Mastercam x6-mill-level-1-tutorial-1

To order more books:
Call 1-800-529-5517 or
Visit www.inhousesolutions.com or
Contact your Mastercam dealer
Mill Level 1 Training Tutorial

Mastercam X6 Mill Level 1 Training Tutorial
Copyright: 1998 - 2011 In-House Solutions Inc. All rights reserved
Software: Mastercam X6
Author: Mariana Lendel
ISBN: 978-1-926955-26-1
Revision Date: November 18, 2011
Notice
In-House Solutions Inc. reserves the right to make improvements to this manual at any time and without
notice.
Disclaimer Of All Warranties And Liability
In-House Solutions Inc. makes no warranties, either express or implied, with respect to this manual or
with respect to the software described in this manual, its quality, performance, merchantability, or
fitness for any particular purpose. In-House Solutions Inc. manual is sold or licensed "as is." The entire risk
as to its quality and performance is with the buyer. Should the manual prove defective following its
purchase, the buyer (and not In-House Solutions Inc., its distributer, or its retailer) assumes the entire
cost of all necessary servicing, repair, of correction and any incidental or consequential damages. In no
event will In-House Solutions Inc. be liable for direct, indirect, or consequential damages resulting from
any defect in the manual, even if In-House Solutions Inc. has been advised of the possibility of such
damages. Some jurisdictions do not allow the exclusion or limitation of implied warranties or liability for
incidental or consequential damages, so the above limitation or exclusion may not apply to you.
Copyrights
This manual is protected under International copyright laws. All rights are reserved. This document may
not, in whole or part, be copied, photographed, reproduced, translated or reduced to any electronic
medium or machine readable form without prior consent, in writing, from In-House Solutions Inc.
Trademarks
Mastercam is a registered trademark of CNC Software, Inc.
Microsoft, the Microsoft logo, MS, and MS-DOS are registered trademarks of Microsoft Corporation; N-
See is a registered trademark of Microcompatibles, Inc.; Windows, Windows XP, Windows Vista,
Windows NT and Windows 7 are registered trademarks of Microsoft Corporation.

Getting Started ...........................................................................................................1
Tutorial #1 - Open Contour and Drill Toolpaths ................................................................................... 11
Tutorial #2 - Facing, Pocket, Contour, Drilling and Contour-Chamfer Toolpaths................................. 59
Tutorial #3 - Open Pocket, Contour Remachining, Circle Mill, Drill and Contour Toolpaths.............. 133
Tutorial #4 - 2D HS Core Mill, 2D HS Dynamic Core Mill, Pocket Island Facing and Pocket
Remachining Toolpaths........................................................................................................................ 231
Tutorial #5 - 2D HS Dynamic Area Mill, Drill, Circle Mill and Contour Chamfer Toolpaths ................ 309
Tutorial #6 - Working with Tool Planes, 2D HS Area Mill, 2D HS Rest Mill,
Drill and Slot Mill Toolpaths ............................................................................................................... 417
Tutorial #7 - 2D HS Dynamic Core Mill, 2D HS Core Mill, 2D HS Blend, 2D HS Peel Toolpaths .......... 567
Tutorial #8 - Feature Based Drilling (FBD) Toolpath........................................................................... 639
Tutorial #9 - Feature Based Milling Toolpath..................................................................................... 703
Mill Level 1 Training Tutorial Contents

Tutorial #10 - 2D HS Dynamic Area Mill, 2D HS Dynamic Rest Mill, 2D HS Dynamic Core Mill, 2D HS
Dynamic Contour and Machine Simulation........................................................................................ 765
General Notes ......................................................................................................... 831
Creating/Editing Tools ............................................................................................ 889
Quiz Answers.......................................................................................................... 897

Mill Level 1 Training Tutorial Page|1
GETTING STARTED
GETTING STARTED
Objectives:
The Student will learn about the Graphical User Interface.
The Student will learn how to navigate through Mastercam.
How to use the Status Bar to set the attributes.
Set the Toolbar States.
Setting the Grid.

