Master Thesis

Numerical Simulation of Thermo-viscoplasticity
Behaviour of Copper under Hot Compression
Test
MOSTAFA PAYANDEH DARI NEJAD
Supervisor: Prof. Hasse Fredriksson
Royal Institute of Technology
Stockholm, Sweden,
January 2011
KTH Industrial Engineering
and Management
THESIS FOR MASTER DEGREE

Abstract
This project is focused on developing user defined subroutines UMAT and VUMAT, in the
commercial finite element code, ABAQUS, to model thermo-viscoplastic hardening behav-
ior in oxygen-free high thermal conductivity (OFHC) copper during hot compression test.
Constitutive equation for finite deformation, isotropic, hypoelastic-viscoplastic solid is formu-
lated and the constitutive relation of J2 flow theory of metal plasticity is employed. Moreover
thermo-viscoplastic model Johnson-Cook (JC) flow stress model calculates the strain-rate
and temperature dependence of the yield stress. Rate-dependent plasticity is formulated by
including the rate of the state variables in the yield function according to the consistency
model. The classical radial returned method and modified explicit integration scheme is used
for updating the stress and other variables.
Due to sufficient rigid body rotations are provided by Abaqus, formulation in term of
deformation gradient is not considered. Also to reduce mesh distortion, the ALE adaptive
remeshing and Mesh-to-Mesh solution mapping technique is performed in Abaqus Explicit
and Abaqus Standard respectively. Hot plain strain compression test on copper have been
conduct. The obtained result from UMAT and VUMAT is discussed and also compare.

Contents
1 Hot Compression Test Simulation 4
1.1 Finite Element Method . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4
1.1.1 Abaqus . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4
1.2 Pre-Processing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5
1.3 Part and Assembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5
1.4 Material . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6
1.5 Contact . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7
1.6 Step . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8
1.6.1 Lagrangian and Eulerian . . . . . . . . . . . . . . . . . . . . . . . . . 9
1.6.2 Increment . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9
1.7 Mesh . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10
1.8 Adaptivity . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11
1.8.1 ALE Adaptive remeshing . . . . . . . . . . . . . . . . . . . . . . . . . 12
1.8.2 Mesh-to-Mesh solution mapping . . . . . . . . . . . . . . . . . . . . . 12
1.9 Boundary Condition . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14
1.9.1 Predeﬁned Field . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14
1.10 Processing and Post-Processing . . . . . . . . . . . . . . . . . . . . . . . . . 15
1.10.1 Job, submit and Running . . . . . . . . . . . . . . . . . . . . . . . . 15
1.10.2 Visualization . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15
2 Constitutive Equation 16
2.1 Consistency viscoplastic model . . . . . . . . . . . . . . . . . . . . . . . . . . 16
2.2 J2 Flow rule . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17
2.3 Nonlinearity . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17
2.3.1 Nonlinear elasticity . . . . . . . . . . . . . . . . . . . . . . . . . . . 18
2.4 Finite Strain Theory . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19
2.5 Rate form and Objectivity . . . . . . . . . . . . . . . . . . . . . . . . . . . . 21
2.6 Constitutive Model for hypoelastic-Plastic base on J2 ﬂow theory . . . . . . 22
3 User Subroutines 24
3.1 General Information . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 24
3.2 Jonson Cook model and UMAT . . . . . . . . . . . . . . . . . . . . . . . . . 25
3.2.1 Procedure for Writing UMAT . . . . . . . . . . . . . . . . . . . . . . 25
3.3 Jonson Cook model and VUMAT . . . . . . . . . . . . . . . . . . . . . . . . 27
1

2 CONTENTS
3.4 UHARD and VUHARD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 29
3.5 Impanation of Subroutine . . . . . . . . . . . . . . . . . . . . . . . . . . . . 30
4 Result and Discussion 32
4.1 Friction and Barreling . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 32
4.2 Empirical test . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 34
4.3 Result and Discussion . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35
4.4 Future Work . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35

Introduction
Finite element analysis is the most famous method in modeling the physical phenomena.
Nowadays, varieties of commercial FEM program are introduced by developing companies.
The powerful designing tools, dominant FEM solver cause many research and development
groups get very effective assistance from the commercial FEM program. ABAQUS as a pow-
erful finite element software package is used in many different engineering fields throughout
the world. ABAQUS performs static and/or dynamic analysis and simulation on structures.
It can deal with bodies with various loads, temperatures, contacts, impacts, and other envi-
ronmental conditions.
In practical regards, Hot Compression test as one the standard test is very famous to
research on the constitutive equation in viscoplastic condition in metals. This constitutive
equations use in more complex simulation when the processes face with multifarious circum-
stance. Developing FEM modeling in material constitutive equation which predicts material
behaviors under different conditions is possible by providing the facility for users to specify
their own material models in commercial FEM program.
In ABAQUS, two user subroutines handle the user material modeling that large amount
of information is passed into the material subroutines relating to the beginning and end of
a time increment. In particular, stress, strain, temperature, and deformation gradient are
provided at the beginning of the time increment. Also some of these variables like Strain
and the deformation gradient are provided at the end of the increment. Three tasks must
be done by code: First, the stresses at the end of the time increment must be determined
and, second, for the case of an implicit analysis using ABAQUS standard,, the material
Jacobian must be updated. Third, any state variables must be updated at the end of the
time increment.
At the present report we discussion about modeling of Hot Compression Test in four
chapters. In chapter 1, the principles of ABAQUS for modeling hot compression test is
introduced. Chapter 2 is deal with developing viscoplastic model in FEM method. Chapter
3 is concerning about the implantation of the material model in ABAQUS. All result and
discussion is presented in Chapter 4.
3

