A critical overview of machining
simulations in ABAQUS
MIKAELA ZETTERBERG
KTH ROYAL INSTITUTE OF TECHNOLOGY
Author: M. Zetterberg
Report No: KIMAB-2014-127 Swerea KIMAB Project No: 11187
Status: Open Date: 2014-11-20
Abstract
Metal cutting is one of the most commonly occurring manufacturing processes in the industry and ma-jor effort is made to improve its pro-cesses. Cutting tools are expensive and have a life length measured in minutes, why predictions of tool wear are of great interest. Finite Ele-ment (FE) simulations have a cen-tral role in the development of tools and cutting processes, but perform-ing simulations of metal cuttperform-ing is not easy. The method chosen for the chip formation has a large im-pact on the result of the simulations. The scope of this work includes a survey on important parameters and different possibilities to form a chip in simulations of metal cutting in ABAQUS/Explicit. Particular em-phases are placed the on prediction of flank wear and how the hard-ening implemented in the material model effects this. The approach has been to start with a literature study and thereafter make simulations in ABAQUS/Explicit. FE simulations, of cutting, with different damage criteria and simulations with SPH (Smooth Particle Hydrodynamics)-method are presented. None of the possibilities to form a chip in ABAQUS/Explicit, as implemented today, seems to be sufficient for
sim-ulations of cutting to predict flank wear. The SPH-method will be a good alternative for simulations of metal cutting in ABAQUS/Explicit if temperature dependency is imple-mented. The material model in gen-eral, the type of hardening in specific, has an impact on the chip-form and the stress state in the chip and work-piece. And thereby effects the flank wear.
Abstract in Swedish
Skärande bearbetning är en av de vanligast förekommande tillverkn-ingsprocesserna i industrin idag och mycket möda läggs ned för att för-bättra dess processer. Skären är dyra och har en livslängd som kan mätas i minuter, vilket gör att möj-ligheten att förstå och förutsäga nöt-ningen av skäret är av stort intresse. Finita element (FE) simuleringar har en central roll i utvecklingen av skärverktyg och skär processer, men att genomföra simuleringar av detta är långt ifrån enkelt. Meto-den som väljs, för att forma en spåna har stor påverkan på resul-tatet av simuleringarna. Detta ar-bete innefattar en utredning kring viktiga parametrar och olika möj-ligheter att åstadkomma spånformn-ing vid simulerspånformn-ingar av skärande bearbetning i ABAQUS/Explicit. Särskiljt har fokus legat på att kunna förutsäga nötning på skärets
släpp-sida och hur hårdnandet, som finns implementerat i materialmodellen, påverkar denna. Angreppssättet har varit att starta med en litter-aturstudie och därefter göra simu-lationer i ABAQUS/Explicit. Re-sultat från FE simuleringar, av skärande bearbetning, med olika brottvillkor och simuleringar med Smooth Particle Hydrodynamics (SPH)- metoden finns presenterade. Ingen av möjligheterna för spån-formning som finns implementerade i ABAQUS/Explicit idag är tillräck-ligt bra för att simulera nötning av skärets släppsida. SPH-metoden kan komma att bli ett bra alter-nativ för simuleringar av skärande bearbetning i ABAQUS/Explicit om temperaturberoendet blir im-plementerat. Materialmodellen, och mer specifikt typen av hård-nande, påverkar spånformen och spänningstillståndet i spånan och ar-betsstycket. Därmed påverkas också nötningen av skäret.
1 Introduction 1
1.1 Aim . . . 1
1.2 Methodology . . . 1
2 Basic concepts of machining processes 2 2.1 Geometric description of orthogonal machine cutting . . . 2
2.2 Deformation zones . . . 2
2.3 Friction . . . 4
2.4 Chip formation process . . . 4
2.5 Thermal processes . . . 4
2.5.1 Heat production . . . 5
2.5.2 Thermal effects in the workpiece and tool material . . 5
2.6 Tool wear . . . 6
2.6.1 Tool wear mechanisms . . . 6
2.6.2 Types of tool wear . . . 6
3 Finite Element Simulation of metal cutting 7 3.1 Arbitrary Lagrangian-Eulerian adaptive meshing . . . 7
3.1.1 Boundaries in ALE methods . . . 9
3.1.2 Mesh-update procedures . . . 9
3.1.3 Motion in ALE . . . 10
3.1.4 Stress-update procedures . . . 10
3.2 Chip - workpiece separation in an FE environment . . . 10
3.2.1 Adaptive Meshing . . . 11
3.2.2 Element failure models . . . 13
3.2.3 SPH simulation of metal cutting . . . 13
3.2.4 Eulerian models . . . 14
3.2.5 Path dependent parting . . . 14
3.3 Friction models . . . 15
3.3.1 Coulomb friction model . . . 15
3.3.2 Constant shear model . . . 15
3.3.3 Sticking zone and sliding zone model . . . 16
3.3.4 Friction in smooth particle hydrodynamic simulations 16 3.4 Heat transfer models . . . 16
3.4.1 Adiabatic assumption . . . 16
3.5 FE models of tool wear . . . 17
3.5.1 Tool wear rate models . . . 17
3.5.2 Cyclic implementation . . . 18 4 Material models 18 4.1 Hardening . . . 18 4.1.1 Yield criterion . . . 18 4.1.2 Flow rule . . . 19 4.1.3 Isotropic hardening . . . 19 4.1.4 Kinematic hardening . . . 20
4.2 The Johnson-Cook model . . . 20
4.3 Damage and failure models . . . 21
4.3.1 Progressive ductile damage initiation . . . 22
4.3.2 Progressive Shear damage . . . 22
4.3.3 Progressive damage evolution . . . 23
4.3.4 Cumulative Johnson-Cook damage . . . 23
5 Present model and simulation of metal cutting 24 5.1 Workpiece modeling . . . 24
5.1.1 Material physical property . . . 24
5.1.2 Workpiece, Johnson-Cook parameters . . . 24
5.1.3 Implementation of kinematic hardening component . . 25
5.1.4 Implementation of isotropic and kinematic hardening components . . . 26 5.1.5 Mesh density . . . 26 5.1.6 ALE . . . 27 5.2 Tool model . . . 28 5.3 System model . . . 29 5.3.1 Cutting conditions . . . 29
5.3.2 Contact and friction . . . 30
5.4 Chip - workpice separation method . . . 30
5.4.1 Ductile damage initiation . . . 30
5.4.2 Damage initiation Shear . . . 30
5.4.3 Damage initiation Shear and Ductile . . . 31
5.4.4 Johnson-Cook progressive Damage . . . 31
6 Results 32
6.1 Chip - workpiece separation . . . 32
6.1.1 Ductile damage initiation tabular . . . 33
6.1.2 Damage initiation Shear . . . 34
6.1.3 Damage initiation Shear and Ductile . . . 34
6.1.4 Johnson-Cook cumulative damage . . . 36
6.1.5 SPH . . . 37
6.2 Material model . . . 37
6.3 Cutting velocity . . . 39
7 Discussion and Conclusions 40 7.1 Contact problems . . . 40
7.2 Mesh, elements and remeshing . . . 41
7.3 Conclusions . . . 42
7.4 Future work . . . 42
8 Acknowledgements 42
1
Introduction
Machining is a very commonly used manufacturing process within the in-dustry and major effort is made to improve its processes. In both product development and customer relations, simulations of cutting is a widely used tool. Due to the large number of affecting parameters and the extreme range of conditions for these, machining is a very complex process [1].
