Brendan Harmon

CNC Surface Milling

CNC surface milling with RhinoCAM

CNC surface milling

Contents


CNC Surface Milling

Use computer numerical controlled (CNC) milling to digitally fabricate a topographic model in Rhino with the RhinoCAM plugin. Download the Rhino model for this tutorial. This model was generated by the Grasshopper definition trigonometric-landforms.gh. This tutorial is written for a 3-axis Forest Scientific CNC Router using VelocityCNCmill as the post processor. Watch at or .

Model of procedurally generated landforms


Machine Setup

Start Rhino and set the units to Inches. In the RhinoCAM menu switch to the MILL module for CNC milling. In RhinoCAM’s Machining Browser in the Program tab use the default 3 Axis machine. In Post set the post processor to VelocityCNCmill. Set the posted file extension to a .nc numeric control file.


Stock

The stock for this CNC milling exercise is a 6” x 6” x 2” block of high-density urethane (HDU) foam board such as Renshape or Signfoam.

In RhinoCAM’s Machining Browser in the Program tab in Stock select Box Stock and set the dimensions to 6” long, 6” wide, and 2” high. In Align select Align Stock and set Z alignment to Top and XY alignment to South West. Then in In Align select Set World C.S. and set the origin to the stock box, set the zero face to Highest Z, and the zero position to South West.

Create stock from box

Align the stock to the part

Align the world coordinate system to the stock


Tools

In the Machining Objects panel create a new tool. This will be a ball end mill made of carbide with a 0.25” diameter and 2 flutes. The feed rate and speed depend on the tool, stock, and machining operation. Set the tool type to Ball Mill, tool length to 3.25, shoulder length to 1.75, flute length to 1.5, and the tool diameter to 0.25. In the properties tab set the material to carbide and the number of flutes to 2. In the feeds and speeds tab set the speed to 15000 RPM, plunge to 20, approach to 180, engage to 180, cut to 200, retract to 180, and departure to 180. Save the tool. Alternatively in the Machining Objects panel load the cnc_surface_tools.csv tool library.

Feeds & Speeds

Speed Plunge Approach Cut Retract Departure
15000 20 180 200 180 180

Ball end mill

Feeds and speeds


Machining Operations

In the Machining Browser in the Program tab in Machining Operations under 3-Axis Advanced select Parallel Finishing. In the tool tab select the 0.25” ball end mill. In the feeds and speeds tab load the settings from the tool. In cut parameters set the stepover to 25% of the tool diameter. Generate the toolpath. Then right click on the parallel finishing operation and select post to export the toolpath as a .nc numerical control file. Save the numerical control file to a USB drive to load onto the computer connected to the CNC machine.

Parallel finishing operation


Simulation

In the Simulation tab of the Machining Browser under Simulate select Play to simulate the machining operation in Rhino’s viewports.

CNC simulation

CNC surface milling


Machining

Checklist


Thermoforming

Checklist

  • Turn power switch on (at the back bottom)
  • Set mode to Acrylic 8 and start heating
  • Raise bed, open cover, add acrylic sheet, close cover, and lower bed
  • Pull heating element forward
  • Wait 90 seconds until acrylic is hot
  • Push heating element back
  • Turn off vacuums
  • Raise bed to form the model
  • Cool model with air hose
  • Puff the acrylic to release the model
  • Open cover and remove model