1. Live Milling for Soft Materials (HDU)
written by Cody Pfleging and Brian Ringley
The City University of New York
Architectural Technology Dept.
Roland MDX-540
Basic 4-Axis Set-Up:

2. 2
This material is based upon work supported by the National Science Foundation
under Grant Numbers 1141234.
Any opinions, findings, and conclusions or recommendations expressed in this
material are those of the author(s) and do not necessarily reflect the views of the
National Science Foundation.

3. 3
Fig. 1 - Machining Objects Menu
Fig. 2 - RhinoCAM Menu
Introduction
RhinoCAM is a plug-in for Rhino used to create
toolpaths for the CNC mill. It works from the modeling
environment in Rhino to create simulations of the
overall milling process before actually performing any
milling. It then creates NC files (G-Code) which then
can be read by the Roland MDX-540 for the milling
process.
Open RhinoCAM Operations Browser: (Fig. 2)
- Toolbar Menu
- RhinoCAM
- Machining Operations Browser
This is where you set up different machining
operations and toolpaths.
Open RhinoCAM Objects Browser: (Fig. 3)
- Toolbar Menu
- RhinoCAM
- Machining Objects Browser
This is where you load different tools for different
machining jobs and regions/boundaries.
Fig. 3 - Machining Operations Menu Roland- 4 Axis

4. 4
Roland- 4 AxisFig. 4 - Post Processor SetupFig. 5 - Machine Type Setup
Fig. 6 - Machine and Post Processor Icons
Step One:
Machine Setup
Set up the type of machine and the post processor
that will be used for the milling process. In this guide,
we will be using the Roland 4-Axis machine and the
.nc output file.
Machine Type: (Fig. 4)
- Machining Operations Browser
- Machine
Set the Number of Axes to 4 Axis (Fig. 5).
Post Processor: (Fig. 5)
- Machining Operations Browser
- Post
Set the Current Post Processor to Roland MDX
540 by selecting it from the drop down menu (Fig.
6). If the post processor is not available, download
the post processor from nycctfab.com/fabrication/
CNCmaching
Make sure the Posted File Extension is set to .NC
by selecting it from the drop down menu if it is not
already set (Fig. 6).

5. Roland- 4 Axis
5
Fig. 7 - Stock Selection
Step Two:
Box Stock Setup
Setting up your digital stock to match your physical
material dimensions.
Create a Box Stock: (Fig. 7)
- Machining Operations Browser
- Stock
- Box Stock
Set the location of the origin of the stock by clicking
one of the corner buttons and set the dimensions of
the Stock by typing in its Length, Width, and Height
into the text boxes (Fig. 8).
NOTE: This setting corresponds to the orientation of
the milling process and must be the same origin at
the mill.
Fig. 8 - Stock Edit Fig. 9 - Stock in Model Space

6. Roland- 4 Axis
6
Fig. 10 - Selecting a Parallel Finishing Toolpath
Step Three:
4-Axis Live Milling
Roughingandfinishingyourgeometryusingtherotary
axis.
Create 2 Parallel Finishing Toolpaths
- Machine Operation Browser
- 4-Axis
- Parallel Finishing
NOTE: Rename toolpaths to indicate their purpose
(e.g. “Parallel Roughing” or “Parallel Finishing”). Use
a ball end mill for all live 4-Axis jobs.

7. Roland- 4 Axis
7
Fig. 11 - Axis: Step Down Control Fig. 12 - Axis: Cut Parameters
Step Three (continued):
4-Axis Live Milling
Important toolpathing considerations.
Step Down Control: (Fig. 11)
In the Step Down Control tab of the Parallel Roughing
toolpath enter the dimension of your stock from its
center to its outer most point. For a 4”x4”block of
wood that value would be 2.835.
NOTE: This can be left unchecked for your Parallel
Finishing toolpath.
Cut Parameters: (Fig. 12)
In the Cut Parameters tab for both the Parallel
Roughing and Parallel Finishing toolpaths, the Cut
Axial Containment parameter should be offset by a
minimum of the selected tool’s radius.
NOTE: Run a simulation and check to see that
the tool holder (collet nut) is not colliding with the
portion of the stock used by the chuck or tailstock for
securing the stock to the rotary.

8. Roland- 4 Axis
8
Fig. 13 - Simulate Tab
Fig. 14 - Simulation Model
Step Five:
Simulate Toolpaths
Confirm that toolpaths are safely producing the
intended results.
Run Simulations: (Fig. 14)
- Select the toolpath to simulate
- Machine Operation Browser
- Simulate
- Play
Detect Collisions: (Fig. 15)
Running a simulation of each of your toolpaths prior
to posting is an essential part of the CNC milling
process. It is very difficult for even an experienced
RhinoCAM user to be confident that based on the
data entered in your toolpathing parameters that
you will produce the model you intend without first
running the simulations. The most important reason
to run the simulation of your toolpaths is to detect
potential collisions.
In this image the collet has collided with the stock.
The areas where the collision has occurred are
shown in red. This type of collision typically occurs
when a endmill with a relatively small diameter is
used (1/8”or less). These smaller endmills typically
have shorter tool lengths, as well. As a result of this
shorter tool length, the collet must move deeper into
the stock in order for the endmill to reach its cutting
surface. The collisions shown in the far left and right
of this image are a prime examples of this type of
collision. The endmill has removed material in order
to get to a certain depth, but because the collet is
wider it collides with the stock.
By default, your original stock is displayed in orange
and, as the simulation plays out, your geometry is
displayed in gray. Collisions will show themselves in
red.