Page|2 Mill Level 1 Training Tutorial
GETTING STARTED
STEP 1: GUI - GRAPHICAL USER INTERFACE
Menu Allows you to select all the functions in Mastercam to create geometry and toolpaths.
Toolbars Can be used instead of the menu to create geometry and toolpaths.
Ribbon Bar Allows you to enter the values and settings that define the entities that you are
currently creating or modifying.
Function prompt Prompts the user for info.
Status Bar Allows you to set the attributes (color, level, style, and width) and the View/Plane and
Z depth currently used.
Toolpaths/Solid
Manager
Lists the history of the toolpath operations and solids.
Origin Geometry origin from which the system measures the point coordinates in X,Y and Z
axes in the current plane.
Graphic Area Workspace area in Mastercam where the geometry displays.
MRU Toolbar Lists the most recently used functions.
Quick Mask Toolbar Lets you select all entities of a specific type.
Scale Shows you a scale of the object on the screen.
View Port XYZ Axes Inform you which Graphics view, WCS and Toolplane/Construction plane you are
working in.

GETTING STARTED
STEP 2: NAVIGATE THROUGH MASTERCAM
In this step you will learn how to use the menu functions in Mastercam to create geometry.
2.1 Using the Menu to select the command Create Line Endpoint
 Left click on Create.
 Move the cursor on the drop-down menu to the Line function. This will open a flyout menu with all the
commands related to create lines.
 Left-click on the desired command Endpoint as shown in Figure: 2.1.1.
Figure: 2.1.1
2.2 Using the Toolbars to select the command Create Line Endpoint
 Left Click on the Create Line Endpoint command icon as shown in Figure: 2.2.1.
Figure: 2.2.1

GETTING STARTED
 To see the commands which are found under Create Line, in the menu bar choose the drop down arrow to the
right of the icon as shown.
2.3 Reorganizing the Toolbars
 To move a toolbar select the left vertical line in front of the toolbar and drag it to the desired location on the
screen as shown in Figure: 2.3.1.
Figure: 2.3.1
2.4 Create Line Endpoint Ribbon Bar example
 To create a line left click on the screen. Then enter the distance and angle if necessary.
 To continue making lines choose the Apply button from the ribbon bar or press enter. To exit the current
command select the OK button or press the Esc button.
 To undo the last command use the Undo button. The Undo button can be used to go back to the beginning
of geometry creation or to the last point of the saved file. Mastercam also has a Redo button for your
convenience.
NOTE: Mastercam is fully customizable meaning you can move the toolbars anywhere you desire allowing you
to work more efficiently.
NOTE: To customize the toolbars please see the General Notes.

GETTING STARTED
2.5 Function Prompt
 Prompts the user to execute a command.
 For example this prompt is used in the Create Line Endpoint command as shown in Figure: 2.5.1.
Figure: 2.5.1
2.6 Status Bar
 The Status bar seen in Figure: 2.6.1 is used to set the drawing attributes, view, plane, Z depth and construction
mode.
Figure: 2.6.1
2D / 3D Construction Toggles between 2D and 3D construction modes. In 2D mode all geometry is created
parallel to the current Cplane at the current system Z depth. In 3D mode you can
work freely in various Z depths, unconstrained by the current system Z depth and
Cplane setting.
Gview Sets the graphics view which you will view your geometry from. You can choose a
different standard Gview, an existing named view, create a new named view or set
the Gview to the current Cplane.
Planes Sets the construction plane in which you create and manipulate your geometry. You
can change the current plane by selecting a different standard plane, selecting an
existing named view, creating a new named view and by setting the plane to equal
the current Gview.
Z Depth Sets the current construction depth. To set this click the drop down arrow and pick
one from the most recently used list or click the Z: label and pick a point in the
graphics window to use the Z depth values based on the selected entity.
Color Assigns the current color. To change the current color click in the color field and
select a colour from the colour pallet.
Level Sets the main level you want to work with in the graphics window. To change the
current working level type the level number in the box or select the level using one
of the following methods.
Attributes Lets you change one or more drawing attributes.
Point Style Displays and sets the systems point style.
Line Style Shows and sets the system line style.
Line Width Displays and sets the current system line width.

GETTING STARTED
2.7 Change the Current System Colour
 Left Click on System Color as shown.
 Select the desired color from the dialog box as shown in Figure: 2.7.1.
Figure: 2.7.1
 Select the OK button to exit the command and begin creating geometry in the color of your choice.
Work Coordinate
System (WCS)
Allows you to redefine the WCS. You can choose from a list of stand views, specify
origin coordinates, access the view manager or use the named function to access the
view selection dialog box.
Groups Defines a collection of entities or operations that can be manipulated as a single
entity.
NOTE: Any geometry on your screen will remain in the previous system colour. This change will only affect the
geometry you create going forward.

