Jeff Quinn
Mastercam for SolidWorks Step by Step Programming Guide
TABLE OF CONTENTS
Page
Lesson 1:
Lesson 2:
Lesson 3:
Lesson 4:
Lesson 5:
Lesson 6:
Lesson 7:
Lesson 8:
Lesson 9:
Mastercam for SolidWorks—Getting Started
Contour Toolpaths—Part 1
Contour Toolpaths—Part 2
Pocket Toolpaths
Advanced Pocket Toolpaths
Manual Drill Toolpaths
FBM Drill Toolpaths
2D (HST) High Speed Toolpaths
Miscellaneous 2D Toolpaths
1 1
2 1
3 1
4 1
5 1
6 1
7 1
8 1
9 1

Lesson 10: FBM Mill Toolpaths
Lesson 11: 3D (HST) High Speed Toolpaths—Part 1
Lesson 12: 3D (HST) High Speed Toolpaths— Part 2
Lesson 13: Assembly Toolpaths: Configurations
Lesson 14: Assembly Toolpaths: Replacing Parts
Table of Contents
10 1
11 1
12 1
13 1
14 1
Mastercam for SolidWorks Step by Step Programming Exercises
LESSON 3 CONTOUR TOOLPATHS PART 2
INTRODUCTON:
This lesson builds on the basic procedures you were introduced to in the first Contour lesson. You will gain ex
perience in additional geometry selection (Chaining) techniques that will allow you to cut most Contour shapes
you come across. The toolpaths will consist of several new types of contours.
Overview of Exercise:
In this lesson we will machine the part shown by first Facing the 5.0 X 8.0 stock, then machining the yellow
areas shown by using several different types of 2D contour toolpaths and tools.
NEW CONCEPTS COVERED IN THIS LESSON:
ξ
ξ
ξ
ξ
ξ
ξ
ξ
Facing rough stock
Multi pass contour to cut an open pocket shape

Removing excess stock
Chamfer contour toolpath
Multiple techniques for contour chain selection
Chain Manager options
Review of basic Mastercam for SolidWorks general workflow procedures
Contour Toolpaths —Part 2 Lesson 3 Page 3—1
Mastercam for SolidWorks Step by Step Programming Exercises
Contour Toolpaths —Part 2 Lesson 3 Page 3—2
Mastercam for SolidWorks Step by Step Programming Exercises
Contour Toolpaths Additional Reference Information:
REFERENCE INFORMATION:
2D GEOMETRY SELECTION OPTIONS
Single Edge: Click the edge.
(The Mastercam Chain Manager gives the option to
automatically propogate along tangencies.)
Multiple Edges: CTRL-Click each edge.
(The Chain Manager will display all individual edges.
The CHAINS tab will show how Mastercam has
connected continuous edges into a single Chain.)
Select Tangency: Right Click on Edge and choose
the option from the menu.
(This will select all of the edges tangent to the one
highlighted and put them in the Selection list in the
Chain Manager.)
Contour Toolpaths —Part 2 Lesson 3 Page 3—3
Mastercam for SolidWorks Step by Step Programming Exercises
Select Loop: Right Click on Edge and choose the
option from the menu.
(This will select every connecting edge on a face,
whether tangent or not. If the wrong Loop is chosen

by SolidWorks, click the yellow arrow to toggle to the
other option.)
Partial Loop: Click the first entity, then CTRL-RIGHT
Click on the second entity to choose the option from
the menu. NOTE: When CTRL-RIGHT Clicking on
the second entity, you must select on the end of the
entity nearest the direction you want to close. For
more information, see the SolidWorks Help menu.
(This will allow a faster method of selecting a large
number of individual edges on complicated contours.)
Select Face: Click on a Face.
(This will select every individual edge on a face,
including interior edges, whether tangent or not. The
Chain Manager gives the option to use only outer loop
on faces. This is useful if you only want to cut the
outer shape.)
Contour Toolpaths —Part 2 Lesson 3 Page 3—4
Mastercam for SolidWorks Step by Step Programming Exercises
CONTOUR TOOLPATHS PART 2 TUTORIAL
Process Step 1: Prepare and Orient Model for
Machining
In this task you will choose the view to machine from
and locate part on the machine. Due to the shape of
the model, there is no good location for the origin. We
will use SolidWorks to create the origin location first.
1. Open the part “CONTOUR 2.SLDPRT”
2. From the SolidWorks Drop Down View Menu, make
sure View Sketches is selected.
(We will need to see Sketches in a later step.)
3. Select this face and select Insert Sketch from the

