Snapmaker CNC Milling Hands-On
β οΈ CNC Safety Guidelines (Must Read)
- A teacher must be present before starting the CNC module
- Wear safety goggles β chips and debris will fly during milling
- Never touch a spinning tool β even at low speeds, it can cause serious injury
- Tie back hair and roll up sleeves β prevent getting caught in rotating parts
- Know where the emergency stop is β the pause/stop button on the Snapmaker touchscreen
- Never leave the machine unattended during operation
A. When Should You Use CNC Milling?
CNC milling uses a spinning cutting tool to remove material from a solid block, leaving behind the shape you want. Unlike 3D printing (which adds material), CNC is a subtractive manufacturing process.
CNC vs Laser Cutting vs 3D Printing
| Comparison | CNC Milling | Laser Cutting | 3D Printing |
|---|---|---|---|
| Dimensions | 2.5D / 3D | 2D (through-cut) | 3D |
| Materials | Wood, acrylic, aluminum | Wood, acrylic, cardboard | PLA, ABS plastic |
| Precision | High (Β±0.1mm) | High | Medium |
| Strength | Depends on material (aluminum is very strong) | Depends on material | Weaker (layer bonding) |
| Typical VEX Uses | Aluminum brackets, precision mounting plates | Acrylic guards, lightweight plate parts | Sensor mounts, custom gears |
VEX Recommendation: If your part needs to withstand impacts (such as chassis brackets or pusher mounting plates), CNC aluminum is much stronger than 3D printing. For lightweight shells or guards, laser-cut acrylic is faster.
B. Luban CNC Workflow
Step 1: Import the Model
- Open Luban and select CNC mode
- Click + Add and import the STL file you exported in Chapter 21
- The model will appear in the work area preview
- Check that the model dimensions are correct (shown in the left panel)
Step 2: Set the Machining Orientation
- Select the model and find Orientation in the left panel
- Decide which face should point up (this is the face the tool can reach)
- For flat parts: have the largest face pointing up
- For parts with pockets: have the face with the pocket pointing up
Step 3: Select the Tool
CNC tools included with the Snapmaker:
| Tool | Diameter | Use Case |
|---|---|---|
| Flat End Mill | 3.175mm (1/8") | Bulk removal, flat surfaces, contour cutting |
| Ball Nose | 3.175mm (1/8") | Curved surface finishing, 3D relief |
| V-Bit Engraving Tool | ~0.2mm tip | Text engraving, fine detail lines |
VEX Parts Recommendation: The flat end mill is sufficient for most jobs. Use it for roughing to cut the general shape, then switch to a ball nose for smooth curved surfaces if needed.
Step 4: Generate the Toolpath
- Click Process (machining settings)
- Select a machining method:
- Contour β cut along the outer profile to shape the part
- Pocket β mill away an interior area
- Relief β 3D surface machining
- Set the Step Down (depth per pass) β don't cut too deep in one pass!
- Click Generate Toolpath to preview the tool path
- Carefully review the preview animation β make sure the path is what you intended
Import an STL file, set the tool and machining method, and generate a toolpath preview. Confirm that the toolpath looks reasonable.
C. Common Material Parameters
β‘ Model-Dependent: We use a Snapmaker 2.0 A350 with a work area of 320 Γ 350 mm and the standard CNC module. The parameters below are based on real tests with this model and can be used directly. For new materials, we still recommend testing with a small piece first.
| Material | Spindle Speed | Feed Rate | Depth per Pass | Notes |
|---|---|---|---|---|
| Wood (basswood, MDF) | 12000 RPM | 400 mm/min | 0.5-1.0mm | Easiest to machine, great for practice |
| Acrylic | 12000 RPM | 300 mm/min | 0.3-0.5mm | Too fast and it melts β keep it cool |
| Aluminum (6061) | 12000 RPM | 150-200 mm/min | 0.1-0.3mm | Take it slow, use cutting fluid to cool |
Aluminum Warning: The Snapmaker can machine aluminum, but you must be very careful. Keep the depth per pass very shallow (0.1-0.3mm), use a slow feed rate, and always use cutting fluid to prevent the tool from overheating. Have your teacher supervise when cutting aluminum for the first time.
