Basic 2D
Machining
mastercam x getting started series tutorials
Basic 2D
Machining
October 2010
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 2D MACHINING
Mastercam® X5 Basic 2D Machining
Date: October 2010
Copyright © 2010 CNC Software, Inc.— All rights reserved.
First Printing: October 2010
Software: Mastercam X5
Part Number: X5-PDF-TUT-2M
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
1. Drilling Holes............................................................... 5
III
Tutorial Goals................................................................................... 2
Before You Begin............................................................................. 2
If You Need More Help.................................................................... 3
Additional Documentation.............................................................. 4
Lesson Goals.................................................................................... 5
Exercise 1: Assigning a Machine Definition.............................. 5
Exercise 2: Setting Up Stock ....................................................6
Exercise 3: Drilling Four Holes ..................................................8
2. Roughing Outside the Part ......................................... 15
Lesson Goals..................................................................................15
Exercise 1: Creating a Dynamic Mill Toolpath......................... 15
Exercise 2: Viewing Your Toolpaths........................................ 23
Exercise 3: Creating a Contour Toolpath................................. 23
3. Machining Inside the Part.......................................... 29
Lesson Goals..................................................................................29
Exercise 1: Creating a Dynamic Mill Toolpath......................... 29
Exercise 2: Creating a Slot Mill Toolpath ................................ 34
4. Previewing Toolpaths ................................................ 39
Lesson Goals..................................................................................39
Exercise 1: Backplotting All Toolpaths.................................... 39
Exercise 2: Verifying All Toolpaths.......................................... 42
5. Posting Toolpaths ...................................................... 45
Lesson Goals..................................................................................45
Exercise 1: Posting All Toolpath Operations ........................... 45
IV • BASIC 2D MACHINING
Conclusion...............................................................................................48
Post Processing Summary: Sending NC Files to Machine ....... 48
INTRODUCTION
This tutorial focuses on applying several mill toolpaths to a part previously designed in Mastercam.
The tutorial then guides you through the steps to take that toolpath data and create NC code to
machine the part.
Mastercam offers a variety of toolpath types that let
you quickly build toolpaths for specific
applications. You access these toolpaths, such as
the mill toolpaths shown here, through the
Toolpa th s menu.
After you create a toolpath, you can use
Mastercam's backplot feature to preview its
operation on the screen. Once you are satisfied
with it, post it from the Toolpath Manager to
generate the NC code for a specific machine tool.
When you first begin this tutorial, you will be
prompted to assign a machine definition to the
part. This tutorial does not go into any depth on
machine and control definitions. However, the
Help and other documentation installed with
Mastercam provide comprehensive information
regarding these Mastercam features.
When you finish this tutorial, your part will look like this:
If you would like to design (create) the part before you begin this tutorial, please follow the Basic 2D
Design tutorial procedures (published separately in document #X5-PDF-TUT-2D).
2 • BASIC 2D MACHINING
Tutorial Goals
Open a part file, assign a default machine definition, and set up stock.
Create four drill holes with one toolpath (including selecting a drill point, choosing tooling,
using tool tip compensation, and setting machining values).
Rough the outside of the part (including chaining entities, selecting tooling, and setting
machining values).
Clean out the inside of the part (including chaining entities, choosing tooling, and setting
machining values).
View all toolpaths in the graphics window.
View a specific toolpath by temporarily turning off the display of selected toolpaths.
Backplot (view the path the tools take to cut the part) all toolpaths.
Customize your backplot display.
Simulate (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 Series 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.
IMPORTANT: Screen colors in the tutorial pictures were modified to enhance image
quality; they may not match your Mastercam settings or the tutorial results. These color
differences do not affect the lesson or the exercise results.
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.
®
operating system.
INTRODUCTION • 3
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 X5 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.
®
Flash® compatible video
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.
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 ...\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:
4 • BASIC 2D MACHINING
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.
Additional Documentation
You can find more information on using Mastercam in the following materials, located in the
\Documentation folder of your Mastercam installation:
Mastercam X5 Installation Guide
Mastercam X5 Administrator Guide
Mastercam X5 Quick Start
Mastercam X5 Reference Guide
Mastercam X5 Transition Guide
Mastercam X5 Quick Reference Card
Mastercam X5 Wire Getting Started Guide
Version 9 to X Function Map
Mastercam X5 NCI & Parameter Reference
Mastercam X5 Post Debugger User’s Guide
LESSON 1
1Drilling Holes
The first step to machining the tutorial part is to drill the four holes. By beginning with drilling, you
can then use the holes to fixture the part on the machine tool.
