This document provides instructions for using MasterCAM version Mill9.1 to generate G-code files for routing various materials like wood, plastics, and foam using an AXYZ4008 router. It outlines the steps to import an IGES file, set up toolpaths including roughing and finishing cuts, set toolpath parameters, verify toolpaths for collisions and gouges, post process to create NC files, and upload files to the router computer. The overall goal is to enable generating NC files from 3D models to machine parts on the AXYZ router.

1. MasterCAM version Mill9.1
Tutorial chapters:
1. Importing IGES file into MasterCAM
2. Tool path setup
a. Setting job parameters: stock boundaries,
creating a bounding box, selecting the stock
origin.
3. Surface toolpaths:
a. Rough cut
b. Finish cut
4. Setting toolpath parameters
a. Creating a new tool
5. Preparing for machining; post processing
a. Checking toolpaths for collisions and gouges
6. NC file upload
7. Router Functions
Routing is an effective method for machining materials such as
wood (or wood byproducts), plastics, and rigid or high-density
foam. The tutorial chapters will enable you to generate g-code
.NC files from an imported 3-D model to be machined by the
AXYZ4008 router at the GSD.
1. Importing IGES file into MasterCAM
Surface and solid models can be imported into MasterCAM from
environments that create watertight models. The Rhinoceros
platform is successful for exporting watertight .igs or .iges models.
(Note: FormZ is not suited to producing these models.)
Exporting your model from Rhinoceros
1. Prior to exporting your surfaces the entire Rhino model
needs to be located in the Cartesian positive X- and Y-axes
and the negative Z axis.
2. In Rhinoceros select File / Export Selected (follow the
Command prompt instructions and select the appropriate
surfaces.) An Export dialogue box will appear: create file
name and save as an IGES *.igs, *.iges.

2. 3. An IGES Export Options dialogue box will appear: scroll
through the IGES types, select Mastercam and select OK.
Importing your IGES file into MasterCAM
1. Open the MasterCAM Mill9.1 icon.
2. Using the prompts at the top left of the screen select: File /
Converters / IGES / Read File.
3. Browse to find your file and open it.
4. A dialogue bow will appear, accept defaults and click OK.
An addition dialogue box will appear, asking, “Delete the
Current Part?” Click Yes. Your model should now appear.
5. Press F9 to toggle on/off the X, Y, Z-axes. The MasterCAM
location of your model will correspond to the Rhinoceros
exported position. To view your model obliquely, Right-
click for “dynamic spin” options.
Verify Surface Viability
1. Any initial machining problems can be identified by the
following sequence.
2. First, testing the normals: select Main Menu / Analyze /
Surfaces / Test Norms / All / Surfaces / Done. A pop-up
window will then appear informing you of your model’s
integrity. If you have reversed normals, follow the
onscreen prompts to adjust the surfaces of rebuild your
model and re-import.

3. 3. Second, testing the model for sharp internal corners that
may not be machinable: select Main Menu / Analyze
/ Surfaces / Check Model / All / Surfaces / Done. A
tolerance will be shown at the bottom left of the screen,
select Enter to accept
4. A pop-up window will appear with diagnostics of your
model. Click OK. If you had internal sharp corners,
MasterCAM will ask you if you wish to draw the internal
sharp curves. We recommend that you say no and either
proceed knowing that the machine may not be able to
reproduce your model as precisely as you have drawn it
or to redraw your model in the original modeling program
avoiding sharp internal corners and re-import. Take note
of the location of the curves that MasterCAM indicates
contain sharp internal corners before proceeding. And also
understand that you may be able to set parameters that
will minimize the differential between what is modeled
and what the machine is capable of cutting. See below for
details
2. Tool path setup
Setting Job Parameters: stock boundaries
The stock boundaries help you visualize the part you are
machining during the toolpath verification.
1. Choose: Main Menu / Toolpaths / Job setup
2. Choose: Select corners
3. Select one corner of the stock using the Point Entry
system and then select the opposite corner. The system
automatically fills in the X, Y, and Z fields based on the
geometry you selected.
4. Choose OK if you accept.
Note: you can only set up rectangular stock
Setting Job Parameters: creating a bounding box
A bounding box defines the stock limits by finding the extents of
the selected geometry.
1. Choose: Main Menu / Toolpaths / Job setup
2. Choose: Bounding box
3. Select the entities around which the bounding box is
defined.
4. Choose: Done

