In this getting started project, we’re machining another handy everyday carry tool: an aluminum bottle opener! While this project is fairly straightforward on the Bantam Tools Desktop CNC Milling Machine, it gives you the opportunity to add custom features to your part and get more comfortable with working in Fusion 360.
- Workflow for moving from Fusion 360 to setting up a job in the Bantam Tools software
- Setting up multiple files in the Bantam Tools software
- Programing tabs in Fusion 360
- sing the Bantam Tools software’s plan placement probing routines
- (Optional) Customizing your part using SVGs
- (Optional) Customizing your part in post-production, once you remove it from the Desktop CNC Milling Machine
- Bantam Tools Desktop CNC Milling Machine
- Computer with Bantam Tools Desktop Milling Machine Software installed
- Computer with Fusion 360 installed
- Probing pin, 1/4” diameter
- Datron stepped end mill, 12 mm
- Flat end mill, 1/8"
- Datron single-flute flat end mill, 4 mm
- Metal engraving bit, 80º, 1/8” or engraving bit of choice
- High-strength, double-sided Nitto tape
- Collet, ER-11, 1/8”
- Collet, ER-11, 4 mm
- Isopropyl alcohol, 91%
- Swiss file (Optional)
- Ultra-fine-grit sandpaper (Optional)
- Aluminum stock, 4” x 4”x 0.25”
- Aluminum-Bottle-Opener.f3d file downloaded
A Note Before You Start Milling
The Fusion 360 project files we provide are programmed specifically for the tooling and materials listed above. If you don’t have these end mills or stock, you will need to adjust the speeds and feeds parameters for the tooling and stock you're planning to use before you post-process your G-code files and set them up in the Bantam Tools Milling Machine Software. For more insight into programming toolpaths in Fusion 360, see our Fusion 360 Workflows: Programming CAM support guide.
Step 1: Download and save the Bantam Tools CAM post processor.
In order for your Bantam Tools Desktop CNC Milling Machine to read the G-code files you export from Fusion 360, you’ll need a CAM post processor specific to your CNC machine. Think of the post processor as a language translator that takes the settings you’ve programmed in Fusion 360 and translates them into a language the Desktop CNC Milling Machine can understand.
We’ve partnered with Autodesk to ensure a seamless experience when using Fusion 360 and our Desktop CNC Milling Machine. You can download and save a custom Bantam Tools CAM post processor for Fusion 360 locally on your computer. Our support guide teaches you how to download and save the Bantam Tools CAM post processor.
Step 2: Update and generate your G-code for Setup 1 and 2 in Fusion 360.
Now that you’ve saved your Bantam Tools CAM post processor locally, let’s start by generating your G-code files! Launch Fusion 360. Then, go to File > Open > Open from my computer and select the Bottle-Opener.f3d file that you downloaded. The bottle opener design will populate in what we call the Manufacture workspace. If this is your first time in Fusion 360, this workspace is where you program your CAM toolpaths, simulate your toolpaths, and post-process your G-code files.
For this project we’ve pre-configured the toolpaths for the bottle opener, but you’ll still need to tweak the setup to ensure that the size of the stock is correct. This is incredibly important, and failing to do so will prevent the Desktop CNC Milling Machine from machining your bottle opener accurately.
In the Bantam Tools software, users set both the position of the stock in the Desktop CNC Milling Machine and the position of your file relative to the stock. With these two locations identified, the software is able to create an accurate preview of the job.
Here’s how these 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. By default, our software aligns the plan work coordinate system (WCS) to this point. Adjustments to X, Y, or Z offsets in the Bantam Tools Desktop Milling Machine Software's Plan Setup tab will always be relative to this point.
These relative positions are important to keep in mind when you’re programming CAM in Fusion 360, particularly when you’re creating a new setup or adjusting an existing one. It’ll ensure that you have an accurate real-time preview in the Bantam Tools software and that the Bantam Tools Desktop CNC Milling Machine is able to machine your G-code files accurately. You’ll want to not only check the WCS, but also that the X, Y, and Z dimensions for your stock are exactly the same in Fusion 360 and the Bantam Tools software.
