With the Bantam Tools Desktop CNC Milling Machine
In this project, you’ll machine a pocket-sized machinist rule using both the basic and advanced SVG workflows in the Bantam Tools Desktop Milling Machine Software. What's the difference between a "rule" and a "ruler"? Generally, a rule measures straight from its edge (while a ruler's measurements start a little in from the edge) and is more accurately calibrated. And what better way to make a precise tool, than by using a precise CNC machine!
Through building this project, you’ll learn how to:
- Work with color-coded SVG files in the Bantam Tools software.
- Align your material and plan with alternate probing techniques.
- Use high-strength, double-side Nitto tape to fixture your material to the T-slot bed.
- Perform a flip operation.
- Bantam Tools Desktop CNC Milling Machine
- Computer with Bantam Tools Desktop Milling Machine Software installed
- Probing pin, 1/8”
- Datron single-flute flat end mill, 4 mm
- Metal engraving bit, 80º, 1/8”
- High-strength, double-sided Nitto tape
- ER-11 1/8” collet
- Isopropyl alcohol, 91%
- Aluminum stock, 4” x 4”x 0.125”
SVG (scaled vector graphic) files are 2D drawings that the Bantam Tools software can interpret and generate toolpaths. Any object in an SVG file with a border or fill will be machined. The Bantam Tools software looks at strokes and fills to determine the inside and outside of shapes in a design. The software combines the resulting shape with the tools you’ve selected, as well as the scaling, placement, and any other settings you specify. Then it calculates the toolpaths that the Desktop CNC Milling Machine will follow.
The Bantam software can interpret SVG files in two ways. Basic SVG handling reads fills as engravings and strokes as cutouts.
Advanced SVG handling allows you to do multiple cutout operations in one file using color coding. This project uses advanced SVG handling.
To learn more about working with SVGs, check out these resources:
- Download the Illustrator SVG Quick Guide template
- Download the Inkscape SVG Quick Guide template
- Read our Basic & Advanced SVG Workflows support guide.
With this in mind, let’s dive in!
Step 1: Install your ER-11 1/8” collet.
The collet that comes with your Desktop CNC Milling Machine supports 1/4” tooling. However, if you’re going to use smaller tooling––like we are in this project––you’ll need to use a collet that supports smaller tooling. To ensure accuracy and compatibility, we recommend using the ER-11 collet in our store.
To install the collet:
- Remove the collet nut from the bottom of the tool holder. Use the smaller wrench on the flat part of the tool holder to secure it in place, and then use the larger wrench to unscrew the nut.
- Remove the 1/4” collet from the collet nut.
- Insert the 1/8” collet into the collet nut—you’ll hear it snap into place.
- Screw the collet and collet nut back onto the tool holder with two or three turns, or use the wrenches, if necessary. Remember, don’t fully tighten the nut without a tool inserted.
Step 2: Install and locate the 1/8” engraving bit.
Click the Install Tool dropdown menu and choose the Install Tool button. Load the 1/8” metal engraving bit and follow the prompts to perform a tool touch-off. Because 1/8” bits tend to be shorter than 1/4” bits, you’ll need to insert the tool less than 3/4” into the collet. See our Installing & Locating a Tool support guide for more details.
Step 3: Import and set up your SVG file in the Bantam Tools software.
Connect your Desktop CNC Milling Machine to your computer, turn on the machine, and launch the Bantam Tools software. Home the machine and then navigate to the Initial Setup tab and import the Machinist-Rule.svg file. The file dropdown menu will look like this:
To set up your file:
- In the Milling Tools dropdown menu, select the “Datron 4mm Single-FL” and the “1/8” Metal Engraving Bit (80º)”. If you click the gear icon next to each tool you’ve selected, you’ll open the Custom Tool Library, where you can copy a tool and customize the speeds and feeds. We’ll be using the default speeds and feeds in the tool library for these two tools.
- Then, under Toolpaths, change your Engraving Depth to 0.003”.
- Scroll down to the Advanced SVG dropdown menu. Select “Use Advanced SVG Handling”. This tells the Bantam Tools software to read the colors in our SVG, designed to tell the Desktop CNC Milling Machine how to mill the fills and strokes.
Step 4: Prep and load your stock.
Once your tool is loaded, it’s time to prep and load your stock into the Desktop CNC Milling Machine. Navigate to the Material Setup tab. Using digital calipers, measure the dimensions of your stock and enter them into the X, Y, and Z values 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 this stock. We won’t use the toe clamps for this job, so you can remove them from the machine if they’re installed. We’ll be using the L-bracket to act as a backstop for our material.
Double-sided tape is a great fixturing option for when you’re machining thin pieces of stock. And don’t worry, it’s so strong that you may need 91% isopropyl alcohol to remove your part from the T-slot bed.
To prep your stock:
- Ensure the surface of your aluminum stock is clean, and cover as much surface area as you can with double-sided tape. Make sure the strips don’t overlap or wrinkle because this will affect your Z thickness.
- Remove the paper backing after applying.
- Now press the material into place on the T-slot bed using the L-bracket as a backstop, and center it on the bed.
Step 5: Manually locate your stock.
Because we’re working with such a thin piece of stock, we’ll use the Manual Stock Location routine to configure the X and Y offset for our material, as opposed to the Automatic Stock Probing routine. This is an alternate way to locate material, and given that our file fits well within our stock, this manual approach is acceptable.
Follow these steps:
- Under the Material Placement dropdown menu, click the Probe Material button.
- Select Manual Stock Location and click Next.
