Roland MDX-40A User manual

HARVARD GSD BEGINNER’S GUIDE TO ROLAND MDX 40-A
prepared by Alexander Matthias Jacobson

AXYZ 4008
3 Axis (X 96”, Y 48”, Z 6”)
MDF Screw-down anchoring
Pneumatic non-automated tool change
Automatic Dust collection
Max Rotations Per Minute (RPM): 18,000
Max Feed Rate: 300 inches per minute
Software: Mastercam X7
Gund Hall’s CNC Milling Equpiment
ONSRUD 96C18
3-Axis (X 48” , Y 96”, Z 8”)
Vacuum hold-down
Automatic tool change
Automatic Dust collection
Max Feed Rate: 1200 inches per minute
Max Rotations Per Minute (RPM): 24,000
Software: Mastercam X7
ROLAND MDX 40-A
3 Axis (X 12”, Y 12”, Z 4”)
Double-stick tape anchoring
Hand tool change
No dust collection
Max Rotations Per Minute (RPM): 8,000
Max Feed Rate: 120 in/minute (3000mm/min)
Software: Mastercam X7 or Roland SRP
Typical Milling Procedures
Flip Mill
Goal: Create a form milled on two or more sides.
Machine: ONSRUD, AXYZ, ROLAND
Typical Materials: blue foam, white
foam, high-density foam, mdf
plywood, solid wood, laminated
pieces of solid wood
Topography Model
Goal: Represent landscape or surfaces,
including roads, textures, topo
lines and buildings.
Machine: ONSRUD, AXYZ, ROLAND
Typical Materials: blue foam, white
foam, high-density foam, mdf
plywood, solid wood, laminated
pieces of solid wood
Mold Making
Goal: Create two halves of a mold which
can be mated together and used
for casting.
Machine: ONSRUD, AXYZ, ROLAND
Typical Materials: blue foam, white
foam, high-density foam, mdf
plywood, solid wood, laminated
pieces of solid wood, wax
2D Contour Cut-out
Goal: Cut out 2D pieces of material.
Machine: ONSRUD, AXYZ
Typical Materials: plywood, acrylic
sheet, mdf

2. SRP Player Software
- Import geometry
- SRP Player mill settings
- Available bit sizes: .25” Ball /Flat
.125” Ball/Flat
Others can be purchased.
- Design tool motion to creat part
Roland MDX 40-A Workflow Overview
1. Create Geometry
- Center on the origin
- Maximum size: 11” x 11” x 3.5”
- Max vertical wall height: 1.6”
- Export as closed .stl
3. Preparing the Machine
- Starting the machine
- Anchoring material
- Installing endmills
- Setting the origin (X,Y and Z)
4. Run your job
- VPanel controls
- Safety precautions + observations.
- Trouble-shooting
- Changing endmills
5. Extract Piece / Clean Up
- No compressed air, use a vacuum
- Shut down the machine
Detailed instructions follow...

Create Geometry
Steps:
1) Create your geometry in Rhino. The maximum size of anything that can be milled on the
Roland MDX-40 is 4 tall (Z-axis)” x 12 wide (X-axis)” x 12 deep (Y-axis)”. Note that the maximum
pocket, hole or channel depth is limted by the dimensions of the cutting tools. On the Roland
MDX 40-A, the maximum length of a 1/4” bit is 1.7”, and the maximum length for a 1/8” bit is .9”,
so be aware that you will not be able to cut features deeper than this on the Roland MDX 40-A
unless you cut from more than one side.
2) Move to Origin. The coordinate plane of Rhino’s X,Y and Z axis correspond to the milling bed
of the Roland MDX 40-A, where the point (0,0,0) is the center of the bed, the Z-axis points up,
and X&Y are in the plane of the bed. Once you are satifsfied with your geometry, move it so that
the bottom surface of your part it is centered on the origin, as pictured above.
3) Export as .stl SRP Player uses a file format called Stereolithography, which articulates
solids and voids. It is best practice that the model is ‘closed’ when exporting as .stl. If you were
exporting a cube, for example, it would have to have six sides that are all perfectly matched
and touching without any gaps. A cube with 5-sides present and one side missing would b
considered open. Select your geometry and type “Export” into the command line. You will be
promted with the following three windows.
Under “Save as type” select “Stereolithography (*.stl).”
Set this to .001, so that your geometry is
more precise than the machine.
Use binary. If you get errors resulting
from your geometry in SRP Player, try
unchecking “Export open objects”.
Exporting as Stereolithography (.stl)
0.001