Chapter 1
Hot Compression Test Simulation
Hot compression test is famous method for researching on bulk workability and formability
and due to absent of neckline as occurs during tension test, makes compression suitable
test to conduct high strain test. But the friction resistance is major problem which cause
non-uniform stain and consequently non-uniform stress. Therefore finite difference analysis
is major assistance to calculate strain and stress through sample. In this chapter we discuss
about FEM method which is used to model the hot compression test in Abaqus.
1.1 Finite Element Method
The finite element method (FEM) is a numerical technique for finding approximate solu-
tions. Mostly these results must be obtained from partial differential equations or integral
equations. All FEM analysis generally consists of three steps:
• Pre-processing: consist of creating an model and mesh it, defined the boundary condi-
tion
• Processing : Solved the problem numerically according to the type of simulation
• Post-processing Results of simulation which is shown as charts and render pictures.
1.1.1 Abaqus
Abaqus FEM is the one of the famous program in the Finite Element Method which is
mostly write by python language and developing by designing some GUI development which
makes the program more user friendly. There are three core available in Abaqus to run pre
processing simulation or processing and post processing , ( Abaqus/CAE),Abaqus/Standard
and Abaqus/Explicit. [6]
4

5 CHAPTER 1. HOT COMPRESSION TEST SIMULATION
• ( Abaqus/CAE), which is used for drawing the subject meshing, define boundary condi-
tion and load for model (Pre-Processing) and also viewing the result (Post-Processing).
Also complex model can be imported to Abaqus/CAE.
• Abaqus/Standard: a general-purpose Finite-Element analyzer that employs implicit in-
tegration scheme (traditional).This method is used mostly in case of static and some
special quasi static problem. Due to high stability of standard method it has more
accurate result.
• Abaqus/Explicit: a special-purpose Finite-Element analyzer that employs explicit inte-
gration scheme to solve highly nonlinear systems with many complex contacts under
transient loads. Explicit method can handle dynamic problem and most quasi static
models. This method is very useful in case of Failure in material or in the model.
1.2 Pre-Processing
Pre processing of simulation are the main task in make simulation in Abaqus. There are
eight modules which must be consider during the design of the Hot Compression Test in the
Abaqus. These modules are:
• Part - Create individual parts
• Property - Create and assign material properties
• Assembly - Create and place all parts instances
• Step - Define all analysis steps and the results of important vaiables
• Interaction - Define any contact information
• Load- Define and place all loads and boundary conditions
• Predefined Condition-Define initial Condition
• Mesh - Define nodes and elements
• Job - Submit job for analysis
• Visualization- View results
1.3 Part and Assembly
( Abaqus/CAE) is Computer-Aid Engineering to help for pre-process and post-process in
Abaqus. The main application of this feature is the designing the simple to complex model.
In this project, part module of the ABAQUS/CAE is utilized to design two parts

Figure 1.1: Assemble of the model
• Bulk as deformable body
• Press as a analytical rigid body.
Another valuable module in ABAQUS/CAE is Assembly module that helps to assemble
individual parts by position constrain option. Also the coordination of part assembly must
be defined in assembly modules. Figure 1.1shows the final assembly of 2D model which is
consist of quarter of bulk and also the half of the above press. In rigid body is showed by
Wire that the properties and boundary condition must be defined by Referencee Point.For
both Press and Bulk the Surfaces and Set must be defined in the assembly for describing
contacts and boundary condition in the model.
1.4 Material
The material library in Abaqus is intended to provide comprehensive coverage of linear and
nonlinear, isotropic and anisotropic material behaviors. These material libraries consist of
constitutive model for Metals behaviors, Composite, Polymers and much general type of ma-
terial which is used in industries and research area.Generaly these materials can categorized
as below:
• general properties (material damping, density, thermal expansion);
• elastic mechanical properties;
• inelastic mechanical properties;
• thermal properties;

• electrical properties; and
• acoustic properties;
• hydrostatic fluid properties;
• mass diffusion properties;
• Failure properties
But in reality there are many types of constitutive models which describe unusual material
behavior and new models for research that they are not included in the Abaqus material
library. Therefore for developing new models especially in the failure condition researching,
the Abaqus have interfaces that allow the user to implement general constitutive equations
for specific model.This user subroutines allow the programs to be customized for particular
applications. These constitutive equations must first be adopted to the ABAQUS language
and written by user as code either in Fortran or C++. In ABAQUS material user subroutines
divided in two groups [3, 6]:
• In ABAQUS/Standard the user-defined material model is implemented in user subrou-
tine UMAT.
• In ABAQUS/Explicit the user-defined material model is implemented in user subroutine
VUMAT.
The characteristic and difference of these two types of subroutine are discussed in the
next chapter.
1.5 Contact
Contact establishing in ABAQUS for simulation compression test is consist of three steps:
• Define one surface as hard surface which is rigid so it is defined as Master Surface
• Define one surface as deformable surface which is defined as Slave Surface
• Define properties of contact like friction, heat generation.
Contact condition between rigid body and the deformable bulk is established by using
Abaqus Surface-to-Surface and Node-to-Surface formulation. The difference between this
two technique lies in the
• stress result accuracy: Surface-to-Surface discrimination provides more accurate stress
and pressure results than Node-to-Surface discrimination.

• penetration of nodes of surface of deformable body as slave surface into the surface of
rigid body as master surface.
In this project the contact condition are not very complicate and also the results are not
very sensitive to the contact properties so surface-to-surface is the best choice. Moreover,
the friction properties which discussed later is included.
1.6 Step
Step option defined the analysis technique, period time and increments and other parameters
which program must be run the simulation according to them. Simulation can have a simple
step or multi steps.
Correct solution depend to select suitable analysis technique for specific problem.Analysis
techniques in Abaqus is designed for different conditions and problems which makes this
FEM program very effective. Explicit method calculate the solution at a later time from the
solution at the current time but implicit methods is solving an partial equation by considering
both the current and the later state.In specific case for Abaqus implicit and explicit deafened
as below:
• Implicit Analysis:
An Implicit FEM analysis is the same as Explicit with the addition that after each
increment the analysis does iterations to enforce equilibrium of the internal structure
forces with the externally applied loads. The equilibrium is usually enforced to some
user specified tolerance. So this is the primary difference between the two types of
analysis, implicit uses iterations to enforce equilibrium. This type of analysis tends to
be more accurate and can take somewhat bigger increment steps. One drawback of the
method is that during the iterations one must update and rebuild the stiffness matrix in
each iteration. This can be computationally costly and make the procedure not stable
in some case. Also for the reason of dependance of the next step to previous step the
failure condition cannot model by implicit method.
• Explicit Analysis:
An Explicit FEM analysis does the incremental procedure and at the end of each in-
crement updates the stiffness matrix based on geometry changes. Then a new stiffness
matrix is constructed and the next increment is applied to the system. In this type of
analysis,the increments should be small enough for accurate results. One major problem
with this method is many small increments for good accuracy makes it time consuming
procedure. If the number of increments is not sufficient the solution tends to drift from
the correct solution. Furthermore this type of analysis cannot solve some problems. In
some cases there are very hard to reach stabilized solution in explicit

