next we'll set the parameters specific to scan processing mode. In the bottom of the pane, we'll select the scan mode to be X Swing. There are four options here, X Swing, X Unidirectional, Y Swing, and Y Unidirectional. The X and Y options determine which directly the raster lines move, and we want X because that's fastest (it only moves the cutting head, rather than the whole armature). The Swing options specify that engraving should happen when the cutting head moves both left and right, whereas Unidirectional specifies that engraving happens only in one direction of motion. Swing is faster, but produces lower quality engraving. We pick X Swing because this project doesn't require very high detail.
We also have to specify the line separation. This is the distance between raster lines, and the smaller the number the higher detail we can produce, but the more raster lines (and so more time) is required to produce the image. We'll pick 0.1mm, as this is a good quality, and works well for the speed and power we used.
Finally, we'll select the red layer. This layer will also be Cut mode, with the same speed and power as the black layer. However, unlike the black layer, we need to adjust the position of the cut because this will need to fit snugly with the black acrylic insert. To do this, click the advanced button and make sure Sew Compensation is checked. RDWorks gives this a strange name; to the rest of the laser cutting world, this is called kerf compensation. We need to specify the kerf size, which for acrylic is about 0.15mm, as listed in the manual. We might end up adjusting this later depending on how well the fit is. Because we want to keep the part of the acrylic that's outside the path, not inside, we set the compensation direction to inward.
We're now finished with assigning layers their parameters, so make sure you click the OK button in the layer parameters pane. If you click the pane's X/close button on the top right, or if you just hit enter, the software will forget all of the settings you just put in, so be sure to click OK.
Optimizing Cut Order
We now need to specify the order that the paths should be cut/engraved. We do this because the laser cuts at a very specific focal length, and if a piece moves after being cut free from the bulk material, its focal length will change, making it bad to cut on it again. If we work inside out, we guarantee that nothing ever falls out of focus until we've finished working on it (so long as the pieces are completely non-overlapping).
First, let's make sure that we have path previewing turned on, so we can see where the laser will move. Make sure the tool is enabled in the tool bar.
You can see where the laser will move, and the inflection points tell us where the laser enters and leaves a path. For this path, it's obviously not working inside to outside, so let's fix that.
Select everything (control-A) and open the cut optimization tool (Handle > Cut Optimize). Make sure that Inside-to-Outside is checked, and click ok.
The laser's movement preview changed, and now we can see it working inside to outside.
We'll now simulate the process, to ensure that everything is working correctly, and to find out how long it will take. Click the little monitor in the tool bar to open the simulation tool.
Click the Simulation button on the right. If the movement is too slow, adjust the Simulate sider, which specifies the simulation speed as a proportion of the actual speed.
Here we can see that everything looks good.
Now we'll note down the Light Time listed on the top right. Because this project has mixed cutting and engraving, the time might be inaccurate, so we'll compare it later to what the machine says. We need this information to determine how much we need to pay for the laser usage.
Downloading to the Machine
We're now ready to download the file to the machine. Click the download button on the bottom right of the workspace.
When prompted, give your file a name. The name must be alphanumeric only, and at most 8 characters. The choice is mostly arbitrary, as it's only used to identify the file on the machine. In this case, I'll use "blue", since this will be the blue piece of acrylic.
Similar steps for the Black Acrylic
We'll also perform some similar steps for the black acrylic piece. We'll use the current design as a starting point. First, we'll delete everything except the inner part of the Noisebridge logo, since that's all we want from the black acrylic.
Next, we'll change the layer parameters. Use the appropriate processing mode (cut) and appropriate speed and power. For the acrylic I'm using, it's 6mm thick, so the speed is 8mm/s and the power is 55%.
We'll also adjust the kerf compensation. We'll use the same kerf width, but because we now want to keep the inside of the shape, we'll set the direction to outwards.
We'll download this onto the machine as "black".
Part 3: Laser Cutter Machine Operation
This part of the class will go over the parts of the laser machine and its operation, both project-specific operation and also more general operation that you might need in course of using the machine.
Parts of the Laser cutter
In this section, we'll look at the main parts of the laser cutter. In the picture below, you can see the outside of the laser cutter. There are two main parts to be aware of: the control computer on the right, and the scrap collection bin at the bottom.
Opening up the lid, we can see the cut head and the cut bed. The bed has a mesh on it usually, but underneath, there are rails.
The cut head itself has multiple parts. The mirror on the top redirects the laser down into the focusing tube, where it passes through a lens and then out the bottom aperture of the tube. You can also see the air blower connector, which has a screw to control air flow. The wing nut secures the focusing tube in place.
Moving the Cut Head and Cut Bed
On the control computer, we can use the arrow keys to move the cutting head around the bead as shown. The cut head will automatically stop when it reaches its maximum positions.
If the speed of the cut head is too fast or too slow, you can change it by pressing the Speed key on the control computer, and then adjusting the speed. The interface here is slightly clunky: you must select a column (1s, 10s, 100s) in the speed number using the left and right keys, and then use the up and down keys to set the value for that column.
To raise the cut bed up and down, press the Z/U key in the center of the arrow keys, and make sure the Move Z option is highlighted, then use the left and right keys to lower and raise the bed. Be careful not to crash the cut head into the cut bed!
