While it can seem daunting at first, Fusion 360 is an amazing tool. It’s a cloud-connected system that enables you to model your design via CAD (computer-aided design) and program your CAM (computer-aid manufacturing) in one place, across multiple devices. Fusion 360 also allows you to share your design files with other users in the community. And the best part is that the G-code it generates can be imported right into our Bantam Tools Desktop Milling Machine Software.
In this support guide, you'll learn how to
- Import a custom tool library into Fusion 360
- Create a New CAM Setup
- Program your toolpaths
- Simulate your toolpaths
- Post process your toolpaths to generate G-code files
Note: You can download a free trial of the software for professional use or the free version for personal use.
Before you can program your CAM, you’ll need to design your CAD model. For more info about working in Fusion 360’s Design workspace, see our Fusion 360 Workflows: Designing in CAD support guide. To familiarize yourself with navigating the Manufacturing workspace in Fusion 360 (where you’ll program your CAM), check out this Autodesk livestream.
- How is a part programmed? (5:49)
- Post Processing & Types of Code (10:39)
- Setup & Stock in the Manufacturing Workspaces (11:39)
- CAM Properties (12:25)
- Boundary Selection (13:11)
- Heights (13:59)
- Rest Machining (15:34)
- 2D Strategies (17:10)
- 3D Strategies (18:37)
- Fusion 360 Tool Library (19:46)
- Machining Parameters (speeds, feeds, stepdown, and stepover) (20:57)
- CAM Demo Starts (24:17)
- Designing for Fixturing (24:50)
- Utilizing Stock to Leave (27:46)
- Simulating Toolpaths and Utilizing the Comparison Tool (45:22)
- Setting up G-code Files in the Bantam Tools Software (49:16)
- Q&A (1:00:00)
Importing the Tool Library into Fusion 360
We’ve created a downloadable tool library for our desktop CNC machines. This tool library includes default speeds and feeds recipes that we’ve tested extensively for the tooling we carry in our store.
Here are the steps to import our tool library into Fusion 360:
- Download the Fusion 360 Bantam Tools Tool Library.
- Launch Fusion 360, if you haven’t already.
- Go to the Manufacturing workspace.
- Select the Tool Library icon.
- In the Tool tab, click the Select button. A window will pop up that looks like the screenshot below.
- In the top right corner, select Import Libraries and then select the Bantam Tools’ Tool Library file.
Now you’ll be able to select tooling with speeds and feeds specific to your Bantam Tools Milling Machine. Each of our CNC machines have Fusion Tool Libraries that come with speeds and feeds recipes that are specific to the mill. This is because each Bantam Tools Milling Machine has different specifications (e.g. spindle speed range, max traverse speed, etc.). If you have further questions about importing our Fusion 360 tool library or you want to create your own library with custom speeds and feeds recipes, we suggest starting with this Fusion 360 support guide.
Creating a New CAM Setup
To start programming your CAM, click on the Change Workspace button in the top left corner of Fusion 360 and select the Manufacture workspace. CAM can be broken up into two parts: stock setup and toolpaths.
At a minimum, you’ll need to specify three things to set up your stock:
- Stock size
- Model orientation in the stock
- Work coordinate system (WCS)
Note: You can change the units used for a Fusion 360 design in “Browser” on the left side of the Fusion 360 window.
Begin by clicking the Setup menu in the toolbar and select New Setup. A small panel will open three tabs: Model, Stock, and Post Process. The Model tab sets the work coordinate system (WCS) 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.
Stock size: Click the Stock tab and make sure that “Fixed size box” is selected for the Mode. This will allow you to adjust the dimensions of the stock. Measure your stock using digital calipers and enter the dimensions of your stock by entering exact values into the Width (X), Depth (Y), and Height (Z) boxes.
When choosing the size of your stock, think about how much material is going to be cut away to machine your model. Naturally, the less material that needs to be cleared, the more efficient your toolpaths will be.
Model orientation: 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.
You’ll want to orient the model within the stock to optimize your mill job and your fixturing strategy. For example, in the Stock tab, click Model Position under Height, select Offset from Bottom, and enter 0”. This will make the bottom of your stock and model the same.
Before orientating your model within the stock.
After orientating your model. See how it's now flush with the bottom of the stock?
WCS: This is a very important step in setting up your CAM! Specify the coordinate system that the toolpaths will use to machine your design. To set up a work coordinate system (WCS), you’ll configure the directions of the X, Y, and Z axes to match those on your desktop CNC machine, as well as choose the point that will serve as the origin (e.g., coordinate 0, 0, 0). The Bantam Tools software assumes that this point is on the front, left, top corner of the material.
When you go to set up a job in the Bantam Tools software, you’ll need to specify both the position of the stock on the T-slot bed and the position of your file relative to the stock. With these two locations identified, the Bantam Tools software is able to create an accurate preview.
Here’s a visual for how the positions relate to one another:
- The machine bed origin position is the front left corner of the bed.
- The material position is relative to this machine bed origin.
