Skip to content

7. Computer controlled machining

Group Assignment

This week we had the opportunity to work with the ShopBot PRSalpha CNC Router, diving into both its functionality and operating methods.

As part of our group assignment we covered:

Safety

1. Personal protective equipment (PPE)

Before you start working, make sure you are protected:

✅ Goggles or protective screen - flying chips can injure your eyes.

✅ Respirator (FFP2-FFP3 mask) - when cutting wood, fine dust is generated that is dangerous to breathe.

✅ Earmuffs or earplugs - the CNC router can be very loud.

✅ Gloves are NOT NEEDED - their use when working with a rotating tool is dangerous (can wind up your hand).

2. Clothing and work area

✅ Clothing should be tight-fitting, without hanging elements.

✅ Long hair should be tied up in a bun or under a cap/bandana.

✅ No jewelry (bracelets, rings, chains) - they can get caught on the tool.

✅ The workplace is clean - tools, dust, unnecessary items are removed.

General safety

3. Machine preparation

Before starting, be sure to check:

✅ Workpiece fastening – must be firmly fixed on the table (clamps, vacuum table).

✅ Reliability of the cutter fastening in the collet chuck.

✅ Cleanliness of the work table – nothing extra in the cutting area!

4. Check the program before running

Before running the G-code, do the following:

✅ “Dry run” - run the program without a cutter to check the trajectory.

✅ Correct “zero” (zero point) - especially important for multi-stage processing.

✅ Cutting depth and feed parameters - too high a feed can break the cutter.

✅ No collisions - check if the cutter will touch the fastener or the workpiece in unexpected places.

To avoid collisions with clamps when working in VCarve Pro ShopBot Edition, it is necessary to set the correct parameters in the software. In the Toolpaths -> Material Setup -> Rapid Z Gaps above Material section, set Clearance (Z1) = 100 mm, and in Home / Start position, set Z = 100 mm.

Clearans

This will ensure that the spindle lifts 100 mm when moving between operations, preventing potential collisions with clamps and the workpiece. This approach is especially useful when using clamps or other tall fixtures.

5. Working with the machine

✅ Stay close to the CNC router during operation – do not leave it unattended!

✅ Keep a safe distance – at least 30-50 cm from moving parts.

Safe distance

✅ DO NOT reach into the work area with your hands during operation.

✅ Use a brush or vacuum cleaner to clean the machine – do not remove chips with your hands.

✅ If you hear any strange sounds – STOP!

  • Squeaking, squealing, cracking – the cutter may be skewed, broken or fed incorrectly.

  • Stop work immediately and check the tool.

6. After finishing work

✅ Wait until the cutter has come to a complete stop before approaching the machine.

✅ Unplug the machine if you are no longer working.

✅ Clean the work area, remove dust and sawdust.

✅ Check the wear of the cutter - replace if necessary.

Dangerous situations and what to do

❌ The cutter broke during operation - immediately stop the machine, turn off the power, remove the fragments.

❌ The workpiece was torn off - turn off the machine, fix it more securely.

❌ Smoke or a burning smell appeared - possibly incorrect speed or overheating. Stop work, check the cutter and feed.

❌ The machine behaves unstable - check the connections, calibration and mechanical components.

Material Fixation Methods

As part of our group task, we explored several methods for securing material to the sacrificial table.

🔹 Clamp Fixation – Using clamps to hold the material in place.

Fixation 1

🔹 Fixation through existing holes in the sacrificial table – If the material is smaller than the table, it can be secured along the edges using the existing holes on the table.

Fixation 2

🔹 Fixation through a pre-drilled hole in the material – This method is used when the material is large and does not sit flush with the table, especially in the middle.

For this method, after placing the parts on the material, the CNC machine can mark 1mm spots in free areas. Then, you can manually drill holes and secure the material with screws.

Tool Changing

The tool is changed using two wrenches. For safety reasons, one wrench is attached to the key that controls the spindle power.

Tool changing 1

When tightening or loosening, both wrenches should always be held between your palms. This way, if they slip, they won’t injure your hands.

Tool changing 2

Dust tends to accumulate in the tool holder, making it difficult to loosen over time. To prevent this, applying a silicone lubricant beforehand is a good solution.

Tool changing 3

Zero Point Setting

To set the zero point on the Z-axis, a special metal plate is placed on the material, and a wire is attached to the spindle.

