Editing Laser cutter class

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.

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 [[Laser_Manual#Known_good_materials|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.

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".