GETTING STARTED
2.8 The Toolpath Manager
 The Toolpath Manger displays all the operations for the current part.
 You can sort, edit, regenerate, verify and post any operations.
 For more information on the Toolpath Manager, please refer to General Notes.
 The Manger can be hidden to gain more space in the graphics area for creating geometry. Press Alt + O to hide
the manager and Alt + O to reopen the manager as shown in Figure: 2.8.1.
Figure: 2.8.1
STEP 3: SETTING THE TOOLBAR STATES
 Before starting the geometry creation we should customize the toolbars to see the toolbars required to create
the geometry and machine a 2D part.
Settings
 Toolbar States as shown.

GETTING STARTED
 From the left column select 2D Toolpaths.
 Choose the Load button as shown in Figure: 3.0.1.
Figure: 3.0.1
 Select the OK button to accept the toolbar states.
 The 2D Toolpaths will be displayed to the left of the Operations Manager as shown in Figure: 3.0.2.
Figure: 3.0.2

GETTING STARTED
STEP 4: SETTING THE GRID
 Before beginning to create geometry you will enable the Grid. This will show you where the origin is.
Settings
 Configuration.
 Select Screen from the configuration Topics.
 Select the plus sign (+) beside screen as shown in Figure: 4.0.1.
Figure: 4.0.1
 In Grid Settings enable Visible Grid and change the Spacing to X = 0.25 and Y = 0.25.
 Set the Size to 1.0.
 Choose the Ok button to exit.
 Select Yes to save the setting as shown.

GETTING STARTED
 The grid will appear on your screen as shown in Figure: 4.0.2.
Figure: 4.0.2

TUTORIAL #1

Page |12 Mill Level 1 Training Tutorial
TUTORIAL #11 OVERVIEW OF STEPS TAKEN TO CREATE THE FINAL PART:
OVERVIEW OF STEPS TAKEN TO CREATE THE FINAL PART:
From Drawing to CAD Model:
The student should examine the drawing on the following page to
understand what part is being created in the tutorial.
From the drawing we can decide how to go about creating the
geometry in Mastercam.
Create the 2D CAD Model used to generate Toolpaths from:
The student will only create the Top 2D geometry needed to create the
toolpaths.
Geometry creation commands such as create rectangle, line parallel,
mirror and circle center point will be used.
Create the necessary Toolpaths to machine the part:
The student will set up the stock size to be used and the clamping
method used.
An Open Contour toolpath will be created to remove the material on
the both steps.
A Drilling toolpath will be created to machine the through holes.
Backplot and Verify the file:
The Backplot will be used to simulate a step by step process of the
tool’s movements.
The Verify will be used to watch a tool machine the part out of a solid
model.
Post Process the file to generate the G-code:
The Student will then post process the file to obtain an NC file
containing the necessary code for the machine.
This tutorial takes approximately one hour to complete.

OVERVIEW OF STEPS TAKEN TO CREATE THE FINAL PART: TUTORIAL #11

TUTORIAL #11 SETTING UP THE GRAPHIC USER INTERFACE
GEOMETRY CREATION
STEP 1: SETTING UP THE GRAPHIC USER INTERFACE
Please refer to the Getting Started section to set up the graphics user interface.
STEP 2: CREATE A RECTANGLE
In this step you will learn how to create a rectangle knowing the width, the height and the anchor position.
Step Preview:
2.1 Create a 3.0" by 2.0" Rectangle
Create
 Rectangle.
 Enter the Width and Height as shown.
 Press Enter after typing the values to see a preview of the rectangle.

CREATE A RECTANGLE TUTORIAL #11
 [Select position for first corner]: Select the Origin as shown in Figure: 2.1.1.
Figure: 2.1.1
 Make sure that when selecting the origin, the visual cue of the cursor changes as shown.
 Select the OK button to exit the Rectangle command.
 Use the Fit icon to fit the drawing to the screen.
NOTE: During the geometry creation of this tutorial, if you make a mistake you can undo the last step using the
Undo icon. You can undo as many steps as needed. If you delete or undo a step by mistake, just use the
Redo icon. To delete unwanted geometry, select it first and then press Delete from the keyboard.