Lesson Goals
Open a part file and assign a machine definition.
Define stock.
Create a drill toolpath (including selecting drill points, choosing tooling, and setting
machining values).
Use tool tip compensation.
Exercise 1: Assigning a Machine Definition
In this exercise, you open an existing part, assign a machine definition to the part, and save it under
a new file name.
1 Start Mastercam.
2 From the Mastercam menu bar, choose File, Open.
3 Open BASIC_2D_MACHINING_START.MCX-5, which was provided with this tutorial.
4 Click OK if prompted to switch to a metric
configuration.
5 Press [Alt +S] to shade the part for easier
viewing.
6 From the Mastercam menu, 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
and acts like a template for setting up
machining jobs.
6 • BASIC 2D MACHINING
Note: Parts that have previously been saved with a machine definition automatically load the
associated machine definition.
7 Choose File, Save As and save the part under a different file name than the original file.
This will protect the original tutorial file from being overwritten.
Exercise 2: Setting Up Stock
In this exercise, you define the stock model from which your part is cut. Stock models help you
visualize your toolpaths more realistically. The stock model you define can be displayed with the
part geometry when viewing the file or toolpaths, during backplot, or while verifying toolpaths.
1 In the Operations Manager, click on the
plus sign (+) next to Properties - Mill
Default MM.
It changes to a minus sign (-) and displays
the machine group properties. Machine
groups are created automatically and
displayed in the Toolpaths Manager when
you select a machine from the Machine
Type menu. They include job setup
information for toolpaths, such as tool
numbering, stock models, material
selection, and toolpath defaults and
libraries.
2 Click the Stock Setup icon to display the
Stock Setup tab in the Machine Group
Properties dialog box.
DRILLING HOLES • 7
3 Click the Select corners button near the bottom of the dialog box. Mastercam brings you
back to the graphics window to select the two opposite stock corners.
4 Click the two opposite corners as shown in the following picture. The Stock Setup tab
displays again with X and Y coordinate values from the selected corners.
5 Enter 25 for the Z coordinate in the stock diagram to provide some depth for your stock.
6 Select the Display check box to see the stock model boundaries in the graphics window.
8 • BASIC 2D MACHINING
7 Click OK to complete the stock setup. The stock displays as dashed red lines around the
part.
Exercise 3: Drilling Four Holes
In this exercise, you create a drill toolpath that drills all four holes of the part.
Selecting the Drill Holes
1 From the Mastercam menu, choose
Toolpaths, Drill. The Drill Point Selection
dialog box opens.
Note: You may be prompted for an NC file
name. If prompted, click OK to confirm the
default NC file name, or overwrite the file
name and click OK to modify the default file
name.
DRILLING HOLES • 9
2 Right-click in the graphics window and
choose To p ( W C S ) to switch to a Top
graphics view. This will make it easier to
select the drill holes.
3 Click each of the center points of the four holes of the part. Choose them in a clockwise
order from top left to bottom left as shown in the numbered sequence below.
TIP: When you get close to each hole’s center point, Mastercam displays a Visual Cue that
indicates the center point.
4 Click OK. The 2D Toolpaths - Drill/Circles dialog box opens.
10 • BASIC 2D MACHINING
Page viewTree view area
Quick
View
Settings
area
Exploring the Toolpath Dialog Boxes
Many Mastercam toolpaths, including Drill, use a tree-style dialog interface made up of
three distinct areas:
Tree View - Displays a list of all the available dialog box property pages.
Inactive pages are marked with a red circle and a slash.
Edited pages are marked with a green check mark.
Some pages may have a plus or minus symbol, indicating that the page has subpages
and can expand and contract to either display or hide the subpages.
Page View - Changes with each selection you make in the Tree View area.
Quick View Settings - Summarizes key toolpath information from parameters you set on
the different pages. It updates automatically as you make changes in the pages, and is
always visible.
DRILLING HOLES • 11
1 Click on the Circle Mill toolpath type icon.
This changes the toolpath to a circle mill
toolpath and changes the pages listed in
the Tree View area.
Notice that the Toolpath Type page in the
Tree View area now has a green check
beside it, indicating that you made a
change on that page.
2 Click the Drill toolpath type icon to change
back to a drill toolpath.
3 Click the Cut Parameters page in the Tree View list. The Page area changes to list cut
parameters for the toolpath.
Setting Drilling Parameters
1 Click the To o l page in the Tree View list to pick a tool for the drill toolpath.
2 Click the Select library tool button to pick
a tool from one of Mastercam’s tool
libraries.
The Tool Selection dialog box opens.
Loading...