mastercam x getting started tutorials
Basic 3D
Machining
October 2009
Be sure you have the latest information!
Information might have been changed or added since this document was
published. Contact your local Reseller for the latest information.
II • BASIC 3D MACHINING
Mastercam® X4 Basic 3D Machining
Date: October 2009
Copyright © 2009 CNC Software, Inc.— All rights reserved.
First Printing: October 2009
Software: Mastercam X4
TERMS OF USE Use of this document is subject to the Mastercam End User License Agreement. A
copy of the Mastercam End User License Agreement is included with the
Mastercam product package of which this document is part. The Mastercam End
User License Agreement can also be found at:
www.mastercam.com/legal/licenseagreement/
Contents
Introduction ......................................................................................... 1
Machining the Connector ......................................................... 5
1. Toolpath Setup........................................................... 7
III
Tutorial Goals................................................................................... 1
Before You Begin............................................................................. 1
If You Need More Help.................................................................... 3
Additional Documentation..............................................................4
Lesson Goals.................................................................................... 7
Exercise 1: Assigning a Machine Definition.............................. 7
Exercise 2: Setting Stock for Machining................................... 8
Exercise 3: Creating Toolpath Groups ..................................... 10
2. Roughing the Interior ................................................ 13
Lesson Goals..................................................................................13
Exercise 1: Drilling the Holes .................................................. 13
Exercise 2: Roughing the Pocket ............................................ 19
Exercise 3: Roughing the Slot................................................. 23
Exercise 4: Rest Roughing the Interior.................................... 28
3. Finishing the Interior................................................. 33
Lesson Goals..................................................................................33
Exercise 1: Finishing the Pocket Floor ....................................33
Exercise 2: Finishing the Slot.................................................. 36
4. Machining the Exterior ............................................. 41
Lesson Goals..................................................................................41
Exercise 1: Roughing the Exterior ........................................... 41
Exercise 2: Finishing the Exterior............................................ 46
Exercise 3: Drilling a hole from the Front Plane....................... 49
IV • BASIC 3D MACHINING
Machining the Tool Holder..................................................... 71
5. Adding Details .......................................................... 53
Lesson Goals..................................................................................53
Exercise 1: Lettering with a Project Toolpath..........................53
Exercise 2: Lettering with a Contour Toolpath.........................57
6. Backplot/Verify Your Toolpaths ............................... 63
Lesson Goals..................................................................................63
Exercise 1: Backplotting All Toolpaths ....................................63
Exercise 2: Verifying All Toolpaths.......................................... 64
7. Posting Toolpaths..................................................... 67
Lesson Goals..................................................................................67
Exercise 1: Posting All Toolpath Operations............................67
Sending NC Files to the Machine ................................................69
1. Toolpath Setup.......................................................... 73
Lesson Goals..................................................................................73
Exercise 1: Assigning a Machine Definition ............................73
Exercise 2: Setting Stock for Machining .................................74
2. Roughing the Part..................................................... 77
Lesson Goals..................................................................................77
Exercise 1: Roughing the Part .................................................77
Exercise 2: Creating a Leftover Toolpath................................. 82
3. Semi-Finishing the Part ............................................ 85
Lesson Goals..................................................................................85
Exercise 1: Creating a Surface Finish Blend ............................85
Exercise 2: Creating a Surface Finish Parallel Steep ...............89
Exercise 3: Copy and Modify an Operation .............................91
4. Finishing the Part...................................................... 95
Lesson Goals..................................................................................95
Exercise 1: Creating a Swept 3D............................................. 95
Exercise 2: Creating a second Swept 3D ................................98
Exercise 3: Creating a Flowline ............................................. 101
5. Backplot/Verify Your Toolpaths.............................. 105
Lesson Goals................................................................................ 105
Exercise 1: Backplotting all Toolpaths .................................. 105
Exercise 2: Verifying All Toolpaths........................................ 106
6. Posting Toolpaths ................................................... 109
Lesson Goals................................................................................ 109
Exercise 1: Posting All Toolpath Operations ......................... 109
Sending NC Files to the Machine.............................................. 111
Conclusion .........................................................................................112
V
VI • BASIC 3D MACHINING
INTRODUCTION
This tutorial focuses on applying several milling toolpaths to parts previously designed in
Mastercam. The objective is to provide a general overview of a handful of the toolpath options
available to you. The options and parameters selected are intended to get you started on the path
toward learning and exploring all of the features Mastercam has to offer.
