In many high temperature applications, it is necessary to join together
tubular parts of substantially different chemical, physical and mechanical
characteristics. For example, such applications arise in fossil-fired
boiler construction and in nuclear power stations. In such power stations,
high temperature joints are commonly required in various heat exchanger
components such as boilers, steam generators, intermediate heat exchangers
and recuperators, particularly in high temperature gas-cooled reactors,
etc. The joining of dissimilar metals is generally more challenging than
that of similar metals because of differences in the properties of the
base metals welded. These differences may also complicate the selection
of filler metals compatible to both base metals (Sun and Karppi, 1996;
Sedek et al., 2003).
Firstly dissimilar joints must meet the strength requirements and the
probability of defect formation must be estimated and controlled. One
of the most important defects that may be exists in any welded structures,
are residual stresses. But in dissimilar metal joints because of nonuniform
distribution of temperature field due to different thermal properties,
welding residual stresses may be very complex and it is very difficult
to predict the distribution of these stresses particularly in butt welding
Recently many techniques have been used for measuring residual stresses
in metals including stress relaxation techniques, diffraction techniques,
cracking techniques and techniques by use of stress sensitive properties
(Masubuchi, 1980; Price et al., 2006). In spite of diversity of
experimental methods, they have disadvantages because they only obtain
incomplete stress distribution and most of them are costly and time-consuming
and some of them are destructive. For these reasons it is necessary to
establish other methods of evaluating weld induced residual stresses.
In recent years, advanced numerical analysis has been applied to resolve
the complex engineering problems. The finite element method is the conventional
means of calculating residual stresses. Many authors used finite element
method to perform welding simulation and to predict weld induced residual
stresses in different types of joints and materials. For example the finite
element code ADIANT was used by Karlsson and Josefson (1990) while other
authors as Junek et al. (1999) and Dubois et al. (1984)
have utilized SYSWELD to perform the weld simulation. Teng et al.
(2000) and Sarkani et al. (2000) employed ABAQUS and Fricke et
(2001) employed the computer program FRESA, while Chao and Qi (2000)
estimated residual stresses using the finite element code WELDSIM. Josefson
(1993) estimated residual stresses in a multi-pass weld and in a spot-welded
box beam with SOLVIA, Abid and Siddique (2005) utilized commercial code
ANSYS to evaluate weld induced residual stresses.
In this study, finite element analysis of residual stresses in butt welding
of two dissimilar austenitic stainless steel and carbon steel pipes, is
performed using commercial software ANSYS, which includes moving heat
source, material deposit, temperature dependant material properties, metal
plasticity and elasticity, transient heat transfer and mechanical analysis.
In the first stage of the study after determining suitable filler metal
by Schaeffler diagram, butt welding of two similar plates were simulated
and a macro in ANSYS Parametric Design Language (APDL) generated. The
calculated finite element results were compared with experimental results
of other researchers. In the second stage after gaining satisfactory and
validated results from the simulation of the similar plates, the same
procedure was implemented in welding of dissimilar material pipes to obtain
the residual stresses magnitudes and distributions.
MATERIALS AND METHODS
Filler metal selection: When a weld is made using a filler
wire or consumable, there is a mixture in the weld consisting of parent
metal andfiller metal alloy (percentage depends on welding process, type
of joint and welding parameters). The degree of mixing is defined by percentage
dilution as follow (Bonifaz, 2000):
where, Vfm is the volume of deposited filler metal, Efm
and Es represent the enthalpy change required to melt a given
volume of filler metal and substrate, respectively and the terms ηa.
ηmVI represents the melting power delivered by the arc.
In this expression, ηa and ηm are, arc
and melting efficiency of welding process, respectively. For Manual Metal
Arc Welding (MMAW) reported percentage of dilution is 20-30% (Kou, 2002).
In dissimilar joints any reduction in alloy content of austenitic stainless
steel is likely to cause the formation of martensite on cooling. This
could lead to cracking problems and poor ductility. To avoid this problem
filler metal must be selected so that ferrite content become in the range
of 4-10%. Schaeffler first proposed the quantitative relationship between
the composition and ferrite content of the weld metal. Then Schaeffler
diagram can be used to determine the type of microstructure that can be
expected when a filler metal and parent metal of differing compositions
are mixed together in a weld. The Nickel and other elements that form
austenite are plotted against chrome and other elements that form ferrite,using
the formula 2 and 3 (Kou, 2002):
||The microstructure of weld metal without filler wire
||The microstructure of weld metal with filler wire
Our purpose was to determine suitable filler metal for joining ASTM A36
carbon steel to 304L stainless steel.
