With so many different boxes to check and tools to choose from, programming CAM can be daunting and time-consuming if you’re just getting comfortable with Fusion 360––but it doesn’t have to be. Using CAM templates, you can begin generating toolpaths for the Bantam Tools Desktop CNC Milling Machine within minutes. Just open your CAD model, select a Fusion 360 template with preconfigured speeds and feeds, hit Generate, and you’ll have a toolpath ready for post-processing. Take a look!
Here are the basic steps:
- Download and import the templates.
- Right-click on your Fusion setup file and insert one or more CAM templates.
- Adjust as necessary for your design.
Seriously, it’s that simple!
For a more in-depth look at each of these steps, read on.
Step 1: Import the Bantam Tools Fusion 360 templates.
Download the Basic Bantam Tools Fusion 360 CAM Templates.
Launch Fusion 360 and design your model in the Design workspace. When you’re finished designing your CAD, click over to the Manufacturing workspace. In the Manage tab, scroll down to Template Library > My Templates > Local and click on the basic CAM templates.
Note: You can download a free trial of Fusion 360for professional use or the free version for personal use.
Step 2: Create a new setup.
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 will 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 model.
After orientating model.
WCS: 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 position of the X, Y, and Z axes to match those on your desktop CNC machine. By default, the Bantam Tools software assumes that this point is on the front, left, top 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 up.
- The Z-axis is pointing toward you.
When you’ve gone through each of these steps, click OK.
Step 3: Select your toolpaths using the templates.
Right-click on the Setup you just created and select Create From Template. The templates you imported in Step 1 will pop up.
Each of these templates is set up according to a specific type of toolpath (e.g., facing, 3D adaptive, contour, etc.) and includes a specific tool that has preconfigured speeds and feeds recipes that you’d normally have to input when programming your CAM from scratch.
Clicking Select Template will open up the full template library. Choose the template you’d like to insert into your setup and click Select.
Step 4: Adjust and customize.
Some of the templates, like the roughing and facing strategies, won’t require many adjustments, if any at all. However, other toolpaths, like 2D contours, will require you to select the model geometry that you’d like to apply the toolpath to. In the 2D contour toolpath, for example, it’s necessary to select the bottom edge of the contour you’d like the tool to follow.
Step 5: Generate and simulate your toolpath.
Alright, this is where the magic happens! Click on the toolpath you’ve chosen and press Command + G and watch Fusion 360 generate your toolpath. For this example, we chose a 3D adaptive toolpath using a Datron 6 mm single-flute, but you can choose whatever toolpath and tool suits your design.
When you’re finished generating your toolpath, you’ll want to simulate it to ensure that it’s cutting the way you want and that there won’t be any collisions with the stock. Select the toolpath you just generated and click the Simulate icon under Actions in the toolbar.
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.
Repeat this process each time you wish to add a new toolpath.
Note: Some toolpaths will require manual selections so that the geometries are specific to the model you’ve designed.
One example is the contour toolpath, which is great for finishing passes. You can program 2D and 3D passes. You’ll need to select the boundaries of your contour in the Geometry tab. To do this, select the contour toolpath and tool you wish to use. Then, before you generate the toolpath, right-click on it and select Edit. A pop-up window with five tabs will appear, like this one:
Go to the Geometry tab and select the bottom edges of your contours.
Step 6: Post process your G-code files.
Note: If you haven’t done so already, you’ll need to download and save the Bantam Tools CAM post process locally onto your computer before you can post process your G-code files. For more information, see our CAM Fusion 360 Post Processor support guide.
After you’ve selected, generated, and simulated your toolpaths, it’s time to post process your toolpaths as G-code files. To do this, select a toolpath and then go to Actions > Post Process.
In the Post Process window that pops up, select Personal Posts for your Source. If you have more than one post processor saved locally, click the Post Processor dropdown menu, 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.
- Program Number is a 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.
- Program 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.
- For Units, be sure that “Document Unit” is selected.
- 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 as-is.
Repeat this process for each toolpath you wish to post-process.
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. For more insight into moving from Fusion 360 to the Bantam Tools software, see this support guide.