A Basic Introduction to Mastercam
CAD/CAM Software
By
Kyle Bowker
� 2001
This material is based upon work supported by the National Science Foundation under Grant No. DMII-9624966.
Any opinions, findings, and conclusions or recommendations expressed in this material are those of the author and
do not necessarily reflect the views of the National Science Foundation.
Table of Contents
Introduction & & & & & & & & & & & & & & & & & .. ii
Overview of the CAD/CAM/CNC Process & & & .& & . iii
Safety Instructions & & & & & & & & & & & & & & & iv
Starting Mastercam & & & & & & & & & & & & & & ... 1
Interface Overview & & & & & & & & & & & & & & ... 1
Drafting Utilities & & & & & & & & & & & & & & & ... 2
Importing an AutoCAD File & & & & & & & & & & & . 4
Surface Attributes & & & & & & & & & & & & & & & . 6
Generating Toolpaths & & & & & & & & & & & & & & 7
Simulating Toolpaths & & & & & & & & & & & & & & 16
Post Processing & & & & & & & & & & & & & & & & . 18
Preparing the Workpiece & & & & & & & & & & & & .. 20
Load the NC Program & & & & & & & & & & & & & ... 22
Machine Tool Setup & & & & & & & & & & & & & & .. 22
Run the NC Program & & & & & & & & & & & & & & . 23
Appendix & & & & & & & & & & & & & & & & & & ... 24
i
Introduction
The objective of this tutorial is to provide undergraduate level students in engineering and
manufacturing with an introduction to Mastercam. The tutorial provides students with an
overview of the part design and manufacture process, enabling students to gain hands on
experience with real machine tools. Additionally, students gain invaluable exposure to one of
the most popular and user-friendly industry level CAD/CAM software packages available.
Students will learn the basic procedures needed to create a part on a three-axis milling machine
using a numerical control (NC) program generated with Mastercam. Beginning with a blank
screen students will learn how to use the software s built in drafting utilities and how to import
CAD files from other popular software packages such as AutoCAD�. Next the tutorial explains
how to associate tool paths with various part geometry and adjust program parameters such as
tool clearance positions and feed rates. To complete the program students will learn how to
verify the tool path and translate the data into a machine specific format with a post processor.
Finally, the tutorial demonstrates how to load the NC program file into a milling machine s
controller and execute the program.
While much of the information presented in the tutorial can be applied in a general sense it is
specifically geared towards students enrolled in MAE 192:  Manufacturing Processes and
Systems at The George Washington University. The Manufacturing Laboratory located in
Tompkins Hall Room 206 is equipped with PCs running Mastercam Version 8.1 software and
Light Machines Corp. TMC-1000"! three-axis tabletop milling machines. The NC program
created in the tutorial is designed to run on these machines, although it can be modified to work
on other CNC milling machines.
ii
The CAD/CAM/CNC Process
CAD
1. Generate a dimensioned drawing
" AutoCAD using AutoCAD.
" I-DEAS
" Cadkey 2. Draw the part geometry for each tool
" VersaCAD path on different drawing layers for
" Others organizational control.
Produce a dimensioned drawing. 3. Save the drawing in .DWG format.
Save the drawing in .DWG format.
DWG file from
CAD to CAM
CAM
4. Run the Mastercam software and
open the .DWG file you just created
" Mastercam
with the built-in file converter.
" spectraCAM
" Others
5. Generate all the tool paths from the
part geometry.
Enter the cutting parameters.
Generate the tool path.
6. Verify the tool path and save as a
Verify the tool path.
NC program.
Save the NC program.
NC program file
from CAM to CNC
CNC
7. Run the Mill Control Program and
" TMC-1000 Control Program
open the NC file you just created.
" spectraLIGHT Control Program
" SW Industries Control Program
8. Setup the tool length offsets and stock
origin location.
Setup tools and origin.
9. Dry run the program to check for
Dry run the NC program.
program errors or incorrect setup.
Machine the part on the mill.
