WorkBee

WorkBee

MachineInfoBox Ooznest WorkBee CNC
Synonyms:	DE: CNC-Fräse, CNC-Plattenfräse, Portalfräsmaschine
Type:	CNC Router
Material:	wood
Used with:	6 mm, 8 mm, 1/4" or 1/8" end mills; some kinds of router bits
Location:	CNC Area
Access Requirements:	CNC Router Introduction
Status:	Working
Firmware:	grbl
Software:	LaserWeb, Fusion360, see G-Code Sender
Manual:	product page, click "documentation" tab
Tutors:	NitramLegov Pakue Johannes Luzian Leo
Similar (More or Less):	router, CNC mill

Currently defective due to a buggy/broken controller board! See Issue #307

We have a 1500mm x 1500mm version of the WorkBee CNC router, which is based on the Openbuilds OX. It can currently cut sheet material of up to 50 mm thickness on a work area of approximately 1250 × 1250 mm. The surfaced (plangefräste) spoilboard area is 1260 × 1160 (x × y) mm.

Our plans for further improving it up can be found in our "WorkBee CNC" github project - maybe you would like to help.

Fusion 360 Setup

To use the router in Fusion 360, make sure you add the latest machine definition and post-processor to Fusion 360.

You can find the newest version of these required files here. Feel free to submit improvements.

Router

The router mounted to it is a Dewalt D26200 (GB; known outside Europe as DWP611). You need to consider the sizes of its collets (Spannzangen) when buying your router bits.

• no-load speed: 16000 - 27000 rpm
• max cutter diameter: 30 mm
• available collet diameters:
  • 8 mm
  • 6 mm
  • 1/4 inch (6.35 mm)
  • 1/8 inch (3.175 mm)

The collets of the DW613, DW620 and DW621 also fit the router and are easier to get in Germany than the original ones.

RPM Chart

Dial Setting	Approx. RPM
1	16000
2	18200
3	20400
4	22600
5	24800
6	27000

Spoilboard

Ooznest recommends a 6mm spoiler board, our first one is 20mm thick. It is mounted to the frame using 4 drop-in T-slot nuts. Cutting into the boards will make it uneven, from time to time it is neccessary to surface the spoiler board again.

The total size of the spoilboard is currently 1445 × 1370 mm.

When there is time, we would like to drill workholding holes into the spoilboard.

Electrics

The Machine received a full electrical overhaul in the first half of 2024, here are its current electrical specifications:

• Duet 3 6HC+ Mainboard running RepRapFirmware
• Web- and touch interface
• MT-2303HS280AW 2.8A NEMA23 Stepper Motors
• Dewalt D26200 Router

Dust Extraction

The Workbee Vacuum automatically turns on with the spindle. We have added a cyclone dust separator before the shop vac so the bulk of the chips should be collected in an easily emptied box rather than the shop vac's bag.

The part that attaches the dust extraction hose to the router is called a "dust shoe". We are currently using this one designed by Patrick. The next version should ideally fit the dust extraction hose without an adapter and include a kind of transparent, flexible "skirt" to optimize the airflow.

Other interesting designs:

• https://www.thingiverse.com/thing:2802301

Workflow

This is just an overview and does NOT replace the personal introduction!

1. create the tool paths in a suitable CAM software (e.g. Fusion 360)
2. secure your workpiece on the machine's bed
3. insert the appropriate collet & bit as defined in your tool paths
4. home the machine, jog to your workpiece origin and zero your work coordinates
5. Upload your generated G-Code
6. put on personal protection
7. Run your Program
8. Once the Machine has homed, turn on the spindle & vac on the control panel (only works after homing)
9. Be ready to hit the Emergency Stop in case SHTF. Your Program is running!

Using the WorkBee CNC

This Section explains how to use the Machine to create parts.

General Machine Operation

Interfacing with the WorkBee CNC has changed significantly after the 2024 rebuild. This section will explain its operation.

The machine:

To start the Machine, the Electronics Panel on the left have a power strip (Mehrfachstecker) with a toggle switch. This is the main on/off switch.

After starting, ensure both E-Stops are not pressed. The machine will start up, and you can open the Web Interface on the Tablet, PC or any other device.

Web Interface

The WorkBee CNC is controlled via a Web Interface accessible through the CoMakingSpace network. On any connected device, visit http://comakingcnc/ or http://10.2.0.3 to control the machine and upload jobs.

To start milling, you begin by inserting an endmill, homing the machine, and jogging the machine XY over your workpiece origin (usually the left-front corner). Then, slowly lower down until the tip of the endmill touches the workpiece. This is your workpiece zero point. Save this point by clicking on Set Work XYZ. All this is done through Machine Movement on the Dashboard of the Web Interface:

Then, upload your job to the machine, either on the top right of the Web Interface or through the Jobs tab.

Starting a job

When starting a milling job, make sure the workpiece is secured well and you are wearing proper PPE. Next, start your job via the Web Interface. The machine will home. Then, after homing, you can start the spindle with the button on the front panel interface. This button will not work before homing or if no job is running to ensure someone is present at the start of any operation.

Sit back, relax, and keep an eye out in case you need to use the E-Stop - the machine will now start making your parts.

Fusion 360 Process for Contour Machining

The following section will walk you through setting up a contour milling operation in Fusion 360 for the WorkBee CNC. You will start with a New Fusion 360 Document and end up with a G-Code file ready to upload to the machine.

For further information and the explanation for each step, consult the Fusion 360 Documentation

Prepare

To get started, you will need to create the 2D geometry you’d like to mill out. For testing, a simple square with about 50 mm side length is a good starting point. Extrude it by the material thickness you plan to machine.