- Carefully use the jog wheel to move your tool over the front left corner of the stock using the engraving tip as a pointer. You can get close to the top surface, but keep the tip off of the stock. We’ll configure the height in the next step.
- Select the Center radio buttons for the X and Y axes, and click Set X Zero and Set Y Zero.
- When you’re done, click Okay.
Note: To learn more about the Manual Stock Location routine and other material and plan placement probing routines, check out our Material & Plan Placement Probing Routines support guide.
Step 6: Configure plan placement.
Now that you’ve located your material, it’s time to configure your Z height and enter your plan placement. Plan placement routines allow you to align your plan to a point other than the default location of the top left corner of your stock.
Go to the Plan Setup tab, click the Probing Routines button, and select Automatic Stock Probing to launch the Single-Axis Probing routine.
- Jog the spindle over the workpiece.
- Because the machine isn’t in direct contact with the bed, you’ll need to create a conductive loop. Using one of the collet wrenches, place one end on the stock and the other on the T-slot bed.
- When you’ve closed the loop, click the Probe Z- button.
- When the probe comes in contact with the stock, it will stop. Click the Set Z Zero button. Then use the jog controls to back off of the workpiece.
- Click OK.
The Z value under Manual Placement has now been updated.
Before you start milling, we’ll use the manual plan position controls to adjust your plan placement within the stock. Adjust the X and Y values under Manual Placement as well, so that the plan is 1/4” away from the material edge. Now there’s a healthy buffer between the design and the edge of the material.
Step 7: Start milling!
Go down to the Summary tab to review your job. When you’re satisfied, click the Mill Single File button and watch your Desktop CNC Milling Machine go to work!
Step 8: Change your tool.
When the machine is finished engraving, it’ll pause and you’ll be prompted to swap the 80º metal engraving bit for the 4 mm single-flute end mill.
Remove the metal engraving bit and collet, insert a 1/4” or 6 mm collet into the collet nut, then insert the 4 mm single-flute end mill, and perform a tool touch-off. The mill will proceed to machine the internal and outer cutout.
Step 9: Remove your part from the Desktop CNC Milling Machine.
Use a scraper to remove your machinist rule from the T-slot bed. We also recommend using 91% isopropyl alcohol to break down the adhesive in the double-sided tape, which makes it easier to remove the part. Apply a little bit of 91% isopropyl alcohol around the edges of your stock and within the cutout of your part. Let it sit for a minute or so and then carefully use the scraper to take the part off the bed.
Congrats! You now have a handy machinist rule that you can easily carry around with you. If you want to stop here, go measure some stuff! But there’s one more thing you can do: customize the back.
Advanced: Perform a Flip & Customize Your Machinist Rule
Step 10: Measure, flip, and fixture your part.
Glad to see you’re game for adding a custom design to your machinist rule! Let’s start by performing a simple flip. Using the instructions outlined in Step 4, prep the other side of your machinist rule (the front side that you just machined) by applying double-sided tape.
Step 10: Create a custom engraving.
If you’d like to add the “Measure twice, cut once” inscription on the back of your machinist rule like we did, then download the Machinist-Rule-Inscription.svg file and skip to Step 11 to set up your SVG file. However, if you’d like to create your own SVG design, read on!
There are a number of ways to create designs for your SVGs:
- Create them from scratch in a design program. Some of our favorite programs are Inkscape, Adobe Illustrator, and Sketch. Open the program of your choice and create your SVG. When you’re finished, save your SVG.
- Save an image or clip art (simple, black and white images work best) and format it as a vector graphic.
- Draw your own design or take a picture, and save it as an SVG.
For this project guide, we’ll be using Inkscape because it’s free and its default is to save files as SVGs, which is great since this is the file type we want.
Download Inkscape and open the program. It will automatically create a new document. Before you start designing, set your canvas dimensions to match the size of your machinist rule.
Click File > Document Properties, and in the Custom Size window, change the units to inches (in).
Measure the height and width of your machinist ruler, enter these dimensions under Custom Size, and save your file.
Create a design of your choosing using any of the three methods mentioned above, and format your design as a vector graphic. If you need more information on how to do this, see our Basic & Advanced SVG Workflows support guide.
Basic SVG handling will suffice for this custom design, so you won’t need to worry about color-coding your design.
When you’re done, click Save and head over to the Bantam Tools software.
Step 11: Set up your custom engraving file.
Go to the Initial Setup tab in the Bantam Tools software and remove the Machinist-Rule.svg file, if you haven’t already. Then import the SVG design file you just created. Again, we’ll only be using the basic SVG workflow for this operation. Complete the following steps to set up your SVG file:
- In the Milling Tools dropdown menu, select the tool(s) your plan calls for.
- In the Toolpaths dropdown menu, deselect Cutout.
- Change your Engraving Depth to 0.003”––or to the depth of your choosing.
Step 12: Probe stock location and Z height.
Install your engraving bit and then head to the Material Setup tab. Click the Probe Material button, select Manual Stock Location routine, and follow the instructions outlined in Step 5. Once you’ve located your stock, go to the Probing Routines button and select Automatic Stock Probing to launch the Single-Axis Probing routine. Use the same method outlined in Step 6 to probe the Z height of your stock.
Step 13: Install your end mill, review your job summary, and start milling.
Home stretch! Go back to the Initial setup tab and install your end mill. After you’ve performed the tool touch-off, go to the Summary tab and review your job. Be sure that there are no red marks or warning signs. When you’re satisfied, click Mill Single File.
Boom! You’ve just created your very own custom engraving for your machinist rule. Remove your part from the machine and start measuring. Remember: Measure twice, cut once!