10. Run the program and machine the
part.
iii
Safety Instructions
Safety first! Please read and understand the following safety rules before operating the TMC-
1000 Mill:
1. Always use eye protection
Foresight is better than no sight. During operation any power tool can throw foreign objects
and harmful chemicals into your eyes. Keep the safety shield in place whenever the spindle
or cross slide is moving. Although there is a safety switch that stops all operations when
triggered, it is still possible to operate the spindle or move the machine tool with the safety
shield out of position.
2. Wear proper apparel
Avoid loose clothing that can get caught in moving parts. Tie back long hair or wear a hat.
Wear closed toe shoes (no sandals). Remove all jewelry including necklaces, earrings,
bracelets, rings and wristwatches.
3. Keep the work area clean
Cluttered work areas and bench tops invite accidents. Remove all chips after each operation.
4. Remove the adjusting keys and wrenches
Make it a habit to check that adjusting keys and wrenches are removed from the mill before
turning on the machine.
5. Secure the workpiece
Be certain that you have firmly secured the vise to the table and that the workpiece is held
tightly in the vise without damaging it.
6. Secure the cutting tool
Make sure that the set screw that holds the cutter inside the adapter is secure. Check that
tapered shank on the adapter and the inside surfaces of the tool holder are free of debris.
Make sure the cutting tool is firmly secured inside the tool holder. When using the quick tool
change unit you should see the release button pop out and hear an audible  click when the
collar rotates to its locked position.
7. Do not force a tool
Select the feed rate and depth of cut best suited to the design, construction, and purpose of the
cutting tool. It is always better to take too light a cut than too heavy.
8. Turn the spindle by hand before starting
Manually turning the spindle allows the operator to safely determine that the tool is firmly
secured and will not bind or hit the cross slide, fixtures, or workpiece on the start up.
iv
9. Do not cut metal
Use the TMC-1000 only to machine the blue machineable wax stock provided to you. Do not
attempt to machine any other material.
10. Use the EMERGENCY STOP for added safety when changing tools or fixtures
The main emergency stop has an oversize red cap and is located on the front of the mill next
to the spindle speed control knob. Push in the switch to power off. The machine can still be
operated with safety shield out of position so make sure the emergency button is pressed in
whenever changing tools or fixtures. Whenever executing a program for the first time keep
one hand on the emergency stop at all times. This will allow you stop the machine in case
there is a collision with the tool and the fixture or cross slide.
11. Pay attention
Always pay attention to the task at hand. The TMC-1000 is a power tool and is capable of
doing very serious harm very quickly. You are responsible for your safety as well as for
those around you. If you notice someone doing something unsafe notify that person
immediately to correct the problem. If you have a question or uncertainty about any
procedure please ask first. It will save time and prevent possible injury.
v
Starting Mastercam
" Begin by clicking the icon from the Windows desktop.
" Once the software has initialized and verified that the HASP security device is activated a
blank workspace will be displayed.
Note: The HASP security device is commonly known as a dongle. According to MARX
Software Security (http://www.dongles.com), a dongle is  a hardware-based security device that
attaches to the serial or parallel printer port of a desktop computer. It is a hardware key that uses
codes and passwords embedded inside the key to control access to software applications. A
software program integrated with a dongle will only run when that dongle is attached to the
computer.
Interface Overview
Shown below is the Mastercam working environment, which consists of a graphics window and
menu selections. The graphics window is the area where you create part geometry and generate
toolpaths. The menu selections are located along the left hand side of the screen with the Main
Menu on top and secondary menu items on the bottom. Using the mouse to click on an item will
display a sub-menu or pop-up window with more choices. You may proceed to more menu
options by clicking on Next menu or you may return to the previous or main menu by clicking
the BACKUP or MAIN MENU button.
Menu items can also be selected using the keyboard. The name of each menu item has an
underlined letter. To select the item simply hold the Shift key and press the corresponding letter
on the keyboard. A toolbar, which is displayed across the top of the screen, provides shortcut
buttons to perform many common functions.
In a typical sequence you might navigate through the menu structure to a command, choose an
entity according to the prompts, make parameter choices, and then execute that command. An
Undo function is provided to correct mistakes. (Mastercam Help)
" Take a moment to familiarize yourself with the menu and toolbar items.