In simulations of machine cutting, the simulation model must adequately handle: huge elasto-plastic deformations, thermal processes and complex interactions, all of which acts very rapidly. Due to this, the simulations are not trivial either from a numerical or from a physical point of view. There are quite a large number of parameters that effects the simulation result, and the parameters themself depend on each other in complex relations. One of the main problems in Finite Element (FE) simulations of cutting is to get the material separation around the tool tip to be physically cor-rect. Several techniques for performing FE simulations of chip - workpiece separation has been proposed during the last 20 years. One of the erlier models for chip - workpiece separation is path dependent parting and newer ones include frequent adaptive remeshing and more radical ones such as leaving the FE domain and using meshfree methods like Smooth Particle Hydrodynamics (SPH).
An important aspect for improvements of machining processes is tool life, restricted by tool wear. Tool wear can be divided into crater wear and flank wear, depending on where it acts. Flank wear is the wear on the relief face and crater wear is situated on the rake face of the tool. By increasing the tool life with a fraction of a minute a lot of money can be saved for the company operating the tool.
1.1 Aim
The aim of this thesis is to be a pre-study for coming simulations of orthog-onal cutting (with focus on tool wear, and even more specific flank wear) in ABAQUS. This pre-study covers a wide range of questions related to cutting simulations, of which the main questions for the study are:
Which are the important parameters for performing simulations of orthog-onal cutting?
What are the limitations when performing cutting simulations in ABAQUS/Explicit?
Which are the possible ways to perform chip - workpiece separation in cut-ting simulations?
Which of these possible ways are suitable for simulations in ABAQUS/Explicit?
1.2 Methodology
The questions are explored first in a literature study, presented in the theory Chapter and thereafter the investigation is continued by some simulations
in the commercial simulation software ABAQUS [2]. Both a Finite Ele-ment (FE) model with Arbitrary Lagrangian-Eulerian (ALE) formulation and a Smooth Particle Hydrodynamics (SPH) model is implemented and examined.
2
Basic concepts of machining processes
The process of machining consists of removing material from a workpiece, by means of shear deformation, with a sharp cutting tool. A motion of the workpiece relative to the tool is needed in order to achieve the removal. This motion is in most machining processes defined as a primary motion, called the cutting speed, which for the specific case of turning is the velocity with which the workpiece rotates. A secondary motion called feed rate, which for turning is the axial distance the tool advances in one revolution of the workpiece, is usually also defined.
The metal cutting processes used can be divided into two types: orthogonal cutting, where the tool’s cutting edge is perpendicular to the direction of motion, and oblique cutting where the cutting edge forms an inclination angle relative to the cutting direction [1]. Orthogonal cutting is rarely not existing in industry but it is common in research as a sort of simplification of the cutting process.
A full 3D-simulation of cutting is costly since the relatively sharp edge of the tool require a very fine mesh. Orthogonal cutting can be modelled as a two dimensional plain strain problem and is therefore more frequently investigated in research [3, 4].
2.1 Geometric description of orthogonal machine cutting
Figure 1 visualizes the geometry of the process of orthogonal cutting in two dimensions. It can be seen that the cutting tool has two sides, the rake face and the flank face. The rake face where the chip is formed is situated at an angle, called rake angle, relative the normal of the new surface. The flank forms a relief angle (or clearance angle) to the new surface. The difference in height between the original surface and the new surface is called the cutting depth.
2.2 Deformation zones
The chip formation is restricted to three main deformation zones, also called shear zones, which can be seen in Figure 2, called the primary, secondary and tertiary deformation zones. In the primary deformation zone the workpiece material is forced to a quick change in direction under severe shear plastic straining [1]. In the secondary deformation zone, situated along the rake face of the tool, plastic deformation as well as friction is occurring and both of them are producing heat [6]. In the tertiary deformation-zone there exists shearing due to surface friction [7].
Figure 1: Geometric description of a basic machining process in 2D. Figure
by Emesee [5].
2.3 Friction
Frictional forces is at action between the tool and workpiece. The con-tact area can be divided into two types of regions with different frictional behaviour: the sticking region and the sliding region [9].
The frictional contact does not follow the classical friction models in the sticking region, as it has been observed to e.g. be independent of normal load [1]. This is an effect of the frictional stress being greater then the yield stress in the specific region, causing the material to deform rather then slide along the surface of the tool [10]. Different friction models for simulations are described in Chapter 3.3 on Page 15. More advanced friction models exist but they are hard to verify experimentally due to the extreme conditions in the contact region [1, 9].
2.4 Chip formation process
The chip formation process, which starts in the primary deformation zone, is by some authors described as a material flow around the tool tip while by others it is described as a crack that moves ahead of the tool tip splitting the material like in splitting of wood [1].
The physics of chip separation is a key issue that has not yet been fully understood [9]. A large number of different (but internally related) physi-cal phenomena, e.g. large plastic strain, damage, friction, heat generation, exists in the deformation zone where the chip separation occur.
The process of chip - workpiece separation can be described as follows. In the beginning of the process a stress concentration in front of the tool tip is built up when the tool moves towards the workpiece. When these stresses reaches a certain limit an elasto-plastic zone forms in the workpiece (considering ductile material). The sizes of the elastic and the plastic parts of the zone is related to the ductility of the workpiece material [9]. For more brittle materials it is assumed that a crack opens up in front of the cutting edge [9].
Often the cutting process can be characterized by the type of chip produced. General categories of chips are continuous, discontinuous, continuous with built-up edges and shear-localized as can be seen in Figure 3. The different types of chips indicates different types of physical processes and which type is formed is dependent on cutting and material conditions.
2.5 Thermal processes
With temperatures around the melting point, thermal effects have a signif-icant influence on the tool wear in metal cutting. As can be seen in some wear rate models like those by Usui and Takeyama & Murata’s wear rate model, described in Chapter 3.5.1 on Page 17, the temperature on the tool surface is one of the key parameters of the tool flank wear.
Figure 3: The four most common chip forms for a) discontinuous b)
con-tinuous c) concon-tinuous with built-up edges and d)shear-localized chip formation. Figure from Irander [11]
2.5.1 Heat production
There are two main sources of heat production in metal cutting: heat pro-duced by plastic deformation and heat propro-duced by friction.
For the heat produced by plastic deformation many studies assumes that 90% of the plastic deformation energy is converted to heat [10, 12]. This conversion of energy is mainly localized to the deformation zones since it is there the major part of the plastic deformation occurs [1].
In the case of friction induced shear stress [1] it can be assumed that all the frictional energy is turned into heat [10] and this heat is often considered to be conducted equally to the workpiece and to the tool [12].
The heat generated in the workpiece will be conducted to the tool and dissipated both from the tool and the workpiece by heat convection and radiation.
2.5.2 Thermal effects in the workpiece and tool material
Temperature rise largely effects the material parameters in both workpiece and tool. It induces thermal strains [9] and makes the material expand (thermal expansion). Also the strength of the material generally decreases with increasing temperature[9], this effect is referred to as thermal softening which is a special case of the hardening process and furthermore, increasing temperature also increase the ductility of the material [1].
2.6 Tool wear
Tool wear has a major influence of the economy of the machining operations. Process conditions chosen to optimize economy or productivity often result in a tool life measured in minutes [13]. Thus, improvements in the under-standing and prediction of tool wear in metal cutting are very important. The tool wear also effects the chip formation and the residual stresses in the new cut surface.
