136
568

 

This is to certify that the

thesis entitled

Preliminary FEM Modeling
of Orthogonal Turning

presented by

Alexander Macomb Rucker

has been accepted towards fulfillment
of the requirements for

Master of Science degree in Engineering Mechanics

 

 

Major professor

Date USO/aw;

0-7639 MS U is an Afﬁrmative Action/Equal Opportunity Institution

 

l LIBRARY

Michigan State
University

 

 

 

PLACE IN RETURN Box to remove this checkout from your record.
To AVOID FINE return on or before date due.
MAY BE RECALLED with earlier due date if requested.

 

DATE DUE DATE DUE DATE DUE

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

6/01 cJCIRC/DatoDuopBS-pJS

PRELIMINARY FEM MODELING OF
ORTHOGONAL TURNING

By

Alexander Macomb Rucker

A THESIS
Submitted to
Michigan State University

in partial fulﬁllment of the requirements
for the degree of

MASTER OF SCIENCE
Department of Mechanical Engineering

2002

ABSTRACT
PRELIMINARY FEM MODELING OF ORTHOGONAL TURNING
By

Alexander Macomb Rucker

The purpose of this thesis is to develop a computational model used for
studying the effects of changing parameters involved with machining. The
information given by the FEM model will ultimately be used in the determination of
tool wear. The development of such models are important in the minimization of
expensive and time consuming machining experiments for predicting tool life. Finite
element method modeling was developed for the computational models for machining
of an aluminum alloy (AL319T6) during orthogonal cutting. The model consisted of
2-D, plane strain, reduced integration, and four-nodes bilinear elements with
hourglass stiffness control. A ductile fracture criterion based on predetermined
distance from the tool tip was applied in ABAQUS to describe crack growth in the
chip formation. Chip formation in metal cutting is a large deformation problem.
Large deformation of the ﬁnite elements was corrected by remeshing the model as
needed. The chips predicted by the computational machining model were similar to
continuous chips formed in metal cutting. The speciﬁc parameters analyzed were the
curvature of the formed chip and the reaction forces in the tool during cutting process.
Chip curvature and reaction forces are dependant on the rake angle of the tool and the
cutting velocity. Curvature of the chip plays a major role in breaking the continuous

chip. Reaction forces are important in the design of machine tools and other areas.

ACKNOWLEDGEMENTS

I would like to thank my advisor Dr. Patrick Kwon for the chance to work on
this project and for his support and guidance while working on this project.

I would also like to like to thank Tim Wong for all his hard work and late
nights he spent on this project. It was very much appreciated.

I would like to acknowledge my family for all their support over my entire
college career. Without all your love and support, none of this would have been

possible. Thank you.

iii

Table of Contents

Abstract ............................................................................................ ii
Acknowledgements ............................................................................. iii
List of Figures ..................................................................................... vi
List of Tables .................................................................................... viii
Introduction ........................................................................................ l
Orthogonal Turning ..................................................................... 2
Theory of Metal Machining Applied to Orthogonal Turning ..................... 4
Limitations of the Orthogonal Turning Mechanics ................................. 9
Introduction to Finite Element Methods ..................................................... 10
Previous Works Using ABAQUS... . ... .......................................... 11
General ABAQUS Methods .............. . ......................................... 12
Components of an ABAQUS Model ............................... . ............... 14
Units and Coordinate Systems ......... . .. .. ................................... 16
Model Development.............................. ............................................... 17
Modeling in ABAQUS/Explicit .................. . ................................... 17
Modeling in ABAQUS/Standard ..................................................... 20
Results ............................................................................................. 26
Sample Calculations for Simpliﬁed Mechanics of Orthogonal Turning ....... 26
FEM Results ........................................................................... 27
Validation of FEM Model ............................................................ 36

iv

Conclusions ...................................................................................... 37

Limitations and Future Work ......................................................... 42

References ......................................................................................... 43

APPENDDC A: Reaction Force vs. Time Plots for Fine Mesh .......................... Al
APPENDIX B: Comparison of Coarse Mesh and Fine Mesh Cutting

Force and Thrust Force .................................................... Bl

APPEXDIX C: Input Files .................................................................... C1

Figure 1: Orthogonal Turning ................................................................... 3
Figure 2: Two Dimensional Orthogonal Turning Process .................................. 3
Figure 3: A View of the Primary and Secondary Shear Zone .............................. 4
Figure 4: Geometries of Orthogonal Turning ................................................ 5
Figure 5: Forces Acting on the Cutting System .............................................. 6
Figure 6: Relating Reaction Forces ............................................................ 7
Figure 7: Reaction Force Relative to the Work Material .................................... 7
Figure 8: Orthogonal Turning .................................................................... 9
Figure 9: Constitutive Relationship for AL316-T6 ........................................ 15
Figure 10: Initial Mesh Analyzed with ABAQUS/Explicit ................................ 18.
Figure 11: Second Mesh Analyzed in ABAQUS/Explicit ................................. 19
Figure 12: Course 2-D Mesh Analyzed in ABAQUS/Standard..........................21
Figure 13: Mildly Reﬁned Mesh .............................................................. 21
Figure 14: Chip Formation, Remeshing Required .......................................... 22
Figure 15: Chip Formation, Adaptive Meshing Applied .................................. 23
Figure 16: Chip Formation, Cutting Process Continued After Remeshing ............. 23
Figure 17: Finely Reﬁned Mesh Geometry ................................................. 24
Figure 18: Small Crack Length ............................................................... 25
Figure 19: Large Crack Length ............................................................... 25
Figure 20: Cutting Force vs. Time ............................................................ 29
Figure 21: Thrust Force vs. Time ............................................................ 29
Figure 22: Cutting Force vs. Rake Angle .................................................... 30

List of Figures

vi

Figure 23:
Figure 24:
Figure 25:
Figure 26:
Figure 27:
Figure 28:
Figure 29:
Figure 30:
Figure 31:
Figure 32:
Figure 33:
Figure 34:
Figure 35:
Figure 36:
Figure 37:
Figure 38:
Figure 39:
Figure 40:
Figure 41:

Figure 42:

Thrust Force vs. Rake Angle ..................................................... 31
Cutting Force vs. Cutting Speed ................................................. 31
Thrust Force vs. Cutting Speed .................................................. 32
Chip Curvature for chip6bl ....................................................... 33
Chip Curvature for chip6b2 ....................................................... 33
Chip Curvature for chip6b3 ...................................................... 33
Chip Curvature for chip6b4 ........ . ............................................. 34
Chip Curvature for chip6b5 ...................................................... 34
Chip Curvature for chip6b6 ...................................................... 34
Chip Curvature for chip6b7 ...................................................... 35
Chip Curvature for chip6b8 ........ . ..... . ....................................... 35
Chip Curvature for chip6b9 ...................................................... 35
Fine Mesh Cutting Force vs. Time ............................................. 36
Mild Mesh Cutting Force vs. Time ............................................. 36
Continuous Chip formed at 0.07 m/s ............................................ 38
Cutting Force vs. Time Plot at Cutting Speed of 0.07 m/s ................... 39
Thrust Force vs. Time Plot at Cutting Speed of 0.07 m/s .................... 39
Chip Curled into the Work Material ............................................ 40
Cutting Force vs. Time Plot for Cutting Speed of 0.10 m/s .................. 41
Thrust Force vs. Time Plot for Cutting Speed of 0.10 m/s .................. 42

vii

List of Tables

Table 1: Cutting Parameters of Mildly Reﬁned Mesh ..................................... 28
Table 2: Cutting Parameters for Finely Reﬁned Mesh .................................... 28
Table 3: Summary of Results for Reaction Forces ......................................... 29

viii

Introduction

Great bounds in machining research have been made in the past decade.
These achievements have been mainly due to the ability to establish reliable theories
and incorporate these theories into a ﬁnite element analysis to predict important
cutting parameters. The parameters include reaction forces (cutting forces), chip
formation and curvature, and cutting temperatures. These parameters have to be used
to evaluate surface ﬁnish, tool wear and tool life in a more scientiﬁc approach to
machining studies. Finite element analysis minimizes expensive and time-
consuming gathering of experimental machining information. Finite element analysis
has been performed and discussed in this thesis. This analysis is the preliminary
physical modeling of machining and does not incorporate temperature effects into the
material constitutive equation.

Prediction of reaction forces achieved during the cutting process is important
for machine design and cutting tool design, as well as for the control and optimization
of different machining processes. It is also important that material behavior during
chip formation is understood in terms of cutting conditions. The material constitutive
equation is an important key in obtaining interfacial conditions. However, it is
beyond the scope of this thesis.

Chip curvature plays a major role in breaking the continuous chip. This gives

information about material removal and is important in machining operations.

Machining is a very important manufacturing process. It can be applied to
virtually all metals. Machining can be used to produce many different geometries,
ranging from simple to very complex. Dimensions of these geometries can be created
at very close tolerances with smooth surface ﬁnishes. Because machining is so
widely used, it is of much interest to better describe the phenomenon that takes place
during the machining process.

Machining is a manufacturing process in which a cutting tool is used to
remove excess material from the work piece so that a desired shape is formed. The
cutting action involves primarily shear deformation of the work material for the

formation of the metal chip during machining material removal process.

Orthogonal Turning

The preliminary model discussed in this thesis was developed to simulate
orthogonal metal cutting (orthogonal turning). Orthogonal turning is a metal cutting
Operation in which the work material consists of a cylindrical tube rotating on a lathe
and the cutting tool is brought into contact perpendicular to the work material (See
Figure 1). The work material, as it is being sheared off to form the chip, can be

directly observed.

Figure 1: Orthogonal Turning [6,7]

   

Work Material

 

Orthogonal turning can be simpliﬁed in two dimensions (See Figure 2).

Figure 2: Two Dimensional Orthogonal Turning Process [1]

rake face

   
    

shearing zone ' ﬂank face

   

work material

 

In Figure 2, the cutting tool has an ideally sharp cutting edge, which serves to
separate a chip off of the work material. The tool has two faces of interest deﬁned as
the rake face and the ﬂank face. The rake face generates the chip and directs the ﬂow
of the chip. The ﬂank face allows for clearance of the tool to protect the newly

formed work surface.

The shear defamation of the work material occurs along a thin zone called
the primary shear zone. Another shearing action occurs in the chip after it has been
formed in the secondary shear zone. Primary and secondary shear zones can be seen

in Figure 3.

Figure 3: A View of the Primary and Secondary Shear Zone [I]

 

Secondary shear zone

Theory of Metal Machining Applied to Orthogonal Turning

The most important reason to carry out orthogonal turning is because it is
relatively simple to model with simpliﬁed mechanics equations. Orthogonal turning
is one of two main models used for studying constitutive relationships at extremely

high strain rates.

From the two-dimensional simpliﬁed view of orthogonal turning (Figure 2),
the geometry of the process involved can be described by a series of angles (See

Figure 4).

Figure 4: Geometries of Orthogonal Turning [1]

   
  
   

(p=Shear Plane Angle

a=Rake Angle

Chip

 

Work—CW

 

 

 

 

Figure 4 shows the work material being cut by the tool. The rake angle (0.)
is the angle of the rake face of the tool from a vertical axis. Since the primary shear
zone is thin, it can be assumed to be a plane, called the shear plane angle. The shear
plane angle ((p) is the approximate angle at which shear failure of the material takes

place. The original chip thickness (to), deformed chip thickness (to), and length of the

shear plane (1,) are also included. A description of the forces acting on the system can be

seen in Figure 5.

