TRAINING

GUIDE

LATHE-LESSON-3
FACE, ROUGH, FINISH, DRILL,
TAPPING AND CUTOFF
Mastercam Training Guide
Objectives
You will create the geometry for Lathe Lesson 3, and then generate a toolpath to machine the
part on a CNC lathe. This lesson covers the following topics:

 Create a 2-dimensional drawing by:

Creating lines.
Creating fillets.
Creating chamfers.

 Establish Stock and Chuck Setup settings:

Stock size.
Chuck Configuration.
Material for the part.
Feed calculation.

 Generate a 2-dimensional lathe toolpath consisting of:

Lathe Face.
Lathe Quick Rough.
Lathe Quick Finish.
Lathe Drill and Tap.
Lathe Cutoff.

 Inspect the toolpath using Mastercam’s Verify and Backplot by:

Launching the Verify function to machine the part on the screen.
Generating the NC- code.

Lathe-Lesson-3-1
 Lathe-Lesson-3

LATHE - LESSON - 3 DRAWING

Lathe-Lesson-3-2
Mastercam Training Guide
TOOL LIST
Six tools will be used to create this part.
 Tool #1 Face and Rough the outside diameters
Holder: Outside Diameter Rough Right Hand - DCGNR-164D.
Insert: 80 Degree Diamond Insert – CNMG-432

 Tool #2 Finish the outside diameters

Holder: Outside Diameter Finish Right Hand - MVJNR-164D.
Insert: 35 Degree Diamond Insert – VNMG-431.

 Tool #3 Spot drill the hole

Spot Drill – body diameter 0.500”

 Tool #4 Tap Drill the .3125 diameter hole

Drill 0.3125” diameter

 Tool #5 Tap the .375-16 hole

Right Hand Tap 3/8”-16UNC

 Tool #6 Cutoff the part

Holder: Outside Diameter Cut-off Right Hand.
Insert: 0.125” Wide.

Lathe-Lesson-3-3
 Lathe-Lesson-3

LESSON - 3 - THE PROCESS

Geometry Creation
TASK 1: Setting the Environment
TASK 2: Setting the Construction Planes
TASK 3: Create the Geometry
TASK 4: Create the 18 Degree Angle
TASK 5: Create the Fillets (Radius)
TASK 6: Create the Chamfer
TASK 7: Save the Drawing
Toolpath Creation
TASK 8: Define the Stock and Chuck Parameters
TASK 9: Face the Front of the Part
TASK 10: Rough the Outside Diameters
TASK 11: Finish the Outside Diameters
TASK 12: Spot Drill the 5/16” Hole
TASK 13: Drill the 5/16” Hole
TASK 14: Tap the 3/8”-16 Hole
TASK 15: Cut off the Part
TASK 16: Verify the Toolpaths
TASK 17: Save the Updated Mastercam File
TASK 18: Post and Create the CNC Code File

Lathe-Lesson-3-4
Mastercam Training Guide

Geometry Creation
TASK 1:
SETTING THE ENVIRONM ENT
Before starting the geometry creation, you should set up the grid machine type as outlined in the
Setting the Environment section at the beginning of this text:
1. Set up the Grid. This will help identify the location of the origin.
2. Set the Machine Type to the Lathe Default.

TASK 2:
LATHE CONSTRUCTION PLANES:
 Check that the Construction Plane is set to Lathe diameter +D +Z
1. Select the View tab and in the Managers section, ensure the Planes Manager is enabled.
Using the tabs in the lower left corner, click on Planes.
Once your machine is selected,
Mastercam includes special lathe
construction planes that let you work in
radius or diameter coordinates.

For conventional 2D turning applications,

use the Planes Manager to select the
desired coordinate system, as shown
below right.

Choose to use either radius or diameter

coordinates and then choose the desired
X/D and Z directions.

2. On the Planes Manager, from the pulldown uncheck Tplane follows Cplane and then set
the C column (Construction Plane) to the +D +Z Plane (leave the WCS is set to Top).
+D+Z allows you to create
the geometry of the part in
diameter dimensions instead
of radius dimensions. If you
prefer to use radius, choose
+X+Z from the Lathe Planes
pulldown.

For more information on

Lathe Planes, see the video
in the Tips and Techniques
section.

 Also, make note of the Status bar at the bottom of the screen CPLANE:+D+Z TPLANE:
Top WCS:Top as shown below right.