For optimizations of the cutting processes in order to increase the tool life, tool life models such as the famous Taylor’s equation with extension, that states relations between tool-life and process parameters e.g. cutting speed can be used [12]. In this work, the focus is on tool wear i.e. how and with which rate the tool gets worn down depending on cutting process variables such as normal stress and contact temperature [12]. Why models relating cutting process variables with tool wear is of more interest than tool life models.
2.6.1 Tool wear mechanisms
Tool wear in metal cutting can be described as a combination of several different mechanisms [14]. They can be grouped according to when they act: abrasive and adhesive wear are dominant at lower cutting speeds while temperature-activated wear controls the wear as the cutting speed is in-creased. Diffusion wear, oxidation wear, and chemical wear are examples of temperature-activated wear which is a function of the chemical compatibil-ity of the tool material and the workpiece material [15]. (Abrasive wear is the main focus in this study since this is the mechanism that mainly drives the flank wear.)
Abrasive wear is when hard particles in the workpiece material removes
tool material from the tool by mechanical action. The hard particles are either fragments of the tool material removed at an earlier stage or hard particles of the workpiece material [14]. Abrasive wear occurs mainly on the flank face but it effects both the flank face and rake face [15].
Adhesive wear or attritional wear is a process of small particles from the
tool being removed since they have welded or sicked to the chip surface due to friction. In most cases adhesive wear rates are quite low except for cutting of soft work materials under low speed and drilling [15].
2.6.2 Types of tool wear
There are two types of tool wear, defined by which area of the tool they affect.
Crater wear produces wear by the form of small craters on the rake face
[13]. Low levels of crater wear does not shorten the tool life but severe crater wear, usually induced by temperature-activated wear mechanisms, do [15].
Flank wear occurs on the flank face (also called relief face) and is mainly
rubbing the new formed machined surface, damages the surface and produce large flank forces [15].
3
Finite Element Simulation of metal cutting
Finite Element, FE, simulations of metal cutting is a widely used and ap-preciated tool in product development of cutting tools. The simulations has many advantages: it is relatively quick, relatively cheap and can sometimes show results and processes that are not yet possible to achieve experimen-tally due to the extreme conditions in the cutting zone. But FE simulations of metal cutting also has certain limitations. Among them is to find a re-alistic way to model the chip - workpiece separation, to handle the large deformations, to model the friction and to model the heat transfer.
3.1 Arbitrary Lagrangian-Eulerian adaptive meshing
A large problem when simulating machining with the finite element method is that the mesh gets widely distorted which causes the simulations to abort. To handle this problem it is common to use the adaptive arbitrary Lagrangian-Eulerian formulation of the mesh.
In Finite Element methods there are two common classical mathematical formulations for describing motion: the Lagrangian description, where the mesh moves with the material, and the Eulerian description, where the mesh is fixed in space and the material moves with respect to the grid.
In the Lagrangian description, which is the most widely used method when simulating problems in solid mechanics, the displacement vector is a func-tion of the material particles original posifunc-tion. In the Eulerian descripfunc-tion, which is the standard method in Computational Fluid Dynamics (CFD) the displacement is expressed i terms of the current coordinates [16]. Both of the methods have their advantages and disadvantages, among them is that the Lagrangian descriptions, without frequent remeshing, lack the ability to follow large deformations something that the Eulerian approach does with a relative ease [17]. A main shortcomings of the Eulerian description is that the material flow needs to be defined prior to the simulations [6].
In the Arbitrary Lagrangian-Eulerian description (ALE), which is a com-bination of the Lagrangian description and the Eulerian description, the mesh is allowed to move in an arbitrarily specified way. For an explanatory demonstration of the differences between Eulerian, Lagrangian and ALE de-scriptions see Figure 4. In this work an adaptive mesh approach with the ALE formulation is treated.
The ALE adaptive meshing is a single mesh method. This means that the positions of the nodes in the original mesh is corrected by means of a certain algorithm rather than that a new mesh is imposed. There are two main steps in the ALE adaptive meshing, relocation of the nodes to create the reformed mesh (the so called mesh-update procedure described in Chapter 3.1.2) and
Figure 4: An explanatory demonstration of the Eulerian, Lagrangian and
remapping of the solution variables to this reformed mesh (the so called stress-update procedure described in Chapter 3.1.4).
3.1.1 Boundaries in ALE methods
The ALE method can be applied to a wide range of problems by defining the movement of the mesh and the form of the boundaries. There are two primary types of boundaries for ALE domains, Eulerian and Lagrangian boundaries, with the main difference that the material points are allowed to flow across Eulerian boundaries while across Lagrangian boundaries they are not.
At a Lagrangian boundary the nodes follows the material in the direction normal to the boundary making the mesh cover the same material domain during the entire analysis.
3.1.2 Mesh-update procedures
The mesh-update procedure is defined by several different algorithms and choices e.g. the remeshing criteria - which nodes to move and when, smooth-ing algorithms and geometric aspects such as: geometric enhancement and curvature refinement.
ALE adaptive meshing is not performed equally over the entire mesh but serves to reshape the mesh where necessary. The ALE adaptive mesh algo-rithm in ABAQUS always strives to reduce element distortion by improving element aspect ratio (i.e. to get all sides of the element to be of the same length) sometimes under the option to preserve initial mesh gradation [2]. There are several algorithms for relocating the nodes to the new mesh. In ABAQUS/Explicit there are two quite basic options, either a volume-weighted average of the element centres or an average of the positions of the adjacent nodes connected by an element edge. A more complicated smooth-ing algorithm is based on a higher-order average of the eight (in the 2D case) nearest nodes.
In ABAQUS/Explicit there is an extra choice for the mesh-update proce-dure called curvature refinement. The functionality of this is to "pull more elements into areas of high curvature" [2].
The remeshing criteria in ABAQUS is not based on an error function but simply stated as a frequency telling how often the mesh is to be updated. Another parameter stated is the number of iterations for the relocation of the nodes. In ABAQUS/Explicit these iterations, which are performed according to chosen smoothing algorithm, are called mesh sweeps. The mesh sweeps can be based either on the current nodal position (often used for Lagrangian problems) or on the nodal position in the end of the previous adaptive mesh increment (recommended for Eulerian problems) [2].
3.1.3 Motion in ALE
The ALE conservation equations are very similar to the Eulerian conserva-tion equaconserva-tions and the ALE descripconserva-tion is therefore sometimes called quasi Eulerian description [17]. In both the Eulerian and the ALE descriptions there are advective effects due to relative motion between the material and the grid. These advection terms, which are not a part of the classical La-grangian equations, rises a need for an, from the LaLa-grangian point of view, extended solution algorithm [17]. This extension of the solution algorithm is the so called stress-update procedure.
3.1.4 Stress-update procedures
The conservation equations can be handled in several different ways, which can be classified into two different categories: split and unsplit methods [17]. In an unsplit method the non symmetric system of equations is solved di-rectly [2, 17]. A split method decouples the calculations into two different phases: a Lagrangian (material) phase, for calculations of the material as-pects, and a transport phase, for calculations of the advective terms [2, 17]. The main advantage of using a split method is its computational efficiency but choosing a split method comes at the cost of losing accuracy. For explicit approaches this loss is within acceptable limits since the time increment is sufficiently small.
In the Lagrangian phase the advective effects are neglected and hence the calculations exactly follows the procedure for purely Lagrangian descriptions [17]. It should be noted that it is common to let the Lagrangian phase be executed in the mesh-update loop and then perform the calculations of the transport phase only after the mesh has been updated [17].