Figure 5: Forces Acting on the Cutting System [1]

 

There are various ways to decompose the force involved with cutting. The
reaction force relative to the tool (R) can be broken into force acting along the rake face
(F), and force acting normal to the rake face (N). The reaction force relative to the shear
plane (R’) can be broken into force acting along the shear plane (F,), and force acting
normal to the shear plane (Fa). These forces can then be related (Figure 6) to a reaction

force relative to the work material (See Figure 7).

Figure 6: Relating Reaction Forces [1]

 

 

Figure 7: Reaction Force Relative to the Work Material [1]

 

The reaction force is now relative to the work material, which is described as
a cutting force (Fe), and a thrust force (Ft). These forces are approximated by the

Merchant Equation [1].

t xy't o-cos(B- a)

-The Cutting Force: F c F sin(¢)'cos(¢ '1' B" a)

 

t xy't o-sin(B - a)

sin(¢)-COS(¢ + B- 0!)

 

-The Thrust Force: F t i:

Where Ix). is the shear stress at the yield point (perfectly plastic material assumed).

Orthogonal turning is also used because it provides reasonably good
modeling of chip formation along the major cutting edge of most major cutting
operations. These other cutting operations include turning, milling, drilling (See
Figure 8), and other conventional machining operations. In orthogonal turning, the
cutting speed is uniform along the rake face. However, in drilling, the cutting speed

is directly related to the distance from the center axis of the drill.

Figure 8: Orthogonal Turning

   

Work Material

Rake Face

Flank Face

Orthogonal turning is also extremely useful because it is a very open and
exposed process. This allows experimental data to be obtained much more easily
than cutting operations that are closed to the environment. Plans for carrying out

experiments at NIST are being made as the current models improve.

Limitations of the Orthogonal Turning Mechanics

The Merchant Equation assumes that the shear strength of the work material is
a constant that is unaffected by strain rate and temperature. These assumptions are
not obeyed in practical machining operations. Therefore, the Merchant Equation is
considered to be an approximate relationship of terms, rather than a precise

mathematical statement. This is the main incentive for Finite Element Methods.

Introduction to
Finite Element Methods

Finite Element Methods are used for the local estimation of tractions (stress) and
temperatures during the machining process. The evaluation of these parameters allows
for a prediction of tool wear. The work done in this thesis was to develop a preliminary
machining model, into which a better constitutive model can be incorporated in future
work.

The ﬁrst step of any ﬁnite element simulation is to discretize the actual geometry
of the structure using a collection of ﬁnite elements. Each ﬁnite element represents a
discrete portion of the physical structure. Shared nodes and edges join the ﬁnite elements.
The collection of nodes and ﬁnite elements is called the mesh. The number of elements
used in a particular mesh is referred to as the mesh density. In a stress analysis,
displacements of the nodes are the fundamental variables calculated. Once the nodal
displacements are known, the stresses and strains in each ﬁnite element can be
determined. At any other point in the element, the displacements are obtained by

interpolating from the nodal displacements.

10

 

 

AAAAAA BBBBBBBBB AAAAAA QQQQQQQQ U U 53833533
A A B B A A Q Q U U S
A A B B A A Q Q U U S
A A B B A A Q Q U U S
AAAAAAAAAA BBBBBBBBB AAAAAAAAAA Q Q U U 53838333
A A B B A A Q Q Q U U S
A A B B A A Q QQ U U S
A A B B A A Q QQ U U S
A A BBBBBBBBB A A QQQQQQQQ UUUUUUUU SSSSS SSS
Q

<|> | | <|> <|> <| <|> <|> <|> <|>

<|> |> <| <|> <|> <| <|> | | |

I I I I I I I <|><|><|>

<> <> <|><><><>
<> <><><>

<> <> <><> <> <>

<> <><><><><><>

<><><><><><><> <>

<><><><><><><> <><>

<><><><><><|><><><><>

 

 

 

 

 

 

 

 

Previous Works Using ABAQUS

Many machining researchers have developed their own ﬁnite element code to
model orthogonal turning [9-13]. Only two previous works could be found using
ABAQUS to model orthogonal turning.

Komvopoulos and Erpenbeck [4] used a chip-separation criterion based on
distance from tool. This is presumed to be a speciﬁed crack length for a given time. The
model was assumed to be quasi-static so that initial inertial effects of the simulation could
be ignored.

Lei et a1. [5] also used a chip-separation criterion based on distance from tool,

which was presumed to be the speciﬁed crack length for a given time. The tool-chip

11

interaction was modeled by small-sliding contact. Rezoning of the mesh (remeshing)
was also used in this paper. It was presumably done with the aid of ABAQUS/CAB,

which is a windows environment that allows for model development (Michigan State
University does not own a license for ABAQUS/CAB). A user-deﬁned constitutive

relation for flow stress was incorporated into the material deﬁnition.

General ABAQUS Methods

ABAQUS is a set of powerful engineering simulation programs, based on the
ﬁnite element method [3,4]. A nonlinear analysis was used in this thesis. ABAQUS
automatically chooses appropriate load increments and convergence tolerances. Not only
does it choose the values for these parameters, it also continually adjusts them during the
analysis to ensure that an accurate solution is obtained efﬁciently.

ABAQUS/Standard was utilized for the majority of the analyses described in this
thesis. ABAQUS/Standard is a general-purpose analysis module that can solve nonlinear
problems [3,4]. A complete ABAQUS/Standard analysis usually consists of three

distinct stages: preprocessing, simulation, and post processing.

Preprocessing

In the preprocessing stage, the model of the physical problem must be deﬁned and
an ABAQUS input ﬁle must be created. This was done directly using a text editor.

The simulation is where ABAQUS formulates results. An element's formulation
refers to the mathematical theory used to deﬁne the element's behavior. All elements

used are based on the Lagrangian or material description of behavior [3,4]. This means

12

that the material associated with an element remains associated with the element
throughout the analysis. Two dimensional plane strain elements were used in this thesis
because the thickness of the formed chip is thin compared to the thickness of the work
material. Plane strain elements assume that the out-of-plane strain is zero. This infers
that they are used to model thick structures.