Lathe-Lesson-3-5
 Lathe-Lesson-3

TASK 3:
CREATE THE GEOMETRY
 This task explains how to create the geometry of this part. In this lathe part you only need to
create half of the geometry, the geometry above the center line.
 Lines 1 through 9 will be created first and then the fillet and chamfer will be created.

 Create Line #1
1. Select the Wireframe tab at the top of the screen and in the Lines section click on Line
Endpoints.

 On the graphics screen you are prompted: Specify the first endpoint and the Line
Endpoints panel appears.
Line Endpoints
Use this function to create single lines with two
endpoints, or multiple lines connected at their
endpoints.

Simply click in the graphics window to set the

two endpoints; or enter values in the Length
and Angle fields, and then click in the graphics
window to position the line.

Lathe-Lesson-3-6
Mastercam Training Guide
2. Move the cursor over the center of the grid and as you get close to the origin a visual cue

appears. This is the cue that will allow you to snap to the origin. With this visual cue
highlighted pick the origin.

AutoCursor: Visual Cues detects and highlights endpoints and midpoints of curves, lines, arc
center points, and point entities.

In addition, AutoCursor can snap to angle, nearest, tangent, perpendicular, horizontal, and
vertical conditions.

 The following are Mastercam Visual Cues:

3. You are next prompted to “Specify the second endpoint”. In the Line Endpoints panel
activate Multi-line and Freeform.
Multi-line
Let’s you create multiple lines connected at their
endpoints.

Enter a point for the first endpoint of the first line

and then a point for the second endpoint of the line.
That second point becomes the first endpoint of the
next line that you create.

Double-click the last point or press Escape to end

this function.

Freeform
Allows you to create the lien anywhere on the
plane.

4. You are still prompted to “Specify the second endpoint”. click the middle mouse button
and then hit the spacebar on your keyboard, the Fastpoint now opens. Type 0.6,0. This
is D0.6 Z0. Hit the Enter key when done.

Lathe-Lesson-3-7
 Lathe-Lesson-3

 A vertical line should be visible as shown below:

 Create Line #2
5. To satisfy the prompt “Specify the second endpoint” just type the coordinate, type 0.6,
-1.12 and hit the Enter key to complete this line.

 Create Line #3
6. To satisfy the prompt “Specify the second endpoint” just type the coordinate, type 1.0,
-1.85 and hit the Enter key to complete this line.

 Create Line #4
7. To satisfy the prompt “Specify the second endpoint” just type the coordinate, type 1.0,
-2.25 and hit the Enter key to complete this line.

 Create Line #5
8. To satisfy the prompt “Specify the second endpoint” just type the coordinate, type 1.23,
-2.25 and hit the Enter key to complete this line.

 Create Line #6
9. To satisfy the prompt “Specify the second endpoint” just type the coordinate, type 1.23,
-2.8 and hit the Enter key to complete this line.

10. Right mouse click in the graphics area and click on the Fit icon .
11. Right mouse click in the graphics area and click on Unzoom 80% to shrink the display.

Lathe-Lesson-3-8
Mastercam Training Guide
 Create Line #7
12. To satisfy the prompt “Specify the second endpoint” just type the coordinate, type 1.44,
-2.8 and hit the Enter key to complete this line.

 Create Line #8
13. To satisfy the prompt “Specify the second endpoint” just type the coordinate, type 1.44,
-3.0 and hit the Enter key to complete this line.

 Create Line #9
14. To satisfy the prompt “Specify the second endpoint” just type the coordinate, type 0, -
3.0 and hit the Enter key to complete this line.

15. Click on the OK icon to complete this feature.

16. Right mouse click in the graphics area and click on the Fit icon .

 Your geometry should look like the figure below.

Lathe-Lesson-3-9
 Lathe-Lesson-3

TASK 4:
CREATE THE 18 DEGREE ANGLE
 Create the 18 Degree Angle.

1. Click on Line Endpoints in the Lines section of the Wireframe tab.

2. In the Line Endpoints panel click in the space for Length and input 1.0. Hit the tab key and
for the Angle enter -18.0 and hit Enter.

3. You are prompted to “Specify the first endpoint”. Click on the endpoint of line 8 as shown
below.

 A new line is drawn as shown below.

4. Click on the OK icon to complete this feature.

Lathe-Lesson-3-10
Mastercam Training Guide
5. In the Wireframe tab click on Trim to Entities in the Modify section. Activate Trim 2
entities.

6. Click on line 1 and then line 2 as shown below.

 The line is trimmed as shown below. The line noted below will be deleted in the next step.