Now let’s take a closer look at Setup 1. Right-click on the Setup 1 folder and select Edit. The window that pops up will have three tabs: Setup, Stock, and Post Process.
The Setup tab is where you specify your WCS. You’ll notice that we’ve set the WCS to the top, front, left corner of the stock.
On the Stock tab, notice how we’ve selected “Fixed box size” for the Mode. This allows you to adjust the dimensions of your stock and also adjust how your model is orientated within the stock. Using a pair of digital calipers, measure the width (X), length (Y) , and height (Z) dimensions of your stock, and enter them into Fusion 360. When you’re done, click OK.
Notice how there are warning signs next to all the toolpaths now. Don’t worry, this is one of the beautiful things about Fusion 360: It’s telling you that the toolpaths previously programmed are no longer valid because you’ve made a change to your setup. To regenerate your toolpaths, right-click on the Setup tab and click Generate.
Repeat this process for Setup 2. To recap:
- Right-click on the setup folder and select edit.
- Go to the Stock tab.
- Measure your stock using digital calipers.
- Enter X, Y, and Z dimensions into Fusion 360 and then click OK.
- Right-click on the setup folder and select Generate.
Now you can post-process the toolpaths for Setup 1 as G-code files! Right-click on each toolpath and select Post Process––or go to Actions in the toolbar and click the Post Process icon. You’ll be prompted to name your files. We suggest naming the files so that they either match or are similar to the names we’ve designated.
Fusion 360 Quick Tip
If you machine through the full thickness of your stock, there won’t be anything left to hold the part in place, which means it can move or sometimes even go flying at the end of the milling job. Granted, in this project, we’ve fixtured the part using double-sided Nitto tape. But while this tape is strong, we wanted extra reinforcement while machining the part.
As a result, we programmed tabs in the outer 2D contour of our part. To program tabs, go to the Geometry tab and check the Tabs box. You can then customize the shape, size, and distance between your tabs. Here’s a look at what we programmed:
Here’s a simulated view of the toolpath in Fusion 360 to give you a better understanding.
The tabs will hold your part in place while you’re machining and then can easily be popped out of the stock after you’ve removed it from the machine.
Step 2: Import your G-code files and set them up in the Bantam Tools software.
Launch the Bantam Tools software and connect your computer to the Desktop CNC Milling Machine. Home the machine as prompted and then click the Initial Setup tab. Import your G-code files for Setup 1.
There are four operations in Setup 1. Import the G-code files in the following order:
- 1001 Face
- 1002 3D Adaptive
- 1003 2D Contour
- 1004 2D Contour
After importing your G-code files, the Milling Tools dropdown menu will appear, prompting you to select the tool you’ll use to machine the file. When working with G-code files, the tool you select (see image below) helps create an accurate preview of your job. The speeds and feeds for that tool will be read directly from the G-code file––not from our built-in Custom Tool Library.
As a result, you’ll want to make sure the tool you select in the Bantam Tools software is the same as the one programmed in Fusion 360. Here are the tools that should be selected:
- 1001 Face — Datron 12 mm stepped end mill
- 1002 3D Adaptive — 1/8” flat end mill
- 1003 2D Contour — Datron 4 mm single-flute end mill
- 1004 2D Contour — Datron 4 mm single-flute end mill
Before you install your Datron 12 mm stepped end mill and start machining, you’ll need to set up your material. And for this, you’ll need to use your 1/4”-diameter probe. To install the probe, go to the Jog tab and click Install Tool. Load your probe into the Desktop CNC Milling Machine and follow the onscreen instructions to locate your tool.
Note: If you’re still getting comfortable installing and locating a tool, see our Installing & Locating a Tool support guide for more details.
Step 3: Prep and load your stock.
Navigate to the Material Setup tab. Using digital calipers, measure the dimensions of your stock and enter them into the X, Y, and Z fields in the Material Size dropdown menu. When you’re finished, click Next.
You’ll then be brought to the Fixturing dropdown menu, and you can click Next again since we’ll be using high-strength double-sided Nitto tape to fixture your stock (in other words, to hold the material to the bed). We won’t use the toe clamps for this job, so you can remove them from the machine if they’re installed.