Steps:
1) Open SRP Player software.
2) Open the .stl file you exported from Rhino.
3) Enter the scale at which you would like to mill this geometry. Note: if you would like to mill it
exactly as you modeled it, either press 1/1 scale or enter in the dimensions of your geometry
manually. If you need to mill all the way to the bounds of the material, you can reduce the
amount of scrap material left around your part under Create Toolpaths > Edit > Roughing > Top
Surface > Modeling Form
4) Typically this field can be left alone, but if you would like to reorient your material you can do
so here. Note: this does not refer to orienting the direction of cutting, but rather the material in
the bed.
5) Click ‘Type of Milling’ for next step.
1 - SRP Player - Model Size + Orientation
1
2
3
Steps:
1) Select for Quality vs Speed
2) Indicate the most prevalent characteristic of your geometry
3) For a single surface choose “Block workpiece” and “Cut top only.” “Cut top and Bottom” is
used for flip-mills, or models milled on both the top and the bottom.
4) Click on ‘Create Tool Path’ to continue to next step.
2 - SRP Player - Type of Milling
1
2
3

Steps:
1) Select your material from the drop-down list. If your material is not available, consult with a
TA for selecting an appropriate substitute.
2) Enter in the size of your raw material. Your part should be parallel to the bed, and it will be
centered in X and Y. Note: the maximum size is 12” (X Axis) x 12” (Y Axis) x 4” (Z Axis).
3) Clicking ‘Create Toolpath’ will instruct the SRP player to calculate the path that the tool
should follow in order to cut out your desired geometry. For default settings, you can simply
press “Create Toolpath”, however this often results in extremely long cut-times. If you would like
to edit the settings on your toolpath, press “Edit” and proceed to the next page for guidance.
3- SRP Player - Create Toolpath
1
2
3
Here you can see and edit the details of the toolpaths SRP Player
automatically generates. You must always run a roughing toolpath
before you can run a finishing toolpath, but finishing tool paths need
not cover your entire workpiece.
Roughing passes are intended to remove material as quickly
as possible, but they do not leave as fine a finish. These passes cut
as deep and as fast as is safe, according to the size of the tool and
physical stiffness of the machine.
Finishing toolpaths are intended to control the quality of your
finished piece. They remove a small portion of remaining material
more slowly, leaving a finer cut. This is where you can finely control the
finished appearance of your piece.
3.1 to 3.8 - SRP Player - Create Toolpath > Edit Toolpaths

Each toolpath you create will have 8 sets of settings you can use to
tailor the cutting. Repeat these steps for each toolpath you use.
3.1) ROUGHING / FINISHING assigns names to your toolpath, which may make organizing
complex files easier. Note, you only need to run one roughing pass before beginning final
passes.
3.2) TOP OF SURFACE is where you orient the tool relative to your part. Select “Top + Z” unless
you want to cut into your piece at an oblique angle. Please consult with a TA if you would like to
cut obliquely, this requires rotating the physical part on the bed.
3.3) MODEL FORM This is where you control the margins of scrap material SRP will leave
around your part. If you intend to do a flip-mill (i.e. mill on both sides) this must remain at least
.5”, and it may also be useful to create bounding walls for casting.
3.4) ALL (CUT AREA) These two fields are where you can instruct SRP to mill just a portion of
your part. This can be useful for creating multiple finish passes with different surface qualities,
or for milling only part of your stock material.
3.1 3.2 3.3 3.4
3.1 to 3.8 - SRP Player - Create Toolpath > Edit Toolpaths
3.5 3.6 3.7 3.8
3.5) ALL DEPTH Here you can specify a maximum depth for your mill file. This is useful if you
would like to specify different surface finishes for varying depths of your topography. Note that
the depth is measured from the center of your material. If you want to cut one inch deep, in a
two inch deep piece of material, you would set your starting depth to 1” and your ending depth
to 0”, indicating you want it to go from 1” above the center to the center of your material. If you
want your cut to go deeper than the center, you need to specify negative numbers, so cutting
1.25” into the material would mean that your start heigth is 1” and your ending height is -.25”.
3.6) TOOL Specify the tool size and the shape of the end. Currently, the Roland MDX 40-A is
equipped with a .25” flat cutter, a .25” ball cutter, a .125” flat and .125” ball, all found in the black
toolbox beside the machine. Note, you will need to manually change the bit and re-zero the
machine for each tool change.
3.7) CONTOUR LINE Leave this setting on “up-cut” unless you’re using your own down-cutting
endmills. Downcutting endmills can be useful for avoiding tear-out, or damage to the upper
edge of the cut, however downcutting is not recommended for removing large amounts of
material because it forces the chips into the material and they cannot be evacuated.
3.8) CUTTING PARAMETERS This is where you can control the speed at which the tool will cut
through the material, as well as the amount of material it will remove with each pass. Refer to
the chart in Appendix 1 of this document for Foam Cutting Parameters, and see Appendix 2 for
Field Definitions.