For 304L: Nieq = 11.4, Creq = 20.45 and for ASTM
A36: Nieq = 5.05, Creq = 0.35
In the Fig. 1a, point B represents the microstructure
of weld metal that is in the martensite region then it is susceptible
By considering 25% for percentage dilution in accordance with Schaeffler
diagram (Fig. 1b), 309L selected for filler metal that
has Nieq = 14.45, Creq = 24.9.
||Geometry and meshed model used in the analysis
In Fig. 1b, the point A represents the structure of
weld metal in which ferrite content is in the range of 5-10%. Therefore
in this joint there is not the risk of cracking and 309L filler wire is
suitable for joining of these materials.
Theoretical considerations: Because of thermo-mechanical nature
of welding process theoretical considerations can be assessed either using
a thermal or a mechanical analysis. Welding thermal stresses are calculated
from the temperature distributions determined by the thermal model. The
residual stresses from each temperature increment are added to the nodal
point location to determine the updated behavior of the model before the
next temperature increment. Complete thermal and mechanical models are
represented in reference (Teng and Chang, 1998).
Finite element modeling procedure
Verification: To confirm the accuracy of the present method, welding
process of a butt weld joint of two ASTM A36 steel plates with the dimensions
of those used by Hsiang and Liang (2004) was simulated. Figure
2 shows the geometry and meshed model used in the analysis. The result
of finite element analysis is shown in Fig. 3a and b.
These figures show good agreements between analyzed method and the researchers`
experimental results. Therefore, the procedure presented here is considered
suitable for analysis of residual stresses and distortions due to welds.
After gaining satisfactory results, the validated method implemented in
welding simulation of dissimilar material pipes and residual stresses
magnitude and distribution obtained.
||Comparison of FEM with experimental
results for axial residual stresses
||Comparison of FEM with experimental
results for transverse residual stresses
Present study: In this study the Manual Metal Arc Welding (MMAW)
process of joining 304L austenitic stainless steel to ASTM A36 carbon
steel pipes with 309L stainless steel filler metal were simulated using
general purpose finite element package ANSYS10.0. The overall dimensions
adopted were those used by Lindgren and Karlsson (1998) and Murthy et
al. (1996) except that a full penetration considered here. The geometry
and meshed model are shown in Fig. 4.
Coupled thermo mechanical analysis: The procedure for a coupled-field
analysis depends on which fields are being coupled, but two distinct methods
can be identified: sequential and direct. The sequential method involves
two or more sequential analysis that belongs to a different field. But
the direct method usually involves just one analysis that uses a coupled-field
element type containing all necessary degree of freedoms. To simplify
the welding simulation, it is computationally efficient to perform the
thermal and mechanical analyses separately. In this case physically, it
is assumed that changes in the mechanical state do not cause a change
in the thermal state. But a change in the thermal state causes a change
in the mechanical state. So that in this study computation of the temperature
history during welding and subsequent cooling is completed first and then
this temperature field is applied to the mechanical model as a body force
to perform the residual stress analysis.
The finite element model (Fig. 4) consists of total 15348
nodes and associated 9504 linear elements. Due to high temperature and stress
gradients near the weld, relatively fine mesh is used in both sides of weld
center line. Eight-node brick elements with linear shape functions are used
in meshing of the model. For thermal analysis the element type is SOLID70 which
has single degree of freedom, temperature, on its each node. For structural
analysis the element type is SOLID45 with three translational degrees of freedom
at each node.
||Temperature distribution at t = 5 sec
||Temperature distribution at t = 10 sec
Heat input during welding is modeled in ANSYS by a distributed heat flux
applying on individual elements. The amount of heat input calculated as
follow Dubois et al. (1984):
where, η is arc efficiency; V is travel speed; U and I are arc voltage
and current, respectively. Here, it is assumed that, current 180 A, Voltage
24 V and welding speed 5 mm sec-1. These values are in accordance
with the WPS that has been written by Kavoshgharan Mechanic of Mersade
Gharb Company for welding these pipes. The arc efficiency of the process
considered to be 85% (Kou, 2002).
In the thermal analysis, a total of 216 load steps with maximum 200 sub
steps and minimum 25 sub steps were required to complete the heating cycle.
Automatic time stepping and full Newton-Raphson method was used in each
time step for the heat balance iteration.
Figure 5a and b illustrate the temperature
fields of the butt welded pipe at t = 5, 10 sec after the start of welding.