1.6.1 Lagrangian and Eulerian
Lagrangian and Eulerian analysis technique are very famous in the FEM which effect on
result significantly. In a traditional Lagrangian analysis nodes are fixed within the material,
and elements deform as the material deforms. In opposite side, in an Eulerian analysis
nodes are fixed in space, and material flows through elements that do not deform. Eulerian
elements may not always be completely full of material.
Therefore, The Eulerian material boundary must be calculated in first of each time in-
crement.Eulerian analysis are effective for applications involving extreme deformation, like
fluid mechanics, metal forming and dynamic motion. Due to in traditional Lagrangian ele-
ments become highly distorted and lose accuracy in the case of using it new method which
helps to reduce the distortion is essential .For example for large deformation condition due
to high distortion of mesh during the procedure the Eulerian method is very suitable and
using adaptive mesh is very simple.
By above description about Lagrangian and Eulerian method it is necessary to mention
in Abaqus the Eulerian method is only available in explicit method which design to calculate
the state variable at the current time step. Figures 1.2 and 1.3show the schematic concept
of Lagrangian and Eulerian method.
Figure 1.2: Lagrangian mesh
[h]
1.6.2 Increment
Time Increment is the small fraction of step times period which stress and all state variable
update in the end of of time increment. Stability of system, accuracy of result strongly de-
pend on the time increment. By increasing the time increment the solution accuracy increase

Figure 1.3: Eulerian Mesh
and also system become unstable. By means of small time increment the computational cost
increase significantly.
In ABAQUS/Standard the increment time is calculates either automatically by program
or fixed by user. Fixed time increment cause instability when it is large size and increase
in computational cost when it is small, due to this reason in most case program calculate it
automatically by inserting initial, maximum and minimum values of time increment by user.
The main criterion for program is reaching equilibrium and stability during time increment.
In ABAQUS/Explicit, program calculates the time increment by itself according to boundary
condition, mass scale, load scale and etc.
1.7 Mesh
Mesh technique in finite element method is dividing the whole model in small fraction which
is named element. This element, depend on model can be contained some properties which
satisfy the mechanical, thermal or any scientific properties of real sample. In the case of
dimensional Abaqus has
• one-dimensional elements
• two-dimensional elements
• three-dimensional elements
• cylindrical elements
• axisymmetric elements
• axisymmetric elements with nonlinear, asymmetric deformation

in the case of analytical the Abaqus element library contains the following:
• stress/displacement elements, including contact elements, connector elements such as
springs, and special-purpose elements such as Eulerian elements and surface elements;
• pore pressure elements;
• coupled temperature-displacement elements;
• coupled temperature-pore pressure displacement elements;
• heat transfer or mass diffusion elements;
• forced convection heat transfer elements;
• incompressible flow elements;
• coupled thermal-electrical elements;
• piezoelectric elements;
• acoustic elements
• hydrostatic fluid elements; and
• user-defined elements.
The stress/displacement element is used in this project due to this element is used in the
modeling of linear or complex nonlinear mechanical analysis that possibly involve contact,
plasticity or large deformations. Stress/displacement elements can also be used for thermal-
stress analysis, where the temperature history can be obtained from a heat transfer analysis
carried out with diffusive elements.
1.8 Adaptivity
Adaptivity technique is the method which the mesh at the beginning or through one step
can modified according to results or errors in the system to optimize the results. The
concentration one state variable which needs more accurate calculation in one point, mainly
at corner or mesh distortion in high deformation model can be some reason that force user
to utilize adaptive mesh or remesh during the analysis.
Adaptive mesh cab be increased the computational cost very rapidly, so the good design
for these method can decrease the simulation time. Three adaptivity techniques are available
in Abaqus:
• Arbitrary Lagrangian Eulerian (ALE)

• Adaptive remeshing
• Mesh-to-Mesh solution mapping
The ALE adaptive mesh and Mesh to Mesh solution mapping is used in this project to
reduce the mesh distortion in ABAQUS/Explicit and ABAQUS/Standard respectively.
1.8.1 ALE Adaptive remeshing
Arbitrary Lagrangian Eulerian (ALE) adaptive meshing is very useful tools in ABAQUS/Explicit
but in some specific case it available in ABAQUS/Standard. ALE adaptive meshing pro-
vides control of mesh distortion. ALE adaptive meshing uses a single mesh definition that
is gradually smoothed within analysis steps. Adaptive meshing consists of two fundamental
steps:
• creating new mesh, through a process called as sweeping,
• remapping the solution variables from the old mesh to the new mesh through a process
called as advection.
Figure 1.4, 1.5 and 1.6 shows initial mesh of bulk, mesh configuration at ε = 0.5
without and with using ALE adaptive mesh respectively. As it shows the mesh configuration
without adaptive mesh lost its shape and properties and result from this method is not useful.
By using adaptive the configuration of mesh reach more smooth shape and by increasing
sweeping the results obtain more accurate.
Figure 1.4: The initial mesh size of bulk
1.8.2 Mesh-to-Mesh solution mapping
In the ABAQUS/Explicit the advantage of adaptive mesh can help to reduce the distortion.
In ABAQUS/Standard Mesh-to-Mesh solution mapping is very useful tools when the mesh