4 - SRP Player - Preview Results
This is where you can see what the machine will cut, and estimate how
long it will take. At this point it is your responsibility to ensure that you
are not telling the machine to cut deeper than it is able.
Steps:
1) Press “Preview Cutting” and wait for SRP Player to simulate your job.
2) As you watch the simulation, consider the deepest parts of your model. Note that the depth
of vertical walls and deep pockets is limited by the length of the bit. The maximum depth
at which a ¼” diameter tool can cut without the gantry colliding with your material is 1.7”
and the maximum depth at which a 1/8” tool can cut without such a collision is .9” It is your
responsibility to ensure that the bit is at least as far out of the collet as your specified depth.
You need to check this value in order to prevent a collision between the collet or gantry and the
material to be milled. Be aware that this is different from the amount of material the tool can
cut in one pass-- that’s referred to as the “step-down” and it is determined by the flute length
and chip load given a specific material.
3) If you need to reduce the depth of your model you can do so by either a) rescaling your
geometry (under Model Size and Orientation), or b) specifying that the Roland MDX 40-A ignore
the lower part of your model in under Tool Path Depth (see Step 3.5).
4) If you need to reduce the amount of time it is taking to cut your model, consider using a
larger bit in step 3.6, a larger step-over for your Finish Passes in step 3.8, selecting a faster
cutting time over quality in step 2, or (if you are using multiple finish-passes) eliminating
redundant finishing passes in step 3.3.
Special Note: It is possible to use MasterCAM to generate code, which may increase the
efficiency and/or allow more flexibility in determining tool lengths.
Maximum depth
at which it is possible
to cut into the material
is defined by the
distance the cutting bit
sticks out of the collet.
VPanel is the software that allows you to interact with the mill. You’ll
need to use it as you fasten your material, install your endmill and
“home” (define the origin) the axes.
Steps:
1) Moving the gantry. The red arrows will move in X (left-right), the green arrows will move in
Y (back-forth). The movement in Y is inverted because the X axis is stationary, so move the Y
axis as if you wanted to move the bit around your material. The blue arrows control movement
in Z (up-down), these controls are duplicated in solid orange on the front of the machine itself.
As you move you can control the speed using the step sizes. Use caution when moving at high
speed, because if you collide with anything you might damage the bit, your material or the
machine and you will need to re-zero the X, Y and Z axes.
2) Overrides allow you to adjust the spindle speed and feed rate after you’ve begun milling.
The machine’s maximum spindle speed is 8000 rpm, and the maximum feedrate is 120 inches
per minute, or 3000 mm/min. Overrides are also limited to 100% of the maximum specified in
the job, so you can easily reduce speed, but you cannot increase speed at this stage.
3) Origin Controls are for communicating where the machine should place the origin, or the
point (0,0,0). Use the top of your stock as zero for Z, and the center of your stock for zero in X-Y.
4) Readout will tell you where the tool tip is, according to the location your provide as the
origin. It will also tell you how fast the bit is spinning (rotations per minute) and how fast it is
moving (inches or mm per minute).
5) Send to Cut is where you access preferences, and tell the machine to start or stop cutting.
6) MDX-40A controls allow you to pause the job mid-way. Press “View” to do this, the spindle
will stop and the gantry will retract. If you press and hold “View”, it will resume cutting. Green is
the power button, and the orange buttons allow you to move the spindle up and down
7) Emergency Stop will stop the machine immediately and cause you to lose all work you’ve
done so far. It is not possible to resume a job after an emergency stop.
1
2
3
4
5
6
7
4.1 - 4.3 VPanel - Prepare for cutting