From Fig. 5a and b it is obvious that
heat flow pattern in two dissimilar pipes is nonsymmetrical that is because
of differences in thermal properties of two steels. From this analysis
we can understand that the temperature of carbon steel increases rapidly
in comparison with stainless steel. On the other hand in a certain time
for two points that have same distances from weld center line the temperature
of points that are located in carbon steel side is higher than stainless
Metal deposition and element birth and death technique: Metal
deposition is another important aspect of finite element modeling of the
welding process. The model in this study adopts the technique of element
birth and death to simulate the weld filler variation with time in butt
welded joint. In the element birth and death technique, all elements must
be created, including the substrates and those of deposited weld filler
that to be born in later stages of the analysis. To achieve the element
death effect, the ANSYS program does not actually remove killed elements.
Instead, it deactivates them by multiplying their stiffness (or conductivity,
or other analogous quantity) by a severe reduction factor. This factor
is set to 1.0E-6 by default, but can be given other values. In the same
manner, when elements are born, they are not actually added to the model;
they are simply reactivated.
When an element is reactivated, its stiffness, mass, element loads, etc.
return to their full original values. Elements are reactivated with no
record of strain history (or heat storage, etc.); however, initial strain
defined as a real constant will not be affected by birth and death
operations. Thermal strains are computed for newly-activated elements
based on the current load step temperature and the reference temperature.
Another important aspect of element birth and death that employed in this
study is in structural analysis. In this analysis elements that are in
liquid phase must be deactivated and after heat transfer they gradually
solidified and thus must be reactivated. Because we will not explicitly
know the location of elements that require to deactivated or reactivated
we should identify them on the basis of their ANSYS-calculated temperatures
(Abid and Siddique, 2005; Murthy et al., 1996; Teng et al.,
Material model: In the simulation of welding process, material
modeling is one of the key problems according to ANSYS10.0 Theory Manual.
Different material laws have been utilized in weld simulations. The available
material laws typically include an elastic-perfectly plastic model or
a plasticity model which takes into account strain hardening, either kinematic
or isotropic (Zhu and Chao, 2002). In this study for thermal elasto-plastic
material model, the von Mises yield criterion and the isotropic strain
hardening rule were considered. Most publications in welding simulation
adapted material properties that are dependent on temperature. The material
used here are ASTM A36 carbon steel and 304L austenitic stainless steel
as base metals and 309L stainless steel as filler metal. Their physical
and mechanical properties as a function of temperature are presented in
Table 1, 2 and 3
(Deng and Murakawa, 2006; Masubuchi, 1980).
||Temperature dependent thermal, physical and mechanical
properties of 304 L austenitic stainless steel
||Temperature dependent thermal, physical and mechanical
properties of 309 L filler wire
||Temperature dependent thermal, physical and mechanical
properties of ASTM A36 carbon steel
||Hoop residual stresses in outer surface
||Axial residual stresses in outer surface
RESULTS AND DISCUSSION
The finite element analysis result of the residual stress distributions
in outer and inner surfaces of the pipe in hoop and axial directions are
presented in Fig. 6a-d.
Based on the results of the finite element analysis, the characteristics
of welding residual stress distribution in two dissimilar pipes used in
this study can be described as follows. Because of differences in thermal
properties of two materials that has a direct effect on temperature distribution
and heating and cooling rates of two pipes the distribution of thermal
strains and resultant residual stresses are nonsymmetrical and the effect
of different mechanical properties causes that the position of maximum
residual stress becomes different in compare with similar pipes. In similar
pipes maximum residual stresses are coincided on weld center line but
in the case of dissimilar one as indicated in the Fig. 6a-d
the maximum residual stresses is in the side of metal that has a highest
strength namely carbon steel. Also Fig. 6d indicates
that a tensile axial stress is produced on the inside surface and Fig.
6b shows that compressive axial stress exists on the outside surface.
Moreover on the inside surface, the shape of hoop stress is very similar
to the axial stress. The axial residual stresses on the insider surface
and the outside surface have a contrary distribution.
||Hoop residual stresses in inner surface
||Axial residual stresses in inner surface
||Finite element method is an efficient technique in analyzing
residual stresses in welding.
||With generating macro, different conditions can be examined. This
show that finite element is a flexible method in welding simulation.
||In joining stainless steel to carbon steel Schaeffler diagram can
be helpful in selection of suitable filler metal.
||Differences in physical, mechanical and chemical properties of base
metals cause nonuniform temperature distribution and heat transfer.
||Residual stress distribution in dissimilar joints is nonsymmetrical
and the maximum residual stress is in the side of metal that has a
highest strength namely carbon steel.