1
Drafting Utilities
Mastercam is capable of creating 2D and 3D geometry. Parts may be displayed as wire frames
or as solid objects. The Create Menu gives you options for drafting typical items such as lines,
arcs, and dimensions in addition to more specialized features such as gears. You can access the
Create Menu by choosing Create from the Main Menu. Selecting Solids from the Main Menu
allows you to create solid objects. They may be formed by adding or subtracting basic shapes
such as blocks and cylinders or by extruding, revolving, and sweeping geometric chains.
Let s practice these features by drawing the material stock from which we will cut our desired
part.
" Go to the Create Menu and click on Rectangle, 2 points.
" Mastercam will prompt you to enter the coordinates of the lower left corner. Position the
mouse over the origin in the graphics window and click to select it or choose the Origin
command from the sub-menu.
" Next you will be prompted to enter the coordinates of the upper right corner. Position the
mouse and click to select Width = 5.0000; Height = 2.5000.
" To create a 3D model of our material stock we must extrude our rectangle in the Z direction.
Go to the Solids Menu and click on Extrude, Chain.
Note: According the Mastercam Help File,  chaining is the process of selecting and linking
pieces of geometry so that they form the foundation of a toolpath, surface, or solid. When you
chain geometry, you select one or more sets of curves (lines, arcs, and splines) or points which
have adjoining endpoints. It differs from other selection methods because it associates order and
direction to the selected curves. This order and direction affects the way Mastercam generates
surfaces, solids, and toolpaths.
" Use the mouse to select the rectangle. Clicking on one side of the rectangle will select the
entire object. After the rectangle has been selected the line color will change from green to
white and an arrow will indicate the start position of the chain and its direction. Now click
Done. Click Done again at the next menu and a window will pop-up.
2
" Extend the rectangle by a distance of 1.25 and click OK.
" Change the view by clicking on the Isometric View icon from the toolbar.
" You will see that our rectangle is now a 5 x 2.5 x 1.25 block.
Alternatively, we could have created our stock geometry using basic solid building blocks.
" First create a blank workspace. Choosing the Delete icon from the toolbar allows you
to select the geometry you wish to remove.
" The same results can be accomplished by selecting File, New from the Main Menu.
Mastercam will prompt you asking if you are sure you want to initialize geometry and
operations. Choose Yes. Then you will be asked if you would like to save the MC8 file.
Choose No.
" From the Solids Menu choose Next menu, Primitives, Block.
" Use the Corners command and select the same lower left and upper right corners.
" Click on Height and enter 1.25 in the dialog box at the bottom of the screen.
" The dimensions of the block will be displayed as Block Height = 1.2500; Block Length =
5.0000; Block Width = 2.5000.
" The remaining features of our basic part can be constructed using the same techniques used
above.
3
Importing an AutoCAD File
The file converter option enables you to read from and write to a variety of file types such as
ASCII, IGES, DXF, and STL. This feature allows data to be easily transferred from devices
such as rapid prototyping machines or coordinate measuring machines and among CAD/CAM
software packages from various vendors such as AutoCAD and I-DEAS.
Students who have taken MAE004  Engineering Drawing and Computer Graphics may find it
preferable to create their part geometry using AutoCAD. This software is available in the NT
Engineering Design Lab located at Tompkins Hall 410 in the SEAS Computing Facility (see
http://www.seas.gwu.edu/~seascf/pc.html for more information). The Advanced AutoCAD
converter can convert AutoCAD 2000, R14, and R13 .DWG files into the Mastercam .MC8
format.
Differences in program architecture and the need for software companies to protect proprietary
information means that not all geometric entities transition smoothly from one file format to
another. This must be taken into consideration when importing or exporting different file
formats. For a list of supported entities see the Mastercam Help File by clicking the Help icon
from the toolbar and selecting conversion considerations.
Let s try an example to see how to import an AutoCAD file.
" Click on File, Converters, Adv ACAD from the Main Menu.
" To specify the file you wish to import into Mastercam click on Read File. A pop-up window
will allow you to browse for the file location. Select the file named  Basic Part.dwg
located in C:\My Documents\Mastercam Tutorial and click Open.