In the transport phase the advective effects, in form of hyperbolic partial differential equations, has to be accounted for. The solutions of these equa-tions represent spatial travelling waves, giving them a spatial movement direction. For the calculations in the transport phase an upwind scheme is used, taking this directionality into account [18]. ABAQUS/Explicit offers the possibility to chose between a first- and a second-order scheme, although the first order scheme is not recommended due to its major disadvantage of diffusing sharp gradients over time[2, 18] .
3.2 Chip - workpiece separation in an FE environment
A big challenge when creating an FE model of machining is to get the material separation in the cutting zone to behave like it does in reality. The physical processes of chip - workpiece separation depends on several different parameters, in relations not yet determined and depending on material and cutting conditions. The effects of the limited knowledge of the real world behaviour tend to give the models a sense of arbitrariness.
The challenge has historically been handled with a path dependent parting criteria. During the last decade other techniques such as: multiple
remesh-Separation algorithm Advantages Disadvantages Adaptive meshing No non-physical
criteria needed Computationally heavy
Previously defined parting line
Easy to control the separation
Completely non-physical Damage and failure
criteria
Can be related to physical parameters
Element deletion gives rise to loss of mass Meshless/meshfree
methods
No non-physical
criteria needed Not as exact as FEM ALE- with Eulerian
boundaries
No non-physical criteria needed
Predefined chip formation needed
Table 1: Chip - workpiece separation
ing, fracture models, Eulerian models and a meshfree models among which the SPH model has been used more frequently. All these techniques having their respective area of usage, their pros and cons.
The main ways of performing the chip - workpiece separation are summed up in Table 1 and 2.
3.2.1 Adaptive Meshing
The main idea of adaptive meshing is to optimize the mesh, by revisions during the analysis. When performing chip - workpiece separation by use of this method a remeshing algorithm creating a completely new mesh, not just rearranging the nodes in the old mesh, is needed. This is a so called multiple mesh method and it uses the distorted geometry to build a new mesh, on which the solution of the old mesh is mapped. Proudian [6] applies a multiple mesh approach, Updated Lagrangian Formulation with automatic remeshing, in her simulations. A multiple mesh method can perform the chip - workpiece separation alone (i.e. without any damage criteria) but this comes at the cost of solution diffusion at the solution mapping stage. An adaptive method using a single mesh, for example ALE adaptive meshing as implemented in ABAQUS/Explicit see Chapter 3.1, optimizes the original mesh. Single mesh methods can effectively reduce element distortions but they are limited to smoothing the original mesh, why they alone can not perform chip - workpiece separation.
To use adaptive meshing to perform chip- workpiece separation is computa-tionally costly but it has an advantage in relation to element failure models
Separation algorithm Steady / Unsteady
state model Good for modeling Adaptive meshing Unsteady Residual stresses
Chip formation Cutting forces Previously defined
parting line Unsteady
-Damage and failure
criteria Unsteady Chip formation
Meshless/meshfree methods
Unsteady Chip formation Cutting forces The metal dead zone for cutting with strongly worn tools
Eulerian model Steady
Temperature
distribution in steady state machining
since no material is removed and no non-physically criteria is used. As men-tioned above the solution is a bit diffused every time the solution is mapped to the new mesh making the solutions a bit less accurate.
3.2.2 Element failure models
Modeling chip - workpiece separation with element failure models in FEM means setting a condition, based on a value for a certain parameter or a combination of parameters, for when the material breaks. The failure is a binary parameter of the element with the value one before failure and zero when failed. After failure the element is deleted from the mesh exposing the neighbouring elements.
Element failure is probably the most common way of performing chip -workpiece separation today. In relation to adaptive remeshing and Eulerian models, element failure reduces the computational cost. Today many quite physically realistic damage and failure criterion has been proposed. Among them the Johnson-Cook damage law (presented in Chapter 4.3.4) seems to give good results.
The main disadvantage with element failure is the deletion of material. It is generally non-physical that mass is removed from the process and this removal effects the forces (pressure) between the tool and workpiece and thereby it effects all the results of the simulations. To reduce these effects the mesh density has to be very fine, leading to reduced efficiency gain in relation to frequent remeshing. A discussion about whether the material actually breaks in the cutting zone or not can be held. For the formation of segmented chips it might be necessary with a damage criteria but that is a breakage occurring at the top of the workpiece while the chip - workpiece separation occurs in the surrounding of the nose of the cutting tool.
3.2.3 SPH simulation of metal cutting
In several studies a meshfree, smooth particle hydrodynamics (SPH) model for simulations of metal cutting is used [19, 20, 21, 22, 23]. The SPH method handles the large deformations that occurs during cutting simu-lations through a loss of cohesion between the particles [22].
Despite its name, to say that the SPH method is a particle method is not re-ally correct. A particle method incorporates particle equations but the SPH method is just another way to discretize the continuum equations [2]. One could say that SPH is a meshfree FEM method. When the FEM discretizes the material in finite elements built-up by nodes, with arrangements stated in the connectivity matrix, SPH discretizes the material particles which can be thought of as single node elements with their internal ordering not de-termined by a connectivity matrix.
Instead of assuming connectivity between nodes to build the spatial deriva-tives, as is the case in FEM, the SPH uses a kernel approximation to calculate spatial derivatives [23]. The particle approximation is given by:
h
Y
f (x) =
Z
f (y)W (x − y, h) dy (1)
where h is the smoothing length, and W is the centrally peaked kernel function (often a cubic spline , which for example is default in ABAQUS [2]).
When using the SPH method for chip - workpiece separation in cutting sim-ulations no non-physical separation criterion is needed and no remeshing is needed to handle the mesh distortions. In general the SPH method is less accurate then Lagrangian FEM and ALE FEM, and it is therefore recom-mended only for applications where the deformation is so severe that only SPH is possible. Since this is the case for machine cutting it is an accept-able method. An advantage with SPH compared to FEM is an increased transparency in the assumptions made [20].
For analyses of cutting with strongly worn tools the SPH method has shown to be able to represent the metal dead zone which is a physical phenomena earlier observed in experiments [21, 23], which can explain the increased feed force when cutting with worn tools.
For predicting chip formation and cutting forces the SPH method gives good correlation with experiments and FE simulations [22, 21, 20, 19].
Other meshfree/meshless methods have been tried in some studies like the Element-free Galerkin Method (EFGM) and the Finite Pointset Method (FPM), but the SPH method is by far the most common one within manu-facturing technology [24].
3.2.4 Eulerian models
An Eulerian model of chip - workpiece separation simulates the material flow around the tool-tip, without any non-physically cutting conditions, for steady state machining. Due to the nature of the Eulerian mesh, see Chap-ter 3.1, this type of model requires a predefined chip geometry, making it unusable for modeling chip formation.
An option is to model the chip formation part of the problem with another chip - workpiece separation model or using an experimentally determined geometry to get the form of the chip and than use the Eulerian model for calculating cutting forces, residual stresses and tool wear.
3.2.5 Path dependent parting
When using path dependent parting a cutting line is defined beforehand, usually it is the line from the tool tip and forward. Along this line a sepa-ration indicator criterion, based on either geometrical or physical consider-ations, is calculated and the elements reaching the criteria are deleted (or unhooked if using cohesive elements). A possible geometrical indicator is a
critical distance between the tool tip and the nearest node along a predefined line.
Path dependent parting was a lot more common during the 80:s and 90:s then it is today. With the path dependent parting a crack leaping ahead of the tool-tip is unavoidable. This crack was till not to long ago considered to be in harmony with the theories about real world machining, but recent years this has been reconsidered. Today path dependent parting is concidered completly unphysical. But there are, of course, also advantages with this method. When using it, the chip separation is easy to control and since the cutting line is known in advance the elements can be made very small there and thus reducing the element deletion effects on the simulation.
