FINITE ELEMENT SIMULATION OF COLD UPSETTING PROCESS

CHAPTER 6

FINITE ELEMENT SIMULATION OF COLD UPSETTING
PROCESS

6.1 INTRODUCTION

The upsetting of solid cylinders is an important metal forming process and an
important stage in the forging sequence of many products. Cold forming process
minimizes material wastage, improves mechanical properties such as yield strength
and hardness and provides very good surface finish. The tools used are also subjected
less thermal fatigue [1]. Metal flow is influenced mainly by various parameters like
specimen geometry, friction conditions, characteristics of the stock material, thermal
conditions existing in the deformation zone, and strain rate. Metal flow influence the
quality and the properties of the formed product; the force and energy requirements of
the process. A large segment of industry depends primarily on the predominant
applications of this process which includes coining, heading and closed die forming.

When ever a new component is produced there is usually a trial and error stage to tune
the progress, this helps in obtaining a component without defects, using required
quantity of raw material. Previous experience of designers and manufacturers gives an
important aid in reducing these trails. Use of new materials associated with new
shapes and designs create the possibility of new behaviour. For better understanding
of this behaviour and better knowledge of metal flow free deformation is to be
studied. A systematic and detailed study of free deformation can be used to predict the
metal flow under various working conditions and with various tool and work piece
geometries. This information can then be used to design better forgings, to make
improved intermediate dies, and to avoid the defects and failure of materials during
plastic working. The finite element simulation helps in analyzing the process and
predicting the defects that may occur at the design stage itself. Therefore,
modifications can be made easily, before tool manufacturing and part production,
reducing the trail and error stage and its associated costs [2-8].

The basic idea in the finite element analysis (FEA) is to find the solution of a
complicated problem by replacing it by a simpler one. Since a simpler one to find the
solution replaces the actual problem, we will be able to find only an approximate
solution rather than the exact solution [1]. The existing mathematical tools are not

101

sufficient to find the exact solution of most of the practical problems. Thus in the
absence of convenient method to find the approximate solution of 3-D problem, we
have option for FEA. The FEA basically consists of the following procedure. First, a
given physical or mathematical problem is modeled by dividing it into small
interconnecting fundamental parts called Finite Elements. Next, analysis of the
physics or mathematics of the problem is made on these elements: finally, the
elements are re-assembled into the whole with the solution to the original problem
obtained through this assembly procedure.

6.2 LITERATURE REVIEW

Computer technology became inevitable in the engineering and manufacturing
industry as computing has become cheap and fast enough to simulate metal forming
numerically in a useful timescale. The finite element (FE) method has been used to
solve equations which describe solid metal flow [9]. In the last 15 years considerable
efforts have been made, largely in a research environment, to apply FE modeling to
the simulation of forging operations and in evaluating the results. The technique is
now being adopted tentatively by the forging industry. FE codes which will analyze
the plastic deformation of metals are available but are often not readily useable by
non-experts.

Although a considerable amount of research has been done in developing the FEM
for metal forming simulation since the pioneering work [10] was presented in 1973,
rigorous three-dimensional simulation of metal forming problems still remains a
challenging task from the standpoint of computational efficiency, solution accuracy,
graphics visualization, mesh generation and automatic re-meshing, and so on. As
computer technology and FEM advance, wider and more complicated metal forming
processes are being investigated. It is believed that the further development of FEM
will be continuously challenged by the need from the industry to make the modeling
more accurate, more practical, and more affordable.

To analyze metal forming the FE method requires a mathematical description of the
metal's plastic flow behaviour. Two alternative formulations have been used to do
this [11, 12]. One model of plasticity is a structural formulation derived from the
analysis of solid bodies and the other which is allied to fluid mechanics concepts is a
flow formulation. Calculation of elastic effects such as residual stresses and spring-

102

back can be included in both formulations. Figure 6.1 shows how the mechanical
formulations are categorized in four ways which depend on how plasticity is modeled
and if elastic deformation of the solid metal is neglected or not [13]. Generally the
flow formulation is applicable to hot forging where the mechanical properties of the
metal are sensitive to rate of deformation and the structural formulation applies to
cold forging where the influence of deformation rate can often be ignored.