- The plan position is relative to the top left corner of the material.
To specify your WCS go to the Setup tab, select Stock box point for your Origin point, and then select the top, front, left box point on your stock.
To verify your setup, look at your model from above. You should see that:
- The origin is in the lower-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 upward.
When you’ve gone through each of these steps, click OK.
Advanced Work Coordinate System Setup
As you begin programming CAM for more complex parts, you may want to orientate the WCS for your tooling in a way that differs from the way you've orientated your model within the stock. To give you more flexibility, Fusion 360 allows you to orientate your tool in a few different ways.
- Model Orientation: This aligns your tool with the axis of the WCS associated with your model.
- Select Z Axis/Plane & X Axis: Allows you to choose the Z & X axes yourself, using your model's geometry.
- Select Z Axis/Plane & Y Axis: Allows you to choose the Z & Y axes yourself, using your model's geometry.
- Select X & Y Axis: Allows you to choose the X & Y axes yourself, using the model geometry.
- Select Coordinate System: This allows you to align your tool with a User Coordinate System in the model. This option is helpful if your part doesn't have points or planes that are easy to select.
Note: No matter which of these you choose, make sure that your Z-axis is always pointing away from the stock.
When working with a Bantam Tools Milling Machine, we recommend using the “Select Z axis/plane & X axis” option. To select this option, go to the Setup Tab and under the Work Coordinate System (WCS) > Orientation > "Z axis/plane & X axis." The options available will look like this:
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 your milling machine.
This video features our Tool Holder project for the Bantam Tools Desktop CNC Milling Machine.
You should see the blue Z-axis indicator stick out from the face you selected and pointing in the positive (or “up”) direction—remember to think about how the tool is going to be orientated in the machine in relation to your stock. If the Z-axis indicator isn't pointing the positive direction, click the head of the arrow or check the “Flip Z Axis” checkbox to flip the Orientation.
Next 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.
Finally, select "Stock box point" for the Origin. Beneath the dropdown menu click Box Point and then select the point in the front, top, left corner of the stock.
Note: For more info about the work coordinate system and tool orientation, see this brief Autodesk support guide.
2D vs. 3D Toolpaths
Now that you’ve created a new Setup, you’ll need to program your toolpaths—in other words, the cuts you want your CNC machine to make when milling your part. Keep in mind that some parts may require multiple toolpaths, multiple tools, and even multiple setups. There are many toolpaths to choose from (as shown below) and they all have different strengths and weaknesses. Fusion 360 has helpful information panels that pop up when you mouse over the different toolpaths. To learn more about them, hover your mouse over the toolpath you wish to program.
When you select a toolpath, a new panel will pop up, allowing you to configure this toolpath. This panel has five tabs, each with a number of settings and places to enter your speeds and feeds recipes.
- Tool is for selecting a tool and specifying your speeds and feeds.
- 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. This tab becomes especially helpful when programming multi-operation setups.
Speeds and feeds recipes are essential for CNC machining operations because they’re what we use to define our cutting parameters for the toolpaths we program. For the Bantam Tools Milling Machines, there are five key cutting parameters you’ll need to define when programming your CAM:
- Spindle speed (RPM, revolutions per minute) relates to how quickly the cutting edge spins.
- Feed rate (IPM, inches per minute) controls how quickly the tool moves through the material.
- Axial depth of cut (ADOC), otherwise known as depth of cut (DOC) and stepdown, is how deep your tool cuts into the material.
- Radial depth of cut (RDOC), otherwise known as width of cut (WOC), optimal load, and stepover is the amount of space between tooling passes when cutting a material.
- Plunge rate (inches per minute) is how fast the end mill is driven down into the material. While this isn’t absolutely essential, it’s one more parameter that gives you more control over how your tool is approaching, entering, and exiting the material.
- Ramp angle (inches per minute) is the angle at which your end mill enters the material, which can improve the lifespan of your end mill.
Example: Programming 3D Adaptive Clearing Toolpath
To give you a better understanding of how to program a toolpath, let’s run through an example. Once you’ve set up your stock and orientated your model within the stock, go to the toolbar and select the 3D Adaptive Clearing toolpath. This toolpath clears the bulk of your material in the most efficient way possible using a high-speed machining (HSM) strategy that avoids sharp 90º turns.
When you select the 3D adaptive toolpath, a new window will pop up. In the Tool tab, click the Select button and choose your end mill. For toolpaths where you need to clear a lot of material, we recommend using either 2-flute or single flute 1/4” or 1/8” flat end mills.
When you select your tool, the speeds and feeds parameters will update in the Tool tab. The recipes that come with the Bantam Tools Fusion 360 Tool Library are default speeds and feeds. As you get more comfortable using your Bantam Tools Milling Machine and certain tools, feel free to tweak these recipes to meet your specific needs.