ABAQUS uses numerical techniques to integrate various quantities over the
volume of each element. Using Gaussian Quadrature , ABAQUS evaluates the material
response at each integration point in each element [3,4]. Reduced integration elements
were used in this thesis.

Reduced integration elements have a single integration point located at the
centroid of the element. At this point, average values of the strain components are
computed for the element. This was done to prevent the elements from being too stiff
and shear locking to occur. Shear locking means that strain energy is creating shearing
deformation rather than the intended bending deformation, so the overall deflections are
less.

The objective of the analysis is to determine this response. ABAQUS uses the
Newton-Raphson method to obtain solutions for nonlinear problems [3,4]. In a nonlinear
analysis the solution cannot be calculated by solving a single system of equations.
Therefore, the solution is found by applying speciﬁed loads gradually, and incrementally
working toward a ﬁnal solution. ABAQUS breaks the simulation into a number of load
increments and ﬁnds the approximate equilibrium conﬁguration at the end of each load
increment. Each increment is composed of many iterations. For each iteration,

ABAQUS forms the model's stiffness matrix and solves a system of equations. This

13

means that each iteration is equivalent, in computational cost, to conducting a complete
linear analysis. The sum of all of the incremental responses is the approximate solution

for the nonlinear analysis.

Post Processing

During post processing, the results can be evaluated once the simulation has been
completed and the displacements, stresses, or other fundamental variables have been
calculated. ABAQUSNiewer provides a tidy compilation of large amounts of data,

which aids in the evaluation of results.

Components of an ABAQUS Model

An ABAQUS model is composed of several different components that together
describe the physical problem to be analyzed and the results to be obtained. The model
must contain the following information: geometry, material data, loads and boundary
conditions, and analysis type.

Initially, the geometry must be generated. Finite elements and nodes deﬁne the
basic geometry of the physical structure being modeled in ABAQUS. Each element in
the model represents a discrete portion of the physical structure, which is, in turn,
represented by many interconnected elements. Shared nodes connect elements to one
another. The coordinates of the nodes and the connectivity of the elements make up the
model geometry. The collection of all the elements and nodes in a model is called the
mesh. The mesh is only an approximation of the actual geometry of the structure. The

element type, shape, and location, as well as the overall number of elements used in the

14

mesh, affect the results obtained from a simulation. In general, the greater the mesh
density is, the more accurate the results. As the mesh density increases, the analysis
results are likely to converge to a unique solution, and the computer time required for the
analysis increases. The solution obtained from the numerical model is generally an
approximation to the solution of the physical problem being simulated. The extent of the
approximations made in the model's geometry, material behavior, boundary conditions,
and loading determines how well the numerical simulation matches the physical problem.
Because displacements of the nodes are the fundamental variables calculated, it is
important to have accurate material data for the calculation of other variables. Material
properties for all elements must be speciﬁed. While high-quality material data are often
difﬁcult to obtain, particularly for the more complex material models, the validity of the
ABAQUS results is limited by the accuracy and extent of the material data. The material
AL319-T6 was used for the models developed in this thesis. Material data supplied from
General Motors was used and the simplest constitutive relationship is for AL316—T6 is

shown in Figure 9.

Figure 9: Constitutive Relationship for AL316-T6 [l4]

 

Stress-Strain Relationship for AL316-T6

iiéi

«3%

    

Stress (Pa)

       

0 0.02 0.04 0.06 0.08 0.1 0.12 0.14 0.16 0.18 0.2
Strain

 

 

 

Boundary conditions are used to constrain portions of the model to remain ﬁxed
(zero displacements) or to move by a prescribed amount (nonzero displacements). In a
static analysis, enough boundary conditions must be used to prevent the model from
moving as a rigid body in any direction; otherwise, unrestrained rigid body motion causes
the stiffness matrix to be singular.
An ABAQUS simulation can generate a large amount of output. To avoid
using excessive disk space, a node output frequency was used to limit the output to that

required for interpreting the results. Output was recorded at the frequency speciﬁed.

Units and Coordinate Systems

Before starting to deﬁne this or any model, you need to decide which system of
units you will use. ABAQUS has no built-in system of units. All input data must be
speciﬁed in consistent units. Standard Metric Units were used (Newton’s, meters).

The default global coordinate system in ABAQUS is a right-handed, rectangular

(Cartesian) system.

16

Development of Finite Element Model

Machining is a difﬁcult process to model because of the failure of the material
and large deformations of the chip occuning. At steady states, a rigid surface (the tool)
traveled at a constant velocity into a mesh of elements (the work material), causing them
failure. These large displacements and large deformations in the mesh are difﬁcult to
model. In order for the chip to form, mesh failure along certain nodes must take place. If
no mesh failure takes place, the rigid surface will not penetrate the mesh and the mesh
will react like a balloon poked by a ﬁnger. Therefore, it is imperative to be able to
control failure of the mesh and apply a failure criterion at speciﬁc points of the mesh.

The problem of having a chip form while the tool contacted the material was considered

several ways.

Modeling in ABAQUS/Explicit [4]

Initially, ABAQUS/Explicit was utilized for the modeling of machining. The
motivation behind this was mainly so the adaptive mesh Option could be incorporated
into the model. The adaptive mesh option is desirable because it automatically corrects
for large deformations of elements, allowing for the simulation to be more accurate and
run longer. However, the failure of the mesh was difﬁcult to implement in
ABAQUS/Explicit.

It was attempted to include an element deletion option based on shear failure.
This option was applied where the mesh was expected to fail. This was on a thin layer of

elements that connected the chip elements to the rest of the work material. Initially, a

17

very soft material with much lower material properties was speciﬁed for this thin layer of
elements so that failure would occur rather easily. This soft material was deﬁned in the
user subroutine VUMAT deﬁned. A three dimensional, 200,000—element mesh was
constructed that was 16 elements in height, 50 elements thick, and 250 elements in length

(See Figure 10).