TUTORIAL #11 CREATE THE PARALLEL LINE
STEP 3: CREATE THE PARALLEL LINE
In this step you will learn how to create a parallel line knowing the distance.
Step Preview:
Create
 Line.
 Parallel.
 [Select a line]: Select Entity A as shown in Figure: 3.0.1.
Figure: 3.0.1
 [Select the point to place a parallel line through]: Pick a point below the selected line.
NOTE: The color of the geometry is cyan which means that the entity is "live" and you can still change the line
parameters if needed.

CREATE THE PARALLEL LINE TUTORIAL #11
 Enter the Distance 1.0" (press Enter).
 Select the OK button to exit the command.
 The part will appear as shown in Figure: 3.0.2.
Figure: 3.0.2
NOTE: To continue using the same command you can either select the Apply button or press Enter. To
exit the command you can either start a new command or select the OK button.

TUTORIAL #11 DELETE THE CONSTRUCTION LINES
STEP 4: DELETE THE CONSTRUCTION LINES
In this step you will delete two lines in preparation to mirror the geometry.
Step Preview:
Edit
 Delete.
 Delete Entities.
 Select the two lines as shown in Figure: 4.0.1.
Figure: 4.0.1
 Select the Delete entity icon.
 Select the Repaint icon to refresh the screen.

MIRROR THE GEOMETRY TUTORIAL #11
STEP 5: MIRROR THE GEOMETRY
In this step you will mirror the geometry to create the shape of the part.
Step Preview:
5.1 Mirror about the X-Axis
Xform
 Mirror.
 [Select the entities to mirror]: Click on the All button.

TUTORIAL #11 MIRROR THE GEOMETRY
 Click on the All Entities button in the Select All dialog box as shown in Figure: 5.1.1.
Figure: 5.1.1
 Click on the End Selection button or press Enter to finish the selection.
 Set the parameters to match the following dialog box (ensure Copy is picked to keep the original entities).
NOTE: The entire geometry is highlighted yellow (selection color).

 Choose the option to mirror about the X-axis as shown in Figure: 5.1.2.
Figure: 5.1.2
 Select the Apply button to continue in the same command.
Figure: 5.1.3

TUTORIAL #11 MIRROR THE GEOMETRY
5.2 Mirror about the Y-Axis
 [Select the entities to mirror]: Click on the All button.
 Click on All Entities button in the Select All dialog box.
 Click on the End Selection button.
NOTE: The entire geometry is highlighted yellow (selection color).

 Set the parameters to match the following dialog box (ensure Copy is picked to keep the original entities).
 Choose the option to mirror about the Y-axis.
 Select the OK button to exit the mirror dialog box.
Screen
 Clear Colors.
Figure: 5.2.1

TUTORIAL #11 CREATE ARCS
STEP 6: CREATE ARCS
In this step you will create points which will later be used to drill holes in the part.
Step Preview:
Create
 Arc.
 Circle Center Point.
 Input a Diameter of 0.5" in the ribbon bar and then select the icon to lock the value.
 Select the Fast Point icon from the AutoCursor Ribbon Bar.
 Enter the dimensions -1.75, 0 then hit Enter on your keyboard.
 Select the Fast Point again and enter the dimensions 1.75, 0 and hit Enter on your keyboard once again.
 From the AutoCursor Ribbon Bar, select the drop down arrow to view the AutoCursor’s Override options.

SAVE THE FILE TUTORIAL #11
 Select the option Origin from the list. This will place a circle with the center at the origin.
 Once complete choose the OK button to exit the command.
STEP 7: SAVE THE FILE
File
 Save As.
 File name: "Your Name_1".
 Select the OK button to save your file.

TUTORIAL #11 SUGGESTED FIXTURE:
TOOLPATH CREATION
SUGGESTED FIXTURE:
SETUP SHEET:

SELECT THE MACHINE AND SET UP THE STOCK TUTORIAL #11
STEP 8: SELECT THE MACHINE AND SET UP THE STOCK
In Mastercam, you select a Machine Definition before creating any toolpaths. The Machine Definition is a model of your
machines capabilities and features. It acts like a template for setting up your machine. The machine definition ties together
three main components: The schematic model of your machines components, the control definition that models your
control capabilities, and the post processor that will generate the required machine code (G-code). For a Mill Level 1
exercise (2D toolpaths) we need just a basic machine definition.
 To display the Operations Manager press Alt + O.
Machine type
 Mill.
 Default.
 Select the plus sign in front of Properties in the Toolpaths Manager to expand the Toolpaths Group Properties.
 Select Tool Settings to set the tool parameters.
NOTE: For the purpose of this tutorial, we will be using the Default mill machine.