Then, in the top left corner of Fusion 360, switch from the “Design” workspace to the “Manufacture” workspace. This is where you’ll define your toolpaths and machine settings.

Import Workbee CNC

Before you get started, make sure you have properly imported the latest version of the machine definition and postprocessor into Fusion 360.

Check the last updated date on the GitHub page above. If you haven't imported the latest definitions since then, you'll need to add them.

At the top of the Fusion 360 Interface, select "Manage > Machine Library". Then under "My Machines > Local" you can import (NOT CREATE) the machine definition.

ALSO SEPARATELY IMPORT THE LATEST POST PROCESSOR! Under the machine entry in your machine library, the "Post:" section, you can click the folder icon to import the latest post processor from the GitHub page.

The import process

Create your Milling Tool

At the top of the Fusion 360 Interface, select "Manage > Tool Library" to open the tool library. Navigate to "Local > Library". This is where you'll save all of your endmill data.

Click on "[+]" to add a new tool. Select the appropriate geometry, most likely "Flat End Mill".

Tab 1: General

Here you can name your endmill. Describe them well, you'll mix them up otherwise. Also enter sourcing information (such as aliexpress links) here, you'll thank yourself later.

Tab 2: Cutter

Take Measurements of your tool for dimensions using calipers (Messschieber) and populate the values accordingly.

Adjust number of flutes and the geometry to match your endmill. I recommend setting "length below holder", "shoulder length" and "flute length" to the same value, that being the length of fully formed cutting flutes of your endmill.

Tab 3: Shaft

leave as is

Tab 4: Holder

leave as is

Tab 5: Cutting Data

Cutting Data Tab

The following cutting data is a recommended starting point for a 1/8” (3.175mm) 2-flute flat nose endmill cutting plywood. Many of the values (marked with fx) are calculated automatically and don't need adjusting.

Tweak these values as you gain experience:

• Spindle Speed (Drehzahl): 16,000 RPM
• Cutting Feedrate (Schnittvorschub): 1000 mm/min
• Ramp Feedrate (Helixvorschub): 500 mm/min
• Plunge Feedrate (Eintauchvorschub): 500 mm/min
• Coolant: DISABLE (To prevent errors, the WorkBee doesn’t have a coolant system)

Tab 6: Post Processor

leave as is.

Sanity check all data once over and click "accept" to confirm.

Configure Setup

Create by selecting "Setup > New Setup"

Tab 1: Setup

• Machine:
  • Select the latest machine definition
• Workpiece Coordinate System
  • Origin: Stock Box Point
  • Select Front-Left-Top corner

Tab 2: Stock

• Mode: Relative size box
  • Stock side offset: 5 mm
  • Stock top offset: 0 mm
  • Stock bottom offset: 0 mm

Tab 3: Part Position

leave as is

Tab 4: Post Process

Optional: adjust program name.

leave as is.

Set up 2D contour operation

At the top of the Fusion 360 Interface, select "2D > 2D Contour" to create a new 2D contour milling operation.

Tab 1: Tool

• Select the appropriate Tool
• Ensure the cut parameters are sane and have been properly inherited from the tool

Tab 2: Geometry

• Select the 2D contour you want to machine (the bottom edge of your design)
• Enable tabs
  • Tab Shape: Triangle
  • Tab dimensions example:
    • 6 mm width
    • 4 mm height
    • 30 mm Distance

Tab 3: Heights - leave as is

Tab 4: Passes

• Sideways Compensation: Right (Rechtsfräsen)
• OPTIONAL: Preserve order Check this box if you have nested features (cutouts within cutouts) to maintain the cutting order
• OPTIONAL: Smoothing Filter Enable for smaller file sizes

Tab 5: Multi-Axis

• leave as is

Tab 6: Linking

• Lead-In: Deactivate
• Lead-Out: Deactivate
• Ramp: Enable
  • Maximum Ramp Stepdown: Start with 3-6 mm and adjust based on endmill strength, desired cut quality, and material thickness

Confirm the Operation with OK. Fusion 360 will now display a preview of the operation.

Simulate to check & Export

post processor menu

• At the top of the Fusion 360 Interface, use the “Actions > Simulate” tool to check you haven’t missed anything
• At the top of the Fusion 360 Interface, use "Actions > Post Process"
• Check Use Machine Configuration (“Maschinenkonfiguration verwenden”)
  • Select Machine: “Comakingspace CNC”
  • Check Post-Processor: “WorkBee CoMakingSpace RRF”
• Export

You now have a G-Code file to upload to the CNC via its web interface!

Organization around the Machine

Around the machine, there are plenty of ways to keep all tooling organized. These are for public things. Anything here is free to use for anyone, so leave your leftovers and take what you can use!

As with all other tools, please leave the CNC more organized than you found it. For example, the collet wrench should always return to its intended place:

Gridfinity

In front of the machine, at the table, there are Gridfinity baseplates:

Gridfinity is a 3D Printed organization system based on a 42mm grid. The bins in front of the machine are meant to be freely used, labeled and expanded upon. You can find additional bins to 3D Print on sites like Thingiverse, Printables and Thangs. For example, if we add more collets in the future, re-print the collet holder.

Pegboard

On the wall left of the machine, there is a pegboard system for storing the larger items such as dust shoes. It is a Küpper, also known as “Euro” style pegboard based on a 15 mm grid of 4.5 mm holes. Just as with Gridfinity above, the usual sites offer various ready-made 3D models of hooks and holders to print yourself, and there’s always the option to just buy more hooks from Küpper at Bauhaus or Amazon.