The toolpaths created illustrate possible solutions for machining parts using 3D toolpaths - mainly
surfacing operations. There are many solutions for machining these and similar parts. The goal of
this tutorial is to provide the basic concepts for you to explore and expand upon. Alter and adjust
the outline to fit your learning and programming environment after completing the lessons.
Toolpath creation is a repetitive, step-by-step process as demonstrated by this tutorial.
Comprehensive and conceptual information can be found in the Help and other documentation
installed with Mastercam.
Tutorial Goals
Open multiple part files, assign default machine definitions, and create stock boundaries
for the geometry
Create and rename toolpath groups
Create roughing operations to efficiently remove material from the part
Create semi-finishing operations to safely transition between roughing and finishing the
part
Create finishing operations to create a complete part with final dimensions
Copy operations, change parameters, and regenerate the operation
Assign toolpath parameters to meet the roughing, semi-finishing, and finishing
requirements
Backplot toolpath operations to review tool motion
Verify the machining of the part from a stock model display
Post all toolpath operations to an NC file, review/edit the code as necessary, and save the
NC file
Before You Begin
This is a module of the Mastercam Getting Started Tutorial Series. The series introduces general
Mastercam functions and teaches basic skills for getting started with Mastercam. Other tutorial
series include:
Focus Series: Focuses on a specific Mastercam feature—for example, Setup Sheets or FBM
Drill, and teaches basic and advanced skills.
Exploring Series: Explores a single Mastercam product—for example, Mill, Solids, or Wire,
and teaches in-depth skills for working with the product.
The Mastercam tutorial series is in continual development, and we will add modules as we
complete them. For information and availability, please contact your local Mastercam Reseller.
2 • BASIC 3D MACHINING
Note: Screen colors in the tutorial pictures enhance image quality; they may not match your
Mastercam settings.
General Tutorial Requirements
All Mastercam tutorials have the following general requirements:
You must be comfortable using the Windows
The tutorials cannot be used with Mastercam Demo/Home Learning Edition (HLE). The
Demo/HLE file format (EMCX) is different from Mastercam (MCX), and basic Mastercam
functions, such as file conversions and posting, are unavailable.
Each lesson in the tutorial builds on the mastery of preceding lesson’s skills. We
recommend that you complete them in order.
Focus Series and Exploring Series tutorials require, at minimum, a mastery of the basic
Mastercam skills taught in the Getting Started Series modules. A general knowledge of
machining principals and practices is also required.
You must have a seat of Mastercam X4 Design or higher to complete most of the tutorials in
the Getting Started Series.
The Basic 2D Machining module in the Getting Started Series requires, at minimum, a seat
of Mill Entry or Router Entry.
The Basic 3D Machining module in the Getting Started Series requires Mill Level 3 or Router
Pro.
Additional files may accompany a tutorial. Unless the tutorial provides specific
instructions on where to place these files, store them in a folder that can be accessed from
the Mastercam workstation, either with the tutorial or in any location that you prefer.
The Getting Started Series tutorials are available in an Adobe
format. Additional tutorial videos may also be available. Contact your local Mastercam
Reseller for more information.
You must install Adobe Flash Player to display tutorial videos. You can download Adobe
Flash Player from www.adobe.com.
You must configure Mastercam to work in metric units. Complete the instructions in the
following section Preparing for a Tutorial to set Mastercam to metric.
®
operating system.
®
Flash® compatible video
Preparing for a Tutorial
Before you start a tutorial, be sure you have completed the following tasks:
1 Start Mastercam using your preferred
method:
Double-click Mastercam’s desktop
icon.
Or
Launch Mastercam from the
Windows Start menu.
2 Select the metric configuration file:
a Select Settings, Configuration from
Mastercam’s menu.
b Choose ..\config\mcamxm.config
<Metric> from the Current drop-down
list.
c Click OK.
If You Need More Help
There are many ways to get help with Mastercam, including the following:
INTRODUCTION • 3
Mastercam Help—Access Mastercam Help by selecting Help, Contents from Mastercam’s
menu bar or by pressing [Alt+H] on your keyboard. Also, most dialog boxes and ribbon
bars feature a Help button that opens Mastercam Help directly to related information.
Online help—You can search for information or ask questions on the Mastercam Web
forum, located at www.emastercam.com. You can also find a wealth of information,
including many videos, at www.mastercam.com and www.mastercamedu.com.
Mastercam Reseller—Your local Mastercam Reseller can help with most questions about
Mastercam.
Technical Support—CNC Software’s Technical Support department (860-875-5006 or
support@mastercam.com) is open Monday through Friday from 8:00 a.m. to 5:30 p.m. USA
Eastern Standard Time.