pop up icons or from the SolidWorks Insert menu.
(This will start a new sketch on this top face. The
following steps will have us create a single point at
the theoretical sharp corner of the stock. So we can
locate the machining origin where we want it.)
Contour Toolpaths —Part 2 Lesson 3 Page 3—5
Mastercam for SolidWorks Step by Step Programming Exercises
4. Rotate the model similar to the view shown and
select both of the edges by pressing the Control key
and selecting these two edges.
5. Select the Point icon from the SolidWorks Sketch
toolbar or from the drop down menu Tools – Sketch
Entities – Point, to create a point entity at the
intersection of the two lines.
(Note: You must select the (2) edges first to get
the point at the intersection.)
6. Exit the Sketch.
(Right Mouse Click and Select Icon.)
Contour Toolpaths —Part 2 Lesson 3 Page 3—6
Mastercam for SolidWorks Step by Step Programming Exercises
7. From the Mastercam drop down menu, select
View Manager.
8. View Manager Dialog settings:
9. Select the Geometry button.
10. Rotate the model as needed so you can pick the top
Solid Face to be the Machine View.
11. Rotate XY as desired for Direction.
(We will leave at 0° in this example.)
12. Click OK to accept.
13. Give the new view a Name.

(“2D Machining View” in this example.)
Contour Toolpaths —Part 2 Lesson 3 Page 3—7
Mastercam for SolidWorks Step by Step Programming Exercises
14. Set the Current View and Origin equal to this new
view by clicking the “EQUALS” button.
15. Select button to choose the desired Origin Point.
16. Select the sketch point previously created
as shown.
(In order to see this sketch Point,
View Sketches must be on. See Step # 2)
17. Click OK to accept.
18. Click OK to Accept again to exit and save the View
Manager settings dialog.
(The Mastercam Origin should be located on the
point entity as shown.)
Contour Toolpaths —Part 2 Lesson 3 Page 3—8
Mastercam for SolidWorks Step by Step Programming Exercises
Process Step 2: Create the Job Setup
In this task you will supply Mastercam with information
about tool information and stock size prior to beginning
the machining operations.
19. Select the Mastercam Toolpath Manager Icon from
the Property Manager page.
20. Expand the Properties in the Toolpath Manager.
(Click the plus (+) sign if the Files, Tool Settings
and Stock Setup icons are not visible.)
21. Select the Tool Settings icon
22. Change or confirm the highlighted parameters as
shown:
REFERENCE INFORMATION

For further information on other settings, see the
Mastercam Help file by clicking
Program # Identifies the program in the output NC
machine code.
Feed Calculation from tool uses the feed rate,
plunge rate, and spindle speed directly from the tool
definition.
Assign tool numbers sequentially assigns the next
available tool number. This option overrides the tool
numbers stored in the tool definition.
Warn of duplicate tool numbers informs you when
a duplicate tool number is entered and displays a
description of the duplicate tool.
Override defaults with modal values When
selected, the default values for any of the checked
items will be the value from the previous operation.
These override the values found in the toolpath
defaults file.
Contour Toolpaths —Part 2 Lesson 3 Page 3—9
Mastercam for SolidWorks Step by Step Programming Exercises
23. Select the Stock Setup tab.
24. Select the icon and then set the Stock View to the
previously created view. (“2D Machining View”)
25. Select the Bounding Box button.
26. Accept the default Bounding Box values as shown:
(In this example, the Stock size will be defined as
the extents of the solid model.)
27. Click OK to accept and close the Machine Group
Properties.
Contour Toolpaths —Part 2 Lesson 3 Page 3—10