7. Click on the OK icon to complete this feature.

8. Click on the line as shown above and hit the Delete key on your keyboard.

Lathe-Lesson-3-11
 Lathe-Lesson-3

TASK 5:
CREATE THE FILLETS (RADIUS)

1. Select the Wireframe tab and in the Modify section click on Fillet Entities.

2. The Fillet Entities panel appears. If required activate the Method to Normal and enter a
value of 0.1 for Radius.
3. Ensure the Trim entities box at the bottom of the panel is check marked to turn the trim on.

Lathe-Lesson-3-12
Mastercam Training Guide
4. Move over to the graphic screen and for the prompt “Fillet: Select an entity” click on Line
1 and then for the prompt “Fillet: Select another entity” click on Line 2 as shown below.

5. Click on the OK and Create New Operation icon .

6. Click in the space for Radius, input 0.005 and then hit the Enter key.

7. For the prompt “Fillet: Select an entity” click on Line 1 and then for the prompt “Fillet:
Select another entity” click on Line 2 as shown below.

8. Click on the OK and Create New Operation icon .

9. Click in the space for Radius, input 0.1 and then hit the Enter key.

Lathe-Lesson-3-13
 Lathe-Lesson-3

10. For the prompt “Fillet: Select an entity” click on Line 1 and then for the prompt “Fillet:
Select another entity” click on Line 2 as shown below.

11. Click on the OK and Create New Operation icon .

12. Click in the space for Radius, input 0.5 and then hit the Enter key.

13. For the prompt “Fillet: Select an entity” click on Line 1 and then for the prompt “Fillet:
Select another entity” click on Line 2 as shown below.

14. Click on the OK and Create New Operation icon .

Lathe-Lesson-3-14
Mastercam Training Guide
15. Click in the space for Radius, input 0.2 and then hit the Enter key.

16. For the prompt “Fillet: Select an entity” click on Line 1 and then for the prompt “Fillet:
Select another entity” click on Line 2 as shown below.

17. Click on the OK icon to complete this feature.

 The completed fillet is shown below.

Lathe-Lesson-3-15
 Lathe-Lesson-3

TASK 6:
CREATE THE CHAMFER
1. Select the Wireframe tab at the top of the screen and in the Modify section click on
Chamfer Entities.

2. The Chamfer Entities panel appears. If required activate the Method to 1 Distance and
enter a value of 0.0625 for Distance 1.
3. Ensure the Trim entities box at the bottom of the panel is check marked to turn the trim on.
Method field
Defines chamfer method. Choose to create the
chamfer method based on distance or width as
defined below:

1 Distance - Sets the distance from the

intersection of the two selected lines that each
endpoint of the chamfer is positioned. Activates
only the Distance 1 field for input. Both chamfer
endpoints are positioned equal distances from the
intersection.

2 Distances - Sets the distances from the

intersection of the two selected lines that each
endpoint of the chamfer is positioned. This allows
you to set two separate distances. The value in the
Distance 1 field sets the distance from the
endpoint of the first line you select. The value in
the Distance 2 field sets the distance from the
endpoint of the second line you select.

Distance and Angle - Sets the distance from the

intersection of the entity you select first, and an
angle that determines the angle of the chamfer.
When you are prompted to select the second
entity, your cursor will snap to recognized
chamfers that meet the conditions of both the
Distance 1 and Angle fields. If those conditions
cannot be met, you will not be able to create a
chamfer.

Width - Sets the width of the chamfer and

positions its endpoints along the two selected lines
accordingly.

Lathe-Lesson-3-16
Mastercam Training Guide
4. Move over to the graphic screen and for the prompt “Select Line or arc” click on Line 1
and then for the prompt “Select Line or arc” click on Line 2 as shown below.

5. Click on the OK icon to complete this feature.

 The Chamfer should look like the figure below.

 This completes the geometry for this part.

TASK 7:
SAVE THE DRAWING
1. Select File.
2. Select Save As…
3. Click on the Browse icon.
4. In the “File name” box, type “Lathe-Lesson-3”.
5. Browse to an appropriate location.
6. Select the Save button to save the file and complete this function.

Lathe-Lesson-3-17
 Lathe-Lesson-3

Toolpath Creation
TASK 8:
DEFINE THE STOCK AND CHUCK PARAMETERS

1. Select the View tab at the top of the screen.

2. Select the Fit icon in the Zoom section. Next select Unzoom 50% to shrink the display.

3. Still on the View tab and click on Toolpaths to display the Toolpaths Manager.

4. Switch to the Toolpaths Manager by selecting Toolpaths in the lower left corner.

5. Ensure your screen looks like the image below:

Lathe-Lesson-3-18
Mastercam Training Guide
6. Select the plus in front of Properties to expand the Machine Group Properties, if required.

