Hướng dẫn sử dụng phần mềm Mastercam X3 - P1

4 & 5 Axis Mill Training Tutorials
To order more books:
Call 1 800 529 5517 or
Visit www.inhousesolutions.com or
Contact your Mastercam Dealer

Mastercam X³ Training Tutorials – 4 & 5 Axis Mill Applications
Revised Date: September 26, 2008
Copyright © 1984 2008 In House Solutions Inc. All rights reserved.
Software: Mastercam X³ Mill
Authors: Mariana Lendel
ISBN: 978 1 894487 99 3
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 distributor, 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 the copyright laws of Canada and the United States. All rights are
reserved. This document may not, in whole or part, be copied, photocopied, 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;
Mastercam Verify is created in conjunction with Sirius Systems Corporation; Windows 95, and Windows
NT; Windows XP are registered trademarks of Microsoft Corporation.

TABLE OF CONTENTS
Getting Started .............................................................................................................A 1
Axis Substitution, Rotary Axis Positioning and Transform Rotate Tutorial ................... 1 1
Axis Substitution To Create A Cylindrical And A Conical Helix Tutorial ...........................2 1
Axis Substitution, Rolldie C Hook Tutorial .....................................................................3 1
Chuck Indexing Tutorial ................................................................................................4 1
Rotary4 Axis Toolpath And Axial 4ax Tutorial................................................................5 1
Curve 5 Axis And Drill 5 Axis Tutorial ............................................................................6 1
Swarf 5 Axis With Wall Defined By Using 2 Contours Tutorial........................................7 1
Flow 5 Axis Tutorial ......................................................................................................8 1
Multisurface 5 Axis Tutorial ..........................................................................................9 1
Port 5 Axis Tutorial ................................................................................. 10 1
General Notes ....................................................................................... B 1
TUTORIAL SERIES FOR
CHUCK INDEXING TUTORIAL
4/5 Axis TUTORIAL 4
Objectives:
The Student will design a 3 dimensional drawing by:
Creating the 2D geometry in the Right Side view.
Creating the 3D geometry using translate command.
Creating circles knowing the diameter and the center location.
Changing the view of the part for better visualisation.
The Student will create a 2 dimensional milling toolpath in different Tplanes consisting of:

Using View Manager to select the Tplane for each face.
Create an operation for each face using the same work offset (G54).
Facing one flat surfaces.
Facing the other two flat surfaces using Transform Rotate toolpath.
Drilling the two holes.
Removing the material inside of one groove using contour toolpath.
Machine the second groove using Transform Rotate toolpath.
The Student will check the toolpath using Mastercam’s Verify verification module by:
Defining a 3 dimensional block, the size of the workpiece.
Running the Verify function to machine the part on the screen.
Page 4 2
4/5 Axis
Page 4 3
TUTORIAL 4
4/5 Axis TUTORIAL 4
GEOMETRY CREATION
STEP 1: CREATE THE 2D GEOMETRY IN THE RIGHT SIDE VIEW.
Option 1 The geometry file, Tutorial4_geometry.zip, can be downloaded from
www.emastercam.com/files
The finish part, Tutorial4_finish.zip including the toolpaths, is also provided on the same location
www.emastercam.com/files
Option 2 Create the geometry using the following instructions:
Create the 2D profile in the Righ side view:
Create/Arc/ Create Circle Center Point and set parameters to:
Diameter = 5.0;
Center Origin
Create/Line/ Create Line Endpoint and set parameters to:
Specify an endpoint = Origin
Line length = 2.45
Angle = 165 deg.;

Create/Line/ Create Line Perpendicular and set parameters to:
Select line, arc or spline; Select the existing line
Sketch a point; Select the Endpoint of the existing line opposite the origin.
Select which line to keep; Select the line above the existing one.
Repeat the steps to select the other perpendicular line below the first line that we created.
Delete the first line
Edit/Join entities
Select the two colinear lines; Press enter to finish the command
Edit/ Trim/Break/ Trim/Break/Extend
Enable divide and select the arc left to the line and the two ends of the line.
Select these lines and
the arc here
Xform/ Xform Rotate
Select the line; Enable Copy and set # to 1; Rotation angle 90 deg
Xform/ Xform Rotate
Select the rotated line; Enable Copy and set # to 1; Rotation angle 105 deg
Page 4 4
4/5 Axis
Edit/ Trim/Break/ Trim/Break/Extend
Enable divide and select the two arcs one below and
the other one to the right of the rotated lines.
Select Entity A here
TUTORIAL 4
Create/Line/ Create Line Endpoint and set
parameters to:
Specify an endpoint = Origin
Line length = 2.5
Angle = 120 deg.;
Create/Line/ Create Line Parallel and set parameters to:
Select a line; Select the 120 deg line