Mastercam for SolidWorks Step by Step Programming Exercises
Process Step 3: Toolpath Selection and
Generation
During this section you will select the portions of the
solid model that CNC tool will cut. We will generate 5
separate operations to machine the part in this process
step. These will include:
Facing the Top of the Stock
Open Contour Toolpath with Multiple Passes
Partial Contour Toolpaths
Contour the Entire Outside Periphery
Chamfer the top edge
Facing the Top of the Stock
28. Select Facing Toolpaths from the Mastercam
Drop Down Menu or Command Manager.
(Facing operations will machine the entire top
surface of the model to prepare for subsequent
operations.)
29. Rotate model as needed and select the top face as
shown:
(Note: In this example, the shape is simple enough
to allow selecting the top face. In other cases,
additional sketching may be required to define the
stock shape for the facing operation.)
30. Click OK to accept and close the Chain Manager.
(In facing operations, the entire boundary must be
closed and the facing tool cuts inside the boundary,
so chaining direction and cut side is not required to
be set in this example.)
Contour Toolpaths —Part 2 Lesson 3 Page 3—11

Mastercam for SolidWorks Step by Step Programming Exercises
31. When prompted, enter a name for the NC program
we are going to create.
(“CONTOUR 2” is used in this lesson.)
32. Click OK to accept and close the NC name dialog
box.
33. Facing Toolpath Parameters Dialog Box Preview:
(In the following steps we will be setting the
parameters to make our Facing toolpath.)
34. Toolpath Type:
Facing
35. Tool:
Select Library Tool
(We will choose a 2” Face Mill from the Library of
tools provided by Mastercam.)
Contour Toolpaths —Part 2 Lesson 3 Page 3—12
Mastercam for SolidWorks Step by Step Programming Exercises
36. Select the Filter button.
(The Filter button will allow searching through the
tool library for a specific tool type to make it easier
and quicker to find the desired tool.)
37. Select the None button.
(This will de select all tool types to clear the filter.)
38. Select the Face Mill tool type.
(You can hover your cursor over the icons to see
what tool type is represented by each icon.)
39. Confirm that the rest of your settings match the
screenshot as shown and click OK to accept.
40. Select the 2” Face Mill from the filtered list and
click OK to accept.

41. Other Tool settings:
(Tool numbers should be automatically assigned
from our Job Setup settings.)
Rapid Retract = Selected
Comment: (Enter a description of what the toolpath
does. This will be part of the NC program to assist
the operator of the machine identify what this part
of the program does.)
In this example we inserted “FACE OFF THE TOP OF
THE STOCK”
Contour Toolpaths —Part 2 Lesson 3 Page 3—13
Mastercam for SolidWorks Step by Step Programming Exercises
42. Cut Parameters:
Style = Zigzag
Across overlap = 25%
Along overlap = 110%
Approach distance = 0
Exit distance = 0
Move between cuts = High speed loops
43. Linking Parameters values:
Clearance = 2.0 (Absolute)
Retract = .25 (Absolute)
Feed Plane = 0.1 (Incremental)
Top of Stock = 0.0 (Absolute)
Depth = 0.0 (Absolute)
(Depth value is set from the value of the selected
faces. In this case, Absolute depth of the top face is
at Z 0.0)
44. Set Coolant value:
Flood = ON

45. Click OK to accept the Facing Toolpath parameters
Contour Toolpaths —Part 2 Lesson 3 Page 3—14
Mastercam for SolidWorks Step by Step Programming Exercises
46. Results of Facing parameters:
47. Select the Operation and Backplot and/or Verify
the toolpath operation to confirm your results.
Open Contour Toolpath with Multiple Passes
(In this operation we will remove the cutout area using
Contour toolpath.)
Contour Toolpaths —Part 2 Lesson 3 Page 3—15
Mastercam for SolidWorks Step by Step Programming Exercises
48. Before starting the next operation, turn off the
toolpath display for the Facing operation.
(This will remove selected toolpaths to make it
easier to view and select the model edges for the
next operation.)
49. Select Contour Toolpaths from the Mastercam X4
Drop Down Menu or from the Command Manager.
50. Rotate the model as shown, then Right Mouse Click
on the edge Shown and choose Select Tangency.
(We are using the SolidWorks selection option to
select all of the entities that are Tangent to this
edge instead of selecting each entity individually.)
Contour Toolpaths —Part 2 Lesson 3 Page 3—16
Mastercam for SolidWorks Step by Step Programming Exercises
51. Results:
(You should have 5 edges in the selection list. If you
do not have all 5, you may select the missing edge
from the model or Right Mouse click in the box and
Clear Selections to try again.)