Preparing and Loading the Material
When cutting acrylic, it's useful to cover the back of the material with masking tape, or to place the material on a piece of sacrificial material such as scrap cardboard, to prevent reflections and other heat from marking it. Sometimes the acrylic already comes with a paper backing. We also can put masking tape on the top, which is especially useful when cutting wood, to prevent smoke stains, but this sometimes requires a slight increase of power to cut through the masking tape, depending on what the settings are for the material.
Now move the cut head as far back as possible, and load your material into the machine. Be careful not to hit the cut head!
Focusing the Laser
To focus the laser, get one of the thin ~8mm spacer discs from the laser cutter tool box. Move the cut head over the material you're going to cut, preferably in the region you'll be cutting. Place the space disc under the cut head, so that the guide laser's red dot appears on the disc. While gently holding the air blower connection, loosen the wing nut until the cut head can move freely, and lower it until it's resting on the spacer disc. Tighten the wing nut, and remove the spacer disc. The laser is now focused.
If the focus tube is extended too far, it can wobble and produce non-vertical cuts. To avoid this, raise the cut head, then raise the cut bed a little bit, making sure there's enough room for both material and focusing. This lets the focus tube get a better fit in the cut head, and avoid wobbling.
The laser's focus tube has a lens in it, with a fixed focal length approximately 8mm below the end of the focus tube. If the aperture is dented, however, the tube is shorted, and the focal point is no longer 8mm below the end of the tube but rather further down inside the material, which is why it's important to be careful when moving the cut head or the cut bed to avoid crashes.
Make sure to focus the laser every time you load material of a new thickness into the machine, as the focal point will need readjusting.
On the control computer, from the main screen, press File to bring up the list of files on the machine. Select a file by moving up or down with the arrow keys, then hit enter. The file you've selected should now show up in the file preview.
Changing Layer Settings
Sometimes it's necessary to modify the speed or power of a layer on the machine itself, for instance when adjusting engraving settings, or dealing with material that isn't cutting all the way through.
With your file loaded, press enter. The first layer in the layers list should now be highlighted. Select the layer you wish to modify with the arrow keys, and hit enter again.
This info pane lets you modify a number of settings, but the primary ones we care about are speed and power 1. Use the Z/U key to cycle through the data fields to select the ones you wish to edit, and then use the arrow keys to edit the value. Just as when we edited in RDWorks, we must set the min power and max power to be the same.
Hit enter to save and then again to continue back to the file.
Setting the Origin and Tracing a Bounding Box
With the file now loaded up, we can specify where on the material we want to cut. Move the cut head so that the guide laser is pointing to the position that you want to be the top right of the cut image. Press the Origin button on the control computer to store this location, and press Frame to trace a bounding box. Watch the cut head to make sure that the bounding box is where you want it to be.
You can change the origin's relative position in the image, to set it to be the lower left, for instance, or the center, instead of the top right. You can also reset the origin to the top right if it's been left in a different position. To do this, we need to use RDWorks. Open the file parameters pane (Config > System Setting) and select the location you want to use for the origin. You can also use absolute coordinates, as well, in which case the position of the objects relative to the RDWorks work area matters.
Performing a Dry Run
Now that we have the origin set, and we know that the bounding box is adequate, we can optionally perform a dry run of the job. Make sure the laser power is off and press the Start/Pause key.
If you need to pause the dry run (or a real run), hit Start/Pause again, and then restart with the same key.
If you need to cancel a try run, for instance if it's taking too long, or you've gotten as much information as you needed from it, pause the dry run, then hit the Esc key.
Performing a Powered Run (ie Actual Cutting)
We're now ready to actually cut the merit badge. Turn the power to the laser on and press Start/Pause to begin cutting. Be sure to watch the spot where cutting is happening, to look for fire.
When the job is done, the cut head will return to the origin, and the machine will beep. The parts should separate cleanly, but tall thing parts might need some coercion just because they can get wedged by being at slight angles.
If you need to pause or cancel the job, use the same method as mentioned in the previous section on dry runs.
Cutting the Black Piece
We'll go through the same process for the black piece of the merit badge. After finishing both cuts, I found that the black piece was slightly too big to fit into the hole in the blue piece, so I recut it with a slightly smaller kerf, but your results may differ.
The pointy parts of the merit badge's inner logo also need to be sanded or filed down. This is because when a point is cut in negative space, it's not a sharp point, but a positive space point can be perfectly pointy, and they won't fit together.
I used the files that are in the tool shelf next to the laser computer.
We can now press the black piece into the hold in the blue piece. It's a snug fit, but with a little effort, it now goes through.
Cleaning the Catch Tray
Now that you're done using the laser cutter, it's good practice to check the catch tray below the cut bed to see if any scraps have fallen into it. Open the door and pull the tray out.
If there's scraps in the tray, please clean them out. Open the little quarter circle. This will open up a hole that you can sweep the scraps through, into a dustpan.
It's important to keep the catch tray free of scraps, because any burning material that falls into the catch tray might catch scraps on fire, especially paper and cardboard scraps, as well as charred wood scraps.