Figure 1.5: The mesh configuration of bulk without Adaptive Mesh
Figure 1.6: The mesh configuration of bulk with Adaptive Mesh
distortion during simulation. The procedure can describe as below:
1. Run the job1 until the mesh is not very distort
2. Extract the deformed bulk last from the last increment of job1
3. Make a new model which the extracted deformed bulk is the bulk in the new model
4. Make all modules like steps and boundary condition,... in the new model
5. Make new step
6. Make new mesh
7. Make the job2 and by using the Write Input File option make a input file for new model
8. By using *MAP SOLUTION command in the input file which transfer all the nodes
data to the new mesh
9. Run the simulation and repeated all these steps if the mesh are distort significantly
10. In the ABAQUS/Visualization module these entire files combine together
11. If the result is not very continues or jump significantly, it needs to reduce time of each
simulation.

Figure 1.7: Boundary condition
1.9 Boundary Condition
Boundary condition in Abaqus is varied from symmetric condition, displacement, velocity
and acceleration. This boundary can apply on surface, node or reference point. In this
project according to figure() the one quarter of the sample model due to axisymmetric is
design. Two boundary condition is necessary to defined the axisymmetric condition in the
left(X-Symmetric) and below(Y-Symmetric) surface. The velocity with constant strain rate
is applied to the reference point of the press. Figure 1.7 shows boundary condition.
1.9.1 Predefined Field
Predefined Fields defined the
• temperature
• field variables
• equivalent pressure stress
• mass flow rate
during the analysis.
By using this option we designed the temperature in the initial step.

1.10 Processing and Post-Processing
As mention before each simulation have three steps. The pre-processing step is discussed
previously and the next two step processing and post-processing steps discuss in this section.
In ABAQUS the solving step mostly handles by program. Below modules are used for
running the process and view the results.
• Job - Submit your job for analysis
• Visualization- View your results
1.10.1 Job, submit and Running
Defining Job module is consist of three steps:
1. The type of Job which can be
• full analysis when a job does all the analysis
• restart analysis when the analysis divided into several parts. This option is very
useful in mesh to mesh adaptive mesh.
• recover analysis when the analysis terminated by this option, the simulation can
continue from abrupt point.
2. select the subroutine file in the case of one or several modules use the subroutine.
3. In the ABAQUS/Explicit due to high number of increments which are used for solving
most of simulation the precision of the analysis must be accurately define.
The job must submitted and the input file writing in work directory and analysis running.
After running of analysis is completed, the result is available from Visualization modal.
1.10.2 Visualization
Visualization modules is designed to
• displays the final results of request variables.
• export data from the abaqus to Report,Image or Movie format, Excel and etc.
The usage of result is strongly related to the Result History Request which user defined by
step modules. Also all state variable of user defined subroutine can be visible in visualization
module. These possibilities can be huge assistance to reach accurate answer.

Chapter 2
Constitutive Equation
The viscoplastic consistency model is most popular formulation to integrate of a thermovis-
coplastic constitutive for von Mises or J2 plasticity and adiabatic conditions. The consistency
condition includes strain rate and the effect of temperature on the yield function simultane-
ously. In this chapter basic kinematics of finite deformations and its relation to viscoplastic
consistency model is described. Also nonlinearity in FEM modeling and rate formulation of
high deformation process are defined.
2.1 Consistency viscoplastic model
For modeling viscoplasticity which rate effect on the plastic flow must be considered, two
different models are proposed [8, 9]
• Perzyna viscoplastic model
• Consistency viscoplastic model
Perzyna viscoplastic model feature assumes yield function f can be more than zero which is
lead to overstress condition. Also rate dependency is not included yield function f. In Perzyna
model, the viscoplasticity theory based on overstress, like many other recently proposed
theories, does not consider creep and plasticity separately. They are sometime called unified
theories. In these theories the total strain rate is the sum of the elastic and inelastic strain
rates.
Wang proposed the second model as a consistency model. In this mode rate-dependent
plasticity can be formulate by considering the rate of the state variable like strain.[9]. Otto
M. Heeres et al.[8] demonstrated that consistency model which proposed by Wang has more
coverage compare to Perzyna viscoplastic model.
16

17 CHAPTER 2. CONSTITUTIVE EQUATION
According to the Wang or consistency model yield function f describe by
f = f(σ,
−→
k
˙−→
k ) (2.1.1)
.
in viscoplastic model the only state variable is equivalent plastic strain so
−→
k = and
˙−→
k = ˙
f =
∂f
∂σ
: ˙σ +
∂f
∂ε
˙ε +
∂f
∂ ˙ε
¨ε (2.1.2)
2.2 J2 Flow rule
There is three approaches which is concerned about phenomenological description of large
inelastic (plastic) deformation [7]
• The elementary theory
• Theory of plastic flow
• the general theory of inelastic deformation
The theory that we are concern about it, is Theory of plastic flow which assumes a ideal
plastic material behavior. These theory for satisfy field equation use consistent theory which
is mention in Section 2.1 .[7]
J2 flow theory plasticity is mention to the second stress invariant J2 which is defined as
J2 = (1
2σ : σ)1/2 [5].This theory base on the von Mises yield criterion. The yield criterion
and plastic flow direction are base on deviatoric part of the stress tensor[11].
2.3 Nonlinearity
The Nonlinearity FEM analysis is structure stiffness change during deformation (in general
case force) is applied. The nonlinear arise from three facts
• Material nonlinearity (e.g. polymer)
• Boundary condition nonlinearity
• Geometry nonlinearity

