PRO CNC and Standard CNC Machine Spoilboard¶

Design files for the spoilboard project are provided for use with two CAM packages - Fusion 360 or Vectric software (VCarve Pro and Aspire). Instructions below will guide you through the process of creating the G-code for your specific machine size, followed by machining of the spoilboard.

Fusion 360¶

Download the Fusion 360 Avid CNC spoilboard design file and open in Fusion 360.
In the Design workspace, click on Modify > Change Parameters.
Update the relevant parameters based on your machine configuration and desired spoilboard size. This will set the number and position of the mounting slots used to secure the spoilboard to the machine bed crossmembers.

Crossmember Positions

If a crossmember at the rear of the machine has been moved to line up with the end of the spoilboard, after clicking OK on the Parameters window, roll the timeline forward (at the bottom of the screen) to include the last three features.
Verify the placement and number of mounting slots matches the intended design.
Enter the Manufacture workspace.
Open the menu with the listed toolpaths. Right-click on each toolpath and click Generate to recalculate the toolpath.
Verify the toolpath settings are correct.

Work Coordinate Origin

The Work Coordinate Origin is set by default to Front-Left and Material-Top.

Tool Diameter

The 2D Adaptive Clear for the counterbores, 2D Contour for the mounting slots, and Drill Pattern toolpaths are set by default to 1/4" diameter tooling. The Face toolpath for surfacing the spoilboard is set by default to 1/2" diameter tooling.
If you have not yet installed the Avid CNC Post Processor for Fusion 360, it is available on our Fusion 360 software downloads page.
To export the G-code, begin by clicking the Post Processor button in the Actions section.
Select the Avid CNC post.

Manual Tool Changes

For manual tool changes, it is recommended to deselect the Use M6 option in the Post properties section.
Select an Output folder location and click Post.
Move the exported G-code files to you CNC controller computer and continue to the Spoilboard Machining section.

Vectric (VCarve Pro & Aspire)¶

Download the Vectric Avid CNC spoilboard design file and open in VCarve Pro or Aspire.
Enter the Sheets menu and double-click the sheet that matches your machine bed size. You can hide the other sheets by toggling the lightbulb icon next to each sheet name.
Open the Toolpaths menu and verify the toolpath settings are correct.

Work Coordinate Origin

The Work Coordinate Origin is set by default to front-left and material surface.

Tool Diameter

The Counter Bore Pattern, Mounting Slots, and Dowel Hole Pattern toolpaths are set by default to use a 1/4" diameter tool. The Surfacing toolpath is set by default to use a 1/2" diameter tool.
Right-click on one of the toolpath names and select Recalculate > Recalculate All.
Click the Save Toolpath icon.
Select the desired toolpaths and the saving method (Selected toolpath or Visible toolpaths to multiple files).
Select the Avid CNC (inch) post processor and export the G-code by clicking Save Toolpath(s) button.
Move the exported G-code files to you CNC controller computer and continue to the Spoilboard Machining section.

Spoilboard Machining¶

With your machine powered on and ready for operation, home the machine and run the spindle warm-up routine (if applicable).
Place a sacrificial layer of material on the machine bed, followed by the material you'll be using for your spoilboard. Clamp these to the machine bed.

Warning

Take care to ensure the clamps will not interfere with the router bit's travel.
Install the router bit used in the first toolpath into the spindle (or router). We recommend running the initial toolpaths in the following order:
1. Counterbores
2. Mounting Slots
Use the Auto Z & Corner Finding Touch Plate to set the Work Coordinate Origin, matching the Work Coordinate Origin used when generating the G-code in CAM.

Default Settings

The Work Coordinate Origin is set by default to front-left and material-top (material surface).
Load the appropriate G-code file and verify the toolpath in the Toolpath Preview window.

Soft Limits

The machine origin positions the tool a small distance over the front edge of the machine bed. If you encounter a Soft Limit (software limits) error on the Y Axis (the default table axis), you may need to consider moving the spoilboard closer to the machine origin or editing the CAM files. You can quickly check this prior to running the G-code by verifying the toolpath lines (green or white lines in the Toolpath Preview window) do not extend past the work area (dashed yellow lines).
Click Cycle Start to run the G-code program. Use this procedure to run both the Counterbores and Mounting Slots toolpaths.
With the counterbores and mounting slots machined, remove the spoilboard and sacrificial material from the machine.
Insert Roll-in T-Nuts into the crossmembers, positioning them to match the mounting features machined into the spoilboard.

Spoilboard Fasteners

PRO CNC machines include spoilboard mounting hardware in the Spoilboard Fastener Kit.
Place the spoilboard back on the machine and secure to the crossmembers using M8 Button Head Cap Screws and the previously installed Roll-in T-Nuts.
Load the G-code into Mach4 for any jigs or dowel hole toolpaths.

Tooling

Ensure you're using the correct tooling (size and type) for the current toolpath.
Use the Auto Z & Corner Finding Touch Plate to set the Work Coordinate Origin for the current toolpath.
Verify the toolpath in the Toolpath Preview window and click Cycle Start to run the G-code program.
Load the final G-code program into Mach4, the Surfacing toolpath.

Tooling

Ensure you're using the correct tooling (size and type) for the current toolpath.
Use the Auto Z & Corner Finding Touch Plate to set the Work Coordinate Origin for the current toolpath.
Verify the toolpath in the Toolpath Preview window and click Cycle Start to run the G-code program.
Repeat the previous two steps until the spoilboard is flat across the entire working area.