TUTORIAL #11 SELECT THE MACHINE AND SET UP THE STOCK
 Change the parameters to match Figure: 8.0.1.
Figure: 8.0.1
Program # is used to enter a number if your
machine tool requires a number for a program
name.
Assign tool numbers sequentially allows you
to overwrite the tool number from the library
with the next available tool number. (First
operationtool number 1; Second operation
tool number 2, etc.)
Warn of duplicate tool numbers allows you to
get a warning if you enter two tools with the
same number.
Override defaults with modal values enables
the system to keep the values that you enter.
Feed Calculation set From tool uses feed rate,
plunge rate, retract rate and spindle speed
from the tool definition.

SELECT THE MACHINE AND SET UP THE STOCK TUTORIAL #11
 Select the Stock setup tab to define the stock.
 Set the stock shape to Rectangular if needed and enter the stock dimensions as shown in Figure: 8.0.2.
Figure: 8.0.2
 Select the OK button to exit Machine Group Properties.
 Select the Isometric view from the graphics view toolbar to see the stock.
NOTE: The stock model that you create can be displayed with the part geometry when viewing the file or the
toolpaths, during backplot, or while verifying toolpaths. In the graphics, the plus shows you where the stock
origin is. The default position is the middle of the stock. Click on the corner of the part to set it as the stock
origin.
The Stock Origin values adjust the positioning of the
stock, ensuring that you have equal amount of extra
stock around the finished part.
Display options allow you to set the stock as
Wireframe and to fit the stock to the screen. (Fit
Screen)

TUTORIAL #11 SELECT THE MACHINE AND SET UP THE STOCK
 The stock model will appear as shown.
 Select the Top view from the view toolbar to see the part from the top.
NOTE: The stock is not geometry and can not be selected.

MACHINE THE TWO STEPS USING OPEN CONTOUR TOOLPATH TUTORIAL #11
STEP 9: MACHINE THE TWO STEPS USING OPEN CONTOUR TOOLPATH
Contour toolpaths remove the material along a path defined by a chain of curves. Contour toolpaths only follows a chain;
they do not clean out an enclosed area.
Toolpath Preview:
9.1 Chain Selection
A chain of entities consists of one or more entities linked together in order and direction. The distance between the
endpoints of two consecutive entities of the chain has to be equal or less than the chaining tolerance (0.0001"). In an open
chain, the start point is placed at the end of the chain closest to the selection point and the chain direction points to the
opposite end of the chain. See the User Notes chapter for more information on chaining.
Toolpaths
 Contour.
 If a prompt appears to Enter new NC name, select the OK button to accept the default.

TUTORIAL #11 MACHINETHETWOSTEPSUSINGOPENCONTOURTOOLPATH
 Enable the Chain button in the chaining dialog box to be able to select just the outside contour.
 Select the first chain as shown in Figure: 9.1.1.
Figure: 9.1.1
NOTE: The direction of the chain determines the cutter compensation side (Left or Right) to orient the tool on
the proper side of the geometry. For our example be sure to chain the contour in a CCW direction. Otherwise,
select the Reverse button.

 To be able to machine both contours in one operation select the second chain as shown in Figure: 9.1.2.
Figure: 9.1.2
 Select the OK button to exit Chaining.
 In the Toolpath Type page, the Contour icon will be selected.
9.2 Select a 3/4" Flat Endmill from the library and set the Tool Parameters
 Select Tool from the Tree view list.
 Click on the Select library tool button.
 To be able to see all the tools from the library disable Filter Active.
NOTE: Mastercam updates the pages as you modify them and then marks them, in the Tree view list, with a
green check mark. Pages that are not changed are marked with a red circle and slash.

 Scroll down and select the 3/4" Flat Endmill (# 241) as shown.
 Select the tool in the Tool Selection page and then select the OK button to exit.
 Make all the necessary changes as shown in Figure: 9.2.1.
Figure: 9.2.1
The Feed rate, Plunge rate, Retract rate and Spindle speed are selected from tool definition. You may change these
values as per your part material and tools.
In the Comment field enter a comment to help identify the toolpath in the Toolpaths/Operations Manager such as the
one shown above.