7. Select Stock setup in the toolpath manager window.

8. Select the Stock Properties button in the Stock Setup page as shown in the screenshot
below:
Note:
To learn more about Stock Setup refer to the Tips and Techniques section.

Lathe-Lesson-3-19
 Lathe-Lesson-3

9. In the Machine Component Manager-Stock window click on the Geometry tab and select
Cylinder as shown below. In the Stock setup set the values as shown below. Axis is set
to -Z.

10. Click on the OK icon to complete this feature.

11. Still on the Stock Setup page activate Fit screen to boundaries.

Lathe-Lesson-3-20
Mastercam Training Guide

12. Select the Chuck Properties button in the Stock Setup page as shown in the screenshot
below:

13. On the Chuck Jaws Geometry page, the default settings need no adjusting.

14. On the Chuck Jaws Parameters page, set the values as shown below.

15. Click on the OK icon to complete this feature.

Lathe-Lesson-3-21
 Lathe-Lesson-3

16. Click on the Tool Settings page and make changes as shown below.

17. To change the Material type to Aluminum 6061, click on the Select button at the bottom of
the Tool Settings page.

Lathe-Lesson-3-22
Mastercam Training Guide
18. At the Material List dialog box open the Source drop down list and select Lathe – library.

19. From the Default Materials list select ALUMINUM inch - 6061 and then select .

20. Select the OK button again to complete this Stock Setup function.
21. Right mouse click in the graphics area and click on the Fit icon .

Lathe-Lesson-3-23
 Lathe-Lesson-3

 Note the stock setup outline as indicated by broken lines as shown below.

Lathe-Lesson-3-24
Mastercam Training Guide
TASK 9:
FACE THE FRONT OF THE PART:
 In this task you will use a facing tool to face the front of the part in one cut.
1. If required right mouse click in the graphics area and click on the Fit icon .
2. Select the Turning tab at the top right side of the screen.
3. Now select Face in the General section.

 After selecting the OK button, you are confronted with Toolpath parameters page. The first
task here will be to select Tool #1 an OD Rough- Right – 80 deg.

4. Click on Tool #1 and make changes in the Toolpath parameters page as shown below.
5. Click on Coolant, open the drop-down menu for Flood and set it to On.

Use the Toolpath parameters tab to select a tool, set feeds and speeds, and set other general
toolpath parameters. This tab is very similar for most Lathe toolpaths.

Lathe-Lesson-3-25
 Lathe-Lesson-3

6. Select the Face parameters page and make changes as shown below.

7. Select the OK button to complete this Lathe Face operation.

Finish stepover
Select this option to create one or more finish passes. Enter a stepover distance to define how
much stock gets removed during each finish cut.

Overcut amount
A rectangle is used to define the material removed by the facing toolpath. The overcut amount
determines how far past the rectangle the tool will cut.
Typically, this is a small distance that the tool cuts past the part centerline.

Lathe-Lesson-3-26
Mastercam Training Guide
TASK 10:
ROUGH THE OUTSIDE DIAMETERS
 In this task you will use a new Lathe toolpath called Quick rough.
 In this task you will use the same tool as used for the previous facing operation Tool #1 an
OD Rough- Right – 80 deg.

1. Right mouse click in the white space of the Toolpaths Manager and select:
Lathe toolpaths>Quick>Quick rough.

Quick rough toolpaths coarsely cut the part geometry in preparation for a finish toolpath.

Use this toolpath when you need to quickly create a simple roughing operation and don't need
Mastercam's more advanced roughing features.

In addition, you have fewer options for creating entry and exit passes.

2. In the Chaining window, set the chaining mode to Partial.

Lathe-Lesson-3-27
 Lathe-Lesson-3

3. Select the chamfer, Line 1 as the start of the Partial chain.

After you have selected the chamfer ensure that the arrows are pointing up and to the left of the
part. If it is not select the reverse button in the Chaining dialog box.

4. Then select Line 2 as the end entity in this chain.

5. Select the OK button to exit the Chaining dialog window.

6. In the Toolpath parameters page select the same tool used to face the part Tool #1 an OD
Rough- Right – 80 deg and make any necessary changes as shown below.
7. Click on Coolant, open the drop-down menu for Flood and set it to On.