4
" Check the box labeled Override MC8 Name to automatically name the new Mastercam file
with the name of the DWG file. Click OK at the next pop-up window.
" You will be asked if you want to delete the current part. Click Yes. Mastercam will then
prompt you to save the .MC8 file you have chosen to delete. Click No.
" The display bar at the bottom of the screen will say  ****** Please wait  converting file
****. This may take up to one minute or more depending on the size and complexity of the
part file. Another window will pop-up displaying certain parameters.
" In the Scale field select No change and then click OK. This will ensure that the part
dimensions will remain the same when converted from AutoCAD to Mastercam.
5
" The display bar will say  Creating Solid. Please wait& . After the part has been displayed
in the graphics window a pop-up window will show exactly what has been converted into
Mastercam. After reviewing the information you may close this window.
" You will be prompted to erase the intermediate SAT files. SAT is a solid model format
developed by Spatial Technologies, Inc. During this process each solid in the AutoCAD file
is first written as a unique .SAT file and then converted to .MC8. When the conversion is
complete, you can delete the intermediate SAT files. Click Yes to delete.
" Now displayed in the graphics window is our part that we will create.
Surface Attributes
The part currently displayed in the graphics window appears as a collection of lines and arcs. To
help you visualize the 3D geometry while you work you may want to apply shading parameters
such as colors, materials, and lighting to surfaces on the solid model.
" To do this open the Shading Settings dialog box by selecting Screen, Surf disp, Shading
from the Main Menu.
" To enable shading check the box labeled Shading active.
" Click on All 1 color and select the color bar icon to choose your preferred shading
color. Number 9 is a color that closely resembles the blue machineable wax used to create
our part. Click OK to return to the graphics window.
6
Generating Toolpaths
A toolpath shows where a cutting tool will remove material from the part. Toolpaths can be
programmed to perform a variety of tasks from drilling holes and creating grooves for o-rings to
special text lettering and facing operations. Clicking on Toolpaths from the Main Menu
displays the various types of cutting operations available.
Let s begin by selecting the part origin and material stock dimensions from the Job Setup dialog
box.
" From the Main Menu select Xform, Translate, All, Entities, Done. Now click Rectang and
enter Z-1.25 in the dialog box at the bottom of the screen. A window will pop-up displaying
several options. Select Move and click OK.
Note: This shifts the entire part downward in the negative Z direction by 1.25 and is beneficial
for two reasons. First, it requires that all cuts be in the negative Z direction, which helps us
identify the depth of our part features and provides an instant check to determine if we are
making a cut or have cleared the material surface for traversing operations. Secondly, it assists
in machine tool setup. By setting the top surface of the part at zero in the Z direction we can
easily select the NC machine s reference zero and adjust the offset for multiple tools of varying
length.
7
" To specify the dimensions of the material stock click on Toolpaths, Job setup from the
Main Menu.
" Enter dimension values in their respective data fields as X = 5.0, Y = 2.5, and Z = 1.25.
" Next, choose the location of the stock origin. Click on the red + in the center of the stock
graphic, hold down the mouse button, and drag the + to the same corner as the part origin.
Checking the box labeled Display stock from the Job Setup window will allow you to verify
the correct stock position. Click OK when complete.
Now that our part is properly setup we may now add toolpaths to create the desired features.
" Let s begin by cutting the large rectangular shaped section in the center of the part. From the
Toolpaths Menu select Pocket.
Note: A new window will pop-up asking you to select the output file. According to the
Mastercam Help File,  an NCI file (*.NCI) represents information in a generic or intermediate
format and contains all of the parameter information necessary to create a toolpath. This
intermediate file simplifies post processing of MC8 toolpath operations into the various NC
formats required by milling machine and controls. An NCI file cannot be used to directly control
a machine.
8
" Click Save to save the NCI file in the default directory.
" Select Chain from the Pocket Menu.
Note: According to the Mastercam Help File,  most toolpaths require geometry to be chained.
Usually you chain the geometry that is used in a single operation, such as a contour toolpath or
pocket toolpath. Chaining also determines the direction of tool travel during machining.