Double-sided tape is a great fixturing option for when you’re machining thin pieces of stock. And don’t worry, it’s strong––so strong that you may need 91% isopropyl alcohol to remove your part from the T-slot bed.
To prep your stock:
1. Wipe down the T-slot bed using 91% isopropyl alcohol to ensure the bed of the machine is clean.
2. Make sure the surface of your aluminum stock is clean (if not, clean it with 91% isopropyl alcohol) and cover as much surface area as you can with tape. Make sure the strips don’t overlap or wrinkle because this will affect your Z thickness.
3. Remove the paper backing on the tape after applying.
4. Take one of your parallels and place it so that it’s up against the corner of the L-bracket.
5. Then, press the material into place on the T-slot bed using the parallel as a backstop, and center it on the bed. Be sure to leave about 1.5” of space between the right side of the stock and the L-bracket, to avoid collisions. This will allow us to machine below the top surface of the bracket without running into it.
6. Remove the parallel when you're finished.
Step 4: Locate your stock.
Go to the Material Placement dropdown menu, click the Material Offset Probing Routines button, and launch the Automatic Stock Probing routine. Follow the prompts and carefully lay our wrench across the piece so that it’s touching the aluminum bed, as shown below. This is a trick we use to close the conductive loop between our stock and the T-slot bed when we’re using double-sided tape.
For this job, it’s important to account for the Z-height offset of your material due to the double-sided Nitto tape, to avoidrunning the risk of machining into the T-slot bed.
Enter 0.006” as the Z-offset value in the Material Offset Z input field.
Then complete the following steps to program your Z-height:
- Click the Material Offset Probing Routines button.
- Select Z-only Height Probing and click Next in the pop-up window.
- Jog the spindle to hover over the front, left corner of your stock.
- When you’re ready, click Start.
- When the probing routine is complete, click Accept.
Note: Because our work coordinate system (WCS) in Fusion 360 is aligned to the top, front, left stock box point, you’ll only need to run the Automatic Stock Probing routine (instead of both the Automatic Stock and Conductive Stock Probing routine), since your plan automatically aligns with the top, left edge of the stock.
Step 5: Machine your file.
Now that you’ve set up your material, go to the Jog menu and click the Install Tool button. Swap in the Datron 12 mm stepped end mill and perform a tool touch-off. Then, go to the Summary tab and confirm your job setup. When you’re satisfied, select Mill All.
By clicking Mill All, you’re telling the Bantam Tools software that you want to machine all the files you’ve set up. This includes both the facing and roughing operation files.
Step 6: Install your 1/8” ER-11 collet and the 1/8” flat end mill.
When the Desktop CNC Milling Machine has completed the facing operation, the Bantam Tools software will prompt you to install the 1/8” flat end mill. You’ll need to first install a 1/8” ER-11 collet before you can install and locate your end mill.
Remove the collet nut from the bottom of the spindle shaft by using the smaller wrench on the flat part of the spindle shaft to secure it in place while loosening the nut with the larger wrench.
Insert the collet into the collet nut. It might wiggle a little, but putting it on the tool holder will pop it into place. You might also notice the inside of the collet has an offset. This is part of the collet’s design.
With the collet in place, thread the collet nut back onto the tool holder by hand. Tighten by two or three turns, holding the tool holder in place with the small wrench, if necessary. Do not fully tighten the nut without a tool inserted.
Note: If you need more guidance on installing a collet and/or end mill onto the Desktop CNC Milling Machine, see our Installing & Locating a Tool support guide for more details.
With your collet installed, go to the Jog menu and select the Install Tool button. After installing and locating your 1/8” flat end mill, continue milling in the Bantam Tools software.
When you’re prompted to install the Datron 4 mm single-flute, use the same steps above to install the ER-11 4 mm collet and then install your tool.
Step 7: Break your part out of the stock.
Alright! You’ve successfully machined Setup 1 on the Desktop CNC Milling Machine. Now let’s break the part out of the stock. Use the 91% isopropyl alcohol to loosen the Nitto tape’s adhesive and remove your new bottle opener from the Desktop CNC Milling Machine. Be sure to clean off the T-slot bed so that it’s free of debris.
