Fusion 360 is a cloud-connected CAD/CAM application made by Autodesk. It’s supported on Mac OS X and Windows and is free for students, hobbyists, enthusiasts, and startups. It’s both a powerful design app for 3D objects and a CAM app that can create 3D toolpaths for the Bantam Tools Desktop PCB Milling Machine.
We’ve partnered with Autodesk to ensure a seamless experience when using Fusion 360 and the Bantam Tools Desktop PCB Milling Machine together. An Othermill CAM post-processor is included by default with Fusion 360, and a tool library is available for download from our website.
This guide covers the basics of Fusion 360, with a particular focus on CAM. You’ll need some experience designing with 3D CAD tools, or you’ll need to go through the basic Fusion 360 tutorials. You’ll also need some experience with feeds and speeds as well as knowledge of other CAM terminology like stepover, stepdown, etc.
You can download Fusion 360 from their website.
If you’re new to Fusion 360 or 3D CAD in general, you may want to start with their video training materials.
When Fusion 360 opens, you’ll be asked to sign in or create an Autodesk account. Once signed in, Fusion 360 will open a new, blank document.
To manage your projects and data, click the “Show Data Panel” button at the top left of the Fusion 360 window. From here, you can create new projects, share them with other users, upload models and other data, and open Autodesk’s A360 project collaboration software interface in your web browser.
Fusion 360 has a number of workspaces for modeling, simulation, and CAM features. To switch between workspaces, click the “Change Workspace” button at the top left of the Fusion 360 window, and select the workspace you’d like to switch to. This button is labeled with the name of the current workspace (Model, Patch, Render, Animation, CAM), and will update once you switch workspaces.
Modeling in Fusion 360
There are a variety of methods for 3D modeling in Fusion 360. Follow the step-by-step tutorials (under the Help menu) or use the Fusion 360 Learning and Resources website to learn more.
Import Models from Other Software
Fusion 360 can import a large number of file types from various CAD applications. Note that some file types (such as .step and .iges) are easier to work with than others. Of note, Fusion 360 CAM is now compatible with .stl files.
To import a model, open the Data Panel by clicking the Open Data Panel button at the top left of the Fusion 360 window. If you’re beginning a new project, click New Project and give your project a name. With the project created, click on the project to open it. You’ll now see a new, empty project.
Next, click the Upload button. A window will appear. Drag and drop your files into this window, or click the Select Files button and choose the files you’d like to upload. The files you select will appear in a list. Now click Upload.
A new window will appear showing you the upload progress. You can close this window and the upload will continue. A status bar will show your progress at the bottom left of the Fusion 360 Data Panel. Once the upload is complete, your model will appear in the Data Panel. To open, double-click on your model.
Turn Your Model into a Toolpath (CAD to CAM)
Once you’ve uploaded or created model, you’ll need to turn it into one or more toolpaths so the milling machine can cut them. To do this, switch to Fusion 360’s CAM workspace. Click the Change Workspace button in the top left of the Fusion 360 window and select CAM. Everything you do from this point on, unless you need to make changes to your model, will be in this CAM workspace.
Create a CAM Setup
First, let’s define how your model will be oriented and placed in physical space. Fusion 360 needs to know the dimensions of your material, where to place your model within the material, and where the milling tool will be relative to the material. Finally, you’ll need to ensure that the material is oriented correctly in the milling machine. To do this, create a setup in Fusion 360.
Note: You can change the units used for a Fusion 360 design in “Browser” on the left side of the Fusion 360 window.
Click the Setup menu and select New Setup. A small panel will open three tabs: Model, Stock, and Post Process. The Model tab sets the work coordinate system for your model. The Stock tab sets up the dimensions of the piece of material (or “stock”) you’ll be milling. Ignore the Post Process tab for now.
To set up a work coordinate system, you’ll configure the directions of the x, y, and z-axes to match those on the milling machine, as well as choose the point that will serve as the origin (i.e. coordinate 0, 0, 0). Bantam Tools software assumes that this point is on the front, left, top corner of the material.
Before you begin, it’s helpful to orient the model to match the orientation you plan to mill in the milling machine.
Start in the Model tab. From the Orientation menu, choose “Select Z axis/plane & X axis.” Click the button next to “Z Axis” and then select a face or line on your model that’s perpendicular to the z-axis. In other words, choose a line or face that would be lying flat in the milling machine. You should see the blue z-axis indicator stick out of the face you selected, and the arrow should be pointing in the positive (or “up”) direction. If not, click the head of the arrow or check the “Flip Z Axis” checkbox to flip the orientation.
Now set the x-axis orientation following the same procedure you followed for the z-axis. If it’s already oriented correctly, you don’t need to do anything.
Next, set the origin. Bantam Tools software sets the origin based on the size of your material, so click the Origin menu and select “Stock box point.” Then, click the Stock Point button. A number of points will appear on your model. Click the point that represents the top, left, front of your material.
