Use computer numerical controlled (CNC) milling to digitally fabricate a surface generated by parametric equations in Rhino. Use the Rhino file machining-parametric-surfaces.3dm as a reference. Also see Niloufar Emami's guide to computer aided manufacturing.
The stock for this CNC milling exercise is a 2.75" x 2.75" x 1" sample of Richlite Black Diamond or Rainier. Order here. High density urethane (HDU) foams including Renshape and Signfoam can be substituted for this paper-composite material.
Install the RhinoMath plugin. Then run the MathSurface command with the following equations and parameters to create a meandering mound (see Choma, Morphing, p.128-129).
MathSurface
minimum u: -PI/2
maximum u: PI/2
minimum v: 0
maximum v: PI
PointCount: 4
PointCount: 4
Function X(u,v): v
Function Y(u,v): sin(u)+cos(v)
Function Z(u,v): sin(v)*cos(u)
Scale the parametric surface to the stock box by reference length.
Command: Scale
Then scale the surface by a quarter.
Command: Scale
Origin point: 0,0,0
Scale factor: 0.25
Move the surface 0.3 inches below the top of the stock.
Command: _Move
Point to move from: 0,0,0
Point to move to: 0.70
Create a plane wider than the surface to use as a boundary for extrusion.
Command: Plane
First corner of plane: -1,-1,0
Other corner or length: 4,4,0
Extrude the surface to the boundary plane as a solid.
Command: _ExtrudeSrf
_Solid=_Yes
_ToBoundary
Extrusion distance <-1.6>
Now create an array of solid polysurfaces either manually with object snaps or using the Array command.
Command: Array
Number in X direction: 4
Number in Y direction: 8
Number in Z direction: 1
X spacing: 0.69
Y spacing: 0.4
Combine the array of polysurfaces into a single solid using a boolean union.
_BooleanUnion
Clip the parametric solid to the stock box using a boolean intersection.
_BooleanIntersection
Save your work.
_SaveAs
Launch the RhinoCAM plugin
RhinoCAM
In the RhinoCAM Machining Browser
select the MILL tab for milling operations.
Set the Machine to 3 Axis.
Set the Post to VelocityCNCmill.
Set the Stock length to 2.75, width to 2.75, and height to 1.
Set the World Coordinate System (WCS) to the box stock. Select the SouthWest corner at the bottom of the stock.
In the Machining Operations dropdown menu
select Work Zero.
Generate the work zero for the coordinate 0,0,1.
In the Machining Operations dropdown menu
select 3 Axis Adv > Parallel Finishing.
In the Parallel Finishing dialog
select or create a Ball Mill 0.25.
Tool diameter: 0.25 in
Tool length: 2.5 in
Material: CARBIDE
Speed: 15000 RPM
Plunge: 50 in/min
Approach: 50 in/mm
Engage: 50 in/mm
Cut: 200 in/mm
Retract: 800 in/mm
Departure: 800 in/mm
In the Cut Parameters tab set Stepover Control to
25% Tool Diameter.
Press Generate to compute the
first toolpath.
In the Machining Operations dropdown menu
select 3 Axis Adv > Parallel Finishing.
In the Parallel Finishing dialog
select or create a Ball Mill 0.125.
In the Cut Parameters tab set
the Angle of Cuts to 90 degrees.
Press Generate to compute the
second toolpath.
In the Simulate tab of the RhinoCAM Machining Browser run a simulation to check each toolpath.
Right click on each toolpath under the setup tree
and select Post to export numeric control .nc files with g-code.
Save the first toolpath as parallel-finishing-quarter-inch.nc
and the second toolpath as parallel-finishing-eighth-inch.nc
And of course save again!
_Save