However, you can also chain together separate sets of entities, such as multiple holes for a bolt
circle, to be cut in a single operation.
" Chain the geometry for our pocket by using the mouse to select the four individual lines that
comprise the large inner rectangle of our part.
" Clicking on the first side of our rectangle highlights the line and displays two arrowheads.
The green arrow shows the starting location of the chain and its direction. The red arrow
shows the end point of the chain. The Reverse command allows you to change the direction
of the chain (i.e. clockwise/counterclockwise). If you would like to remove a particular line
or arc from the chain you may use the Backup command.
9
" It is important when chaining to select adjoining geometric entities. Because direction is
matters the next line chosen must be adjacent to the red arrow. Once the chain is complete
the green arrow and the red arrow will have the same end point. Click End here, Done.
" A pop-up window will appear showing the various pocket parameters.
We must select the cutting tool to be used to create the pocket. For efficiency, we will choose a
tool that can effectively create all part features.
" Select the Tool parameters index tab then right click in the large white tool window and
choose Get tool from library& .
10
" Scroll down to Tool Number 239 , 1/2 FLAT ENDMILL and click OK.
Mastercam automatically calculates feed rates that tend to be on the high side, presumably to
reduce machining time and costs for production parts. Therefore, to ensure safety and tool
longevity we will adjust the feed rates by entering values manually.
11
" Change the Feed rate and Plunge rate values by entering 3.0 in their respective data fields.
This value corresponds to a rate of three inches per minute.
" Next, select the Pocketing parameters index tab.
" Check the box labeled Clearance and enter 2.0 as its value. Clearance is the height at which
the tool moves between two separate machining operations. It is necessary to specify this
position high enough to avoid accidentally cutting through your workpiece when traversing.
" Click on the button labeled Top of stock& and select a point that is located on the top
surface of the stock. This value should equal zero.
" Similarly, click on the button labeled Depth and select one of the bottom corners of the
pocket. Since we are making a cut into the material stock and we previously shifted our
entire part into the negative Z plane this value should equal  0.5.
" Clicking on the Roughing / Finishing parameters index tab allows you to adjust the type of
rough cut, the number of finishing passes to complete, and other properties. Leave these
values set to their defaults. However, check to make sure that the box labeled Keep tool
down is NOT selected. This option allows you to override the clearance function and can
cause serious part and machine tool damage if improperly used.
" Hit OK to return to the Toolpaths Menu.
12
You will now see the computer generate the toolpath associated with the pocket we created.
Once this has completed a window will pop-up displaying the Operations Manager. This
window lists all operations in the current MC8 file, including both associative and non-
associative toolpaths, and offers a quick and easy way to access part features to alter parameters,
change the machining order, etc.
Note: Any time you adjust toolpath parameters or geometry you must regenerate the toolpath to
make the changes effective. This can be done by clicking the Regen Path button on the right
hand side of the Operations Manager window.
" Click on OK to close the Operations Manager. The Operations Manager can later be
selected by clicking on Operations from the Toolpath Menu or by typing
Now let s create the stepped feature and the two through holes on the right side of our part. To
do this we must first individually define some part surfaces. Currently, Mastercam observes the
entire object as one continuous surface.
" From the Main Menu select Create, Surface, Next menu, From solid.
13
" Make sure that the Faces option is set to Y and the Solids option is set to N.
" Select the two faces highlighted below. After selecting the first face click Done. Next,
select the second face and click Done twice. The yellow and green highlights will later help
in indicating check and drive surfaces for our machining operation.
14
Note: We could choose to individually identify each surface on the part, however selecting only
these two highlighted faces will suffice for this operation.
" Return to the Toolpaths Menu and select Surface, Rough, Parallel, Unspecified.
" First, click on the surface that is highlighted green according to the image above. This is our
drive surface, or the surface we wish to cut.
" Second, click on the yellow surface. This is our check surface, or the surface we wish to
preserve. After both surfaces have been selected click Done.
" A pop-up window will appear showing the various surface parameters.
" Select the Tool parameters index tab and click the tool icon from the tool
window. This is the same tool used previously to create the pocket feature.
" Change the Feed rate and Plunge rate values by entering 3.0 in their respective data fields.