Finally, click the Model button and choose the body or bodies you plan to mill.
To verify your setup, look at your model from above. You should see that:
- The origin is in the top, front, left corner of your model.
- The red X-axis arrow is pointing to the right.
- The Y-axis arrow is pointing away from you.
- The Z-axis is pointing upwards.
Then look at your model from the side and verify that the origin is in the top corner closest to the surface.
Now it’s time to set up your material. Click the Stock tab, then click the Mode menu and select “Fixed size box.” Enter your material’s X, Y, and Z dimensions, measuring with calipers if possible. Set “Round up to Nearest” to 0.
By default, Fusion 360 will place your model in the exact center of your stock. Depending on the size of your stock and the CAM strategies you wish to use, you may want to align your model to the surface of your stock or offset it by some absolute amount. To do this, choose the “Model Position” for the dimension you want to align to, choose the side you want to offset from, and fill in the Offset field with the amount you want to offset by. Entering 0 will align your model flush to that face of your stock.
Click OK to save your settings.
Set Up Your Tool Library
In order to calculate toolpaths, Fusion 360 needs to know what milling tools you have available. You can configure and store these tool definitions in the Fusion 360 Tool Library.
To open the Tool Library, click the Manage menu at the top of the Fusion 360 windows and select “Tool Library.”
Import the Bantam Tools' Tool Library
To save time, you can download the Tool Library. We’ve preloaded the definitions of the tools we carry in our online store.
After you download the file, unzip it. It will contain two files: Bantam Tools' Tool Library.json for Mac OS X users, and Bantam Tools' Tool Library.hsmlib for Windows users. (The filenames may change depending on the version of the tool library you’ve downloaded.)
Then open the Fusion 360 Tool Library. A new window will appear. Click the Local library, then click the Import Tool Library button in the toolbar. It is the second button in the toolbar, with an arrow pointed downward into a box. Find the file you just downloaded and click Open. The tools should now appear in your library.
Add Tools to the Tool Library
To add other tools to your Tool Library, refer to Autodesk’s documentation.
Now you have to decide which kinds of toolpaths you want to make. There are many to choose from, and they all have different strengths and weaknesses. Fusion 360 has helpful information panels that pop up when you mouse over the different toolpaths.
Open the dropdown list of toolpaths by click the 2D or 3D toolpath menus. Mouse over all the toolpaths, read about them, and determine which ones are right for you. You can also read about the 2D and 3D toolpaths on Autodesk’s website. Keep in mind that some parts may require multiple toolpaths, multiple tools, and even multiple setups.
If you’re completely new to 3D CAM, you may want to follow along with Autodesk’s CAM tutorials.
Set Up a Toolpath
Once you’ve selected a toolpath, you’ll need to configure it. Although the specific settings you see are different depending on the toolpath, the overall workflow is the same: choose a tool, specify your speeds and feeds, select the geometry you wish to mill, and specify settings related to the toolpath algorithm chosen. If you’re confused about what a setting will do, hover your cursor over the field to reveal an explanation of what the setting will do.
We’ll walk through two example toolpaths: 2D Face and 3D Adaptive Clearing.
Toolpath Setup: 2D Face
Facing is a 2D milling operation that mills a flat face onto the material. It’s used to ensure that the material is perfectly flat, and as such, it’s often the first toolpath in a sequence. When configuring a facing toolpath, Fusion 360 will automatically mill the entire piece of material, from the top of the material to the top of the model.
To set up a 2D Face, click the 2D toolpath menu and select Face. A new panel will open and allow you to configure this toolpath. This panel has five tabs, each with a number of settings.
- Tool is for selecting a tool and specifying your feeds and speeds.
- Geometry is for selecting the geometry you wish to mill.
- Heights is for specifying vertical dimensions of the toolpath.
- Passes is for configuring the depth of passes, stepover, and stepdown.
- Linking is for specifying how the toolpath will begin and end.
We’ll discuss each of these tabs in turn.
With the Tool tab opened, click the Select button next to the Tool label. The tool selection window will appear. In this case, we’ll use the 1/8" flat end mill in the Bantam Tools' Tool Library.
- In the left panel, uncheck Workpiece Material and Operation.
- In the left panel under Tool Type, select “Flat end mill.”
- Check the Diameter checkbox, click the chain link graphic, and enter “.125”.
- The 1/8" flat end mill should be in the list under a ”Bantam Tools" heading. If you can’t read the tool name, you can increase the width of the column.
- Select the tool. Information about the tool will be shown in the Tool Info panel on the right side of the window.
- Once you’ve selected the tool you want, click OK.
Back in the Tool tab, ensure that the Coolant menu is set to Disabled.
Now you can set feeds and speeds for this toolpath. Feeds and speeds will differ depending on your tool and material. Make sure to set:
- Spindle speed is the speed at which the spindle turns.
- Cutting feedrate is the rate at which the tool moves through the material horizontally.
- Ramp feedrate is the rate at which the tool descends to begin milling.