Bend the part back and forth until you break the tabs (as shown in the GIF below). Be careful because the metal can be sharp.
Step 8: Set up your G-code file.
Go to the Initial Setup tab and load your G-code file for Setup 2. This setup only requires one facing operation:
- 2001 Face
When you import this G-code file, select the Datron 12 mm stepped end mill in the Milling Tool dropdown menu, but don’t install the tool just yet. You’ll need to probe your material and place your plan before you machine this final operation.
Step 9: Flip, load, and locate your part.
Flip your part over so that the tabs are facing upward, and use the steps outlined in Step 3 to prep and load your stock onto the Desktop CNC Milling Machine. The part is orientated as seen below. Again, notice how there’s about an1.5” of space between the right side of the part and the L-bracket.
Go to the Jog tab and install your probing tool. Use the steps outlined in Step 6 to re-install your ER-11 1/4” collet and 1/4”-diameter probe.
When you’re done, go to the Material Setup tab and complete the following steps:
- Enter 0.006” as the Z-offset value.
- Click the Material Offset Probing Routines button and select Automatic Stock Probing routine. Run through the onscreen prompts like you did in Step 4, and use the wrench trick to close the conductive loop.
When you’re ready, go to the Summary tab and click Mill Single File.
If you want to add a custom design to your new bottle opener, leave your part in the machine. If not, use the 91% isopropyl alcohol to loosen the Nitto tape’s adhesive and remove your new bottle opener from the Desktop CNC Milling Machine.
Remember to vacuum out the machine and wipe down your T-slot bed.
Step 10 (Optional): Set up your SVG file and machine your custom engraving.
You can either machine this wave pattern SVG that we created or make your own design! If you wish to add your own custom engraving, we recommend creating an SVG file ahead of time. To learn more about working with SVG files:
- Download the Illustrator SVG Quick Guide template
- Download the Inkscape SVG Quick Guide template
- Read our Classic & Advanced SVG Workflows support guide.
Once your SVG is ready, go to the Initial Setup tab, import your file, and select the tooling you wish to use. If you’re using a specialty tool that isn’t found in our Custom Tool Library, you can add the geometry and speeds and feeds that you wish to run. To access the Tool Library, either go to Settings > Custom Tool Library or click Control + T on Windows or Command + T on Mac.
Before you install your engraving tool, insert and locate your 1/4” probing pin (or insert your 1/8” flat end mill upside down). Then run through the Automatic Stock Location routine in the Material Setup tab, using the instructions outlined in Step 2.
Next, head to the Plan Placement tab > Plan Offset Probing Routines, and select Conductive Stock Probing. A window will pop up that looks like this.
- Position the tool along the back, left corner of your bottle opener.
- Then click the Probe Z+ button in the menu on the left to locate the material edge using conductive probing. When the probe stops, click the Set X Zero button.
- Retract the probe using the jog controls, and repeat along the Y-axis. Again, position your probe and select the Probe Y– button. When the probe stops, click the Set Y Zero button.
Note: If you’re a software subscriber, you can alternatively use the Rectangular Corner Probing routine to place your plan.
When you’re ready, go to the Summary tab and select Mill Single File.
When you're finished, use the 91% isopropyl alcohol to break down the Nitto tape’s adhesive. Remove the part from the T-slot bed, wipe down the T-slot bed so that it’s clear of adhesive and debris, and vacuum out your Desktop CNC Milling Machine.
Step 11 (Optional): Post-processing your bottle opener.
If you’re up for it, let’s add another custom touch to this bottle opener. Using a Swiss file and ultra fine-grit sandpaper, you can add a unique finish to your part. To add a more tumbled surface finish, lightly rub the ultra-fine-grit sandpaper against your bottle opener until you achieve the desired finish. Then, use your Swiss file to clean up the edges. Again, file the edges gently until you get the finish you want.
We picked up these post-processing tips from our friend Ian Schon, a Philly-based product designer and machinist. Ian makes custom pens and watches. If you’d like to learn more about Ian and his work, follow him on Instagram or Twitter—and be sure to check out Ian’s podcast episode on The Edge.