4. Setting Job Parameters: selecting the stock origin
The stock origin adjusts the position of the stock. You can set the
stock origin to any corner of your model.
1. Choose: Main Menu / Toolpaths / Job setup
2. Choose: Select origin
3. Select a point in the graphics window. The system returns
to the Job Setup dialog box and fills in the stock origin X,
Y, and Z-coordinate based on the point you selected.
4. Click OK and leave the remaining defaults as they are set.
3. Surface Tool paths
Rough Cut
Rough toolpaths remove large amounts of material from surfaces
as rapidly as possible. A rough cut is not required for milling
foam. A rough cut is required when removing wood. Note: be
sure to leave 1/16” of material for your finish cut.
1. Choose: Main Menu / Toolpaths / Surface /
2. Ensure that the Surface settings shown at the top left of the
interface are as follows:
a. Drive: S
b. CAD file: N
c. Check: N
d. Contain: N
3. click / Rough
4. Select the “surface roughing.” Choose from a number of
preset paths that the tool will take (i.e., parallel, radial,
flowline, contour, etc.) These are all options for the
direction or manner in which the tool will make its cuts
over the surface of the object. To learn more about the
differences at this point, click on the help button.
5. If you choose parallel cut you will be prompted to tell
MasterCam whether you are cutting a boss or a cavity. Do
so accordingly (Boss is a positive, cavity is a negative. If
you have both or a complex form, choose unspecified)
6. You will now be prompted to select the surfaces for
machining. Select all surfaces feature by clicking All and
then Surfaces. Do not worry if this automatically selects
an underside. You will verify that the machining is only
cutting the desired surfaces in the next steps. Click Done.
7. If you wish to select only specific surfaces rather than
clicking All as described above, use the pointer and click
on each desired surface. When finished selecting, click
Done. You may use the unselect button at the top left if you
accidentally choose a surface you didn’t intend to.
8. Again, once your surfaces have been selected, click Done.

5. 9. A Toolpath Parameters Dialog Box will open. Follow the
directions in Chapter 4: Setting Toolpath Parameters to
set the parameters of your rough-cut, prior to setting the
Finish Cut parameters.
Finish Cut
Surface finish toolpaths are used to create precise surfaces after
roughing.
1. Choose: Main Menu / Toolpaths / Surface /
2. Ensure that the Surface settings shown at the top left of the
interface are as follows:
a. Drive: S
b. CAD file: N
c. Check: N
d. Contain: N
3. click / Finish
4. Select the Surface Finishing. This is the manner in which
the tool will make its cuts over the surface of the object. To
learn more about the differences at this point, click on the
help button.
5. You will now be prompted to select the surfaces for
machining. Select all surfaces feature by clicking All and
then Surfaces. Do not worry if this automatically selects
an underside. You will verify that the machining is only
cutting the desired surfaces in the next steps. Click Done.
6. If you wish to select only specific surfaces, rather than
clicking All as described above use the pointer and click on
each desired surface. When finished selecting, click Done.
You may use the unselect button at the top left.
7. Again, once your surfaces have been selected, click Done
4. Setting toolpath parameters
Creating a new tool
1. After the defaults are set, a dialogue box will appear.
2. Under the “Tool Parameter” tab, in the Parameters dialog
box, right-click in the tool list area and choose Create new
tool.

6. 3. Enter your bit parameters in the Define Tool dialog box.
4. Choose OK.
5. Set the following parameters for your tool:
a. Feed Rate: 25 (for wood), 200 (FOR FOAM
ONLY!!!)
b. Plunge Rate: 10 (for wood), 200 (FOR FOAM
ONLY!!!)
c. Retract Rates: 200
d. Coolant: off
e. Accept all other defaults
6. Click on the Surface Parameters Tab and adjust the
following parameters according to the specifics of your
project.
(NOTE: BE SURE ALL MEASUREMENTS ARE SET TO
INCREMENTAL)
a. Clearance: This is how high the tip of the bit will
be raised off of the top of the material block when
the arm travels during initial and final non-cutting
movements. It will be important to forecast the
height of any bracing or clamps used to hold down
your material on the router bed when calculating
this figure. THE TIP OF THE ROUTER MUST BE
HIGH ENOUGH SO THAT IT WON’T HIT ANY
OF THEM.