52. Select Chains tab in the Chain Manager.
(Notice that all 5 edges have been combined into
one continuous chain automatically by Mastercam
for SolidWorks.)
53. Click on “Chain 1” in the Chains Selection box.
Contour Toolpaths —Part 2 Lesson 3 Page 3—17
Mastercam for SolidWorks Step by Step Programming Exercises
54. Verify the Direction of cut and Cut side of the
selected chain by selecting the icons.
(Match screenshot shown to Climb Cut
the contour.)
REFERENCE INFORMATION
Change Sides changes which side of the
selected chain the cutter will travel.
Delete Chain deletes the currently selected
chain(s) from the list.
Analyze Chain provides technical information
about the selected chain.
Reverse Chain changes the selected chain cut
direction.
Rename Chain allows changing the name from
Chain #1, etc. to a more meaningful name to
help user recall the purpose of the chain.
Start Point allows user to change the start
point by scrolling through each possible chain
point.
End Point allows user to change the end
point by scrolling through each possible chain
point.
55. Click OK to accept the Chains and close the Chain

Manager.
56. Contour Toolpath Parameters Dialog Box:
(In the following steps we will be setting the
parameters to make our toolpath.)
57. Toolpath Type:
Contour
Contour Toolpaths —Part 2 Lesson 3 Page 3—18
Mastercam for SolidWorks Step by Step Programming Exercises
58. Tool:
Select Library Tool
(We will choose a ½” Flat Endmill from the
Library of tools provided by Mastercam.)
59. Select the Filter button.
(The Filter button will allow searching
through the tool library for a specific
tool type to make it easier and quicker
to find the desired tool.)
60. Select the None button.
(This will de select all tool types to clear the filter.)
61. Select the Flat Endmill tool type.
(You can hover your cursor over the icons to see
what tool type is represented by each icon.)
62. Confirm that the rest or your settings match the
screenshot as shown and click OK to accept.
Contour Toolpaths —Part 2 Lesson 3 Page 3—19
Mastercam for SolidWorks Step by Step Programming Exercises
63. Select the 1/2 Flat Endmill from the
filtered list and click OK.
64. Other Tool settings:
Rapid Retract = Selected

Comment: “REMOVE THE OPEN POCKET AREA”
65. Cut Parameter Settings:
Compensation = Wear
Stock to leave on walls = .005
(We will leave .005 for final clean up contour
operation we will add later. Confirm other settings
match the default values as shown.)
Contour Toolpaths —Part 2 Lesson 3 Page 3—20
Mastercam for SolidWorks Step by Step Programming Exercises
66. Lead In/Out Settings:
Lead In/Out = Selected
Entry = Selected
Entry Line Tangent = 30%
Entry Arc Radius = 30%
Select the Double Arrow to copy all values to the
Exit Values.
67. Set Break Through values as shown:
Break through = Selected
Break through amount = 0.05
68. Set Multi Passes settings as shown:
Multi Passes = Selected
Rough = 3
Spacing = .25
Finish = 0
Spacing = 0
Keep tool down = Selected
(Since there is no danger of cutting through the part
in this toolpath, it is more efficient to keep the tool
down.)
Contour Toolpaths —Part 2 Lesson 3 Page 3—21

Mastercam for SolidWorks Step by Step Programming Exercises
69. Set the Linking Parameters values as shown:
Clearance = 2.0 (Absolute)
Retract = .25 (Absolute)
Feed Plane = 0.1 (Incremental)
Top of Stock = 0.0 (Absolute)
Depth = 0.0 (Incremental)
(Depth value is set from the value of the chained
edges. Incremental value is used in case there are
multiple edges are at different depths. Incremental
values always display 0.0)
70. Set Coolant value:
Flood = ON
71. Click OK to accept the Contour Toolpath Parameters.
72. Results:
Contour Toolpaths —Part 2 Lesson 3 Page 3—22
Mastercam for SolidWorks Step by Step Programming Exercises
73. Select the Operation and Backplot and/or Verify
the toolpath operation to confirm your results.
(If your verify does not look like this result, click the
Parameters icon under the Contour operation in the
Mastercam Operations Manager and confirm your
settings are correct. Then Regenerate the toolpath.)
Partial Contour Toolpaths
(In this Contour operation we will remove the excess
material at the four corners of the stock.)
74. Before starting the next operation, turn off the
toolpath display for the Contour operation you just
completed.
75. Select Contour Toolpaths from the Mastercam

Drop Down Menu or from the Command Manager.
Contour Toolpaths —Part 2 Lesson 3 Page 3—23