3.3 Friction models
The choice of friction model has a major impact on the predicted tool wear since it affects both the heat produced in the contact region and the normal stresses between the tool and the workpiece.
Several different models for the frictional behaviour between the tool and the workpiece has been proposed, a few of them are described below. It is important to note that the mechanisms behind the problem of friction are not yet completely understood [10] and the choice of friction model is therefore often driven by a wish for simplicity.
3.3.1 Coulomb friction model
The Coulomb friction model is the most simple and classical of the fric-tion models. It is basically an implementafric-tion of the Coulomb’s law. The Coulomb friction model states, as can be seen in Equation (2), that the fric-tional stress τf is proportional to the normal stress σn times the constant
frictional coefficient µ.
τf = µσn (2)
The Coulomb friction model was used for simulations of residual stress by Proudian [6] in her thesis at KTH in 2012. It has also been used by Arrazola et al. [25] and by Issa et al. [26] but then with a friction coefficient depending on temperature and sliding velocity at the contact interfaces.
3.3.2 Constant shear model
The constant shear model assumes the frictional stress τf to be constant, and defined as:
τf = mτY (3)
where τY is the yield shear stress of the material, defined [2, 10] as τY =
σY/
√
3.3.3 Sticking zone and sliding zone model
A common friction model for simulations of metal cutting is the stick-slip model defining a sticking region around the tool tip and a sliding region on all other areas subjected to contact. For simulation purpose it can be implemented as follows [10, 27],
τf(x) = µσn µσn< τY (4)
τf(x) = τY µσn≥ τY (5)
where Equation (4) and (5) describes a case where the Coulomb friction model is used up to a certain level of shear stress and for normal stresses above that value a constant shear model is used. Please note the similarity between Equation (4) and (2) and Equation (5) and (3).
3.3.4 Friction in smooth particle hydrodynamic simulations
In some studies of smooth particle hydrodynamic, SPH, simulations of metal cutting both the workpiece and the tool has been modelled with SPH par-ticles. This opens up for the possibility to let go of the applied friction condition and just use contact between two SPH surfaces. This method has shown to give really good results which sometimes can explain which con-tact conditions should be applied in FE simulations [23]. It should be noted that the SPH friction still needs to be validated before it can be considered a reliable tool in the prediction of cutting behaviour.
3.4 Heat transfer models
With temperature differences of 500◦C - 1400◦C [4], the temperature has a large impact on the accuracy of the machining simulation. The heat transfer depends on the cutting velocity, the material of the tool and the workpiece. In real world cutting sometimes cutting fluids are used as coolants, which further increases the complexity in the heat transfer models.
3.4.1 Adiabatic assumption
Sometimes orthogonal cutting is modelled as an adiabatic process, i.e. as if no heat transfer occurs. This can be assumed when the cutting speed is high and when the material points studied are not in the tool but in the workpiece [23, 9, 1].
An adiabatic FE simulation means having no heat transfer between the elements. A way to implement this is to set the heat conduction matrix to zero [9].
3.4.2 Coupled Thermal-Stress analysis
In the physical world cutting is a thermally-mechanically coupled problem and some of the heat produced close to the workpiece surface is conducted to the tool. In many cases the heat transferred to the tool is considered to be around 10% of the heat produced in the workpiece near the tool.
The conductive heat transfer between the tool and the workpiece is often considered to be linear and is then defined as:
q = h(θA− θB) (6)
where q is the heat flux per unit area crossing the interface from point A on the workpiece surface to point B on the tool surface, h is the heat conduction coefficient, θAis the workpiece temperature and θB is the tool temperature. According to some authors the heat conduction coefficient is a constant [14] while according to others it depends on the contact pressure [10, 28].
3.5 FE models of tool wear
The tool wear models describe a rate of local volume loss on the tool face, per unit time, per unit area [28]. In FE simulations these models are often used in a simulation cycle where the tool wear is calculated in a step separated from the FE simulation and thereafter used in further simulation steps.
3.5.1 Tool wear rate models
Uisui et al. [29] derived a wear rate model based on the equation of adhesive wear, which has shown to be adequate for both flank and crater wear of tungsten carbide tools [28].
∂W
∂t = Avsσnexp(− B
T) (7)
where∂W∂t is the rate of volume loss on the tool contact face per unit area per unit time, vs is the sliding velocity at the contact surface, σn is the normal stress, T is the temperature measured i Kelvin and A and B are constants.
Takeyama and Murata, as cited in [28], proposed a wear rate equation
(see Equation (8)) by considering abrasive wear and diffusive wear.
∂W
∂t = G(V, f ) + Dexp(− E
RT) (8)
here the first term G(V, f ) is the abrasive wear in which; G is a constant,
V is the cutting speed and f is the feed rate and the second term is the
diffusive wear in which; D is a constant, E is the process activation energy and R is the universal gas constant [30].
3.5.2 Cyclic implementation
FE simulations of tool wear are often implemented as a cyclic system [12, 30] with three distinctive steps [31]. Here the Usui’s wear rate model, see Equation (7), are used since it is common in literature, gives satisfactory results and the values of the parameters are easily achieved from the FE simulation.
Chip formation The parameters T , vs and σn are calculated in the FE
cutting simulation for nodes on the tool surface that are in contact with the workpiece
Wear rate calculation A wear rate based on Usui’s wear rate model is
calculated from the values for T , vs and σn given from the previous step.
This calculation is often performed in a user subroutine [31].
Tool geometry update Based on the tool wear rate the nodes on the
tool surface is moved in a tool wear direction which is calculated differently depending on the nodes position and method chosen See for example [31, 12].
4
Material models
In metal cutting the material undergoes rapid elasto-plastic deformation un-der extreme conditions. To give an adequate result the material model must be able to describe deformation behavior such as hardening and softening over a great ranges of strain, strain rate and temperature [1].
4.1 Hardening
For many materials the stress after initial yielding keep increasing with in-creasing strain. This phenomena is called strain hardening [32]. For mate-rial subjected not only to increasing strain after yielding but also to reversed loading, two extreme cases of behavior can be defined: isotropic and kine-matic hardening. Hardening can also depend on other parameters, such as temperature and plastic strain rate.
While the hardening rules effects the size and location of the yield surface, the yield criterion defines the shape.
4.1.1 Yield criterion
There are several different yield criteria. Among them the von Mises yield criterion is the most common and it is specially suited for metals since for most metals all volumetric response is linear elastic [16]. Therefor only the von Mises yield criterion is treated and used in this work.
The von Mises condition reads:
f (σij) = (
3 2sklskl)
1/2− σ
where skl is the deviatoric stress tensor and σy is the yield stress, which can
be a material constant or the isotropic hardening component (see Chapter 4.1.3). Equation (9) describes a cylinder with circular cross section and radiusq23σy in stress space.
The von Mises condition for mixed or kinematic hardening reads:
f (σij) =
3
2(skl− αkl)(skl− αkl)
1/2
− σy = 0 (10)
where αkl is the back stress tensor (see Chapter 4.1.4) defining the center
of the circular cross section of the yield stress in stress space. If αkl = 0 Equation (10) reduces to the initial von Mises criterion, i.e. Equation (9).