Lathe-Lesson-3-28
Mastercam Training Guide
8. Select the Quick rough parameters page and make any necessary changes as shown
below.

9. Select the Lead In/Out button select the Lead out page and extend the contour by 0.2 as
shown below.

10. Select the OK button to exit this function.

11. Select the OK button to exit Quick rough Parameters.

Lathe-Lesson-3-29
 Lathe-Lesson-3

TASK 11:
FINISH THE OUTSIDE DIAMETERS
 In this task you will finish the outside diameters in one cut using Tool #2 OD Finish Right –
35 DEG.

1. Right mouse click in the white space of the Toolpaths Manager and select:
Lathe toolpaths>Quick>Quick finish.

Quick finish toolpaths are useful for placing finish passes on an uncomplicated part where you
don't need all Mastercam's more advanced finishing options.

You can chain geometry for this toolpath or simply select an existing roughing operation

2. Select Tool #2 OD Finish Right – 35 DEG tool from the tool list and make any necessary
changes as shown below. Coolant Flood is set to On.

Lathe-Lesson-3-30
Mastercam Training Guide
3. Select the Quick finish parameters page and make changes as shown below.

4. Select the Lead In/Out button select the Lead out page and extend the contour by .2 as
shown below.

5. Select the OK button to exit this function.

6. Select the OK button to exit Quick finish parameters.

Lathe-Lesson-3-31
 Lathe-Lesson-3

TASK 12:
SPOT DRILL THE HOLE
 In this task you will spot drill .20” depth using Tool #3 Spot Drill - .50 diameter.

1. Select Drill in the General section of the Turning tab.

2. Scroll down and select the SPOT TOOL .5 DIA tool from the tool list and make changes as
shown below. Coolant Flood is set to On.

Lathe-Lesson-3-32
Mastercam Training Guide
3. Select the Simple drill – no peck page and make changes as shown below.

4. Select the OK button to exit Simple drill – no peck.

Lathe-Lesson-3-33
 Lathe-Lesson-3

TASK 13:
TAP DRILL THE 5/16” HOLE
 In this task you will drill the 5/16” hole .75” depth using a 0.3125 (5/16”) Drill.

1. Select Drill in the General section of the Turning tab.

2. Click on the Select library tool… button in the lower left corner of the Toolpath parameters
page as shown below.

3. At the top left of this dialog box, click the Select New Folder icon to show the library
tools list, and select LDRILLS. Now click on the Open button to select LDRILLS.

4. Scroll down and select the 0.3125 Dia. 5/16” DRILL from the list.

5. Select the OK button .

Lathe-Lesson-3-34
Mastercam Training Guide
6. Ensure settings are as shown below. Coolant Flood is set to On.

7. Select the Simple drill – no peck page and make changes as shown below. This hole will
be Peck Drilled. The depth of the hole is 1.00” from the front face so click in the space
for depth and type in -1.0.

8. Select the OK button to exit Peck drill – full retract.

Lathe-Lesson-3-35
 Lathe-Lesson-3

TASK 14:
TAP 3/8” – 16 UNC
 In this task you will tap the 3/8”-16 hole 1” deep.

1. Select Drill in the General section of the Turning tab.

2. Click on the Select library tool… button in the lower left corner of the Toolpath parameters
page as shown below.

3. Select the select new folder icon at the top of the dialog box and then the LTAPS
from the list as shown below. Now click on the Open button to select LTAPS.

4. Scroll down and select the 0.375 Dia. 3/8”-16 RH TAP from the list.
5. Select the OK button .
6. Ensure necessary settings are as shown below. Coolant Flood is set to On.

Lathe-Lesson-3-36
Mastercam Training Guide
7. Select the Peck drill – full retract page and make changes to tap as shown below.

8. Select the OK button to exit Tapping – feed in, reverse spindle – feed out.

Note:
The depth at which you can tap this hole will depend on the type of tap used. If you are using a
spiral flute bottoming tap than you will be able to go much closer to the bottom of the previously
drilled hole. Here, we have assumed the use of a non-bottoming tap and one that is pushing the
chips forward. So, we have had to stop well short of the bottom to accommodate the packing of
the chips.

Lathe-Lesson-3-37
 Lathe-Lesson-3

TASK 15:
CUT OFF THE PART
 In this task you will cut off the part using Tool #6 - Cutoff Right - Width .125.