D. Workholding and Tool Setting
Workholding (Securing the Material)
The material must be firmly secured during CNC milling. Otherwise, the cutting forces will move the material β at best ruining the part, at worst breaking the tool.
- Double-sided tape + wasteboard (simplest):
- Place a sacrificial piece of wood on the Snapmaker's work surface
- Use strong double-sided tape to stick the material to the wasteboard
- This way, if the tool cuts through the material, it won't damage the work surface
- Bolt clamping (more secure):
- Use the Snapmaker's T-slot and bolt-down clamps
- Best for harder materials like aluminum
Tool Setting (Setting the Origin)
Tell the Snapmaker "where to start cutting":
- Enter CNC mode on the touchscreen
- Manually move the tool to the front-left corner above the material
- Slowly lower the tool until the tip just touches the material surface (use the paper test: if a piece of paper can't slide under the tip, it's touching)
- Tap Set Work Origin on the touchscreen
- Zero all three axes (X, Y, Z)
Paper Test Method: Place a sheet of A4 paper on the material and slowly lower the tool. When the paper can just barely no longer slide freely, the gap between the tool tip and the surface is about 0.1mm. This precision is sufficient for VEX parts.
Answer: (1) Why do you need a wasteboard? (2) How do you know when the tool tip is at the right height using the paper test?
E. Common Troubleshooting
| Problem | Cause | Solution |
|---|---|---|
| Finished part is larger than designed | Tool diameter compensation not applied | Enable "contour offset" in the Luban toolpath settings |
| Visible tool marks on the surface | Feed rate too fast or step-over too large | Reduce feed rate and decrease the step-over value |
| Material shifted during cutting | Workholding not secure enough | Improve clamping or reduce depth per pass |
| Acrylic melted and stuck to the tool | Speed too high or feed too slow (heat buildup) | Lower spindle speed or increase feed rate; add a cooling fan |
| Tool broke | Depth per pass too deep, material too hard, or hit a clamp | Reduce depth per pass; check toolpath for clamp interference |
| Didn't cut all the way through | Z-origin was set too high | Re-set the tool origin, or increase total cut depth in Luban |
Beginner Tip: For your first CNC job, start with wood. It's cheap, easy to cut, won't melt, and won't break tools. Once you have a feel for the parameters, move on to acrylic and aluminum.
Use a piece of wood to mill a simple part (such as a block with a hole). Check the dimensional accuracy and surface quality.
F. Record It in Your Engineering Notebook
The VEX engineering notebook should document your manufacturing process. Judges especially look for evidence that you actually built things yourself, not just assembled off-the-shelf parts. CNC machining is a strong differentiator.
Notebook Entry Template
π Manufacturing Log β CNC Milling
Date: ____/____/________
Part Name: ________________
Material: ________________ Thickness: ____mm
Machine: Snapmaker 2.0 A350
Tool: ________________ Diameter: ____mm
| Parameter | Value |
|---|---|
| Spindle Speed | ________ RPM |
| Feed Rate | ________ mm/min |
| Depth per Pass | ________ mm |
| Total Machining Time | ________ minutes |
Problems Encountered:
Solutions:
Improvement Plan:
Judge Bonus Points: Include in your notebook: (1) Onshape design screenshots (2) Luban toolpath screenshots (3) Photos of the machining process (4) Photos of the finished part. Showing the complete "design β manufacture" workflow makes a strong impression.
Chapter Summary
- CNC milling is ideal for load-bearing parts (aluminum brackets, mounting plates)
- Luban CNC workflow: Import STL β Select tool β Set parameters β Generate toolpath β Machine
- Start with wood for practice; move to acrylic and aluminum once you're comfortable with the parameters
- Document the manufacturing process in your engineering notebook β judges value this highly
In the next chapter, we'll use the Snapmaker's laser module to cut acrylic parts.