9.3 Set the Cut Parameters
 From the Tree view list, select Cut Parameters and make the changes as shown in Figure: 9.3.1.
Figure: 9.3.1
Figure: 9.3.2
Compensation type set to Computer allows Mastercam to compensate the toolpath based on the tool diameter and
does not output G41/G42 in the code.
Compensation direction set to Right compensates the toolpath to the right of the chain based on the chaining
direction. See the Figure: 9.3.2.
Roll cutter around corners set to Sharp inserts arc moves around corners in the toolpath. The radius of the arc moves
is equal with the radius of the tool.
Infinite look ahead prevents the toolpath from crossing itself (fish tail).

9.4 Set the Lead In/Out
 From the Tree view list, select Lead in/out and change the parameters as shown.
 Make sure that you disable the Entry and the Exit options and enable Adjust start/end of contour as shown in
Figure: 9.4.1.
Figure: 9.4.1
Lead In/Out allows you to select a combination of a Line and an Arc at the beginning and/or end of the contour
toolpath for a smooth entry/exit while cutting the part.
Adjust start/end of contour moves the starting/ending position in open contours by adding (Extend) or removing
(Shorten) the specified length.

9.5 Set the Linking Parameters
 From the Tree view list, select Linking Parameters and change the parameters as shown Figure: 9.5.1.
Figure: 9.5.1
 Select the OK button to exit the contour parameters.

TUTORIAL #11 BACKPLOT THE TOOLPATHS
STEP 10: BACKPLOT THE TOOLPATHS
Backplotting shows the path the tools take to cut the part. This display lets you spot errors in the program before you
machine the part. As you backplot toolpaths, Mastercam displays the current X, Y, and Z coordinates in the lower left
corner of the screen.
 Make sure that the toolpath is selected (signified by the green check mark on the folder icon).
 Select the Backplot selected operations button.
 Make sure that you have the following buttons turned on (they will appear pushed down) to see the tool and
the rapid moves.
 Select the Isometric view from the view toolbar to see the stock.
 Select the Fit button.
 You can adjust the speed of the backplot.
 You can step through the Backplot by using the Step forward or Step back buttons.
 Select the Play button in the VCR bar.

VERIFY THE TOOLPATH TUTORIAL #11
 The part should appear as shown in Figure: 10.0.1.
Figure: 10.0.1
 Select the OK button to exit Backplot.
STEP 11: VERIFY THE TOOLPATH
Verify allows you to use a solid model to simulate the machining of a part. The model created by verification represents
the surface finish, and shows collisions, if any exist.
 In the Operations Manager choose the Contour operation.
 Choose the Verify selected operations icon from the Operations Manager.
 Set the Verify speed by moving the slider bar in the speed control bar as shown.

TUTORIAL #11 VERIFY THE TOOLPATH
 Select the Play button to start simulation.
Figure: 11.0.1
 Select the OK button to exit Verify.

ADD MULTI PASSES TUTORIAL #11
STEP 12: ADD MULTI PASSES
Multi Passes lets you define multiple cutting passes. The tool approaches the part geometry at the cutting depth in steps
instead of cutting right to the part geometry.
Toolpath Preview:
 Select Parameters for the contour toolpath.

TUTORIAL #11 ADD MULTI PASSES
 From the Tree view list select Multi Passes and make the necessary changes as shown in Figure: 12.0.1.
Figure: 12.0.1
 Once the changes have been made to the parameters select the OK button to exit the 2D Toolpaths- Contour
parameters.
 Select the Regenerate all dirty operations button to recalculate the changes made to the toolpath.
 Once the operation has been regenerated Backplot and Verify your toolpath page 38 to review these
procedures.
NOTE: We made a change to the Contour parameters, this toolpath is now marked as a dirty toolpath/
operation. A dirty toolpath or operation occurs anytime you make changes to the toolpath parameters.
Rough Passes/Finish Passes allows you to enter the number of passes and amount of material you want to remove per
pass.
Machine finish passes at: performs the finish pass at the final depth. All depths performs the finish passes at all depths.
This option only applies if depth cuts are enabled.

DRILL 3 HOLES TUTORIAL #11
Figure: 12.0.2
STEP 13: DRILL 3 HOLES
A drill toolpath is used for cutting holes in material.
Toolpath Preview:
Toolpaths
 Drill.

TUTORIAL #11 DRILL 3 HOLES
 The Drill point Selection dialog box will appear prompting you to select the arc center points as shown.
Figure: 13.0.1
 Select the center of all three arcs on the part.
 Ensure the Auto Cursor icon appears as shown before selecting the points as shown.