Next, go to the Geometry tab. Rather than machine away all the material, program this toolpath to clear only what you need to optimize your milling operation. To do this, create a machining boundary by selecting Silhouette and then enter a value for the boundary. When deciding on how large or small the boundary should be, take into account the size of your tooling and your fixturing so you don’t break an end mill or have a collision.
The Heights tab is where you'll program the way in which you want your tool to approach your part, machine the part, and leave the part. In this tab you’ll have four different heights you can adjust.
- Clearance Height: This height should always be set above all features on the model so that you avoid plunging your tool into any part features when doing linking moves or moving at a rapid feedrate.
- Retract Height: This height tells the milling machine how far to retract after performing an operation.
- Top Height: This allows you to set an upper boundary for certain operations and will usually be just the top of your model.
- Bottom Height: This setting specifies the lowest height you want the operation to machine.
When working with the Heights tab, we recommend working from the bottom up. This will help you first define the bottom and top boundaries you want to work off. And once you’ve defined these boundaries it will be easier to determine how/if you wish to adjust your Retract and Clearance Heights.
To input your stepover and stepdown, you’ll notice the options in the Passes tab look a little different for the 3D adaptive toolpath. For adaptive toolpaths, the Optimal Load is essentially the stepover, and Maximum Roughing Stepdown is the stepdown.
The settings you program in the Linking tab are very specific to your job. Perhaps you don’t want your spindle to fully retract after every cutting pass. Maybe you want to specify stock to leave that you plan to clean up in the proceeding operations. When it comes to setting up this tab, it really depends on what operation(s) you’ll be machining next.
Note: To learn more about each of these tabs, especially the Heights and Linking tabs, we recommend checking out this NYC CNC walkthrough.
Repeat this workflow for each toolpath you program. Remember, you'll need to enter values for speeds, feeds, stepdown, and stepover. These values will be dependant on a number of factors (e.g. tool selection, material, and much more). You'll also need to enter settings into each of the five tabs in the programming pop-up window. But be aware the process for setting up these tabs will differ. If you're just getting started with Fusion 360 be patient, stay curious, and be sure to always simulate your toolpaths.
Simulate Your Toolpath
When you’re finished programming your toolpath, select OK and watch the toolpath generate. To ensure that the toolpath is cutting the way you want and that there won’t be any collisions with the stock, it’s a good idea to simulate your toolpaths. Select a toolpath and click the Simulate icon under Actions in the toolbar.
Your screen will look similar to the screenshot below. Make sure Stock is checked so that you can see the toolpath being machined. When you’re ready, click the Play button at the bottom of your screen. If the tool turns red, there will be a tool collision, but don’t worry—this is why you simulate! Head back into the toolpath and make adjustments as needed.
Post Process: Generating G-code Files
We’ve partnered with Autodesk to ensure a seamless experience when using Fusion 360 and our desktop CNC machines. There are two post-processors available for Bantam Tools users. The first is the Batam Tools CAM post processor for Fusion 360 that you can save locally on your computer.
When you’re finished programming your CAM and simulating your toolpaths, the next step will be post-process your G-code files. Post processing is the component of your CAM software that translates the CAM toolpaths you’ve programmed into the exact G-code dialect that your Bantam Tools Milling Machine can read. You can post-process your toolpaths two different ways. The first, is by right-clicking on the toolpath you wish to post-process and selecting Post Process in the menu.
The second is selecting the toolpath and then clicking the Post Process icon under Actions in Fusion 360’s toolbar.
We point this out because you’ll find that folks use and talk about these methods interchangeably. Which method you choose comes down to personal preference.
When you select Post Process, a new window that looks like this will pop up:
In the Post Process window that pops up, click the three dots next to Post if you don't have a post-processor selected. If you have more than one post processor saved locally, select “Bantam Tools / bantam tools,” and enter the rest of the information as needed.
You’ll also notice there are other pieces of information you can fill out.
- Name/Number is a program number 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.
- Comment allows you to enter a description. Again, it’s just a comment inside the file that you can read to determine what’s going on in the file.
- Output Folder is where you select where you want your G-code file to be saved.
- For Document Unit, be sure that “Document Unit” is selected.
- Leave “Post to Fusion Team" unchecked.
- Make sure the NC Extension will be greyed out and will read .gcode.
- Uncheck “Open NC file in editor” unless you want to make manual changes to the G-code.
- Leave all the Properties values as-is.
Alright! Now that you’ve post-processed your G-code files, you can import them into the Bantam Tools Milling Machine Software, set up your job, and start machining with your Bantam Tools Milling Machine. To learn more about how to setup your G-code files in the Bantam Tools software see our Fusion 360 to Bantam Tools Software support guide.
Additional Links & Resources
We know this is a lot of information to soak in and that there’s even more to explore. As you create new designs and dive deeper into programming CAM, you’ll have more questions. Feel free to reach out to us. In the meantime, here are some of our go-to resources when programming CAM:
- Haas’ Tip of the Day
- Haas’ How to Calculate Speeds & Feeds
- NYC CNC’s CAM for Beginners
- Lars Christensen Fusion 360 YouTube Series