Select the point to place a parallel line through; Pick a point above the line; enter the distance 0.25
Select the flip buton several times until you make both parallel lines (above and below the 120 deg. line)
Edit/ Trim/Break/ Trim/Break/Extend
Enable Break in the ribbon bar.
Select an entity to break; Select the first parallel line end that is further away from the origin.
Enable the length button in the Ribbon bar and enter 0.25
Repeat the command to break at 0.25 distance the other parallel line that we created in the previous
step
Delete the center line and the parallel lines closes to the origin.
Select these entities
Create/Line/ Create Line Endpoint and set parameters to:
Select the endpoints of the parallel lines left to close the slot.
Edit/ Trim/Break/ Trim/Break/Extend
Enable Divide in the ribbon bar.
Select the arc between the two parallel lines.
Edit/ Trim/Break/ Trim/Break/Extend
Enable Trim 2 entities in the ribbon bar.
Select the entities at the top corners of the slot.
Xform/ Xform Rotate
Select the three lines of the slot; Enable Copy and set # to 1; Rotation angle 180 deg
Edit/ Trim/Break/ Trim/Break/Extend
Enable Divide in the ribbon bar.
Page 4 5
4/5 Axis
Select the arc between the two parallel lines that you rotated in the previous step.
Create the cylindrical shape
Xform/ Xform Translate
Select all entities;
Enable Join; # =1;z = 6.0
Create the circles in the Front plan

TUTORIAL 4
Set the plane to Front.
Select Entity A
Set the Z depth at the holes plane. ( 2.45)
Create/Line/ Create Line Parallel and set parameters to:
Select a line; Select line A as shown
Select the point to place a parallel line through; Pick a point below the line; enter the distance 0.50
Select a line; Select line B as shown
Select Entity B
Select the point to place a parallel line through;
Pick a point to the right of the line; enter the distance 1.50
Select a line; Select line C as shown
Select the point to place a parallel line through; Pick a point
to the left of the line; enter the distance 1.50
Select Entity C
Create/Arc/ Create Circle Center Point and set parameters to:
Diameter = .375;
Center at intersection between two of the lines created in the previous step.
Diameter = .375;
Center at intersection between two of the lines created in the previous
step.
Delete the construction lines
File/Save as
File Name: Tut4_Rotary axis indexing.mcx
Page 4 6
4/5 Axis TUTORIAL 4
TOOLPATH CREATION
STEP 5: DEFINE THE STOCK.
To display the Toolpaths Manager press Alt + O.
If a machine definition is already selected see Tutorial # 2 page 2 4 to learn how to change it.

Otherwise follow next step.
Set the construction plane to Top Plane.
Select Mill 4 AXIS VMC.MMD
Page 4 7
4/5 Axis
Select the plus in front of Properties to expand the Toolpaths Group Properties.
Select the plus
Select the Stock setup.
Select Stock setup
The stock shape should be set to
Cylinder.
Enable X Axis
Enter the Diameter and Length values
of the stock size.
Enable Display stock as Wireframe
and enable Fit Screen to the stock.
The Stock Origin values adjust the
positioning of the stock, ensuring
that you have equal amount of
extra stock around the finish part.
Display options allows you to set
the stock as Wireframe and to fit
the stock to the screen.(Fit
Screen)
Page 4 8
TUTORIAL 4
4/5 Axis
Select the Tool Settings tab to set the tool parameters and the part material.
Change the parameters to match the following screenshot.
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 OK button to exit Toolpath Group Properties.
Page 4 9
TUTORIAL 4
4/5 Axis TUTORIAL 4
STEP 6: FACE THE FLAT SURFACE AT 165 DEGREES ANGLE.
6.1 About Tool Planes
The tool plane (Tplane) is the plane in which the tool approaches and machines the part. The
Tplane represents the CNC machine’s coordinate system (XY axis and origin). This is the cutting
plane for a toolpath, typically normal to the tool axis
The Rotary axis for our part is A axis. The axis orientation for different views should look as shown
in the following picture.
Compare the planes axis orientation when rotating the part about B axis. (horizontal machining
centers).