" Next, select the Pocketing parameters index tab
" Check the box labeled Clearance and enter 2.0 as its value.
" Click on the Roughing / Finishing parameters index tab.
" Change the Cutting method from One way to Zigzag.
" In the Max stepdown data field enter 0.4 as the value. This will allow us to remove all the
necessary material in a single pass.
" In the Machining angle data field enter 90 and click OK. This change causes the tool to
sweep in a direction parallel to our check surface and leaves behind a smooth finish.
" The Operations Manager window will now display our new surface feature in addition to the
pocket. Click on OK to close.
Now we can create our final two part features.
" From the Toolpaths Menus select Drill, Entities.
" Choose the two � diameter arcs located on the stepped surface and click Done twice.
" Select the Tool parameters index tab and click the tool icon from the tool
window.
" Change the Feed rate to 3.0.
" Go to the Simple drill  no peck index tab and set the Clearance to 2.0.
" For this operation specify the Top of stock& as the height of the stepped surface. This value
should equal -0.4.
15
" Change the Depth& by manually entering  0.9 in the data field. Because the two holes are
through-holes we want to make sure that the depth is set a little deeper than the actual depth
of the hole (-0.85). This ensures that the tool will cut completely through the material and
won t leave behind any rough edges.
Note: It is very important when making through-holes to avoid damage to the machine table.
This can be done by raising the workpiece above the machine table with parallels.
The Operations Manager now shows all three main features we want to create. We may now
graphically verify our toolpath.
Simulating Toolpaths
The Verify command uses solid models to simulate the material removal process. The stock
shape is updated as the tool moves along the toolpath and produces the final part. The resulting
model can be inspected, ensuring that programming errors are eliminated before they reach the
shop floor. (Help)
16
" From the Operations Manager click on Select All to choose all three machining operations
and then choose Verify. A blue checkmark will appear next to the name of each feature
selected.
" To begin the toolpath simulation click the play button on the Verify Toolbar.
17
" A model of the cutting tool will follow the toolpaths and expose cut surfaces as a contrasting
color. You may adjust the speed of the simulation using the
control. If the simulation has completed and there are no problems return to the Operations
Manager by clicking the close window button on the Verify Toolbar.
Post Processing
Now that we ve generated the necessary toolpaths to make our part we must use a program to
translate the NCI data to a format usable by a machine. A post processor converts the toolpath
information to a NC part program, which is also known as G code. This term refers to the word
address format used to identify different NC commands. Typically, each NC controller requires
its own specific post processor. In our case we are using a Light Machines Corporation TMC-
1000 Controller.
The post processor file for this machine is called MPMLIGHT.PST and is located in
C:\Mcam8\Mill\Posts. It has been chosen as the default although you may choose different post
processors for other NC machines. For example, the newest Clausing-Kondia mill in the
Tompkins Hall Machine Shop is equipped with a Dynapath, Inc. Systems 10 Controller. To run
a NC program on this machine simply run the post processor file name MPDYPTH.pst.
" Begin by clicking on Post from the Operations Manager.
18
" Check the box labeled Save NC file and click OK.
" Specify a number as the file name. Although many NC controllers will accept a text name
for a NC file, some controllers may only be able to interpret numeric data. Therefore, it is a
good habit to name all NC programs using numbers.
" Save the file onto a 3 � floppy disk located in drive A:. We will use this floppy disk to
transfer the program from the design PC to the NC controller.
Note: Although we are using a floppy disk to load the program onto the NC machine some
systems may support data transmission via an RS232 interface. Refer to your specific
machine s owner s manual for more information.
" The display bar at the bottom of the screen will say,  Processing the file with MPMLIGHT.
Once this task is complete the Operations Manager will be displayed. Click OK to close this
window and return to the Main Menu.
Now is a good time to save your completed .MC8 file. This will allow you to make later
changes in your NC program.
" Click on File, Save to save the Mastercam file.
You may now exit Mastercam by clicking the close window button or by going to File,
Next menu, Exit from the Main Menu.
19
Preparing the Workpiece
We are now ready to start cutting our part.