Zero point 1

In the ShopBot3 control software, there is a dedicated Z zero button that lowers the spindle until the end mill touches the metal plate.

Zero point 2

When the end mill tip touches the metal plate, an electrical contact is created, allowing the machine to register the Z = 0 position. The thickness of the plate is automatically subtracted to ensure precise calibration.

Zero point 3

To change the zero points for the X and Y axes, move the end mill to the desired position. Then, in the ShopBot3 control software, click on Zero Axes select the required axis, and press OK.

Zero point 4

Types of End Mills for Cutting

As part of a group assignment, we looked at several types of end mills for cutting material.

End mills

🔹 Upcut End Mill – Provides good chip evacuation but may cause tear-out on the top surface. Best for deep cuts in soft materials.

🔹 Downcut End Mill – Produces a clean top edge but pushes chips downward, requiring good dust extraction.

🔹 Compression End Mill – Prevents tear-out on both the top and bottom surfaces of laminated materials like plywood and MDF.

🔹 Straight End Mill – No lifting or pushing, ideal for consistent cuts. Ideal for wood, MDF, plywood, and acrylic.

VCarve Pro ShopBot Edition

VCarve Pro ShopBot Edition is a powerful software specifically designed for use with ShopBot CNC machines. It allows users to create, edit, and manage toolpaths for 2D and 3D CNC machining.

When creating a new project in VCarve Pro ShopBot Edition, you can set up the following parameters:

  • Material Dimensions – Specify the length, width, and thickness of the material to fine-tune the workspace.

  • XY Orientation – Select how the material will be oriented relative to the X and Y axes, which helps to correctly position the workpiece for machining.

  • Zero Point Position (0) – You can set the zero point relative to the top or bottom of the material, which is important for accurate calibration and ensuring correct coordinates when milling.

V Curve 1

The program has good tools for creating and editing drawings.

V Curve 2

After completing the design, it must be placed in the desired places on the material. In the Toolpaths section, there are tools with which we can cut or engrave the material, or make a hole in the material.

V Curve 3

2D Profile Toolpath

To cut the material, we select the 2D Profile Toolpath. The first step is to set the Cutting Depth (C). In our case, the material thickness is 10.1mm, so to ensure a complete cut, we set the value to 10.2mm.

V Curve 4

Tools

Next, we select the tool for cutting the parts. In the pop-up window, we can choose, create, or edit a tool. In our case, we selected a 6mm end mill.

V Curve 5

A crucial parameter in material cutting is Pass Depth, which defines how deep the tool cuts in a single pass. To extend tool life, it is recommended to keep this value around half the tool diameter.

The Stepover value is essential for engraving; for good material processing, it should not exceed 50% of the tool diameter.

Additionally, Feeds and Speeds play an important role. Here, we set the spindle speed (RPM), along with Feed Rate and Plunge Rate.

Machine Vectors

In the Machine Vectors section, we define how the tool should follow the path. There are three options: Outside, Inside, and On. In our case, we want the final part to match the specified dimensions, so we select Outside.

V Curve 6

As it later turned out, the choice of movement direction played a crucial role in our case. There are two options: Climb and Conventional. Each has its own advantages and disadvantages. You can find more details here.

Tabs

If we leave everything as is, the part will be completely cut out and may shift due to vibrations, leading to defects.

To prevent this, we can secure the material to the sacrificial table with screws or use Tabs. Tabs have two main parameters:

  • Length – The horizontal size of the tab.

  • Thickness – The vertical thickness that remains uncut.

V Curve 7

After cutting, the part remains attached to the material via Tabs, ensuring a clean cut without damage.

V Curve 8

By selecting Add tabs to toolpath and clicking Edit tabs, a menu opens where we can place tabs in the required positions.

V Curve 9

It is best to place Tabs at the edges of the part, especially if they are thin. If, during the final pass, the thin edges are not secured, they may break or shift, affecting the cut quality.

ShopBot3 Control Software

ShopBot3 is the official control software for ShopBot CNC machines, allowing users to operate the machine, execute toolpaths, and fine-tune settings. It provides a user-friendly interface for both beginners and experienced machinists.

Key Features

  1. Machine Control & Movement

    • Allows manual and automated movement of the spindle along the X, Y, and Z axes.

    • Supports jogging and precise positioning.

  2. Zeroing Axes

    • Enables users to set zero points for X, Y, and Z axes.