Figure 10: Initial Mesh Analyzed with ABAQUS/Explicit

Vlewpori: 1 068: IIIomémsrmckerauahaquslaaﬁub "T—_’ 'TF

REFII‘IED MESH 'SEC'ME C'F A CUFTII‘I:
ODE: aal.odb RE 1 T

TC-C'L
hu Mar (17 15:05 :16 EST .3303

. ANALY'.
2.1311 Ci t

Time = 0.1500

«mention Scale Factor: *l.‘CJ'30~30C|0

 

It can be seen from Figure 10 that the chip is much too stiff and is behaving
similar to a rigid body. This can be explained by the large difference in material
properties of the soft connecting layer. A problem can be seen as the rear end of the chip

is penetrating the rest of the model. Even though the failed elements are still being

shown, it can be seen that they are carrying zero stress. Due to the large size of the mesh,
it took much too long to process this simulation (nearly a day).

Another mesh was created that was much smaller in size to cut down on processor
time. This was a three dimensional, 1,000-element mesh that was 5 elements in height, 5
elements in thickness, and 40 elements in length (See Figure 11). In addition to the
variation in the number of elements, added boundary conditions (ﬁxation in the Y-
direction) were added to the rear end nodes of the work material to prevent penetration of

the chip layer into the rest of the work material.

Figure 11: Second Mesh Analyzed in ABAQUS/Explicit

manned: 1 008: Ihameld3fnrckewrajlalﬁﬁuslorthogl $0711;

ADAFTI 'v'E H EEHI I): EKANF'LE . l ... 2 _
ODE: orthogl4.oﬂh ABAQL /Explicit L l :5 I;

= 0.1000

ormation ~cale Factor: +1

 

 

Figure 11 shows the chip still behaving much too rigidly, because of the soft layer
of material. It can be seen that the additional boundary conditions to the rear end of the
work material corrected the previous penetration problem. The soft material layer is still
failing very easily and carries no stress.

The next step was to make the material properties of the thin connecting layer of
elements similar to those of the rest of the work material. When this request was made in
the user subroutine, the ABAQUS analysis would not run. After ABAQUS/Explicit

attempts were exhausted, focus was switched to the use of ABAQUS/Standard.

Modeling in ABAQUS/Standard [3]

A major motivation for the use of ABAQUS/Standard is that it allows for the use
of fracture mechanics, which is not allowed in ABAQUS/Explicit. This allows for the
modeling of material failure in the mesh. A double layer of nodes was speciﬁed along
the surface where failure of the material was expected to occur. The double layers of
nodes were deﬁned to be initially bonded, bonding the chip elements to the rest of the
work material. A ductile failure criterion was applied along this double layer of nodes.
As the tool progresses, a crack length was speciﬁed, allowing the bonded nodes to
separate and the chip to form. A coarse two-dimensional mesh was constructed (See
Figure l) to apply the fracture mechanics options in a timely manner. This mesh
consisted of 200 elements (5 elements in height and 40 elements in length) and can be
seen in Figure 12. Once the fracture mechanics options were used with some success, the

mesh was mildly reﬁned (See Figure 13). An offset of the ﬁrst few elements was

20

included to make the model initially less stiff, giving the simulation a greater chance of

running.

Figure 12: Course 2- D Mesh Analyzed In ABAQUS/Standard

    

 

erm-qiortn —ODB: (researctrfnrckemllalstuortlrﬂs. ad!)

.11 turning uzinrg ' tand . . 21.1002
23:3: rcho‘. .odk- AER ._ ._ "— Thu Mar

3 : Step-l
an 0.5000

: m1r- Jar
Def: -rm:.=d . v r ' - . ale F1: t 3:: «4.0009900

Fig—ure 13: Mildly Reﬁned Mesh

Viewportzt ODB . Imsearchlruckerrrllsldortlrs. udh

usin-I A ' . . . Mar. 3'1, 200.3.
REA-NJ. mdnrfl (- 1 Mon Ar-r 01 19:51:53")

Ste-p Ti ..Z.C

21

As the simulation proceeded in ABAQUS/Standard, the chip formed and data was
recorded. During the simulation, large deformations of the elements were evident (See
Figure 14). The simulation would stop once elements became severely distorted. The
increment was noted when elements approached severe distortion as seen through
ABAQUSNiewer. In order to correct these highly distorted elements, data was imported
from the speciﬁed increment into ABAQUS/Explicit. An adaptive meshing option was
applied with a Lagrangian constraint (See Figure 15) to the mesh, correcting the severely
distorted elements.

The data was then imported back into ABAQUS/Standard after the ﬁrst increment
in ABAQUS/Explicit. The simulation was then continued (See Figure 16) to the end of

the simulation or until the remeshing process needed to be repeated.

Figure 14: Chip Formation, Remeshing Required

Viewportn ODB:Iresearchimckéﬁlglﬁdrtthtth “T

0.4052

cale Factor:

 

22

Figure 15: Chip Formation, Adaptive Meshing Applied

 

 

 

 

T ABAQUS ?TAHCARD IHT‘ EXFLICIT T? "5 THE ADAPTIVE MEﬂi-PFTIOH
rem-ashlnzdb AEIFUQLU Explicit; '5...“ '1" ‘Jr {12 19:55:17 EST 2002
.. Step-l

I _ amen:

Primary Var: S .

Deformed Var: , . I ; elujloﬂewgn

Figure 16: Chip Formation, Cutting Process Continued A

 

 

Viewport: 1 ODE: Iresearchfnrckeralirenmndb

 

 

 

 

'. 71'5””;
“—459

import-3:1 from explicit
‘ rerIm.~:--_.- AEIr‘d;IIJ$.’Stan-dard 6.2-1 Wed Apr 03 15:55 :05 EST 2003

‘: Etep Time = O .5004

Deformation Scale Factor: 91.000e0-00

 

Once these operations were carried out with the course mesh, the next step was to
greatly reﬁne the mesh. A new mesh was created (see Figure 17) consisting of a total of
4,000 elements (16 elements in height and 250 elements in length). In addition to the
reﬁnement in element size, crack tip location was also reﬁned. It was seen that large
element deformations did not occur for the ﬁne mesh simulations. Therefore, remeshing

was not needed.