Figure 2.1: Rotation and displacement of the mesh after 60 percent deformation
In the case of material nonlinearity the metal has linearity in elastic region and nonlin-
earity in plastic region. Polymer and Rubber mostly behave nonlinearity in both elastic and
plastic region. Nonlinearity in boundary conditions happens when during the simulation the
boundary conditions change. The case of compression test the boundary conditions due to
change in amount of force and speed and at high deformation, the new surfaces make contact
with tools are not linear. Moreover, Large deformation cause nonlinearity in geometry which
is considerable when both rotation and displacement. This means in the FEM approach,
the mesh has both displacement and rotation due to frictional force which appears between
the tools and the surface of materials. Figure 2.1 shows the rotation of the mesh due to
frictional force.
The fact is the main nonlinearity in the FEM modeling of large deformation problem arise
from geometrical condition. In coming section the more focus is on the solutions to obtain
reasonable response.
2.3.1 Nonlinear elasticity
Three constitutive laws were published to define nonlinear elasticity. Two models are more
popular for describe nonlinear elasticity during high deformation [13]:
• Hyperelasticity which is mostly use when nonlinearity of material in elastic region is
significant. For instant, during simulation of rubber or elastic foam polymer. Assump-
tion of existence of a specific free energy per unit volume ψ which is function of left
Cauchy-Green strain and internal variable. In the linear elasticity the relation between
stress and strain defined by stored energy W by
σ =
∂
∂ε
(
1
2
: c : ) (2.3.1)

For nonlinear regime a hyperelastic constitutive model is
σ =
2
J
F
∂ ˆW
∂C
.FT
(2.3.2)
• Hypoelasticity is the main important constitutive law to defined material with re-
versible elastic. In linear elasticity the relation between stress and strain rate introduce
by
˙σ = c : ˙ (2.3.3)
and in nonlinear relation it can be introduced by
ττ
= a : d (2.3.4)
The constitutive equation (2.3.4) is called hypoelastic model. This model is not a good
constitutive equation but in the case of an axisymmetric upsetting problem it seems
same result is obtained[13].
2.4 Finite Strain Theory
Finite strain theory or large strain theory is mathematical theory which deals with the
situation that deformation and rotation both has large magnitude. In this case the deformed
and undeformed configurations of the sample are significantly different from each other. On
other hand, infinitesimal strain theory or small deformation-rotation theory emphasizes on
the case of small deformation and rotation.
During FEM simulation of Hot Compression Test, large deformation is occurred. Ro-
tation and displacement of mesh both are considerable. The change in body which is con-
tinuum has two part, displacement and deformation. Also displacement part of is consist of
translation and rotation.
In general approach, finite deformation theory attempts to relate velocity gradient L = dv
dx
to stress and strain rate. For reaching this point F as the deformation gradient which maps
the dX as reference configuration to dx in the deformed configuration is proposed. The F
is major parameter which can calculate elastic and plastic strain. In figure 2.2 F and the
elements of F is shown.
dx = F.dX (2.4.1)
Multiplicative decomposition of deformation gradient in finite deformation is introduce
by separation F to two part elastic part of deformation Fe and plastic part of deformation
Fp which means the deformation gradient in free force condition.

Figure 2.2: Deformation gradient F has two parts elastic and plastic part
F = Fe
Fp
(2.4.2)
By substitute Eq. (2.4.1) in Eq. (2.4.2)
dx = F.dX = Fe
Fp
.dX (2.4.3)
so by get derivative from both side
˙dx = ˙FdX = ˙FF−1
dx (2.4.4)
L =
d ˙x
dx
= ˙FF−1
(2.4.5)
by assumption of small elastic strain (which is discuss in future section), can approxi-
mately write the multiplicative decomposition into additive decomposition of the velocity
gradient
L = Le
+ Lp
(2.4.6)
L as velocity decomposition has two part L = D + W which D is symmetry part of
velocity gradient and is called the the rate of deformation and antisymmetric part W is
named continuum spin, so
L = D + W (2.4.7)
which

D =
1
2
(L + L−1
) (2.4.8)
and
W =
1
2
(L − L−1
), (2.4.9)
Dunne [5] shows for small elastic stretches and by using Eq. (2.4.8) and (2.4.9)
D = De
+ Dp
(2.4.10)
Eq. (2.4.10) is the base assumption of constitutive equation which hypoelastic -plastic
material is expressed which we shall return to it later.
2.5 Rate form and Objectivity
In nonlinear finite element, many constitutive models are proposed in rate form as the relation
between stress rate and strain rate (deformation rate). The important subject is constitutive
equations must be frame indifferent or objective. However, objectivity (frame independently)
of constitutive equations is very important by making strain and stress objective. To reach
the
x ∈ Ωt → x+
= c(t) + Q(t).x (2.5.1)
Which c(t) is a ”rigid” translation and Q(t) a rigid rotation.
The Doghri[2] prove that the deformation gradient F, right Cauchy-Green strain C, veloc-
ity gradient L, rate of deformation d, spin tensor ω, Cauchy stress σ and Kirchhoff stress τ
are objective. But the material time derivative of Kirchhoff or Cauchy stress is not objective.
Non-objective stress rate cause huge oscillation happen during solving when our algorithm
is rate-depend. .Three type of objective derivative of stress or stress rate are defined
• The Truesdell rate
• The Green-Naghdi rate
• The Jaumann rate