4.1 - Fastening Material
4.2 - Install/Change Cutting Tool
Anchoring refers to the process of holding your material in place so the
mill can begin cutting.
Steps:
1) Mark the material prior to mounting. make a mark on top of your material at the center that
you can use to zero the X-Y Axes.
2) Tape the material. Double-stick tape your material to the bed of the machine (pictured in
orange, above center). Be sure to cover all four edges of your material securely enough that it
will not loosen during cutting.
3) Mount material to the bed. Be sure to mount your material onto the center of the bed,
parallel to the edge in the same orientation in which you modeled it. The Y Axis goes from front
to back, and the X Axis goes from right to left, refer to your Rhino Model if necessary.
Steps:
1) Choose Cutting Tool. Install the tool you intend to cut with first. In most cases this will be
either a 1/4” Flat or a 1/4” Round, because these are most often used for roughing.
2) Place the bit in the appropriate collet. There are two collet sizes, 1/8” and 1/4”
3) Measure how far you need the cutting tool to protrude from the collet, according to your
desired geometry and maximum cutting depth.
4) Finger tighten the collet into the spindle. Ensure that the cutting flutes are not inside the
collet, because tightening the collet on an area of the tool meant for cutting will damage the
tool and the collet.
5) Fully tigthen the collet firmly into the gantry with two wrenches (pictured above, right). One
prevents the spindle from rotating (top) and the bottom tightens the collet.
6) Repeat this for each tool change when prompted.
4.3 - Setting Origin in Z Axis + X-Y Axes
Setting the origin is how we communicate to the machine where (0,0,0)
is located. Without this step, the machine will not know where to begin
cutting. We will set the origin in Z seperately from in X & Y.
Steps for Setting the Origin in the Z-Axis:
1) Connect Z-Sensor. We store the sensor in the black toolbox that sits beside the machine. The
sensor sends a signal to the machine when the cutting tool has touched its surface. Place the
sensor in the bed and feed the cable through the black flap-port in the rear left of the machine.
Pull the cable up gently and plug it into the port called ‘Z0 Sensor’ (pictured above left)
2) Place the sensor on top of your material (pictured above center).
3) Position Mill. Ensuring that the cutting tool is above the tallest part of your material before
moving it, use the red and green X-Y controls in VPanel to position the bit directly above the
center of the detector, or place the detector beneath the center of the bit.
4) Detect. Move the tool down until it is about .25” or 7 mm above the sensor, and then, in
VPanel, select the blue bullet for “Set Z origin using sensor” and then press the button for
“Detect”. VPanel will ask you to confirm that the sensor is in place. Once you press “OK” , the
machine will being to slowly move down in the Z direction until the tool tip touches the sensor.
Your Z-zero point will be set at the bottom of the sensor, which should be at the top of your
material. If you do not place the sensor beneath the tool, the MDX 40-A will lower the tool until it
hits something and meets resistance, possibly damaging the tool or the material. After touching
it will retract.
5) Unplug the sensor from the rear of the machine, remove it from the bed and place it back in
the case.
Steps for Setting the Origin in the X-Y Axes:
1) Measure to the center of the material with a ruler, make a mark and place your material so
that it s parallel to the edges of the bed (pictured above right).
2) Navigate using the red and green x-y arrows in VPanel to the center of your material, lower
the bit so that it is within 1/4” of the top of your stock and you can easily see that it is centered,
the tool center should be above the point you have drawn.
3) Confirm. Under ‘Set’ in Set origin Point click XY origin, and press “Set” when you have the
tool centered on your material / point (picture above right).