Figure 17: Finely Reﬁned Mesh Geometry

‘— “*H 0 D73: Iresearchl‘ruckertulc—rzE‘KBEJIT—I

 

 

Viewporf: 1

'1

Thu Apr 04 10:24:36 E91" 2002

Figure 18 and Figure 19 show the difﬁculty in correctly specifying the crack
length. The crack opening is desired to be as close to the tool tip as possible to model
what is happening in reality of the machining process. Initially, if the crack length is not

large enough, the crack will not be allowed to open and the tool will crash into unopened

24

nodes (Figure 18), stopping the analysis. Also, the crack opening must initially be larger
than what is actually observed in machining. This is because if the model is initially too
stiff, the simulation will terminate. If a large crack opening is speciﬁed (Figure 19), the
analysis will be allowed to run, but what is modeled does not resemble the actual

machining process.

Figure 18: Small Crack Length

Vtawpor‘: ! on": lmsoarcnlnurbuvrnlln/crnckz.ouh

    

A
Dob-axmutncal Rena.‘ Factocl val 'Z‘I'iu-‘m’lo

wa'rur‘: 1 0|)“: ViruiéamII/nrckerallcrauk'lndb 7

err-"rum; I
"-nru. .-r

D tar-:9” our”: III
'7. rib Al'JagIll.

“I

 

Once an acceptable crack length vs. time was established, results were taken.

25

Results

Results were calculated according to the Merchant Equation [1] to obtain an

approximate solution.

Sample Calculations for Simplified Mechanics of Orthogonal Turning:

-Calculations made for a ten degree rake angle

 

 

F ._ ty-to~w-cos(B-a)
t '- .
Cutting Force (N): cu sm(¢)-cos(¢ + B‘- a)
._ t y-t o'wsinﬂi— a)
1:thrust " .
Thrust Force (N): srn(¢) 'COSW + B" (I)

Where:

Young's Modulus (Pa): E := 73000000000
Poisson’s Ratio:

Axial Yield Stress (Pa): Y

.. 2, _ 8
ry.-J;oy ty—1.08610

Shear Yield Stress (Pa):
Width (m): W .=
it
(p := 18 -_
Shear Plane Angle (Rad): 180

Original Chip Thickness (m): t 0 '— .006

26

or := 10-—
Rake Angle (Rad): 180
It
I} := .—
Beta Angle (Rad): 130
F -4011106 F -552106
cut ‘ ° ° ' thrust " ‘ ° '

Results (in Newton’s):

It is important to note that the forces are very high. This is because some of the
assumed parameters are unrealistic. For instance, a machined chip of six millimeters is
very large. Original chip thickness is commonly on the order of tenths of a millimeter.
Also, a width of one meter is extremely large. It is usually along the order of millimeters.
This width was used because the FEM model uses plane strain, which assumes a
thickness of one.

The results obtained from the Merchant Equation are an approximation of the
forces involved in the machining process modeled by FEM in this thesis. These results
were used to determine if the FEM results were along the same order of magnitude as

these simpliﬁed equations. FEM results are expected to be more accurate.

FEM Results

Results were recorded for three different rake angles (10°, 15°, 20°) at three
different cutting speeds (70mm/sec, lOOmm/sec, 130 min/sec) for the ﬁnely reﬁned mesh
(Figure 17). Results were also recorded for the mildly reﬁned mesh (Figure 13) to show

similarities of results. Table l and Table 2 shows the cutting parameters associated with

27

the ABAQUS ﬁle name for the mildly meshed model and the ﬁnely meshed model,

respectively. Each simulation for ﬁles chip6b1-9 took approximately 15 hours to run.

Table 1: Cutting Parameters of Mildly Reﬁned Mesh

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

File Name Rake Angle (deg) Cutting Speed (m/sec) Chip Thickness (m)
rest 10 0.07 0.006
r632 15 0.07 0.006
res3 20 0.07 0.006
res4 10 0.1 0.006
resS 15 0.1 0.006
resG 20 0.1 0.006

Table 2: Cutting Parameters for Finely Reﬁned Mesh

File Name Rake Angle (deg) Cutting Speed (In/sec) Chip Thickness (m)
chip6b1 10 0.07 0.006
chip662 15 0.07 0.006
chip6b3 20 0.07 0.006
chip6b4 1 0 0.1 0.006
chip6b5 15 0.1 0.006
chip6b6 20 0.1 0.006
chipr7 10 0.13 0.006
chip6b8 15 0.13 0.006
chip6b9 20 0.1 3 0.006

 

 

 

 

 

The cutting forces and thrust forces were recorded for each of the ﬁles. Chip

curvature was also noted for general comparison.

Reaction forces were estimated from the force versus time plots when the curves

leveled off and reached an approximate steady state (See Figure 20 and Figure 21). Table

3 and shows a summary of results for the reaction forces (cutting force and thrust force)

for the ﬁne mesh. All reaction force versus time plots is included in APPENDIX: A.

28

 

 

Figure 20: Cutting Force vs. Time Figure 21: Thrust Force vs. Time

_1

O 6’
O o
’— I—
l— I—
“J UJ
U) U)
2 2
E- E
O

O 8
O o
O o
O o
g s
0 0
Z 2
ii a
'— N
[L u.
U: o:

 

Table 3: Summary of Results for Reaction Forces

 

29

An incremental decrease of cutting force can be seen with and increasing rake
angle at all three cutting speeds (Figure 22). An incremental increase in cutting force can
be seen with and increasing rake angle at cutting speeds of 0.07 m/sec and 0.10 m/sec
(Figure 23). There is also and incremental increase in cutting force and thrust force at all

three cutting speeds for rake angles of 10 deg. and 15 deg. (Figures 24 and 25).