EŽ ůĂƐƚŝĐ tŝƚŚ ůĂƐƚŝĐ

σ σ

^ƚƌƵĐƚƵƌĂů ε
ĨŽƌŵƵůĂƚŝŽ
ůĂƐƚŝĐͲWůĂƐƚŝĐ
ε

ZŝŐŝĚͲWůĂƐƚŝĐ

σ ε σ
ε
&ůŽǁ
ĨŽƌŵƵůĂƚŝŽ ε

ε ůĂƐƚŝĐͲsŝƐĐŽƉůĂƐƚŝĐ

ZŝŐŝĚͲsŝƐĐŽĞůĂƐƚŝĐ

Fig.6.1 Different types of material behaviour

The elasto-plastic constitutive equation together with contact conditions are used for
metal forming analysis. The radial return mapping algorithm is used to compute the
stress and internal variables (Krieg and Key, 1976) [14], and the consistent tangent
operator (Simo and Taylor, 1985) [15], which preserves the quadratic convergence
rate of the Newton method is also used.

J.Babu Rao et.al [16], reported the deformation behaviour of Al-4Cu-2Mg alloy
during cold upset forging, and found the relationship between the circumferential
strain and axial strain increments is continuously changing with increasing
deformation.

103

J. Appa Rao, J. Babu Rao, Syed Kamaluddin et.al [17], reported the cold workability
limits of Brass, as a function of friction, aspect ratio and specimen geometry, they
also conducted the ring compression test to determine the friction factor, and finally
validated the experimental results with the finite elements software.

S. Dikshit, et.al [18], have studied and evaluated the effect of homogenization and
deformation behaviour of AA2014/SiC/10p composite billets, having dispersions in
size range of 20–40 µm, by conducting cold upsetting experiments under
unlubricated conditions and made comparison with finite elements software.

6.3 PROCEDURE ADOPTED IN MODELING THE PROBLEM UNDER
TAKEN.

The computational modeling of each forming process stage by the finite element
method can make the sequence design faster and more efficient, decreasing the use of
conventional “trial and error” methods. In this study, the application of commercial
general finite element software ANSYS-10 has been applied to model a forming
operation

Finite element analysis of deformation behaviour of cold upsetting process was
carried out for all the HSA(P) composites and base alloy (A356) with aspect ratios of
1.0 and 1.5 in dry condition. Due to axisymmetric nature of the geometry only
quarter portion was modeled with symmetric boundary conditions. Rigid-flexible
contact analysis was performed for the forming process, so that the die appears like a
thin plate, and the stress analysis was done on the billet only. The billet geometry was
meshed with 8-node Brick elements (solid 185 in ANSYS Library). Element size was
selected on the basis of convergence criteria and CPU time. Too coarse mesh may
never converge and too fine mesh requires long CPU time without much improvement
in accuracy.

6.3.1: Contact Analysis

The contact problem is a kind of geometrically nonlinear problem that arises when
different structures or different surfaces of a single structure, either come into contact
or separate or slide on one another with friction. Contact forces, either gained or lost,
must be determined in order to calculate structural behavior [19]. The location and
extent of contact may not be known in advance, and must also be determined.

104

Contact algorithms in FM analysis allow contact elements to be attached to the
surface of one of two FE discretization’s that are expected to come in contact. A
contact element is not a conventional finite element. Their functions is to sense
contact and then supply a penalty stiffness or activate some other scheme for
preventing or limiting interpenetration. Contact analysis is highly complex and
nonlinear analysis. Contact problems fall into two general classes. One is rigid-to-
flexible and flexible-to-flexible. In rigid-to-flexible contact problems, one or more of
the contacting surfaces are treated as rigid, i.e., it has a much higher stiffness relative
to the deformable body it contacts.