 Once the 3 arcs have been selected choose the OK button to exit the Drill Point Selection dialog box.
 In the Toolpath Type page, the Drill icon will be selected.
13.1 Select a 1/2" Drill from the library and set the Tool Parameters
 Select Tool from the Tree view list.
 Click on the Select library tool button.
 To be able to see all the tools from the library disable Filter Active.
 Scroll down and select the 1/2" Drill (#141) as shown in Figure: 13.1.1.
Figure: 13.1.1
 Select the tool in the Tool Selection page and then select the OK button.

 Make the necessary changes as shown in Figure: 13.1.2.
Figure: 13.1.2

 Select the Cut Parameters page and change the Cyclce to Peck Drill as shown in Figure: 13.1.3.
Figure: 13.1.3
Peck Drill retracts fully out of the drill hole to remove material chips. Often used with chips that are hard to remove.

 Choose Linking parameters, enable Clearance and set the Depth to -1.0" as shown in Figure: 13.1.4.
Figure: 13.1.4

 Choose the option Tip Comp, enable this option and make the necessary changes as shown in Figure: 13.1.5.
Figure: 13.1.5
 Select the OK button to generate the toolpath.
 To Backplot and Verify your toolpath page 38 to review these procedures.
 To select both operations click on the Select all operations button.
 The finished part will appear as shown.

TUTORIAL #11 POST THE FILE
STEP 14: POST THE FILE
Posting refers to a process where the toolpaths in Mastercam are converted to a format that can be understood by the
machines control, specifically the G-codes. In most cases every machine will require its own post processor; customized to
produce code formatted to meet the machines exact requirements.
 Ensure all operations are selected, if they are not use the button Select all operations in the Operations
Manager.
 Select the Post selected operations button from the Operations Manager.
 In the Post processing window make the necessary changes as shown in Figure: 14.0.1.
Figure: 14.0.1
 Select the OK button to continue.
NC File enabled allows you to keep the NC file and to assign the
same name as the MCX file.
Edit enabled allows you to automatically launch the default editor.

SAVE THE UPDATED MCX FILE TUTORIAL #11
 Select the OK button to save the NC file.
 A window with the NC program will appear.
 Select the red "X" box at the upper right corner to exit the editor.
STEP 15: SAVE THE UPDATED MCX FILE
 Select the Save icon.

TUTORIAL #11 SAVE THE UPDATED MCX FILE
REVIEW EXERCISE -STUDENT PRACTICE

CREATE THE GEOMETRY FOR TUTORIAL #1 EXERCISE TUTORIAL #11
CREATE THE GEOMETRY FOR TUTORIAL #1 EXERCISE
Use these commands to create the geometry:
 Create 1/4 of the geometry.
 Create a rectangle.
 Create Line Parallel.
 Create Point Position (position using Fast Point).
 Delete Entities.
 Xform Mirror.
 Edit Join Entities.

TUTORIAL #11 CREATE THE TOOLPATHS FOR TUTORIAL #1 EXERCISE
CREATE THE TOOLPATHS FOR TUTORIAL #1 EXERCISE
Create the Toolpaths for Tutorial #1 Exercise as per the instructions below.
Set the machine properties including the stock.
Remove the material in the center of the part Contour (2D).
 Use a 7/8" Flat Endmill.
 Based on your chaining direction ensure the Compensation
direction is set correct.
 No Depth Cuts.
 Lead In/Out ensure the arc radius is set to zero.
 No Break Through, Multi Passes.
 Set the depth according to the drawing.
Drill the holes through the part.
 Use a 5/16" Drill.
 Choose the Drill/Counterbore cycle.
 Depth set according to the drawing.
 Enable Tip Comp and input a Breakthrough amount.

NOTES: TUTORIAL #11
NOTES:

TUTORIAL #11 NOTES:
TUTORIAL #1 QUIZ
 What is a Contour Toolpath used for?
 What does Backplot do?
 When would you use Multi Passes?
 When would you use the drill cycle Peck Drill?

NOTES: TUTORIAL #11

TUTORIAL #11 NOTES:

Mastercam x6-mill-level-1-tutorial-1

More Related Content

What's hot (19)

Viewers also liked (16)

Similar to Mastercam x6-mill-level-1-tutorial-1 (20)

Recently uploaded (20)

Mastercam x6-mill-level-1-tutorial-1