5- SRP Player - Peform Cutting
We are now ready to begin the milling process. Ensure that the MDX lid
is closed and that the workspace inside is clear of any tools or debris.
Steps:
1) Press Start Cutting in SRP Player.
2) Confirm Tool the first tool you use will almost always be a 1/4” Flat or 1/4” Round for
roughing. If you do not see the tool you intend to use first here, press cancel and return to step
3.6 where we selected the bit. Confirm each of your toolpaths use the tool you intend and that
the desired tool is actually installed in the machine.
3) Set Surface here you should select the top surface of the material, because we placed the
z-sensor on the top of our material when we zeroed the Z-axis. It is also ok to set the z-sensor
on the orange bed of the MDX, however you must then also check the bottom surface here to
be consistent (otherwise the cutting tool will plunge into the table and cause damage to the
tool, material and the machine).
4) Proceed with mill. Place your hand over the stop button and watch for problems.
5) Await instructions for changing tools. Refer to step 4.2 if necessary, but be certain that you
are leaving enough of the bit out of the collet for your job.
Note: If the computer shuts off, you will lose the progress on your job.
Type of toolpath Roughing
Size of Bit 1/4”
MAX .4”
.18”
.05” .05” .05”
3000 mm/min
(120 in/min)
8000 rpm
3000 mm/min
8000 rpm
3000 mm/min
8000 rpm
1/4”
.1”
.125” to .05”
1/8”
.0625”
.0625” to .01”
Finish Finish
Spindle Speed
Feed Rate
Cutting-in Amount
Path Interval
Finish Margin
Appendix 1: Foam Cutting Parameters
Appendix 2: Field Definitions
(120 in/min) (120 in/min)

Appendix 1: Posting from Mastercam: The Roland Template
Mastercam provides more precise control over your milling job,
however the process is not fully automated. The first step is to prepare
toolpaths in mastercam for output to code that the Roland MDX 40-A
can interpret.
Steps:
1) Open the template Mastercam 7 file for the Roland MDX 40-A.
2) Ensure that the machine definition and posting protocol for the Roland MDX 40A have been
loaded into the file. (Right-click ‘Files’ under the Properties tab of the Operation Manager and
ensure C:\Users\Public\Documents\shared mcamx7\CNC_MACHINES\ROLAND MDX40 3
AXIS MILL INCH-1 is selected)
3) Import geometry into the model (File > “File Merge/Pattern” > Browse to your geometry).
Your Geometry should be located in positive Z, positive X and positive Y. When in Rhino’s TOP
View, with Y positive facing UP and X positive facing RIGHT, locate the lower left hand coorner
of the bounding box representing your material at the origin, with its lower face at 0 in the
Z-direction. See image on next page.
4) Apply toolpaths to your geometry. Detailed tutorials for this process are available on the
CNC tools main page, linked from http://www.gsd.harvard.edu/#/gsd-resources/fabrication-
laboratory/
5) Post the NC Code, one fil
2 3
3

Now that we have prepared toolpaths, it is necessary to post them
to G-code, which contains information about spindle speed, and
movement. The the Roland MX40-A cannot automatically change tools,
so it is necessary to post the toolpaths one at a time.
Steps:
1) Select the first toolpath. TA green check will appear after you have single-clicked on the
name of the toolpath. Note the lack of a green check box on the other toolpaths (indicated with
dotted lines).
2) Click on the icon for ‘G1’, which is for posting the toolpaths to NC-Code. You will receive a
warning indicating that you have not selected all the toolpaths. This is normal, click No.
3) Repeat this step for all toolpaths in your file. Name the toolpaths with numbers indicating the
sequence in which they will be milled, and the size of the bit. For example: “Path1_quarter inch”
12
Exporting Toolpaths from Mastercam
With the NC files in hand, its now time to mill. Here we will walk through
the process of starting the machine, and fastening your material to the
bed.
Steps:
1) Turn on the computer. Sometimes the computer will have trouble booting if the Roland
MDX 40-A is connected, simply unplug the USB at the base of the machine for startup, and plug
it in again once you see the Windows Desktop.
2) Turn on the Roland MDX 40-A. First ensure that there is no material in the bed because the
startup routine of the machine can cause a collision. Press the green Power Button on the Front
of the machine.
3) Install the tool for the first toolpath. Each tool change will need to be done mannually.
Install the tool that your first toolpath uses, ensuring that the length of the tool protruding from
the collet is in line with the assumptions you made in Mastercam when programming the
toolpaths.
Milling on the MDX 40-A
IMage of USB Image of Power Button