4.1.2 Flow rule
The associated flow rule for isotropic hardening is given by:
˙ εplij = ˙¯εpl ∂f ∂σij = ˙¯εpl3skl 2σy (11)
where ˙¯εpl = (32ε˙plijε˙plij)1/2 is the equivalent plastic strain rate. The associated flow rule for kinematic or mixed hardening is given by:
˙ εplij = ˙¯εpl ∂f ∂σij = ˙¯εpl3(skl− αkl) 2σy (12) 4.1.3 Isotropic hardening
Isotropic hardening describes a process where the elastic region in the stress space expands with increasing effective plastic strain. This means that the yield surface is represented by a circle (considering a von Mieses material) with a radius depending on the effective plastic strain [32].
For isotropic hardening processes the yield stress is given by:
σy = σy0+ K(¯εpl, ˙¯εpl, T ) (13)
where σy0 is a constant initial yield stress and K(¯εpl, ˙¯εpl, T ) can be modeled
in several different ways, most common as a linear function K(¯εpl) = H ˙¯εpl
or as a power law K(¯εpl) = h( ˙¯εpl)awhere H, h and a are material constants [32].
4.1.4 Kinematic hardening
Opposed to isotropic hardening, the elastic region is invariable in a process of kinematic hardening. Instead it can be visualized as if the center point of the yield surface translates (see Equation (10)) in the stress space by a back stress vector which depends on the effective plastic strain [32]. The observation of kinematic hardening is sometimes called Bauschinger effect [16].
There are many possible choices for modeling evolution of the back stress
α. A classical model is the Melan-Prager’s evolution law [16] which reads:
˙
αij = c ˙εplij (14)
where c is a material parameter. Another evolution law, proposed by Arm-strong and Frederick [16] is
˙ αij = c 2 3ε˙ pl ij − αij α∞ ˙¯ εpl = C 1 σy (sij − αij) ˙¯εpl− γαijε˙¯pl (15)
where α∞, C and γ are material parameters and the equivalent plastic strain
rate is given by the flow rule for kinematic hardening, see Equation (10). Note that if α∞ goes to infinity then γ goes to zero and the
Armstrong-Frederick evolution law in Equation (15) reduces to the Melan-Prager’s evo-lution law in Equation (14).
The Armstrong-Frederick model was generalized by Chaboche [16] by su-perposing several Armstrong-Frederick terms after each other
αij = X k αkij (16) ˙ αkij = Ck 1 σy (σij − αkij) ˙¯εpl− γkαkijε˙¯pl (17)
where k is the number of back stresses and Ck and γk is the Chaboche material parameters.
4.2 The Johnson-Cook model
The Johnson-Cook constitutive material model, which is in implementa-tion of isotropic hardening, is a common material model for describing the thermo-visco-plastic behavior of the workpiece in a cutting process [4]. To attain the data for deriving the material parameters, torsion tests over wide ranges of strain rates, static tensile tests, dynamic Hopkinson bar tensile tests and Hopkinson bar tests are performed [6].
The flow stress is formulated as a function of strain, strain-rate and tem-perature as can be seen in Equation (18).
The Johnson-Cook equation reads:
¯ σ = (A + B(¯εpl)n) 1 + Clnε˙¯ pl ˙ ε0 1 − ˆθm (18)
where ¯σ is the equivalent flow stress, A is the initial yield strength of the
material, ¯εpl is the equivalent plastic strain and ˙¯εpl is the equivalent plastic strain rate which is normalized with a reference strain rate ˙ε0. The
param-eters B, n, C and m are material model paramparam-eters. ˆθ is the homologus
temperature given in Equation (19).
ˆ
θ = (θ − θroom)
(θmelt− θroom)
(19)
here θ is the instantaneous temperature of the workpiece, θroom is the room
temperature and θmelt is the material melting temperature.
The Johnson-Cook model can be seen as a multiplication of three distinctive terms σ = f (ε)g( ˙¯εpl)h(θ) (20) where f (ε) = A + B(¯εpl)n (21) g( ˙¯εpl) = 1 + Clnε˙¯ pl ˙ ε0 (22) h(θ) = 1 − θ − θroom θmelt− θroom m (23)
Equation (21) describes an isotropic strain hardening behavior, Equation (22) describes strain rate sensitivity and Equation (23) describes a thermal softening behavior [33].
The Johnson-Cook model has been criticized for neglecting the coupling effects of strain, strain rate and temperature [33]. It also lacks ability to capture some important behavior during high strain and high strain rate (for example flow softening) [33], a very important comment in the environment of cutting since the simulations are then including strain rates up to 106and strains up to 10 [1].
4.3 Damage and failure models
There are two different types of damage models in ABAQUS, dynamic dam-age and progressive damdam-age. The main difference between them is that the materials load carrying capacity is reduced progressively after a certain cri-teria is met in the progressive damage while it is changed discretely when the dynamic damage parameter has reached a critical value for dynamic dam-age. ABAQUS recommends the later one to be used only for high strain rate dynamic problems [2].
Considering e.g. metals under tension, the FE model of progressive damage is based on the assumption that the material, after a linear elastic phase and a plastic yielding phase, reaches a phase of strain softening. In the strain softening phase, which starts at a damage initiation point, the material undergoes a reduction of load carrying capacity, i.e. a damage evolution phase, before a final failure [2].
In the dynamic damage model the material undergoes the linear elastic phase and the plastic yielding phase with stress strain curves just as for the model with progressive damage. But instead of damage initiation and evolution the element just fails when the damage criteria is met at all integration points in the element.
There are several possible choices for the damage initiation criteria, e.g. Ductile damage (see Chapter 4.3.1) and Shear damage (see Chapter 4.3.2) as described below, and damage evolution criteria (see Chapter 4.3.3) in ABAQUS/Explicit. For elements where the material has reached failure, i.e. when it no longer has any load carrying capacity, a deletion criteria can be imposed. This means that failed elements are deleted from the simulation. For further discussion on effects of element removal see Chapter 3.2.2.
4.3.1 Progressive ductile damage initiation
In the ductile damage initiation criterion the critical equivalent plastic strain, ¯
εplD, is a function of stress triaxiality, η, and plastic strain rate, ˙¯εpl, i.e. ¯
εplD(η, ˙¯εpl). The onset of damage is met when the following criterion is satis-fied: ωD = Z 1 ¯ εplD(η, ˙¯εpl)d¯ε pl= 1 (24)
where ωD is a monotonically increasing state variable. The model of ductile
damage is based on phenomenological observations of damage related to voids in the material [2]. The ductile damage initiation criterion is specified as a table with ¯εplD(η, ˙¯εpl).
4.3.2 Progressive Shear damage
The shear damage initiation criterion assumes that the critical equivalent plastic strain, ¯εplS, depends on shear stress ratio, θS, and plastic strain rate,
˙¯
εpl. With the shear stress ratio defined as:
θS =
(q + ksp) τmax
(25)
where q is the Mises equivalent stress, p is the pressure stress, τmax is
the maximum shear stress and ks is a material parameter. We then have ¯
εplS(θs, ˙¯εpl). The onset of damage is met when the following criterion is
ωS =
Z 1
¯
εplS(θS, ˙¯εpl)d¯ε
pl= 1 (26)
where ωS is a monotonically increasing state variable. The model of shear damage is based on phenomenological observations of damage related to shear bands in the material [2]. The shear damage initiation criterion is specified as a table with ¯εplS(θS, ˙¯εpl).