1. Click on the Select all operations icon .

2. Now click on the Toggle display on selected operations button or ALT and T to
show/hide the tool path.

Toolpath Lines visible: Press Alt T to hide toolpath Lines:

3. Click on the Expand gallery down arrow to view additional options in the General toolpath
section.

4. In the General section select Cutoff.

Lathe-Lesson-3-38
Mastercam Training Guide
5. Pick where Line 8 and Line 9 meet as shown below. (Move the cursor over the corner until

the visual cue for End point displays and then click on this point.)

6. Click on the Select library tool… button.

7. Select the select new folder icon at the top of the dialog box and then the
lathe_Inch from the list as shown below. Now click on the Open button to select
lathe_Inch.

8. Scroll down and select OD Cutoff Right Width .125 from the list.
9. Select the OK button .

Lathe-Lesson-3-39
 Lathe-Lesson-3

10. Make changes as shown below in the Toolpath parameters page. Coolant Flood is On.

11. Click on the Stock Update… button.

12. Activate Keep both pieces.

Keep separated piece
Select to display the part boundary after the part is cut
off.
Keep piece in active chuck
Select to display the stock boundary after the part is cut
off.

Keep both pieces

Select to display both the separated piece and the
leftover piece. This is useful when the separated piece
will be transferred to a sub spindle and you will be
machining on both spindles at the same time.
These options are available only with cutoff operations.

Lathe-Lesson-3-40
Mastercam Training Guide
13. Select the Cutoff parameters page and make sure the settings are as shown below.

Note:
The use of CSS with this part off combined with a Max RPM of 2500 would result in the part
being separated at the max RPM. We can still use CSS and a high max RPM but reduce the
RPM when we are close to separating the part.
The Secondary Feed Rate/Spindle Speed allows setting new speeds and feeds once you
reach a specific Radius. Here, we switch to an RPM call of 1500 once a radius of 0.15 is
reached, 0.30 diameter.

14. Select the OK button to exit Cutoff parameters.

Lathe-Lesson-3-41
 Lathe-Lesson-3

TASK 16:
VERIFY THE TOOLPATHS
 Mastercam's Verify utility allows you to use solid models to simulate the machining of a part.
The model created by the verification represents the surface finish, and shows collisions, if
any exist.
1. Right mouse click in the graphics area and click on the Fit icon .
2. In the Toolpaths Manager pick all the operations to Verify by picking the Select all

operations icon .
3. Select the Verify selected operations icon shown below.

4. Maximize the Backplot/Verify window if required.

5. Now select the Home Tab if required.

6. Activate the options shown below in the Visibility section of the Home tab. Initial Stock not
activated.

7. At the top of the screen select the View tab, the Isometric icon and then select Fit.

Lathe-Lesson-3-42
Mastercam Training Guide
8. Select the Verify tab and activate the Color Loop to change the color of the tools for the
verified part.
Color Loop
Changes the color of the toolpath or cut stock by operation or by
tool change.

Choose File Options to set the colors.

9. In the lower part of the screen now set the run Speed to slow by moving the slider bar
pointer over to the left as shown below.

10. Now select the Play Simulation button to review the toolpaths.

11. Select the Close button in the top right-hand corner to exit Verify.

TASK 17:
SAVE THE UPDATED MASTERCAM FILE

1. Select the Save icon from the Quick Access toolbar at the top left of the screen.

Lathe-Lesson-3-43
 Lathe-Lesson-3

TASK 18:
POST AND CREATE THE CNC CODE FILE
1. Ensure all the operations are selected by picking the Select all operations icon from
the Toolpaths manager.
2. Select the Post selected operations button from the Toolpaths manager.
 Please Note: If you cannot see G1 click on the right pane of the Toolpaths manager window
and expand the window to the right.

3. In the Post processing window, make the necessary changes as shown below.

About Post Processing

NC file:
Select this option to save the NC file. The file name and extension are stored in the machine
group properties for the selected operation. If you are posting operations from different machine
groups or Mastercam files, or batch processing, Mastercam will create several files according to
the settings for each machine group.

Edit:
When checked, automatically launches the default text editor with the file displayed so that you
can review or modify it.

4. Select the OK button to continue.

Lathe-Lesson-3-44
Mastercam Training Guide
5. Ensure the same name as your Mastercam part file name is displayed in the NC File name
field as shown below.

6. Select the Save button.

 The CNC code file opens in the default editor.

7. Select the in the top right corner to exit the CNC editor.

 This completes Lathe-Lesson-3.

Lathe-Lesson-3-45
 Lathe-Lesson-3

LATHE-LESSON-3 EXERCISE

Lathe-Lesson-3-46
Mastercam Training Guide

Lathe-Lesson-3-47