" Begin by turning both the NC machine and the controller  ON . The power switch for the
NC machine is located on the front of the TMC Controller Box. The PC based TMC-1000
Control Program runs on an IBM compatible Dell 486P/25. The control program should
load automatically when the PC is switched on. If the program fails to load, type cd TMC
to change directory and then enter TMC to execute from the DOS C:\ prompt.
" Using the mouse or the keyboard select M MANUAL CONTROL from the Main Menu.
This option allows us to control machine tool movements using the nine key number pad
located on the right hand side of the keyboard. The TMC-1000 system uses right-hand
Cartesian rectangular coordinates to describe the machine tool position in 3D space. The
image shown below depicts machine various components and how the coordinate axes relate
to them.
" Take a moment to familiarize yourself with the manual control commands.
20
Next, you will use the manual controls to perform facing operations on the workpiece surfaces.
The material stock was originally rough cut from a larger piece to the approximate dimensions of
the part. Facing each side allows you to create the exact outer dimensions of the part. In
addition, facing makes sure that each surface is perfectly flat and the edges are square with one
another. This improves the part s accuracy and helps firmly secure the workpiece in the vise.
" Begin by lowering the safety shield to gain access.
" Clamp the material stock in the vise so that the ~ 2 � width is along the Z-axis and the ~ 5
length runs along the X-axis.
" Insert a large end mill cutter into the tool holder and make sure it is securely locked in place.
Carefully rotate the tool by hand to make sure it will not bind or hit the cross slide, fixtures,
or workpiece on the start up. Using a large end mill (greater than � diameter) allows you to
remove significant amounts of material in fewer passes, thereby saving time.
" Raise the safety shield.
" Press the F1 button on the keyboard to turn on the spindle.
" Adjust the spindle speed control knob to 2000 RPM.
" Select C-CONTINUOUS/INCREMENTAL to set the tool to continuous motion. Carefully
lower the machine tool to the top surface of the workpiece.
" You can adjust the jog speed by selecting S SET JOG SPEED from the Manual Control
Panel. Slow down the jog speed to 2 IN/MIN when the tool gets close to the surface.
" Make a light cut (approximately 0.2 deep) into the workpiece surface. Traverse the tool
across the workpiece until the entire surface is at the same level. Depending on the condition
of the material stock it may be necessary to make several light passes before the entire
surface becomes flat.
" Move the tool away from the workpiece in the vertical direction and press F2 to stop the
spindle.
" Raise the safety shield, remove the workpiece from the vise and flip it over to machine the
opposite side.
" Repeat the steps above to face the surface. Make light cuts and stop frequently to measure
part dimensions. Stop removing material when the width of the workpiece is exactly 2 � .
" Face the remaining four sides of the workpiece by following the steps outlined above. Be
sure to make light cuts and measure the dimensions of the workpiece frequently. Remember,
the final dimensions of the material stock are 5 L x 2.5 W x 1.25 D.
" Finally, secure the workpiece in the vise in the same orientation as our drawing. Make sure
not to over tighten the vise as this can result in part damage.
21
Load the NC Program
Now that the material stock is cut to the proper dimension we can load the NC program to create
the rest of the features.
" Press ESC to return to the Main Menu.
" Insert the 3 � floppy disk with the NC program into drive B:.
" Select L-LOAD/DELETE and highlight the name of your NC program to load it into the
controller s memory.
" Once the program has successfully loaded you will return to the Main Menu.
Machine Tool Setup
The next step is to set up the cutting tools and the machine s local origin.
" Remove the large end mill cutter used for the facing operations and insert the � end mill.
This tool, labeled #1 in our NC program, is used to create the rest of the part features.
" Go to the Manual Control Panel by selecting M MANUAL CONTROL.
" Slowly lower the tool to the top surface of the workpiece. Set the tool motion to incremental
when the tool gets close to the surface. Stop when the tool has just barely touched the top
surface to avoid damage. The NC program defines this location as zero in the Z direction.
Note: You may wish to place a thin sheet of paper between the end mill and the part surface
when lowering the tool to set the Z position. This helps reduce the possibility of damaging the
workpiece. Gently slide the piece of paper back and forth over the workpiece surface as you
lower the tool. Stop when the paper catches on the cutter and no longer slides smoothly.