7. b. Retract: This is the height the tip of the bit will be
raised off of the top of the material block in between
cutting movements.
c. Feed Plane: This is distance off of the machined
material to which the feed rate will continue and
after which the Plunge Rate will begin. In other
words, the tool will move very quickly when it is
above this height, and will move at the feed rate
when it is below this height.
d. Tip comp: This is the point on the bit from which
the cutting measurements are drawn. You do not
want to use center comp.
(NOTE: BE SURE ALL MEASUREMENTS ARE SET TO
INCREMENTAL)
7. Click on the Finish Parallel Parameters Tab to adjust
tolerance, max stepover, cutting method, and machining
angle.
a. The Tolerence will help determine how accurate the
bit interpolates your surface curvature. The smaller
the number, the more accurate and longer the cut-
time. Most jobs will be fine accepting the default of
0.001
b. The Max Stepover determines the distance the bit
will move over for the next parallel cut. This will
affect the “smoothness” of your final surface Here
a larger number will result in more “stepping”
(if using a flat-end bit) or “scalloping” (if using a
rounded bit). Consider the width of your bit and
some fraction of that width as a Max Stepover.
c. Cutting Method: select “zig-zag” to allow the
machine to cut while traversing both positive and
negative directions or “one-way” to restrict cutting
to a single direction. The most efficient is “zig-zag.”
d. Machining Angle: this will allow you to dictate
which angle the parallel lines are cut.
8. Select OK and the lines of your toolpath will appear along
the surface of your object/model along with an Operations
Manager Dialog Box. Fron this dialog box you will be able
to complete the final steps to Verify and Post your file.
CHAPTER 5. Preparing for machining; post processing
A post processor is a program that converts a toolpath, which
contains all information necessary to machine a part, into an NC
program, which is the code, required by a particular machine and
control combination to machine the part.

8. Checking toolpaths for collisions and gouges
By checking your toolpaths for collisions and gouges, you can
prevent future problems while machining a part. Collisions and
gouges can cause damage to a part, tool, CNC machine, and
the machine operator. A collision occurs when the tool contacts
material during a rapid move. A gouge occurs when the tool
removes more material than desired, usually during a linear or arc
move. The system compares a surface toolpath to an STL file that
represents the finished shape of the part to see where gouges have
occurred.
You can check more than one toolpath for gouges and collisions
at the same time if the toolpaths are all in the same tool plane.
You can also set the color and level of the geometry that marks
collisions and gouges. This function works with flat, bull, or ball
endmills.
(NOTE: TOOL HOLDER COLLISIONS AND GOUGES ARE
NOT REPORTED)
Verifying Toolpaths
The model created by Verify represents the surface finish, and
shows collisions, if any exist the simulation will pause to identify
the location, so that any program errors can be eliminated before
they are sent to the router.
1. Verify your toolpath:
a. If the Operations Manager Dialog Box is open,
select Verify
b. Or, select: Main Menu / NC utils / Verify
2. To preview multiple toolpaths highlight the name in the
post box by holding the Ctrl and LMC.
3. To run the verify, click the play button.
4. If you are unsatisfied for any reason, return to the
Operations Manager and click on the Parameters line
to return to the tool parameters dialogue box. Make any
necessary adjustments and say OK.
5. IMPORTANT: If you have altered the parameters, you must
return to the Operations Manager and click Regen. This
will regenerate the tool path. Then repeat the steps outlined
above to re-verify the new tool path. Repeat these steps
until you are satisfied with the tool path demonstrated in the
verify.
6. If you are satisfied with the verify, close the verify bar
by clicking on the X at the top right. This will reopen
the Operations Manager. From within the Operations
Manager, highlight the tool path in the window on the left
and click on the Post button on the right.
7. This will open the Post Processing dialogue box. You

9. should use the AXYZ postprocessor (axyz_Harvard.pst). If
it is not shown in the dialogue box, choose change post and
choose it from the list (it will be the first one on the list).
Click on save NCI, as well as save NC. You do not need
to click the edit box. When prompted, save the file to your
desired location.
8. Saving the file will cause your G-Code to be written.
9. You now have a rough cut tool path ready for the uploading
to the mill/router.
6. NC file upload
Log on to the computer in L40d and transfer your file onto the
desktop.
7. Router Functions
In L40d a laminated sheet titled AXYZ CNC Router Table
– Instructions for Milling your Part is located with the bits. The
sheet walks the operator through the simple Functions in machine
operation.