In general, any time a soft material comes in contact with hard material, the problem
is assumed to be rigid-to-flexible, instances like: metal forming problems. The other
class, flexible-to-flexible, is the more common type. In this case, both contacting
bodies are deformable, i.e. have similar stiffness. Example, bolted flanges. Ansys
supports three contact models; node-to-node, node-to-surface and surface-to-surface
contact. In problems involving contact between two boundaries, one of the boundaries
is conventionally established as the target surface and the other as the contact surface.
For rigid-flexible contact, the target surface is always the rigid surface and the contact
surface is the deformable surface. For flexible-to-flexible contact, both surfaces are
associated with deformable bodies. These two surfaces together comprise the contact
pair. Ansys provides special elements for contact pair. Different contact elements are
CONTAC12, CONTAC52, CONTAC 26, CONTAC 48, CONTAC 171,172,
TARGET 169, CONTAC 173, and TARGET 170. Figure 6.2 shows the contact pair
between die and composite model.

Contact elements are constrained against penetrating the target surface. However,
target elements can penetrate through the contact surface. In the present problem
rigid-to-flexible analysis is performed. For rigid-to-flexible contact, the choice of
target was tooling (upper and bottom platens) which need not require meshing.
Obviously the soft billet surface was considered as contact

105

Figure 6.2: Contact pair between die and composite model

6.3.2 Material Properties and Real Constants
The material models selected were based on the properties of the tooling and billet
materials. Due to high structural rigidity of the tooling, only the following elastic
properties of tooling (H13 steel) were assigned assuming the material to be isotropic
[20].

Young’s Modulus E = 220 GPa (for steel)
Poisson’s ratio ȣ = 0.3

As the nature of loading is non-cyclic, Bauschinger effect could be neglected and the
non-linear data was approximated to piecewise multi linear with 10 data points. The
material was assumed to follow the Isotropic hardening flow rule. Suitable elastic
properties were also assigned for the material under taken for analysis. As the
experiments were conducted at room temperature, the material behaviour was
assumed to be insensitive to rate of deformation

106

6.4 RESULTS AND DISCUSSION

Figure 6.3 and 6.4 shows the meshed models of billets and tooling for the aspect
ratios of 1.0 and 1.5 respectively. Figure 6.5 and 6.6 shows the 50% deformation
specimen with zero friction for the aspect ratios of 1.0 and 1.5 respectively. Since
there was no friction at metal-die contact, the deformation can be treated as
homogeneous since no bulging was seen. The maximum radial displacement
corresponding to 50% for the aspect ratio of 1.0 is shown as 2.435mm in figure 6.7.
This means that the diameter after 50% deformation equals to 12 + 2 X 2.435 = 16.87
mm. The value of analytically determined diameter after 50% equals to 12 X 2 =
16.970 mm, (assuming volume constancy) leading to a very little error of 0.59%
usually can be discarded in non-linear finite element analysis such as in large
deformation / metal forming applications. Hence the analysis procedure adopted is
validated.

For the present study the friction factor ‘m’ was found to be 0.36 (explained in
chapter 5) and the extent of barreling with this friction at 50% deformation for alloy
and composites under investigation was shown in figures 6.9-6.40 respectively. These
results were supported by many authors [11-30]. Lower aspect ratio (H0/D0 = 1.0)
samples has shown more barreling affect compare to higher aspect ratio (H0/D0 = 1.5).
The above results were experimentally evidenced, as discussed in chapter 5.
The notations used in the analysis were, radial displacements (UX): circumferential
stress,σ θ (SY), axial stress σ z (SZ), hydrostatic stress, σ H (NLHPRE), Von-Mises
equivalent stress σ (SEQV).

The variations in FEA results compared to analytical results obtained in chapter 5
were shown in figures 6.41 to 6.44. The obtained FEA results revealed that these
values are closely matching with the experimental values with a maximum deviation
of less than 5%. Hence the FEA model adopted for solving the present upsetting
analysis was validated with the analytical results of chapter 5.

