Once we have our case designed, we need to setup CAM operations to tell the CNC machine how to cut out the design. We need to think about which bits and operations are best and determine what material we want to use. A good goal to have is optimizing for minimal machining time. This can mean having less operations or getting the most usage from a given tool.
There's a whole slew of operations that we can use to make our part. In Autodesk Fusion 360, you can hover over each type in the 2D/3D drop down menus within the CAM workspace. If you keep your cursor over the operation title, you'll get a handy tool tip with a description and thumb nail. This is really helpful and gives you an idea of what they do and when to use them. For this project, we can make our part with just a few of them.
This operation will remove material to get our stock to be the same height as our model. It generates straight passes that will mill away a given area/selection.
Let's you select an edge and generates a tool path that sweeps across the edge. This can take several parameters like number of step downs and starting positions.
Good for cutting out cavities and holes. Instead of just going in a single path (like a 2D contour), it generates concentric outlines that follow the edge of a given selection.
This is good for handling lots of different geometry. It'll analyze the model and automatically generate tool paths that will clear out the material. This will follow the contours of a surface and sequentially step down until the stock resembles the model.
Setting Up CAM
Now that we have a basic understanding of what operation types we can use, we need to create a "setup" for our parts. Since we have two halves and buttons, we'll need to create a "setup" for each part. A "setup" is a group of tooling operations that will makeup our part. In the setup, you'll need to define the size of the stock, it's coordinates and if we're using fixtures or jigs.
In Fusion 360, you can create a new setup by clicking on the setup icon within the CAM workspace. Once it's open you'll have various settings contained in a properties panel.
Under Work Coordinate System, select "Box Point" and choose one of the white dots that appear in corner of your model. You're basically picking the origin of the setup. On the Othermill, the origin for getting the best alignment will be on the lower left of the spoilboard. If the model is upside down, you can click on the blue Z arrow to flip the direction. Next, we need to select the correct model we want to mill. By default, everything will be selected. Under Model, click the X to clear the selection. Then, click on the part to select it as the model.
Set Stock Dimensions
In the "Stock" tab, you have the option to specific the dimensions of your stock. Under the "mode" drop down menu, are several options for choosing size and shape. I normally use the "Fixed" size and enter the dimensions of the stock. For the model position, I set offsets to the sides. I like to add a 4mm offset on the X and Y to ensure I get clean outline. I zero out the Z offset so the model is positioned to the bottom of the stock and not in the middle of it. Click the OK button to save your setup.
Othermill Tool Library for Fusion 360
Before we start adding some operations, it's a good idea to import Othermill's tool library into Fusion 360. A tool library contains info and details about the bits that are compatible with the Othermill. I suggest following the guide on Othermachine's website to get the library and installation. It'll walk you through the steps on how to do it, pretty straight forward.
Once we have our tool library installed, we can set our first operation. We'll use a facing operation. This will get our stock to the height of the model. In this specific job, our stock is 12mm thick and our model is 8.5mm tall. The face operation will therefore remove 3.5mm of material from the top.
Click on the 2D icon in the tool bar and select 2D Face. In the properties panel, select the 1/8in flat end mill. Then, change the following parameters.
- Cutting Feedrate: 800mm/min
- Plunge Feedrate: 381mm/min
We only need to change these two parameters. The rest of the settings are already set, all we're changing is the "speed" of the cut and how fast the tool should "plunge" down onto the material. Since we're cutting hardwood, it's best to cut at a speed that isn't too fast or slow. For softwood, you could cut faster, such as birch plywood – 1500mm/min is suffice. For other types of wood, you can refer to Othermachine's material support page.
The next settings to modify will be under the "Passes" tab. Here, we'll change the direction from "both ways" to "climb". When milling from both directions (left and right), it can leave behind some excess material – thin strips. If we tell the operation to mill from only one side, we'll get cleaner cuts – especially if we're cutting along the grain of the wood. Select "Multiple Depths". Here, we should set the maximum stepdown to 1mm. This is telling the operation how deep to cut. If we limit the depth to just 1mm, we avoid the risk of breaking our bit. Going too deep can cause the tool to snap from too much load. 1mm is a safe depth for the 1/8th flat end mill. OK to save the settings.