4.3.3 Progressive damage evolution
The damage evolution defines the material behavior after damage initiation. The stress in the material is in this phase given by:
σ = (1 − D)¯σ (27)
where ¯σ is the undamaged stress, i.e. the stress that would exist in the
material in absence of damage, and D is the damage variable which is zero at damage initiation and one at complete failure. This is a softening of the material, a reduction in material stiffness. If there are several different failure mechanisms active, ABAQUS calculates a damage evolution that takes them all into account [2].
4.3.4 Cumulative Johnson-Cook damage
This model is a dynamic shear failure model in ABAQUS/Explicit which is used for the chip - workpiece separation in orthogonal cutting simulations by Agmell et al.[10] and Zouhar et al. [34].
For the shear failure model, failure occurs when the damage parameter ω defined by Equation (28) reaches the value one.
ω = ε¯ pl 0 + P ∆¯εpl ¯ εplf (28)
where ¯εpl0 is the initial value of the equivalent plastic strain, ∆¯εpl is an increment of the equivalent plastic strain and ¯εplf is the critical strain at failure. The summation is performed over all steps of the analysis.
For the Johnson-Cook damage law the strain at failure is given by:
¯ εplf = D1+ D2exp D3( p σ) 1 + D4ln(ε˙ pl ˙ ε0 ) 1 + D5 θ − θroom θmelt− θroom (29) The element has failed when the shear failure criterion is met for the inte-gration point (since in this work only first order quadrilateral elements with reduced integration and first order triangular elements, both having only one integration point) in the element [2]. Then all the stress components will be set to zero and the element will be deleted from the simulation.
20NiCrMo5 AISI 4041 Density [kg/m3] 7800 7850 Poisson’s ratio 0.3 0.29 Youngs modulus [P a] 2.1 · 1011 2.19 · 1011 Thermal conductivity[W/m◦C] 47.7 42 Specific Heat [J/kg/◦C] 556 Thermal expansion [1/◦C] 1.2 · 10−6
Table 3: Workpice material physical property data
5
Present model and simulation of metal cutting
In previous chapters important parameters, and possible ways of model-ing them in simulations of cuttmodel-ing, has been looked at through a literature study. In this chapter a 2D model for simulations of metal cutting is pre-sented. Focus is on trying to achieve a good way to perform chip - workpiece separation in ABAQUS/Explicit.
5.1 Workpiece modeling
The workpiece is a 5 mm long and 2 mm high piece of steel. Two different types of steel are used in the simulations, the first one is 20NiCrMo5 steel with Johnson - Cook parameters evaluated at Swerea KIMAB and the sec-ond one is AISI 4041, chosen because Johnson - Cook damage parameters for this material existed in literature [10].
5.1.1 Material physical property
The workpiece material is 20NiCrMo5 steel and AISI 4041 steel, both of which are considered elastic-plastic von Mises materials throughout the study. General thermal and mechanical properties for the workpiece ma-terial are listed in Table 3.
5.1.2 Workpiece, Johnson-Cook parameters
Cook material parameters (for more information on the Johnson-Cook model see Chapter 4.2 on Page 20) for 20NiCrMo5 steel and AISI 4041 are listed in Table 4. The constants for 20NiCrMo5 were experimentally determined by machining tests in the Swerea KIMAB lab and evaluated by Håkan Thoors [27]. The Johnson-Cook material parameters for AISI 4041 was given by Agmell et al. [10] and are used in some simulations for testing the Johnson-Cook cumulative damage model. Figure 5 shows the equivalent plastic flow-stress as a function of equivalent plastic strain for both 20NiCrMo5 and AISI 4041.
20NiCrMo5 AISI 4041 A [P a] 4.9 · 108 5.95 · 108 B [P a] 6 · 108 5.8 · 108 n 0.21 0.133 C 0.015 0.023 m 0.6 1.03 ˙ ε0 1 1 Tmelt [K] 1900 1850 Troom [K] 300 300
Table 4: Johnson-Cook constitutive material model constants for 20NiCrMo5
and AISI 4041 0 0.2 0.4 0.6 0.8 1 0.8 0.9 1 1.1
Equivalent plastic strain
Equiv ale n t plastic flo w stress [GP a ] 20NiCrMo5 AISI 4041
Figure 5: Johnson-Cook stress-strain curves for 20NiCrMo5 and AISI 4041,
with T = Troom= 300K and ˙¯εpl= ˙ε0= 1
5.1.3 Implementation of kinematic hardening component
For trying out the possibilities with the SPH model, a material model with kinematic hardening is implemented. This implementation is written as a tabular data on the form of ABAQUS/Explicit built in function Com-bined Hardening, which takes in yield stress as a function of plastic strain and possibly temperature (although here the temperature dependency is ne-glected). The tabulated data is fitted to imitate the curves generated from the Johnson-Cook equation achieved with the parameter values from Table 4.
ABAQUS/Explicit then automatically finds the parameters for the Chaboche model, see Chapter 4.1.4 on Page 20, for a given number of back stresses
Table 5: Chaboche parameters for kinematic hardening component of workpice material C1 1.9 · 108 C2 1.125 · 1011 C3 1.9 · 109 γ1 0 γ2 500 γ3 10
here chosen to 10 for the best accuracy. Since only a few load cycles are under consideration only half cycle data is provided for the hardening im-plementation. Then the Chaboche parameters are calculated according to:
αkij = Ck
γk
(1 − e−γkε¯pl) (30)
During the evolution of the implementation of this material model, different possibilities for implementing a strain rate dependency for the kinematic hardening component was considered. This since the Chaboche model in ABAQUS/Explicit has no built in possibilities for dependency on strain rate. Among the ideas tried was writing a user defined field which was supposed to calculate and pass on the strain rate to the kinematic hardening. Due to limited time this idea had to be turned down before finalized. And it should be noted that this implementation of the kinematic hardening is not really sufficient for showing hardening behaviors of the workpiece material but can only give a glimpse of it.
5.1.4 Implementation of isotropic and kinematic hardening components
A mixed hardening, i.e. a combination of isotropic and kinematic hardening as in Equation 10 in Chapter 4.1.1 on Page 19, is implemented by the built in function Combined hardening in ABAQUS/Explicit.
The kinematic hardening component is given as a parameter list, implement-ing the Chaboche model. Equation (30) has been used to obtain values for the Chaboche parameters given in Table 5. The back stress α in Equation (16) is optimized to give a resulting yield stress similar to the Johnson-Cook yield stress for fixed strain rate ( ˙ε0).
The isotropic hardening component is implemented as a rate-dependent tab-ular data.
5.1.5 Mesh density
When meshing the workpiece, a very fine mesh of first order linear quadri-lateral elements, CPE4R, of size 3.12 µm is assigned in the cutting zone,
(a) Full mesh (b) Close up of the cutting zone in the
mesh
Figure 6: The meshed workpiece with 67020 elements
which is considered 87.5 µm broad. Above and under the cutting zone a coarser triangular mesh, with first order linear elements of type CPE3, is assigned. Here the element sizes range from 3.12 µm close to the cutting zone to 53 µm at the top of the workpiece and 175 µm at the bottom of the workpiece.
The quadrilateral mesh is a structured mesh and the triangular mesh is meshed by using the free meshing technique in ABAQUS. To achieve an acceptable quality for the triangular elements; the workpiece was partitioned in stripes aligned with the cutting direction, and each stripe was seeded (i.e. node density was defined on the edges) and meshed separately. This procedure made it possible to achieve quite a large gradient in element size moving from the cutting area to the bottom of the workpiece.
All in all the workpiece is meshed with 67 020 elements as shown in Figure 6.