107

Figure 6.3: Undeformed sample (H0/D0 = 1.0)

Figure 6.4: Undeformed sample (H0/D0 = 1.5)
108

Figure 6.5: Deformed sample (H0/D0 = 1.0) at 50% deformation for zero friction

Figure 6.6: Deformed sample (H0/D0 = 1.5) at 50% deformation for zero friction
109

Figure 6.7: Radial displacement at 50 % deformation for zero friction (H0/D0 = 1.0)

Figure 6.8: Radial displacement at 50 % deformation for zero friction (H0/D0 = 1.5)
110

Figure 6.9: Axial Stress at 50% deformation of A356 alloy (H0/D0 = 1.0)

Figure 6.10: Axial Stress at 50% deformation of A356 alloy (H0/D0 = 1.5)
111

Figure 6.11: Circumferential Stress at 50% deformation of A356 alloy (H0/D0 = 1.0)

Figure 6.12: Circumferential Stress at 50% deformation of A356 alloy (H0/D0 = 1.5)
112

Figure 6.13: Hydrostatic Stress at 50% deformation of A356 alloy (H0/D0 = 1.0)

Figure 6.14: Hydrostatic Stress at 50% deformation of A356 alloy (H0/D0 = 1.5)
113

Figure 6.15: Von-Mises Stress at 50% deformation of A356 alloy (H0/D0 = 1.0)

Figure 6.16: Von-Mises Stress at 50% deformation of A356 alloy (H0/D0 = 1.5)
114

Figure 6.17: Axial Stress at 50% deformation of 5% composite (H0/D0 = 1.0)

Figure 6.18: Axial Stress at 50% deformation of 5% composite (H0/D0 = 1.5)
115

Figure 6.19: Circumferential Stress at 50% deformation of
5% composite (H0/D0 = 1.0)

Figure 6.20: Circumferential Stress at 50% deformation of
5% composite (H0/D0 = 1.5)
116

Figure 6.21: Hydrostatic Stress at 50% deformation of 5% composite (H0/D0 = 1.0)

Figure 6.22: Hydrostatic Stress at 50% deformation of 5% composite (H0/D0 = 1.5)
117

Figure 6.23: Von-Mises Stress at 50% deformation of 5% composite (H0/D0 = 1.0)

Figure 6.24: Von-Mises Stress at 50% deformation of 5% composite (H0/D0 = 1.5)
118

Figure 6.25: Axial Stress at 50% deformation of 10% composite (H0/D0 = 1.0)

Figure 6.26: Axial Stress at 50% deformation of 10% composite (H0/D0 = 1.5)
119

Figure 6.27: Circumferential Stress at 50% deformation of
10% composite (H0/D0 = 1.0)

Figure 6.28: Circumferential Stress at 50% deformation of
10% composite (H0/D0 = 1.5)
120

Figure 6.29: Hydrostatic Stress at 50% deformation of 10 % composite (H0/D0 = 1.0)

Figure 6.30: Hydrostatic Stress at 50% deformation of 10% composite (H0/D0 = 1.5)
121

Figure 6.31: Von-Mises Stress at 50% deformation of 10% composite (H0/D0 = 1.0)

Figure 6.32: Von-Mises Stress at 50% deformation of 10% composite (H0/D0 = 1.5)
122

Figure 6.33: Axial Stress at 50% deformation of 15% composite (H0/D0 = 1.0)

Figure 6.34: Axial Stress at 50% deformation of 15% composite (H0/D0 = 1.5)
123

Figure 6.35 Circumferential Stress at 50% deformation of 15% composite
(H0/D0 = 1.0)

Figure 6.36: Circumferential Stress at 50% deformation of 15% composite
(H0/D0 = 1.0)
124

Figure 6.37: Hydrostatic Stress at 50% deformation of 15% composite (H0/D0 = 1.0)

Figure 6.38: Hydrostatic Stress at 50% deformation of 15% composite (H0/D0 = 1.5)
125