The Truesdell rate has very accurate but implantation of this model is not very easy.
Green-Naghdi rate is simplification of Truesdell rate when we get R W and the Jaumann
rate Jaumann rete is defined by
τ = ˙T − W.τ + τ.W (2.5.2)
which is most useful rate form formulation in nonlinear FEM modelin.
Using this type of algorithm Abaqus uses a Green-Naghdi rate and Jaumann, i.e., the
stress and rate of deformation are rotated to the reference configuration before the constitu-
tive relation is evaluated. Everything is then rotated back to spatial coordinates.
2.6 Constitutive Model for hypoelastic-Plastic base on J2 flow the-
ory
For this project which performed in ABAQUS, some of the above steps run by FEM software.
The strain is calculated. The information before imported to UMAT or VUMAT for writing
codes is rotated automatically by program. In UMAT and VUMAT the formulation is
Hypoelastic and rotation for reaching objective stress is performed by Jaumann rate. So
these two steps eliminated from our subroutines.
Only the updating stress and state variables must be done. For describing the relationship
between stress- strain we must establish constitutive equation which must contain[10]:
• The trial stress must be calculate according to Von Mises or J2 plasticity.
• Yield criteria: predict whether the solid responds elastically or plastically
• The decomposition of strain into elastic and plastic parts
• Strain hardening law which is related strain hardening and plastic strain
• Update the Jacobian Matrix for UMAT and state variables
In this project the yield function is defined by
f = ¯σ − σY (¯p
, ˙¯p
, T) (2.6.1)
The σY can be one of Johnson and Cook , Bodner, Zerilli, Litonski or Rusinek and
Klepaczko model. These models
¯σ is effective or equivalent stress and ˙¯p is effective plastic stress rate which are defined
by Von Mises

¯σ =
√3
2
S : S (2.6.2)
So the Von Mises yield function is obtained
In the next the implantation of these steps in User Subroutine is discussed.

Chapter 3
User Subroutines
User Subroutines in finite element programs are very common to specify the properties of
the simulation. The properties might be boundary conditions, material constitutive model,
mesh, adaptive mesh properties and etc. The abilities of program and simulation task define
that the new user subroutine is required or not. But using this application increases time
of simulation and also equipment cost. In this chapter the subroutine code for defining
viscoplastic behavior is describing.
3.1 General Information
The user subroutines in Abaqus mostly write in Intel Fortran as professional compiler.
This code must be linked to simulation code by setting environment in operating system.
Two parts are important in writing the subroutine codes:
• The interface of subroutine which is constant for all of the subroutines. It is consist of
introduce the input and output variable, dimensions and parameters which are using in
code.
• The constitutive model which is finally update stress and state variables and store them
in output variables. This constitutive model can be elastic, plastic, viscoplastic or any
type of materials.
Moreover, variables in user subroutines are also can classified in three groups
• Variables to be defined like stress, effective stress, plastic strain and etc.
• Variables that can be updated like stored energy
24

25 CHAPTER 3. USER SUBROUTINES
• Variables passed in for information like increment time and Number of direct compo-
nents in a symmetric tensor, Number of indirect components in a symmetric tensor and
etc. This variable is very important when user have non uniform constitutive model.
In the coming section, the UMAT and VUMAT subroutine for viscoplastic constitutive
model is described.
3.2 Jonson Cook model and UMAT
As mention in chapter 2 the viscoplastic is a theory in mechanical engineering which mainly
describe the material behavior under rate-dependant inelastic. The UMAT Model of vis-
coplastic material are available by using ﬂow stress (or yield stress) model. These models
can be empirical or empirical-Theoretical. The below list shows some important viscoplastic
models
• Johnson-Cook model
• Zerilli-Armstrong model
• Mechanical Threshold Stress model
• Preston-Tonks-Wallace model
• Steinberg-Cochran-Guinan-Lund model
Among these models Johnson-Cook model is purely empirical.
σ = (A + Bεn
p )(1 + Clog( ˙εp/ ˙εp0 ))(1 + (T∗
)m
) (3.2.1)
which
T∗
= (T − T0)/(Tm − T0) (3.2.2)
The A constant is yield point and B, C, m and n are material constants. Also Tm is
melting temperature, T0 is reference Temperature and ˙ε0 is reference strain rate which is
used for determination of A,B and n.
3.2.1 Procedure for Writing UMAT
Implicit ABAQUS / Standard is very eﬀective to achieve a more accurate constitutive in-
tegration, and application of Johnson-Cook model. This needs to ABAQUS / Standard

Figure 3.1: UMAT insert for calculation new stress and Jacobian Matrix
UMAT user material subroutine programming. In the UMAT Programming with the rate
dependent plasticity theory, and fully implicit stress update algorithm.
UMAT subroutine with powerful features:
• can be used to deﬁne the material constitutive relationship; using the ABAQUS material
library materials are not included in the calculation, the expansion program function.
• can be used for the mechanical behavior of almost any analysis can take ABAQUS user
material properties given in any unit;
• must be provided the Jacobian (Jacobian) matrix, that is, the stress increments to
strain increments The rate of change
 = ∂ σ/∂ ε
The below ﬁgure shows how UMAT insert to the simulation.
As mentioned above, the Abaqus subroutines must update the stress and state variables
and return the Jacobian matrix to help simulation to reach accurate coverage in result. For
implantation of implicit integration for isotropic hardening viscoplastic material the below
procedure is applied in the subroutine:

1. calculate the trial elastic stress
2. call UHARD to calculate yield stress σy by using Johnson Cook thermo-viscoplastic
model.
3. calculate f = σ − σy
4. if the f is more than zero, then by irritation processes we must find the plastic strain εp
and plastic strain rate ˙εp until f = σ − σy reach zero
5. Update the stress, plastic strain and other variables
6. Make jacobian matrix
Integration in UMAT
According to implicit model first assume the material goes only in elastic part and then by
using yield point the f = σ − σy is calculated. If the f is more than zero the material goes
in plastic region which is means the strain has two part 1) elastic 2) plastic. So according
to additive theory of strain ε = εe + εp. The plastic strain must be calculated to obtain new
yield point from Johnson Cook model. Below iteration process finds plastic strain:
1. estimate the plastic strain that the classical radial return algorithm for strain hardening
is done by assuming no strain rate and temperature effects are considered.
εp =
f
3G + H
(3.2.3)
which H is strain hardening H = ∂σ
∂ε . G is elastic constant G = E
2(1+ν)
.
2. estimate the strain rate according incremental time step and plastic strain ˙p = p/ t .
3. the yield point and hardening is calculated and if it is not satisfy the criteria the new
plastic strain must be defined.
4. this process is continued until the best coverage obtain
3.3 Jonson Cook model and VUMAT
The VUMAT interface is completely different with what the UMAT has. In this case the
explicit integration must be done to find the plastic strain. Also the Jacobian matrix which
must define by UMAT in the end of inclement is not necessary. In the case of VUMAT
the nodes identification does not insert into the subroutine. So all of the nodes information
insert to the VUMAT by matrix. Figure 3.2 shows how generally the VUMAT works.

