Turning

By D Cheshire Page 1 of 11
This tutorial introduces the concept of machining of turned parts using a
CNC lathe. A sample model of a turned part is provided for you to work
with in this tutorial. There is a link to it next to this tutorial at
and it is called
turnedpart.prt. This part should be downloaded to your working directory
before starting the tutorial.
Machining Setup
To start the tutorial, create a new file for the machining data using FILE >
NEW. Select MANUFACTURING and NC ASSEMBLY as shown in Figure
1 and type in a name such as turnedpart. In the New File Options dialog
that follows choose EMPTY.

Figure 1 : Creating a New Machining File
The blank file created is ready to store all of the manufacturing
information. The first data to be inserted into the file is the actual model to
be machined. This is specified by the command from the right side menu
MFG MODEL  ASSEMBLE  REF MODEL and choosing turnedpart.prt
in the file list box. After the model to be machined appears in the window
choose DONE/RETURN.

Figure 2 : The Mould Part to Be Machined
As an aid to visualising the machining process it is beneficial (though not
essential) that the stock material from which this part will be machined is
defined. To do this choose MFG MODEL  CREATE  WORKPIECE
and type in the name turnedpart_work. Now choose PROTRUSION 
EXTRUDE | SOLID | DONE to enter the extrude dashboard. If you have
completed the modelling tutorials you will be familiar with this function.

of the workpiece.

Figure 5 : Defining the Coordinate System
It is ESSENTIAL that the Z axis is correctly oriented if the turning operation
is to be correct. The Z axis defines the rotation of the work in the lathe
chuck. If the Z axis is incorrectly oriented then Pro Engineer will try and
machine from the wrong direction. Click OK to close the dialog and ACS0
should appear in the model tree.
It is also useful to define the location of the position that the tool will return
to before/after each cut is taken. To specify this point we will define a
datum point with INSERT > MODEL DATUM > POINT > OFFSET
CORDINATE SYSTEM... As a reference point, choose the coordinate
system ACS0. Type a name of HOME and add a value of 30 in the X
column and 5 in the Z. Click OK to close the dialog and create this point.
Defining the Machining Operation
An operation is the term Pro Engineer uses to define the type of machine
that will be used for a sequence of cuts. Choose the command
MACHINING from the side menu and the dialog shown in Figure 6
appears in which you define the Operation. Type in an Operation Name of
Turning. Press
to go to the machine Tool Dialog and type in a
machine name of CNCLathe, choose a Machine Type of Lathe then press
OK to return to Operation Setup. Next click on
next to Machine Zero
and pick on the coordinate system ACS0. Close the dialog with OK.

Figure 6 : Operation and Machine Tool Setup Dialogs

Turning


curve shown in blue in Figure 9a before pressing DONE/RETURN.

Figure 9 : Defining a Profile by Section
This has defined the profile which the tool will follow but the shape
includes the grooves around the part and the hole in the end. These
should not be included so they need to be removed. In the CURVE: TURN
PROFILE dialog double-click on ADJUST TURN PROFILE to show the
ADJUST PROFILE dialog. In this dialog click ADD to create a new
adjustment then pick the points in Figure 10. Press PREVIEW to see that
Pick here
then here
Negative Z
Positive Z

Turning

By D Cheshire Page 4 of 11
the machine profile now misses out the groove – the two points you chose
are joined by a straight line. Add a similar adjustment to the other groove.
Click OK in the ADJUST PROFILE dialog and OK in the CURVE: TURN
PROFILE dialog. ProEngineer next offers the opportunity to extend the
profile at each end to ensure a clean cut – choose the options NEGATIVE
Z | DONE for the first end and POSITIVE Z | DONE for the second end as
shown in Figure 9b. Then choose DONE CUT and the toolpath will be
previewed. Choose OK in the CUSTOMIZE dialog to finish the definition of
this cut.

Figure 10 : Profile Adjustment
This has defined all of the parameters needed to perform the cut. To see
the result of this machining exercise choose PLAY PATH  SCREEN

wrong! To see this more clearly choose PLAY PATH  NC CHECK. This
Pick here
then here
Pick this
profile

Turning

By D Cheshire Page 5 of 11
uses software called Vericut to simulate the machining process. A
graphical representation of the part should appear on the screen after a
few moments. You can use the buttons in the bottom right of the screen to
play the toolpath
. Use the solid green arrow to
play the path now.

Figure 13 : Cut Verification for Finish Cut
The yellow material shows the starting shape. The grey material is
correctly machined. The red colour shows the error. In its rush to get to the
home position the tool went straight through the part trying to cut at very
high speed. How can we stop this happening?
Close Vericut with FILE > EXIT. In the NC SEQUENCE menu choose SEQ
SETUP and tick PARAMETERS to redefine some of the settings for this
toolpath. Choose DONE then tick NC SEQUENCE | DONE SEL > SET.
The PARAM TREE dialog shown in Figure 12 should be shown. Only the
simple parameters are shown – there are many more parameters which
are hidden until you press the ADVANCED button. Press this and scroll to
the bottom of the list where you will see a parameter called START
MOTION. Change this to Z FIRST (select then use the INPUT list box at
the top of the dialog). You will see a second parameter called END