Documentation feedback—For questions about this or other Mastercam documentation,
contact the Technical Documentation department by email at techdocs@mastercam.com.
Mastercam University—CNC Software sponsors Mastercam University, an affordable
online learning platform that gives you 24/7 access to Mastercam training materials. Take
advantage of more than 180 videos to master your skills at your own pace and help prepare
yourself for Mastercam Certification. For more information on Mastercam University,
please contact your Authorized Mastercam Reseller, visit www.mastercamu.com, or email
training@mastercam.com.
4 • BASIC 3D MACHINING
Additional Documentation
You can find more information on using Mastercam in the following materials, located in the
\Documentation folder of your Mastercam installation:
Mastercam X4 Installation Guide
Mastercam X4 Administrator Guide
Mastercam X4 Quick Start
Mastercam X4 Reference Guide
Mastercam X4 Transition Guide
Mastercam X4 Quick Reference Card
Mastercam X4 Wire Getting Started Guide
Version 9 to X Function Map
Section 1
Machining the Connector
6 • BASIC 3D MACHINING
LESSON 1
1Toolpath Setup
Before generating toolpaths for a part, you must select a machine definition. Defining stock creates
a visual representation of the stock placed in your machine. Creating and naming toolpath groups
will organize operations and maintain a logical structure for the part. This lesson covers these
topics.
Lesson Goals
Open a part file and assign a machine definition.
Define stock to be used in machining the part.
Rename toolpath groups.
Exercise 1: Assigning a Machine Definition
Toolpaths are organized in machine groups and toolpath groups. A machine group is created when
a machine definition is assigned. This exercise guides you through selecting a machine definition.
1 Open the tutorial part file Basic_3D_Machining_Part1_Start.MCX, which was provided
with the tutorial.
8 • BASIC 3D MACHINING
2 Click OK if prompted to switch to a metric
configuration.
3 Choose Machine Type, Mill, Default to
open the default Mill machine definition.
In Mastercam, you select a machine
definition before creating any toolpaths.
The machine definition is a model of your
machine tool’s capabilities and features. It
acts like a template for setting up
machining jobs.
Note: Parts that have previously been saved with a machine definition automatically load the
associated machine definition.
4 Choose File, Save As, and save the part under a different file name. This protects the
original tutorial file from being overwritten.
Exercise 2: Setting Stock for Machining
Define stock to help you more clearly visualize toolpaths. The stock can help to generate toolpaths,
or be used when backplotting or verifying toolpaths. This exercise guides you through creating a
stock boundary for your part.
1 In the Toolpath Manager, select Stock
setup. If necessary, click the [+] next to
Properties to expand the list.
The Machine Group Properties dialog box
opens to the Stock Setup tab.
2 Click Bounding box.
The Bounding Box dialog box opens.
Bounding box is a quick and convenient
method for creating stock around the outer
boundary of your geometry.
3 Set the options and parameters as shown,
then click OK.
SECTION 1: TOOLPATH SETUP • 9
4 Click OK in the Machine Group Properties
dialog box.
10 • BASIC 3D MACHINING
5 Press [Alt+F1], or right-click and select Fit, to fit the geometry to the screen.
6 Choose File, Save or click the Save button
to save the part with the machine
definition and defined stock.
Exercise 3: Creating Toolpath Groups
Toolpath groups aid in organizing toolpaths logically. A well organized part file makes it easy for
any user to understand the process involved in making the part. This exercise guides you through
creating and renaming toolpath groups.
1 In the Toolpath Manager, right-click
Toolpath Group-1, select Groups,
Rename.
SECTION 1: TOOLPATH SETUP • 11
2 Ty pe Interior and press [Enter].
3 In the Toolpath Manager, right-click on
Machine Group-1, select Groups, New
Toolpath Group.
The new toolpath group is named
Toolpath Group-1. If you create the second
toolpath group before renaming the first,
the new group is named Toolpath Group-2.
TIP: Right-clicking the machine group name creates the new toolpath group at the same
level in the tree as the Interior toolpath group. You can right-click Interior to create a new
toolpath group one level below Interior.
4 Ty pe Exterior and press [Enter].
The Toolpath Manager should look as
shown.
5 Choose File, Save or click the Save button
to save the part.
12 • BASIC 3D MACHINING
LESSON 2
2Roughing the Interior
The first toolpaths for a part typically involve removing large amounts of material. This is referred
to as roughing the part. This lesson guides you through several roughing toolpaths. These include
drilling the holes, roughing the inner pocket, roughing the inner slot, and rest roughing the interior
portion of the part.