Figure 3.2: VUMAT Subroutine ABAQUS/Explicit Flow chart

Integration in VUMAT
The implicit method to reach final answer for plastic strain was possible in the UMAT.
But in the VUMAT the irritation is not possible, instead for numerical integration of elastic
viscoplastic models with hardening and rate dependence model in the VUMAT, the modified
return algorithm which was first proposed by O.Yu.Vorobiev [12] in AUTODYN program.
According to this modified algorithm:
εp = (1 − λ)σe/(3µ) (3.3.1)
λ is scale factor and σe is effective stress
Y = Y +
∂Y
∂εp
∆εp +
∂Y
∂ ˙εp
∆ ˙εp + . . . (3.3.2)
so by changing the last part
Y = Y +
∂Y
∂εp
εp +
∂Y
∂ ˙εp
∆εp
∆t
− ˙εp (3.3.3)
By using the value of λ as scale factor:
λ =
Y
σe
=
Y + A + B
σe + A
(3.3.4)
which
A =
σe
3µ
[
∂Y
∂εp
+
∂Y
∂ ˙εp
1
∆t
(3.3.5)
B =
∂Y
∂ ˙εp
˙εp (3.3.6)
If A → 0 and B → 0 the classical return algorithm is derived. This scheme mostly use
when the dependence of yield point to a variable and its derivative is significant.
3.4 UHARD and VUHARD
The UHARD and VUHARD are two subroutines in ABAQUS/Standard and ABAQUS/Explicit
respectively which use to calculate yield point and hardening ∂σ
∂ε . The main important fea-
tures of these subroutines are:

• called at all material points of elements for which the material definition includes user-
defined isotropic hardening or cyclic hardening for metal plasticity;
• can be used to define a material’s isotropic yield behavior;
• can be used to define the size of the yield surface in a combined hardening model
• can include material behavior dependent on field variables or state variables
• requires that the derivatives of the yield stress (or yield surface size in combined hard-
ening models) be defined with respect to the appropriate independent variables, such
as strain, strain rate, and temperature.
• In the case of dependence of the yield to strain, strain rate and temperature, the hard-
ening is a matrix with three elements. These elements are
H(1) =
∂σy
∂ε
, H(2) =
∂σy
∂ ˙ε
, H(3) =
∂σ
∂T
, (3.4.1)
The general features of UHARD and VUHARD subroutines are mostly like UMAT and
VUMAT and base on the input, output and consecutive model which update new yield point
according to input data.
3.5 Impanation of Subroutine
The UMAT and VUMAT are written under Visual Studio and Visual FORTRAN 11 envi-
ronmental setting and upload in the simulation. The code is verified [3] by using below tests
and the results are compared with standard results.
• Single and multiple element uniaxial tests.
• Single element simple shear test.
• Non-uniform strain and stress field
The main problem during the implantation is the simulation time. The simulation time
due to program refer for every increment to the subroutine, it takes very long time to
perform the simulation. Table shows the details for some simulation by using ABAQUS
material library and UMAT and VUMAT subroutine. These dates show significant increase
in time consuming when subroutines add to simulation.
In the next chapter the results from simulation are compared with experimental results.

hr:min:sec
Simulation Type Abaqus Library VUMAT UMAT
Elastic 00:00:5 00:00:25 00:00:21
Simple plastic 00:01:35 00:08:52 00:07:50
Viscoplastic 00:09:19 03:29:46 02:17:50
Project Model 00:17:19 28:55:32 42:49:20
Table 3.1: Comparing Simulation Cost Between Abaqus Library And Subroutines

Chapter 4
Result and Discussion
In this chapter, method to calculate stress in hot compression test in present of barreling is
discussed. Then the results of two compression tests are discussed with obtain results from
simulation. To compare the obtained results from experimental test and simulation, due
to variation results in simulation by changing the simulation method, the best results from
simulation is selected.
4.1 Friction and Barreling
Barreling during hot forming originates from this fact that the friction between tools and
sample is the phenomena which cannot eliminate, but it reduces by using good lubrication.
The friction factor m is measured to insert in formula for calculating correct amount of stress.
Also the main assumption for calculation is the value of m is constant during compression
test. This is true in small strain which is less than one but by increasing strain the new
surfaces are contacted with tools surface and cause in increasing the m value. There is two
methods are introduced for calculating or estimating the friction factor
• Numerical Simulation: In this method the best function is introduce for the relation
between m and other parameters like strain, strain rate, Temperature and etc, then
by running the simulation by changing the value of parameters we find the function
between m and other parameters.
• Analytical evolution: this method is introduced by R.Ebrahimi and A. Najafizadeh [4]
who are found the formula for calculation the m value by measuring final and initial
dimensions.
The second option is more accurate and faster than the first one. For these method the
below equations are proposed:
32

33 CHAPTER 4. RESULT AND DISCUSSION
Figure 4.1: Barreling in Hot Compression Test
m =
R
h b
4√
3
− 2b
3
√
3
(4.1.1)
where
b = 4
∆R
R
H
∆H
(4.1.2)
and
R = R0
H0
H
(4.1.3)
Also ∆R is the diﬀerence between maximum radius and minimum radius after compres-
sion. The ﬁgure 4.1 shows schematically these values.
By using these equations the friction factor is equal to 0.65 which shows high friction
between tools and sample. The strain calculate according equation 4.1.4