Page 4 10
4/5 Axis TUTORIAL 4
6.2 Create the new view at 165 degrees angle.
Select WCS in the Status Bar.
Select View Manager.
Select Geometry button.
[Select a flat entity, 2 lines, or, 3 points]: Select the two lines as shown in the following picture
Select the second line here
Select the first line here
Page 4 11
4/5 Axis TUTORIAL 4
The axis should be orientated as shown in the following picture. Otherwise select Next View
Select Next View
Select the OK button to accept the view.
Enter the Name for the new view as
shown.
Disable Associative and Set new origin.
Select the OK button to exit.
Change the
parameters to match
the following
screenshot.
Make sure that X, Y, Z
for the Origin are set
to 0 and Associative
is disable.
The Work Offset #
should be change to
0 (G54 for Fanuc).
We will set only one

work offset at the center
of the cylinder.
Page 4 12
4/5 Axis TUTORIAL 4
6.3 Set both Cplane and Tplane to the flat at 165 degrees angle.
Click on Set your current tool plane and origin to the selected view button.
Click on Set your current construction plane and origin to the selected view button.
The View Manager will
look as shown to the right
Select the OK button to exit the View Manager name.
Set Z to 0.
The grid orientation and origin should look as shown in
the following picture.
Page 4 13
4/5 Axis
6.3 Face the plane.
Toolpaths
Face toolpath
Select the OK button to accept the NC name.
Enable C plane in the Chaining dialog box.
[Select OK to use the defined stock or select chain 1]:Select the
chain as shown
Select the
chain here
Select the OK button to exit Chaining.
Click on the Select library tool button.
Select the Filter button in the Tool Selection.
Page 4 14
TUTORIAL 4
4/5 Axis

In the Tool Types field select the None button to disable all tools.
Select the Face mill tool type as shown.
In the Tool Diameter field click the pull down arrow and select Equal.
Enter the Tool Diameter value to 3.0.
Select the OK button to exit Tool List Filter.
Make sure that the tool is selected (highlighted) in the Tool Selection screen.
Select the OK button to exit the Tool Selection dialog box.
Make the necessary changes to match the parameters with the screenshot below.
Page 4 15
TUTORIAL 4
4/5 Axis TUTORIAL 4
The Tool parameters dialog box allows you to select the tool used in this operation. It also allows you to
change the Spindle speed, the Feed rate, Plunge rate and Retract rate. You can insert a comment that will be
output in the NC file after running the post processor.
Select the Facing parameters and change the parameters as shown in the following screenshots.
Make sure that
you change the
Cutting
method to One
pass.
The Facing parameters dialog box allows you to establish the heights for rapid movement (Clearance)and
(Retract); the height from where the tool moves with feedrate (Feed plane); the Top of stock and the final
depth (Depth). Depth and Top of Stock set to Incremental values are relative to the location of the chained
geometry. Clearance, Retract, and Feed plane are relative to the Top of stock.
Select the OK button from the Facing
parameter screen.
Page 4 16
4/5 Axis TUTORIAL 4
STEP 7: FACE THE FLAT AT 255 DEGREES ANGLE USING ROTATE TRANSFORM
TOOLPATH.

Toolpaths
Transform Toolpath
Enabled Rotate and the Method should be set to Tool plane to be able to create a new tool plane
for the transform toolpath.
Enable Maintain source operation’s to keep the same Work offset number.(G54).
Note that the Facing operation is selected
Page 4 17
4/5 Axis
Select Rotate tab and change the parameters as shown.
Enable Rotation view and select the arrow button.
Select the Right Side View.
Select the OK button to exit View Selection
Select the OK button to exit Transform Operation
Parameters
Page 4 18
TUTORIAL 4