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

Figure 22:
Cutting Force vs. Rake Angle
*speed=0.07 mls
800000 +speed=0.1 rule
A 700000 ‘speed=0.13 mls
.2. mm :5 I
8 < _
3 500000 ' ‘71
u.
at 400000
.5
3; 300000
0 200000 $
4
100000 . . . . .
10 12 14 16 1e 20
Rake Angle (deg)

 

 

 

30

Figure 23:

 

 

   
 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

Thrust Force vs. Rake Angle
300000 *speed=0.07 mls
+speed=0.1 rule
A 250000 ‘- 'I'~speed=0.13 rule 443—.
E .'
., 200000
2
.2 150000
‘2'
E 100000 .
50000 «L— 4”
o T T l l l
10 12 14 16 1e 20
Rake Angle (deg)
Figure 24:
Cutting Force vs. Cutting Speed
800000 -
700000 —

 

 

 

 

 

 

 

 

 

  
  

 

 

 

Cutting Force (N)

 

 

 

 

 

 

*rakeﬂo deg
200000 - +reke=15 deg —
100000- 0 " "~reke=20deg——
o I I I l I I I 3
0.06 0.07 0.08 0.09 0.1 0.11 0.12 0.13 0.14
Cutting Speed (mls)

 

 

 

31

Figure 25:

 

 

 

 

 

 

  

 

 

 
 

 

 

 

 

 

 

 

 

 

 

Thrust Force vs. Cutting Speed
300000-
A 250000 —"'-
E.
on 200000
0
h
.2 150000
76
E 100000 -————— *reke=10 deg
.: +reke=15deg
'— 50000
rake=20 deg
0 V I 1 T I I I 1
0.06 0.07 0.08 0.09 0.1 0.11 0.12 0.13 0.14
Cutting Speed (mls)

 

 

 

Chip Curvature

The chip curvatures were noted at a constant cutting distance of 0.028 m for each
of the ﬁles. This was done because it is easiest to view chip curvature and changes in

chip curvature at the beginning of the analysis. Figures 22 to 30 show chip curvatures for

each of the ﬁnely meshed models.

32'

Figure 26: Chip Curvature for chip6b1 Figure 27: Chip Curvature for chip6b2

   

Figure 28: Chip Curvature for chip6b3

.-» ,qwﬁcah‘qwxvf!nn:—1 L: ,

 

It can be seen that chip6b1 (Figure 26) has more curvature that chip6b2 (Figure

27) and chip6b2 has more curvature than chip6b3 (Figure 28).

33

Figure 29: Chip Curvature for chip6b4 Figure 30: Chip Curvature for chip6b5

 

It can be seen that chip6b4 (Figure 29) has more curvature that chip6b5 (Figure
30) and chip6b5 has more curvature than chip6b6 (Figure 31). It can also be seen that
chip6b4 has more curvature than chipbl , chip6b5 has more curvature than chip6b2, and

chip6b6 has more curvature than chip6b3.

34

Figure 32: Chip Curvature for chip6b7 Figure 33: Chip Curvature for chip6b8

 

Figure 34: Chip Curvature for chip6b9

 

It can be seen that chip6b7 (Figure 32) has more curvature that chip6b8 (Figure

33) and chip6b8 has more curvature than chip6b9 (Figure 34).

35

Validation of FEM Model

It can be seen that the FEM results are on the same order of magnitude as the
results from the Merchant Equation. This shows that the FEM model is generating
somewhat realistic results.

It can be seen from Figures 35 and 36 that the reaction forces generated from the

ﬁne mesh and the mildly reﬁned mesh are similar.

Figure 35: Fine Mesh Cutting Force vs. Time Figure 36: Mild Mesh Cutting Force
vs. Time

.L_L1_LLLI_LLL.L‘I_LLL LLL! ,_:_ LLLLLLI

.1}
O
O
I...
I...
Lu
(I)
2
C
O
O
O
O
O
O
"C
0
2
P3
E
I

RF1 at Node 10000 In NSET TOOL

-i.1

 

The cutting force versus time plot of the ﬁne mesh is much smoother that the
mildly reﬁned mesh but follows a similar path. This shows the FEM model converging

to a solution with mesh reﬁnement.

36

Conclusions

Reaction forces (cutting force and thrust force) computed by the FEM model were
along the same order of magnitude as the simpliﬁed mechanics calculations. This shows
that the FEM model is computing realistic values for the given machining parameters.

An increase in chip curvature can be seen as the rake angle is decreased for all
three cutting speeds. Therefore, this model shows that a decrease in rake angle will
increase chip curvature. This is an observed and expected phenomenon. It gives
conﬁdence that this machining model is an accurate predictor of chip curvature. This
theory must be backed up with experimental data. Chip curvature gives insight to when
the chip might break off and become debris. This is very important in today’s automated
machining processes. If a continuous chip is formed, it may interfere with other
operations of the machine that is cutting the work material.

Cutting forces were seen to decrease linearly with an increase in rake angle for all
three cutting speeds. It is expected that an increase in rake angle will decrease the cutting
force because less of the resultant force is directed along the X-axis. Conversely, thrust
forces were seen to increase linearly with an increase in rake angle for all three cutting
speeds. It is expected that an increase in rake angle will increase the thrust force because
more of the resultant force is directed along the Y-axis. These results give further
conﬁdence that the model is properly modeling orthogonal turning.

Both the cutting force and the thrust force increased as cutting speed was
increased from 0.07 m/s to 0.10 m/s. It is expected that increasing the cutting speed will
increase the reaction forces. This was not the case as the cutting speed was increased

from 0.10 m/s to 0.13 m/s. This obvious modeling ﬂaw can be explained by the chip

37

formation phenomenon during the simulation of the increased cutting speeds (0.10 m/s
and 0.13 m/s). The simulation run with a cutting speed of 0.07 m/s yields a nice
continuous chip (Figure 37) and smooth reaction forces versus time plots (Figures 38 and

39) that approach a steady state solution.