ε = ln(−
h
h0
= ln(1 −
∆h
h0
) (4.1.4)
Stress has more complicated condition. Due to friction and consequently inhomogeneity
through sample, equation 4.1.5 has not accurate results. So the equation 4.1.6 is the proposed
[1] for calculating actual stress. These equation shows lower stress actual stress compare to
true stress.
σ0 =
4P
πD2
(4.1.5)
σa = σ0(1 +
mD
3
√
3h
) (4.1.6)
4.2 Empirical test
The empirical tests are performed in MTS machine. This machine has three parts:
• The control system
• The compression tools
• Three lamps which reach the temperature to desirable temperature.
After sample is placed between two tools the lamps start to heat it to around test temper-
ature. Sample hold for around 30s in test temperature to make uniform temperature through
sample. After the test start to run at constant strain rate the force and temperature are
recorded by control system.
This part of this project held by conducting two tests which the geometrical data of
samples and test conditions are deﬁnes in table 4.1.
Sample Data
Sample Height Diameter Strain Strain Rate Temperature
SV17 12.3 9.7 0.35 0.5 300
MG79 12 10 0.75 0.5 300
Table 4.1: Sample Geometrical and Test Data

Figure 4.2: The schematic of MTS machine
4.3 Result and Discussion
The figures 4.3 and 4.4 show comparison between the results from simulation and experi-
mental test. According these figures the elastic parts in stress-strain experimental curves
are not very fit to the simulation curve. The one probable reason for this inaccuracy is raise
from the temperature of the test. Test is conducted at 300C which is not hot compression
test and it categorized in warm working. In this condition maybe it is better to change from
Hypoelastic modeling to Hyperelastic modeling which can handle the material with larger
plastic region. Also, the plastic parts of experimental stress-strain curve has good trend
with simulation but the differences between these two curves are not significant. In the high
strain, the result from simulation shows more softening compare to experimental test.
4.4 Future Work
This project is a initial step in the field of FEM simulation of high deformation compression
process. The more investigation is essential to improve integration algorithm and adaptive
meshing. Also writing new subroutine according to the Hyperelastic formulation of constitu-
tive equation is recommended. The VUMAT code also can be developed to model the Shear
Bands in the metals. Also more experimental test must be conduct to have more comparing
and accurate conclusion.

Figure 4.3: The comparison between SV17 and the simulation
Figure 4.4: The comparison between MG79 and the simulation

List of Figures
1.1 Assemble of the model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6
1.2 Lagrangian mesh . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9
1.3 Eulerian Mesh . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10
1.4 The initial mesh size of bulk . . . . . . . . . . . . . . . . . . . . . . . . . . . 12
1.5 The mesh conﬁguration of bulk without Adaptive Mesh . . . . . . . . . . . . 13
1.6 The mesh conﬁguration of bulk with Adaptive Mesh . . . . . . . . . . . . . . 13
1.7 Boundary condition . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14
2.1 Rotation and displacement of the mesh after 60 percent deformation . . . . 18
2.2 Deformation gradient F has two parts elastic and plastic part . . . . . . . . 20
3.1 UMAT insert for calculation new stress and Jacobian Matrix . . . . . . . . . 26
3.2 VUMAT Subroutine ABAQUS/Explicit Flow chart . . . . . . . . . . . . . . 28
4.1 Barreling in Hot Compression Test . . . . . . . . . . . . . . . . . . . . . . . 33
4.2 The schematic of MTS machine . . . . . . . . . . . . . . . . . . . . . . . . . 35
4.3 The comparison between SV17 and the simulation . . . . . . . . . . . . . . . 36
4.4 The comparison between MG79 and the simulation . . . . . . . . . . . . . . 36
37

List of Tables
3.1 Comparing Simulation Cost Between Abaqus Library And Subroutines . . . 31
4.1 Sample Geometrical and Test Data . . . . . . . . . . . . . . . . . . . . . . . 34
38

Bibliography
[1] H.A. Kuhn Design G.E. Dieter and S.L. Semiatin. Handbook of Workability and Process
Design. 2003.
[2] Issam Doghri. Mechanics of Deformable Solid,linear and nonlinear Analytical and Com-
putational Aspects. Springer, 2000.
[3] FIONN DUNNE and NIK PETRINIC. Introduction to Computational Plasticity, chap-
ter 6. OXFORD Uuniversity Press, 2005.
[4] R. Ebrahimi and A. Najafizadeh. J. Mater. Proc. Technol, 152:136–142, 2004.
[5] Nik Petrinic Fionn Dunne. Introduction to computational plasticity. Oxford University
Press, Republish 2006.
[6] ABAQUS Inc. ABAQUS/Explicit and ABAQUS/Standard v6.10 User Manual. 2010.
[7] Theodor Lehmann. Some remarks on the recent development of the foundations of the
theory of plasticity. Steel Research, 56(3):101–107, 1986.
[8] Ren de Borst Otto M. Heeres, Akke S.J. Suiker. A comparison between the perzyna vis-
coplastic model and the consistency viscoplastic model. European Journal of Mechanics
A/Solids, (21):1–12, 2002.
[9] J.Fernández-Sáez R.Zaera. An implicit consistent algorithm for the integration of ther-
moviscoplastic constitutive equation in adiabatic conditions and finite deformation.
Journal of Solids and Structures, 43(6):1594–1612, 2006.
[10] Henry Tan. Flow theory of plasticity. 2009.
[11] Brian Moran Ted Belytschko, Wing Kam Liu. Nonlinear Finite Elements for Continua
and Structures. Willy, 2000.
[12] O Yu Vorobiev. Improved numerical integration of elastic-viscoplastic models with
hardening and rate-dependence in autodyn. Structures under Shock and Impact VII,
pages 457–466, 2002.
[13] Gustavo Weber and Lallit Anand. Finite deformation constitutive equation and a time
integration procedure for isotropic, hyperelstic-viscoelastic solid. Computer Method In
Applied Mechanics and Engineering, 79(2):173–202, 1990.
39

Master Thesis

Recomendados

Recomendados

Más contenido relacionado

La actualidad más candente

La actualidad más candente (20)

Similar a Master Thesis

Similar a Master Thesis (20)

Master Thesis