- Plunge feedrate is the rate at which the tool descends during milling.
Next are the Geometry and Heights tabs. For a Face operation, Fusion 360 will automatically mill the entire region from the top of the material to the top of the model. Unless you want to change this, you can leave the default settings on these tabs as-is.
Now switch to the Passes tab. Set a stepover value that’s at least half the diameter of your tool. You may want to reduce this value further depending on the surface finish you desire and the tool/material you’re using.
You also may want to check the Multiple Depths checkbox. By default, Fusion 360 will do a facing operation in one pass, cutting all of the material away in one go. Depending on your material, you may want to limit the Maximum Stepdown to between .003” and .01”.
With all of these settings entered, click OK. Fusion 360 will generate the toolpath and superimpose it on top of your model.
Now let’s simulate. In the Browser, select the toolpath you just created. It’s probably titled something like “Face1.” Then click the Actions menu and select Simulate.
The Simulate panel will appear. You can choose to display the tool, toolpath, and stock by clicking the checkboxes. To begin the simulation, click the Play button in the bottom of the window. An animation will show the tool milling through the material.
If the animation looks like what you expect, great! If not, double-click on your toolpath and change the settings. Keep doing this until you’re satisfied with the toolpath.
Toolpath Setup: 3D Adaptive Clearing
3D Adaptive Clearing is a Fusion 360 milling strategy for roughing out large areas of material. It’s a great way to quickly set up a toolpath for a complex part and is also a good first step if you don’t know what type of toolpath to choose.
To set up a 3D Adaptive Clearing toolpath, in the 3D toolpath menu, select Adaptive Clearing. Like with the 2D Face, a new panel will open and allow you to configure this toolpath.
With the Tool tab opened, click the Select button next to the Tool label. Use the tool selection window to choose an appropriate tool. (We’re using an 1/16” ball end mill in these screenshots.)
Back in the Tool tab, ensure that the Coolant menu is set to Disabled and set the feeds and speeds for this toolpath. (Refer back to “Toolpath Setup: 2D Face” above for more details.)
Switch to the Geometry tab. Deselect Stock Contours to ensure that the toolpath mills the entire piece of stock configured. Disable Rest Machining to disregard previous toolpaths. (Rest Machining is a powerful way to combine multiple toolpaths.) Leave Tool Orientation and Model unchecked.
Click the Heights tab. For a 3D Adaptive Clearing operation, Fusion 360 will automatically mill the entire region from the top of the stock to the bottom of the model. Unless you want to change this, leave the default settings on this tab as-is.
Switch to the Passes tab. Although there are many options on this tab, the most important are Optimal Load and Maximum Roughing Stepdown. These set the amount of material the tool will cut on each pass. Set values for both that are no more than half the diameter of your tool. You may want to reduce this value further depending on the surface finish you desire and the tool/material you’re using.
If you don’t plan to set up a separate finishing pass, uncheck Stock to Leave.
With all of these settings entered, click OK. Fusion 360 will generate the toolpath and superimpose it on top of your model.
Now, let’s simulate. In the Browser, select the setup that contains this and all other toolpaths you’ve set up. It’s probably titled something like “Setup.” Then click the Actions menu and select Simulate. By clicking the setup instead of the toolpath, the simulation will show the entire milling process in order.
If the animation looks like what you expect, you’re ready to export! If not, double-click on your toolpath and change the settings. Keep doing this until you’re satisfied.
Export a Toolpath File
Now that you have toolpaths configured, you’re finally ready to export toolpath G-code files. For each toolpath, do the following:
- Select it in the Browser panel.
- Click the Post Process button under Actions.
- In the Post Process panel that pops up, set Post Processor to “othermill.cps - Generic Othermill (Otherplan).”
- Under Program Number, enter a number. This is a comment that will show up in the file so you can tell which order the file is supposed to be cut, just by looking at the contents of the file.
- Optional: For Program Comment, enter something descriptive. Again, it’s just a comment inside the file that you can read to determine what’s going on in the file.
- For Units, select Document Unit.
- Leave “Minimize tool changes” unchecked.
- Uncheck “Open NC file in editor,” unless you want to make manual changes to the G-code.
- Leave all the Properties values alone.
- Click OK and choose a destination to save your file, making sure that it has an .nc extension, otherwise the Bantam Tools Software won’t recognize it.
Open Toolpath Files in Bantam Tools Software
Open the Bantam Tools Desktop PCB Milling Machine Software and set up as you would normally for a project. Measure and set up your material, and install and locate a tool.
Open the toolpath files in the Bantam Tools Software. The 3D preview should match what you saw in Fusion 360. Make sure it shows up the way you expect it to, and that it’s not sitting on top of your material when it should be beneath the surface of your material. If the toolpaths are in the wrong place, check your Setup configuration in Fusion 360 and re-export.
In the panel for your imported toolpath, select the tool or tools you’ll be using for this toolpath. Then, simply click Start Milling.