Figure 37: Continuous Chip formed at 0.07 m/s

Viewport: 1 OﬁﬁﬂﬁmickeﬁmMm .0111)”—

EEFIHED 3-D 3H DIiIl‘lE Ill STAl'lDAFD
DDS: :hif 6h __ AE=H MIS/St1ndard 6 -1 Thu Apr :3 11:29:19 EDT 2002

p Time = 2.000

ormation _ .c . : *1 "'*

 

38

Figure 38: Cutting Force vs. Time Plot at Cutting Speed of 0.07 m/s

_I
O
O
i...
'—
LlJ
(D
Z

c
o
o
o
o
0

<0
ti

0
2
E
E
El:

 

Figure 39: Thrust Force vs. Time Plot at Cutting Speed of 0.07 m/s

RF2 at Node 100000 in NSET TOOL

 

39

During the simulation of the faster cutting speeds of 0.10 m/s and 0.13 m/s, the chip

curvature became extreme and the chip curled into the work material (Figure 39).

Figure 40: Chip Curled into the Work Material

VIEWER: 1 008: InseamIiIhTélTeFm??theBSToliir'__

u ...n
~1——-—.uqnq.‘[
' . l

FEFII‘IED :J-D HE'FH 03113
(DB: chip6b5.odh AE

CARD
andarcl 6' l'l:n Apr 3'? 09:39:17 EDT 2100::

 

The model was deﬁned so that the front surface of the chip could not penetrate the top
surface of the chip. It was attempted to implement a similar deﬁnition so that the bottom
surface of the chip could not penetrate the top surface of the chip (which is occurring in
Figure 39). Such a deﬁnition was not allowed to run in ABAQUS. The extreme nature
of the deformations taking place during the simulation could not be modeled for this chip

thickness. A much thinner chip may yield better modeling and better results.

40

Also, the reaction forces vs. time plots (Figures 40 and 41) were not smooth and
difﬁcult to approximate. This is believed to be caused by the forces involved with the
chip contacting itself. The results for cutting speeds of 0.10 m/s and 0.13 m/s may not be

accurate.

Figure 41: Cutting Force vs. Time Plot for Cutting Speed of 0.10 m/s

..J
O
O
*—
*—
LU
(D
Z

r:
o
o
o
o
o

a)
'1:

0
2
iii
II
Cf

 

41

Figure 42: Thrust Force vs. Time Plot for Cutting Speed of 0.10 m/s

._l
O
O
1....
’—
LlJ
(D
Z
.S
o
o
o
o
0

<0
*0

0
2
iii
N
Ll.
o:

 

Limitations and Future Work

The chip curling and penetrating into the work material at cutting speeds of 0.10
m/s and 0.13 m/s is major limitation of this ﬁnite element model. This problem affects
the reliability of results.

This machining model does not include temperature and strain rate into the
constitutive equation. Elastic and plastic deformation is incorporated into the model
(according to Figure 9). The incorporation of these variables into a user deﬁned
constitutive equation is left for future works.

Also, the chip-separation criterion of increasing crack length with time is
unrealistic to actual machining. In the future, a stress failure criterion will be

incorporated for chip separation. This way, the failure plane is not deﬁned by the user.

42

[1]

[2]

[3]

[4]

[5]

[6]

[7]

[8]

[9]

References

Grooverl(996). Fundamentals of Modern Manufacturing. Prentice-Hall
Publishers. Pg:543-557

Hibbit, Karlsson, Sorensen (2001). ABAQUS/Standard User’s Manual Version
6.2. Hibbit, Karlson, Sorensen, Inc.

Hibbit, Karlsson, Sorensen (2001). ABAQUS/Explicit User’s Manual Version
6._2_._ Hibbit, Karlson, Sorensen, Inc.

Komvopoulos, Erpenbeck (1991, August). Finite Element Modeling of
Orthogonal Metal Cutting. Journal of Engineering for Indusﬂ. Volume 113,
Pg:253-267

Lei, Shin, Incropera (1999, November). Material Constitutive Modeling Under
High Strain Rates and Temperatures Through Orthogonal Machining Tests.
Joumgl of Manufacturing Science and Engineering. Volume 121, Pg:577-585.

Shaw (1991). Metal Cutting Principles. Oxford University Press. Pg:11-47

Tlusty (2000). Manufacturing Processes and Equipment. Prentice-Hall
Publishers. Pg:419

Kwon (2000, January). Predictive Models for Flank Wear on Coated Inserts.
Journal of Tribology-Transactions of the ASME. Volume 122, no.1, sz340-347.

Obikawa, Usui (1996, May). Computational Machining of Titanium Alloy-Finite

Element Modeling and a Few Results. Journal of Manufacturing Science and
Engineering. Volume 118. Pg:208-215.

43

[10]

[11]

[12]

[13]

[14]

Strenkowski, Athavale (1997, November). A Partially Constrained Eulerian
Orthogonal Cutting Model for Chip Control Tools. Journal of Manufacturing
Science and Engineering. Volume 119, Pg:681-688.

Poulachon, Moisan, J awahir (2001 , November). Evaluation of Chip Morphology
in Hard Turning Using Constitutive Models and Material Property Data.
Proceedings of 2001 ASME International Mechanical Engineering Congress and
Exposition.

Shih (1995, February). Finite Element Simulation of Orthogonal Metal Cutting.
Journal of Engineering for Industry. Volume 117, Pg:84-93.

Strenkowski, Carroll (1985, November). A Finite Element Model of Orthogonal
Metal Cutting. Journal of Engineering for Industg. Volume 107, Pg:349-354.

Provided by General Motors

 

‘-
-
- A
-
_ -
-
-
-

“
...—..—~~
..