Lesson Goals
Create a drill toolpath (including drill point selection, choosing tooling, and setting
machine values).
Create High Speed and surface roughing operations.
Create a High Speed rest roughing operation (including toolpath refinement).
Exercise 1: Drilling the Holes
1 In the Toolpath Manager, click the Move
insert arrow up one item button.
The Toolpath Manager should look as
shown after performing this step.
The insert arrow controls the location
where new toolpaths will be added to the
Too l pa th M an a ge r.
14 • BASIC 3D MACHINING
2 Right-click in the graphics window and
choose Isometric (WCS) from the menu to
view the part and toolpath in the isometric
view.
You may need to center the part in the
graphics window to see it. The easiest way
to do this is to use the graphics window
right-click menu and select Fit to fit the
part to the screen size [Alt+F1]. Then
unzoom using [Alt+F2]. You can also use
the fit/zoom/unzoom buttons in the View
Manipulation toolbar.
3 Choose Toolpaths, Drill.
4 Click OK when prompted to enter new NC
name.
The name displayed will be the name you
chose to save the file under. You may
change the NC file name now if necessary.
5 Use the default option for Select drill
point position in the graphics screen in
the Drill Point Selection dialog box.
SECTION 1: ROUGHING THE INTERIOR • 15
6 Select the arc centers of the four holes as
indicated.
The autocursor changes to indicate the arc
center as you approach.
7 Click OK in the Drill Point Selection dialog box.
The 2D Toolpaths dialog box opens to the Toolpath Type page. Drill is selected as the
toolpath type. (Do not click OK on the 2D Toolpaths dialog box until all pages are
complete.)
16 • BASIC 3D MACHINING
8 Select To o l from the Tree View pane on the
left.
9 Click the Select library tool button.
The default metric tool library opens.
10 Select the 10mm drill and click OK.
TIP: Use the default tool settings for the purposes of the tutorial. Tool speeds, feeds,
number, and other parameters should be changed to fit your machine and tooling before
cutting the part.
SECTION 1: ROUGHING THE INTERIOR • 17
11 Select Linking Parameters from the Tree View pane and enter values as shown.
These values will control the depth the tool will move to, where the top of stock is located,
as well as the height to retract the tool to.
12 Select Tip Comp from the Tree View pane.
Click the Tip Comp checkbox to activate
this feature. Use default values for the tip
comp parameters.
18 • BASIC 3D MACHINING
13 Click OK in the 2D Toolpath dialog box to generate the drill toolpath.
14 Click the Toggle toolpath display on
selected operations button. If necessary,
select the Drill/Counterbore operation.
The toolpath display for the Drill toolpath
is turned off. Perform this step after the
creation of each operation for clarity in
selecting geometry for subsequent steps.
15 Save your part file.
SECTION 1: ROUGHING THE INTERIOR • 19
Exercise 2: Roughing the Pocket
1 Choose Toolpaths, Surface High Speed.
2 If the New 3D Advanced Toolpath Refinement Feature! dialog box opens, select the
option to eliminate this dialog box and make refinement available for use. Click OK to close
the dialog box.
Note: This dialog box introduces the 3D Advanced Toolpath Refinement feature. Use this feature
to fine-tune your toolpath motion.
20 • BASIC 3D MACHINING
3 Follow the prompt to select drive surfaces as shown.
4 Press [Enter] or click the End Selection
button to accept the selection.
5 Click the Select button in the
Containment area of the Toolpath/Surface
selection dialog box.
The Chaining dialog box opens.
6 Click the C-plane radio button.
C-plane selection limits chaining to
entities that are parallel to the current
construction plane.
SECTION 1: ROUGHING THE INTERIOR • 21
7 Select the chain on the top of the part. The
selection can be in either direction for a
closed containment boundary.
8 Click OK on the Chaining dialog box to return to the Toolpath/Surface selection dialog box.
9 Click OK on the Toolpath/surface selection dialog box.
The Surface High Speed toolpaths dialog box opens on the Toolpath Type page.
10 Select Roughing and Area Clearance on
the Toolpath Type page.
11 Select To o l from the Tree View pane.
12 Click the Select library tool button. The
default metric tool library opens.
13 Select the 10mm bull endmill with 2mm
corner radius and click OK.
TIP: Adjust the Filter options on the right of
the dialog box to limit the types of tools
displayed.
22 • BASIC 3D MACHINING
14 Select Cut Parameters from the Tree View pane. Set the parameters as indicated.
Loading...