Figure 6.39: Von-Mises Stress at 50% deformation of 15% composite (H0/D0 = 1.0)

Figure 6.40: Von-Mises Stress at 50% deformation of 15% composite (H0/D0 = 1.5)
126

COMPARATIVE GRAPHS BETWEEN EXPERIMENTAL AND FEA VALUES

Figure 6.41: Comparative graphs between experimental and FEA values of Effective

stressσ , stress componentsσθ , σ and σ as a function of effective
z H

strain ε for A356 alloy up to 50% deformed in dry condition with aspect

ratio: (a) H0/D0 = 1.0, (b) H0/D0 = 1.5.

127

Figure 6.42 Comparative graphs between experimental and FEA values of Effective
stressσ , stress componentsσθ , σ z and σ H as a function of effective
strain ε for 5 % composite up to 50% deformed in dry condition with
aspect ratio: (a) H0/D0 = 1.0, (b) H0/D0 = 1.5.

128

Figure 6.43 Comparative graphs between experimental and FEA values of Effective
stressσ , stress componentsσθ , σ z and σ H as a function of effective
strain ε for 10 % composite up to 50% deformed in dry condition with
aspect ratio: (a) H0/D0 = 1.0, (b) H0/D0 = 1.5.

129

Figure 6.44 Comparative graphs between experimental and FEA values of Effective
stressσ , stress componentsσθ , σ z and σ H as a function of effective
strain ε for 15 % composite up to 50% deformed in dry condition with
aspect ratio: (a) H0/D0 = 1.0, (b) H0/D0 = 1.5.

130

6.5 CONCLUSIONS
Detailed comparisons of the experimental variables with the finite element method
(FEM) results were carried out to ascertain the accuracy with which the deformation
process can be modelled. Predictions from the simulation results were found to be in
good agreement with the actual experimentation

1. The cold upsetting process was modeled, simulated and analyzed with a
sufficient accuracy.

2. The accuracy of results depends on the accuracy of the input data (true stress-
true strain behaviour and friction factor obtained from the experiments) and
friction model used in the analyses.

3. The analysis is useful in reducing the lead time of design cycle.
4. The machine down time can be reduced at production stage.

131

REFERENCES

1. Jolgaf, M., Hamouda, A.M.S., Suleiman, S and Hamdan, M.M, 2003,
Development of a CAD/CAM system for the closed–die forging process, Journal
of Material Processing Technology, 138: pp.436-442.

2. Altan T Male, and Vincent Depierre, 1970, Transactions of the ASME J of
Lubrication Technology, July 1970: pp.389 – 397.

3. Samantha S.K, 1975, Effect of friction and specimen geometry on the ductile
fracture in upset. Institute of Engineering Materials and Technology.
Transactions of ASME, Jan 1975: pp.14-20.

4. Santos, Duarte, D. J.F., Anareis, Rur Neto, Ricardo Paiva, and Rocha, A.D,
2001. The use of Finite Element Simulation for optimization of Metal Forming
and Tool Design. J of Material Processing Technology. 119: pp.152 -157.

5. Kobayashi, S., Oh, S.I. and Altan T, 1989, Metal Forming and Finite Element
Method, Oxford University Press, New York.

6. Lee, C.H., and Kobyashi, S, 1973, New solutions to rigid plastic deformation
problems using a matrix method. J of Engineering for Industry Trans. of ASME.
95: 865.

7. Jackson, J.E, J.r., and Ramesh, MS, 1992. The rigid plastic finite element
method for simulation of deformation processing, Numerical Modeling of
Material deformation Processes. Springer-Verlag, London, pp 48 – 177.

8. Bathe K.J, 1996, Finite Element Procedures- Prentice – Hall, pp 622.

9. Kobayashi, S and Altan T., “Metal Forming and the Finite Element Method”,
Oxford University Press, New York, 1989.

10. Lee C.H. and Kobayashi S., “New Solutions to Rigid-Plastic Deformation
Problems Using a Matrix Method”, J. Eng. Ind. (Trans. ASME), vol. 95, 1973, p
865.