" Click P-SET POSITION and set Z POSITION = 0.
" Now raise the tool slightly and traverse across the workpiece to the corner you defined as the
origin in the NC program. Try to line up the center of the cutter with this corner. You may
wish to insert a smaller diameter cutter such as a center punch to help you  eyeball the
origin. Position the cutter as best you can. Because this is a practice part and does not
contain any critical dimensions this method of locating the origin will suffice. For more
precise work you may wish to use a mechanical audible edge finder such as the
Brown&Sharpe units shown below.
22
" Click P-SET POSITION and set both the X POSITION and the Y POSITION = 0.
" Hit ESC to return to the Main Menu.
Run the NC Program
Now you may run the NC program. You may wish to perform a dry run the first time you
execute a new program. This allows you to check for any errors in the program that were not
evident during toolpath simulation or to check for proper machine tool setup. To perform a dry
run simply remove the adapter and end mill from the tool holder and run the program as outlined
in the steps below.
" Select R-RUN and click START.
" The NC machine moves the tool to its default home position and pauses.
" Hit RETURN on the keyboard to continue. The tool then moves to the start position of the
first feature and begins cutting. Notice that the tool moves to the clearance height between
each cutting operation.
" You may manually override the feed rate using the + and  keys. This is particularly useful
in eliminating chatter caused by resonant frequencies. Usually increasing or decreasing the
feed rate slightly will remove unwanted vibrations. This feature can also be used to speed up
various machining operations. For example, if the original feed rate specified in the NC
program is very slow and can safely be increased, you may do so using this feature.
Note: Be very careful when overriding the feed rates specified in the program. While a 20 /min
feed rate might be okay for one part feature it might be much to fast for another such as a finish
cut or a part that requires especially high accuracy or surface finish. The feed override feature
can only be used during cutting operations in which the program specifies a particular rate. You
cannot adjust the override during rapid traverse moves in between individual machining
operations. Therefore, by the time you realize a particular feed rate override is to high for the
next operation it might be too late to change it before damage occurs.
" When the program has completed a pop-up window will appear stating a normal program
stop has occurred. Click OK and you will return to the Main Menu.
Congratulations! You re done and may now remove the completed part from the fixture. This
tutorial provided you with a basic introduction to Mastercam CAD/CAM software and CNC
machining principles. Going through the all the motions has equipped you with the knowledge
necessary to start creating parts of your own design for class assignments or any one of the great
student engineering projects such as Mini-Baja� and FutureTruck.
23
Appendix
NC Program Code
123.nc
; T
T1 M06
G90 G80 G40 G17
G0 X.76 Y.7601
S1069 M3
Z.25
Z.1
G1 Z-.5 F3.
X2.74
Y1.0867
X.76
Y1.4133
X2.74
Y1.7399
X.76
G0 Z.25
X.75 Y.75
Z.1
G1 Z-.5 F3.
X2.75
Y1.75
X.75
Y.75
G0 Z.25
Z2.
X5. Y0.
Z.49
G1 Z-.01 F3.
Y2.5
G0 Z.09
Z.25
Z.49
X4.625 Y0.
G1 Z-.01 F3.
Y2.5
G0 Z.09
Z.25
Z.49
X4.25 Y0.
G1 Z-.01 F3.
Y2.5
24
G0 Z.09
Z.25
Z.49
X3.875 Y0.
G1 Z-.01 F3.
Y2.5
G0 Z.09
Z2.
X5. Y0.
Z.11
G1 Z-.39 F3.
Y2.5
G0 Z-.29
Z.25
X4.625 Y0.
Z.11
G1 Z-.39 F3.
Y2.5
G0 Z-.29
Z.25
X4.25 Y0.
Z.11
G1 Z-.39 F3.
Y2.5
G0 Z-.29
Z.25
X3.875 Y0.
Z.11
G1 Z-.39 F3.
Y2.5
G0 Z-.29
Z2.
G81 X4.25 Y.75 Z-1.3 R-.3 F3.
Y1.75
G80
M05
M2
%
25