    • Uses a touch plate for automatic Z-zero calibration.

  3. Toolpath Execution

    • Loads and executes toolpath files generated in software like VCarve Pro ShopBot Edition.

    • Supports multiple file formats, including .sbp (ShopBot’s native format).

  4. Speed and Feed Rate Adjustments

    • Users can modify spindle speed, feed rate, and plunge rate during operation.

    • Real-time adjustments help optimize cutting performance.

  5. Emergency Stop & Safety Features

    • Includes an E-stop function to immediately halt operations in case of an emergency.

    • Provides alerts for errors or potential collisions.

  6. Preview Mode

    • Simulates toolpaths before actual cutting, helping prevent mistakes.

  7. Shortcut Commands

    • ShopBot3 supports keyboard shortcuts and custom macros for quick execution of commands.

This software is essential for managing all aspects of a ShopBot CNC router, from setup to final machining.

Test results

As part of a group assignment, we conducted several tests demonstrating the capabilities and accuracy of our CNC milling machine. We wanted to demonstrate the results of end mills of different diameters (Ø3 mm and Ø6 mm), and since we only have an Up-cut Ø3 mm end mill, the tests will be conducted using only Up-cut mills.

As mentioned earlier in the Machine Vectors section, there are two movement direction options for the end mill when cutting material: Climb and Conventional.

During our initial tests, we chose Conventional, which led to inaccurate results, particularly significant deviations from the intended dimensions.

For example:

A square part that was supposed to be 100mm ended up measuring 99.24mm x 99.72mm.

Test Con

A square pocket intended to be 50mm turned out to be 50.61mm x 50.31mm.

Test Con

A square piece with a width of 50mm resulted in 49.43mm x 49.74mm.

Test Con

The most noticeable inaccuracies occurred along the X-axis.

From various sources, we learned that the Conventional cutting method is best suited for edge finishing rather than full-depth cutting.

All our subsequent tests were conducted using the Climb method.

Squareness test – “Diagonals”

Idea:

  • Cut out a 100 x 100 mm square.

  • Measure both diagonals – they should be equal.

  • Cut out the part with Ø3 mm and Ø6 mm end mills

What are we testing?

✅ Are there any distortions in the X and Y axes.

For the Ø3 mm end mill, we got the values ​​of 141.31 mm and 140.75 mm

Test 1

For the Ø6 mm end mill, we got the values ​​of 141.01 mm and 141.15 mm.

Test 1

Both tests showed satisfactory results, since in ideal conditions the diagonal of a square with a side of 100 mm should be approximately 141.42 mm. Considering the possibility of incorrect measurement, this is a pretty good result.

“Groove in groove” - ​​precision fitting test of parts

Idea:

  • Cut a 50 mm wide groove and a separate insert also 50 mm.

  • Cut the part with end mills Ø3 mm and Ø6 mm

  • Try to insert the part into the groove without glue.

  • If it does not fit, measure how much it needs to be adjusted.

What are we testing?

✅ How correctly does the CNC maintain the dimensions.

✅ How does the width of the cutter and kerf (cut thickness) affect?

✅ Is it necessary to adjust the “tool compensation”.

The result of cutting the insert using a Ø6 mm end mill showed the following result:

Test 2

And in the case of using a Ø3 mm end mill, it showed the following result:

Test 2

We did not photograph the results of cutting the grooves, but they fluctuated in the region of 49.8 mm.

In the case of using a Ø6 mm end mill, we changed the width of the insert to 49.8 mm, and we were able to insert the insert into the groove using a rubber hammer and get the following result:

Test 2

And in the case of using a Ø3 mm end mill, without changing the dimensions, we were able to insert the insert into the groove using a rubber hammer.

Test 2

Feed change test – “Depth ladder”

Idea:

  • We make a ladder-shaped milling, 3 steps of 2 mm depth.

  • We measure the depth of each step.

Test 4

What are we testing?

✅ Compliance of the actual depth with the declared parameters.

✅ Effect of load on the machine.

As a result, we measured the following values: 1.94 mm, 2.03 mm and 1.99 mm.

Test 4

The test turned out to be excellent, some errors may be associated with the roughness of the plywood. We can say that the depth corresponds to the declared parameters. When the cutter is deepened by 2 mm, the load on the spindle is not great.

Last update: March 14, 2025