In some simulations the workpiece is meshed in a similar way but with 5 µm size on the quadrilateral elements over a 25 µm broad stripe giving a total number of elements of 21 115.
5.1.6 ALE
An Arbitrary Eulerian Lagrangian domain, as described in Chapter 3.1, with Lagrangian boundaries is defined on the area of quadrilateral elements in the cutting zone of the workpiece. The parameters given to the simulation software are listed in Table 6.
For the mesh-update procedure the smoothing objective is set to uniform, telling there is no need to try to keep initial mesh gradation, and the new mesh is predicted from the current node positions. It is here important to note that the part of the mesh where the ALE adaptive meshing is performed has no initial grading. During the development of the model several attempts to define an ALE domain over the entire workpiece was made and then the condition of keeping the initial mesh gradation was used. These attempts did not fall out well, maybe because the obligatory splitting of the ALE domain due to two types of elements in the same domain.
In the evolution of the workpiece model and parameters for the ALE an initial incorrect assumption, that the ALE algorithm by it self were able to
Remeshing criteria Frequency 1
Mesh sweeps 20
Initial mesh sweep 0
Mesh-update Smoothing objective Uniform Volume smoothing 1
Curvature refinement 2 Geometric enhancement on Meshing predictor Current Stress-update Advection algorithm second order
Momentum advection Element center projection
Table 6: ALE parameters
perform chip - workpiece separation, was investigated. During that work the value of the curvature refinement parameter was varied in quite a wide range. The purpose of the curvature refinement is to drag nodes to concave areas where the mesh density is decreased since the mesh is stretched out. In the case of the chip - workpiece separation the curvature refinement parameter did not really effect the outcome, probably because the development is to quick for the pulling of nodes to be efficient. After some considerations the curvature refinement was set to 2 and kept constant for the rest of the study. A volume weighted average algorithm is used for the relocation of the nodes, since this is the algorithm best suited when there are large distortions of the mesh [2], and this relocation is performed 20 times every time step.
Because of its computationally efficiency an element center projection algo-rithm of second order (as recommended, see Chapter 3.1.4 on Page 10) is used for the stress update procedure.
It is worth noting that the ALE algorithm requires the ALE domain to be unsplit and therefore domain-level parallelization (i.e. splitting the model in topological domains) for computations on multiple CPU:s is not an option when using the ALE method. Instead loop-level parallelization (which par-allelizes low level loops in the code) can be used. Unfortunately the speedup factor may be significantly lower using loop- level parallelization compared to domain-level parallelization and the loop-level method may scale poorly for more than four processors [2].
5.2 Tool model
The tool is considered an analytic rigid body throughout the analysis. The geometric properties of the tool are given in Table 7.
Rake angle, α[◦] +6 Relief angle, c[◦] +6 Tool nose radius, [µm] 20 Cutting velocity, [m/min] 100
160 260 Uncut chip thickness, [mm] 0.2
Table 7: Cutting conditions
Figure 7: Tool and workpiece boundary conditions
5.3 System model
Metal cutting can be performed in several ways and under several different conditions. FE simulation of a system also require specific conditions, such as contact conditions, to be explicitly defined.
5.3.1 Cutting conditions
A constant cutting velocity of 160 m/min (if nothing else is stated, in some simulations a cutting velocity of 100 or 260 m/min is used) is applied to the tool in the negative x direction, all other degrees of freedom are constrained. The workpiece is fully restrained at the bottom surface and a symmetry condition, in the x direction is applied at the left and at the lower part of the right surfaces as can be seen in Figure 7.
It is of great importance to note that the simulations are all performed without taking the temperature dependencies into account. This choice is made, although heat effects have a major impact on the result of simulations of machine cutting, in order to reduce the computational time and it does not falsify the conclusions from the investigation since the investigation is at a very initial step and no detailed results are needed.
Equivalent plastic strain at damage initiation Stress triaxiality Strain rate 5.0 -0.33 0.0 4.0 -0.3 0.0 3.0 -0.2 0.0 2.0 -0.1 0.0 1.0 0.0 0.0 0.3 0.33 0.0
Table 8: *Damage Initiation, criterion=DUCTILE
5.3.2 Contact and friction
The contact between the workpiece and the tool is a penalty based hard contact in the normal direction where the tool is defined as the master surface and the workpiece is defined as the slave surface. This means that the surface of the workpiece is not allowed to penetrate the tool at any point, but that the opposite might occur if the mesh of the slave surface is too coarse [2].
In the tangential direction a Coulomb friction model, with friction coefficient 0.4, has been used.
5.4 Chip - workpice separation method
In this work a few different separation methods have been tested, among them are several different types of failure applied both on the workpiece as a whole and a distinct part of the workpiece. An SPH model is also implemented in ABAQUS/Explicit and tested.
5.4.1 Ductile damage initiation
At first a simple ductile damage imitation criteria (for further information see Chapter 4.3.1) of ¯εplD = 2.5 is tested in ABAQUS/Explicit. Then a more complex tabular implementation of the progressive ductile damage initiation criterion as given in Table 8, a plot the later one can be seen in Figure 8.
5.4.2 Damage initiation Shear
A simple shear damage initiation criteria (for further information see Chap-ter 4.3.2) of ¯εplS = 2.5 is tested in ABAQUS/Explicit.
−0.2 0 0.2 0 1 2 3 4 5 Triaxiality, η Equiv alen t plastic strain at damage initiation, ¯ε pl D
Figure 8: Equivalent plastic strain at damage initiation, as a function of
triaxiality, for the ductile damage initiation according to Table 8.
D1 1.5 D2 3.44 D3 −2.12 D4 0.002 D5 0.1
Table 9: Johnson-Cook progresive damage parameters. From Agmell et al.
[10]
5.4.3 Damage initiation Shear and Ductile
A combination of the progressive shear and ductile damage initiation crite-rion as used by Prasad [27] has also been tried. This critecrite-rion is on the form ¯
εplD = 1.5; ¯εplS = 1.5, where these two separate damage initiation criteria are evaluated individually and then captured in a overall damage variable [2].
5.4.4 Johnson-Cook progressive Damage
A Johnson-Cook dynamic failure model is tried for the AISI 4041 material. The Johnson-Cook damage parameters, as achieved from Agmell et al. [10], are given in Table 9. A plot of Johnson-Cook strain at failure as a function of triaxiality is seen in Figure 9.
−0.4 −0.2 0 0.2 0.4 0.6 0.8 1 2 4 6 8 10 Triaxiality, η Equiv al en t plastic strain at failure, ¯ε pl f
Figure 9: Johnson-Cook strain at failure as a function of triaxiality for AISI
4041
5.4.5 SPH
A SPH model of the workpiece has been tried in some simulations. Since ABAQUS/Explicit only allows for 3D implementation of SPH models, a model with only two particles in thickness (z- direction) and complete con-straints to move in the z-direction was constructed. Except for this thickness the workpiece has the same geometrical properties as in Chapter 5.1 and is assigned the 20NiCrMo5 material parameters given in Table 3 and 4. The workpiece is meshed with 32563 particles, giving an initial in plane particle distance of 25 µm. The tool is considered rigid and has the geometrical properties given in Table 7.
6
Results
Results from simulations with different damage criteria, chosen in order to achieve the chip - workpiece separation, are presented. They are compared to results from SPH simulations. Also different models for the hardening are tried and results from simulations showing the effect of the cutting velocity on the chip - workpiece separation are presented.
6.1 Chip - workpiece separation
In this chapter results for different methods to separate the chip from the workpiece is presented.