132

11. Zeinkiewiez O.C., “Flow Formulation for Numerical Solution of Forming
Processes”, in. Pittman J.F.T et al. (Eds), “Numerical Analysis of Forming
Processes”, Wiley. New York, 1984, pp. 1- 44.

12. Jackson J.E., JR and Ramesh. M.S., “The Rigid-Plastic Finite Element Method for
Simulation of Deformation Processing” in Hartley. P. et al. (Eds), “Numerical
Modelling of Material Deformation Processes”, Springer-Verlag, London, 1992,
pp 148-177.

13. Forging Modelling Project, School of Mechanical Engineering, University of
Bath, Report FMP -3, 12-12.

14. Krieg, R.D and Key, S.W., “Implementation of a Time-Independent Plasticity
Theory into Structural Computer Programs” in “Constitutive Equations in Visco-
plasticity: Computational and Engineering Aspects”, Stricklin. J.A and Saczalski.
K.J. (eds.), AMD-20, ASME, NY, 1976.

15. Simo, J.C and Taylor, R.L., “Consistent Tangent Operators for Rate-Independent
Elasto-Plasticity”, Compute. Meth. Appl. Mech. Engg., Vol 48, 1985, pp 101-118.

16. J Babu Rao, Syed Kamaluddin, J Appa Rao, MMM Sarcar and NRM Bhargava
Deformation behavior of Al-4Cu-2Mg alloy during cold upset forging,
International Journal of Alloys and Compounds, Vol. 471, 2009, pp. 128-136.

17. J Appa Rao, J Babu Rao, Syed Kamaluddin, MMM Sarcar and NRMR Bhargava
Studies on Cold Workability Limits of Pure Copper using Machine Vision System
and its Finite Element Analysis” International Journal of Materials and Design -
Vol. 30, 2009, pp. 2143–2151.

18. S.Dikshit, V. Gurjar and R. Dasgupta, Studies on cold upsetting behaviour of
A2014 based metal-matrix composites, fem simulation, and comparison with
experimental results, J Mater Sci, 2010, 45: pp.4174-4179.

19. ANSYS 10.0 Help manual documentation.

20. http://www.matweb.com

133

21. Jolgaf, M., Hamouda, A.M.S., Sulaiman, S and Hamdan, M.M., “Development of
a CAD/CAM system for the closed–die forging process”, Journal of Material
Processing Technology, Vol 138, 2003, pp 436-442.

22. Taylan Altan and Dan Hannan “Prediction and Elimination of Defects in Cold
Forging Using Process Simulation” R&D Update Forging, The Engineering
Research Center for Net Shape Manufacturing, 2002, http://www.erensm.org.

23. Bramley, A.N, and Mynors, D.J., “The use of forging tools” Materials and Design,
vol 21, 2000, pp 279-286.

24. Weronski, W., Gontarz, A., and Pater, Zb., “The reason for structural defects
arising in forgings of aluminium alloys analysed using the finite element method”
Journal of Materials Processing Technology, vol 92-93, 1999.

25. Kusiak,J., Pietrzyk,M., Chenot,L., “Die Shape Design and Evaluation of
Microstructure Control in the Closed-die Axisymmetric Forging by Using
FORGE2 Program” ISIJ International, vol 34, 1994, No 9, pp 755-760.

26. Chitkara,N.R., and Kim,Y, “Simulation of Upset Heading, Application of Rigid-
Plastic Finite Element Analysis and some Experiments” The International Journal
of Advanced Manufacturing Technology, vol 20, 2002, pp 589-597.

27. Ph.D Thesis of J. Babu Rao, Department of Metallurgical Engineering Andhra
University, 2006.

28. Syed Kamaluddin, J Babu Rao, MMM Sarcar and NRMR Bhargava, “Studies on
Flow Behavior of Aluminum Using Vision System during Cold Upsetting”. Met
and Mater. Trans. B, 38 B, 2007: pp.681-688

134