With your material fastened, its now necessary to instruct the Roland
where 0,0,0 is relative to your part.
1) Set the Z Origin. , First, set the origin in Z, by moving the spindle away from your part, and
lowering it to touch the bed. Use fast moves until you about 1/2” above the orange bed, then
use slow moves until you are about 1/8” above the bed. Place a slip of paper on the bed and
slide it back and forth as you incrementally lower the tool the rest of the way down to the bed,
stop as soon as the tool touches the paper. With the tool in this position, select “Set Z Origin’ in
VPanel.
2) Set the X-Y Origin. Lift the spindle in the Z direction, and reposition it above your material, on
the left hand corner closest to the door to the machine. With the tool in this position, select ‘Set
X-Y origin’ in VPanel.
Setting the Origin
Image of setting
Z in machine
Image of setting
Z in soware
Image setting
X-Y
Image for Send-
ing NC code
Set the Ma-
chine in NC
code mode
Image setting
X-Y in soware
With the origin set, all that remains is to send the tool paths one at a
time, and chang the tool when necessary.
Steps:
1) Select ‘Run’ From inside the Vpanel Window,
2) Load the first one of your toolpaths.
3) Press ‘Cut’.
4) Keep watching the part through the glass, being prepared to stop the milling if anything
unexpected happens.
5) When the toolpath completes, refer to 4.2 for changing the tool, and repeat the above steps
for each toolpath.
Running the Mill

Please clean up the workspace after yourself by completing the
following tasks.
1) Vacuum the bed. Do not use an airhose, as this may lodge debris in areas of the Roland
MDX 40-A that will prevent it from operating properly.
2) Remove double-stick tape from the bed
3) Return all tools to their plastic sleeves and place them in the toolbox
4) Place the toolbox on top of the Roland MDX 40-A.
5) Shut down the computer.
Cleaning Up
Image Vacuum-
ing Chips
Image of setting
Z in soware
Image setting
X-Y
Image setting
X-Y in soware

18234567
Each toolpath you create will have seven sets of settings you can use
to tailor the cutting. Repeat these steps for each toolpath you intend to
use.
Steps:
1) Here you can assign names to your toolpath, which may make organizing complex files
easier. Note, you only need to run one roughing pass before beginning final passes. If you
would like to create multiple finish passes, duplicate one of the finishing passes and adjust the
settings for each.
2) Here you orient the tool relative to your part. Select Top + Z unless you want to cut into your
piece at an oblique angle, and please consult with a TA if you would like to cut obliquely.
3) This is where you control the margins of scrap material SRC will leave around your part. If
you intend to do a flip-mill (i.e. mill on both sides) this must remain at least .5”, but if you intend
to mill just a single side it can be reduced to zero.
4) If you would only like to cut part of your material, here is where you define those bounds.
This can be used for creating multiple finish passes with different surface qualities, or for milling
only part of your stock material.
5) Here you can specify a maximum depth for your mill file. This is useful if you would like to
specify different surface finishes for varying depths of your topography.
6) Specify the bit size. Currently, the Roland is equipped with a .25” flat cutter, a .25” ball cutter, a
.125” flat and .125” ball. Note, you will need to manually change the bit and re-zero the machine
for each tool change.
7) Leave this setting on up-cut.
8) This is where you can control how fast the machine cuts and how aggressively it removes
material. Refer to the chart in the Appendix:Foam Cutting Parameters for filling in these settings.
COTNENTS:
Types of Milling Jobs:
Topography
Flip-Mill
Mold-making
2D Contours
Robot Arm
Gund’s Machines:
Roland
AXYZ
ONSRUD
6-Axis Robot Arm
5-Axis Robot Arm
Guide to Tooling:
By Toolpath
By Desired Articulation of Form
Starter Guide to Mastercam
Creating Geometry in Rhinoceros
Material Preparation
Importing Geometry
Articulating Toolpaths
Simulating operations
Submitting the Job
Trouble-shooting strategies
Running the job
- Machines
- Anchoring
- Dust Collection
- Timing + expectations from student
-