Under the 3D icon is Adaptive Clearing, click on it and choose the 1/8th" flat end mill. If the feedrates appear to have changed, go ahead and adjust them like we did for the facing operation. Under the Geometry tab, click on the machining boundary dropdown and choose "selection". Then, select the outer edge of the part. We're essentially telling the operation to only cut within the bounds of our part. This prevents the operation from milling out the entire stock. This saves a lot of time and lets us use any of the excess stock that doesn't need to be milled. It's also a good idea to set the Tool Containment to "Tool inside boundary". Next, under the "height" tab, look for "Bottom Height" and choose "Selection". Then, click on the inside inner surface of the part. By doing this, we're telling the operation to only cut until it reaches this surface. The cutout for the joystick and buttons are just too small for the 1/8th" flat end mill. So, we'll limit the adaptive clearing and finish the cutouts with a smaller tool. Last thing, go "Passes" tab and set the Maximum Roughing Stepdown to 1mm. Just like we limited the stepdown for facing, we don't want to cut too deep. After that, click OK to save and generate the tool path.
Before we switch out the tool, we should try to use the 1/8th" flat end mill as much as we can. The next operation is a 2D contour, found under the 2D icon. The 1/8th" flat end mill should already be selected along with our feedrates. If not, go ahead and set those up. In the Geometry tab, Contour selection should already be active, so you can click on the outer bottom edge of the part. In the Heights tab, make top height "model top" and bottom height, "model bottom". Under the "passes" tab, check the multiple depths option and set Maximum Roughing Stepdown to 1mm. So, here we're telling the operation where to start the cut, which is the top of the model because our face operation has cleared out the material to be the same height as the model. We've limited the stepdown to a safe amount, so we won't cut too deep on each pass. The toolhead will keep cutting along the outer edge of the case until it has reached the bottom of the model, which is also the bottom of the stock. That's basically all we need to tell the contour what to do. Click OK to save it.
Last operations to make are 2D pockets. Click on it and select the 1/16" flat end mill from the tool library. You'll need to adjust the feedrates like we did for the other operations. Under the Geometry tab, we need to make our pocket selections. Go ahead and select the edges that make the cutout of the joystick and buttons – that's 7 chains in total. In the Heights tab, set the Top Height to Selection and select the inner face. In the Passes tab, enable Multiple Depths and set maximum roughing stepdown to 0.5mm. It's important we don't cut too deep with the 1/16" flat end mill because it is thinner than the 1/8". So here we've told the operation where to start, what to geometry cut and how deep. Click OK to save.
We'll need a second 2D Pocket to make the holes in the corner standoffs. This setup will be similar to the first pocket, but we'll make a few changes. First, switch the tool to a 1/32" flat end mill. The 1/16" is too big to make our mounting holes. The 1/32" is just the right size. Under Geometry, select the bottom surface of each hole (not the top). Under Heights, make the Top Height a selection – click on one of the top surfaces on the standoff. For Passes, enable multiple depths and set the maximum stepdown to 0.25mm. Here, we've told the operation to mill out the holes, where to start, when to stop and how deep to cut. And that's it for our the top halve of the case. Click OK to save.
Now that our operations are set, we can simulate them. Click on Setup icon in the browser and then click on the simulate button in the tool bar. In the simulate panel, disable tool path and enable stock. Fusion 360 will generate a preview of how it thinks the operations will actually play out. You'll get a new set of icons across the bottom, they look like media buttons. You have the option to play, rewind, and fast forward as if it were a movie. It's pretty cool. When you hit the play button, it'll animate a tool head and follow the tool paths we setup. They're segmented across the bottom of the work area as a green bar. If you encounter any red tick marks in here, that means we have a tool collision. If we setup everything properly, we shouldn't have any. If you do, double check your operations and ensure we have all the right settings and chain selections. If everything looks good, we can move onto post processing (saving out gcode files for Otherplan). When your done with the simulation, click the close button.
Now we'll save out the gcode for our operations. For starters, I recommend saving out a separate gcode file for each operation. Right click on one of the operations (order doesn't matter), and select "Post Process". Then, in the post process panel select othermill.cps from the dropdown menu. Click OK, navigate to a directory where you want to save it and name your file. For example, I'd name the face operation, "joybonnet-1-8-face.nc". We need to use the ".nc" file extension in order for Otherplan to recognize it. I like to name the file so I know what operation type it is, and which tool it needs. You'll need to repeat this process for the rest of the operations. Next up, we'll set up our gcode in Otherplan – The software that interfaces with the Othermill Pro.
So far we've only setup our first part. We still have to do the bottom half of the case and our buttons. It's a pretty similar process, so I won't cover them in full detail like I did for the top half of the case. I hope I've provided enough information for you to take and apply to your own designs. It's a bit much at first, but I think the main concepts are there to learn from. There's lots of opportunity to make the tool paths optimized to reduce machining time. The more you practice, the better you'll get with experience.