TOPOGRAPHY MODELS:
- Size & Time considerations + planning the job
- When to talk to a TA, expected scheduling
- Maximum Dimension: 4’ x 8’ x 6” tall
- Small: 6” x 12” x 2” (or whatever the Roland is)
- Large: more than 6” x 12” x 2” up to a maximum of 4’ x 8’ x 6”
- Material choice + considerations
- Wood
- Plywood
- Single piece of solid hardwood
- Laminated solid wood
- Foam
- Blue Foam
- White foam
- High Density Foam
- Anchoring strategies
- Desired Geometry + Appropriate Milling Strategies
- General overview of advantages to milling + limits of milling
- Tooling considerations with regard to desired geometry
- Buildings:
- Pockets for inserting buildings
- Solid Buildings integrated into topography
- Overall strategy
- Height limitations + relationship with the bit
- Distance between buildings
- Pocket Strategy
- Rough Parallel Strategy
- Sloped topography
- Smooth continuous surfaces
- Stepped topography
- Surface Articulation
- Recessed roads
- Up-cutting + downcutting
- Contours and marking lines or points on the surface
- Holes for trees/inserting pins
- Peck Drilling
- Size + time considerations
-
FLIP MILL
- Maximum size: 4’ x 8’ x 6” tall for your entire end piece
- BUT, must be supported throughout
- Anchoring Strategy
- Registration Holes
- Multiple World Axes in Master Cam
- Tabs
- Thickness of resulting Geometry
- Tolerances
- Vibration + part stability
- Part removal

2D CUTOUTS IN SHEET MATERIAL
- (maximum 4 ‘ x 8’ x 1.5” tall)
- Tabs
- Size + Depth limitations
- Types of cutting bits
- Up-cutting
- Down-cutting
- Material Specific
- Engraving Bits
-
MOLD FOR CASTING
- Size & time considerations + planning the job
- When to talk to a TA, expected scheduling
- Mill the positive, or the negative?
- Maximum Dimension: 4’ x 8’ x 6” tall for each half of the mold)
- Small: 6” x 12” x 2” (or whatever the Roland is)
- Large: more than 6” x 12” x 2” up to a maximum of 4’ x 8’ x 6”
- Material choice + considerations
- Wood
- Plywood
- Single piece of solid hardwood
- Laminated solid wood
- Foam
- Blue Foam
- White foam
- High Density Foam
- Wax, plastic or other mold making material
- Anchoring strategies
Desired Geometry + Appropriate Milling Strategies
- General overview of advantages to milling + limits of milling
- Tooling considerations with regard to desired geometry
- Female Molds - Surface milling
- Male Molds - Flip Milling (see next section)
- Registration Holes
- Grooves
- Size + Depth limitations
- Ramping
- Speed Considerations
- Surface Geometry
- Steep slopes
- Deep holes
- Surface Patterning
- Flowline
- Constant Scallop
- Parallel
- Radial
-
-

Robotic Arm / 6-Axis Jobs
- When to consider the Robot
- Tolerances, Precision + expectations in planning the job
- Assembling readymade pieces
- Fiber-winding
- Circular Saw
-
- Size & time considerations + planning the job
- Material choice + considerations
- Anchoring strategies
Desired Geometry + Appropriate Milling Strategies
- Grasshopper + HAL -
-
GUIDE TO TOOL PATHS
BY TOOLPATH - Don’t know what that toolpath does? Look here.
BY DESIRED GEOMETRY - Want to articulate a form, but don’t know how? Look here.
SURFACES
GROOVES
POCKETS
HOLES
ABB 6 - Axis Small Robot
6 Axis
ABB 6- Axis Big Robot
6 Axis