Three-Dimensional Thermo-Elastic-Plastic Finite Element Method Modeling for Predicting Weld-Induced Residual Stresses and Distortions in Steel Stiffened-Plate Structures

The objective of the present paper is to develop nonlinear finite element method models for predicting the weld-induced initial deflection and residual stress of plating in steel stiffened-plate structures. For this purpose, three-dimensional thermo-elastic-plastic finite element method computations are performed with varying plate thickness and weld bead length (leg length) in welded plate panels, the latter being associated with weld heat input. The finite element models are verified by a comparison with experimental database which was obtained by the authors in separate studies with full scale measurements. It is concluded that the nonlinear finite element method models developed in the present paper are very accurate in terms of predicting the weld-induced initial imperfections of steel stiffened plate structures. Details of the numerical computations together with test database are documented.

Simplified methods to predict weld-induced initial distortions are available in the literature [13]- [18].However, weld-induced initial imperfections are affected by various parameters such as weld joint details, plate thickness, thickness transition (when the joint consists of plates with different thicknesses), stiffener spacing, numbers of attachments, corrugated constructions, mechanical restraint conditions, assembly sequences and overall construction planning [19].In this regard, more refined method is still required to accurately predict them.
Nonlinear finite element method is a powerful tool to predict the weld-induced initial imperfections as it can deal with the distribution of heat transfer and general deformation due to welding.Ueda and Murakawa [20] undertook a pioneering work using two-dimensional finite element method to predict weld-induced residual stresses.Lindgrean and Karlsson [21] are the first to use three-dimensional finite element method for predicting weld-induced residual stresses.Chen and Guedes Soares [22] also used the three-dimensional finite element method to predict the weld-induced residual stresses with a validation by a comparison with test database on small scale models.Studies on predicting the weld-induced initial distortions using finite element method are also found in the literature [23]- [28].It was realized from the studies that the computing times are very expensive, and thus simplified methods using inherent strain have been suggested [27] [29] [30].Michaleris and DeBiccari [31] developed a useful method to predict weld-induced distortions of large and complex structures, where two-dimensional thermal analysis was performed while three-dimensional structural analysis was undertaken.Regardless of the useful contributions in the literature, more efforts are still required for predicting the weld-induced initial imperfections of ships and offshore structures in association with welding and repair methods as well as robust design [32].
And, studies on repair welding using finite element method and experiment are also found in the literature [33] [34] [35].
In this paper, a three-dimensional thermo-elastic-plastic finite element method model is developed to predict the weld-induced distortions and residual stresses of thin-walled structures while achieving the goals in resulting accuracy and computational cost.The validity of the method is confirmed by a comparison with test database separately obtained from the full scale measurements by the authors.

Finite Element Modeling for Predicting the Weld-Induced Residual Stresses
In this section, the finite element model is presented to predict the weld-induced residual stresses.The three-dimensional thermo-elastic-plastic finite element analysis method is applied.
Welding residual stress analysis is a complex problem requiring a lot of knowledge such as solid mechanics, heat transfer, materials science and so on.
An important feature of this problem is the nonlinearity of the material.That is, material properties such as thermal conductivity, heat capacity, elastic modulus, yield stress, and Poisson's ratio vary sensitively with temperature.Particularly in the case of welding, there is sudden change of the temperature from the atmospheric temperature to the melting temperature of the metal.In addition, during the thermal transition period, the material experiences state changes from the solidus to the liquidus, or vice versa.These state changes produce changes in material properties and specific volume.This is generally explained by the coefficient of thermal expansion.For this reason, it is very difficult to obtain an analytical solution to the temperature and stress field.However, recent advances in finite element analysis using computer have led to many improvements in the residual stress analysis of welding.In general, the finite element method provides very detailed information on transition temperature, displacement, strain and stress.This FE method provides an accurate solution to the welding problem.This is possible because the temperature-dependent changes in the material properties of the material can be taken into account and properties such as the state of the weld and the phase change can be sufficiently modeled.As described above, the features of the welding problem requires consideration of many physical phenomena.Figure 2 shows the form of the connection between thermal, mechanical and metallurgical processes for the phenomena occurring during the welding process.This method is used to analyze the weld-induced residual stress.
The validation of the finite element model is made by a comparison with test database obtained by Paik and Yi [36].The MSC/MARC computer program [37] is used for computations in the present study.

Modeling of Heat Source
As heat source moves associated with welding, the heat input can change accordingly.Rosenthal [38] suggested a model to simulate the moving heat source although the distribution of heat input was not considered due to the change of heat source.Goldak et al. [39] suggested a model to consider thermal distribution through moving heat source using Gaussian surface or double-ellipsoidal distributions.For welding with low depth of penetration, the Gaussian surface distribution model is well more suitable to apply.However, as the weld penetration becomes deep like in shipbuilding industry practice, heat transfer is of significance in the thickness direction.In this case, the double-ellipsoidal distribution model is more suitable.
Figure 3 presents the configuration of the heat source distribution with a double ellipsoidal shape.The heat flux for the first half-ellipsoidal internal area located at the front of the welding arc can then be defined as follows: ( )  the voltage.x, y and z are the coordinate where the origin is located on the weld surface below the heat source as shown in Figure 2.
The arc efficiency η is defined as the ratio of the heat transferred from the arc to the base material and the total heat generated by the arc, which is a constant simply indicative of the complex heat loss between the substrates in the arc.
Since the arc efficiency is influenced by various factors such as welding conditions, melting depth and protective gas, it is very challenging to predict it theoretically and it is usually determined experimentally.This is because the arc efficiencies given in the literature are somewhat different from each other.For flux cored arc welding considered in the present method, 0.75 η = is usually taken.
The heat flux at any point ( ) , , x y z in the second semi-ellipsoid covering the rear part of the arc can be defined as follows: ( ) , , r q x y z is the heat flux at any point ( ) , , x y z in the second semi-ellipsoid covering the rear part of the arc, r c is the geometric parameter, and r f is the heat input proportion in the rear part.It is realized that approximately taken as far as the following conditions are satisfied:

Thermal Loading Load and Boundary Conditions
As mentioned earlier, a quarter model of the target structure is applied as the extent of the finite element analysis as shown in Figure 4 in association with the symmetric condition.Figure 7 shows the sample model of the thermo-elastic-plastic finite element analysis together with loading and boundary conditions where the welding sequence is divided into 8 zones in the same order as the actual welding sequence.The structure is modelled using eight-node 3D brick thermal-mechanical finite elements or Solid 7 (full integration type) elements which treat plasticity, hyper-elasticity, stress stiffening, creep, large deflection, and large strain capabilities [37].
Welding heat input is applied using the dual heat source model where thermal loading and boundary conditions with convection and radiation are allocated.
With convective conditions, the related constants depending on elevated temperature are defined from the database obtained from experiments and computational fluid dynamics simulations [41].Figure 8 shows the variation of the temperature-dependent convection coefficient values [41].
Table 3 indicates the heat input defined from welding parameters associated with weld bead length applied in the present study.Table 4 gives the values of double ellipsoidal moving source model [22].

Computed Results and Discussion
Figure 9(a) shows the process of the moving heat source and resulting temperature distributions when welding is performed at the second weld zone.Figure 9(b) shows the equivalent von Mises stress distribution for the structure with a plate thickness of 6 mm after welding and cooling are completed.
Figure 10 shows the residual stress perpendicular to the weld line in relation to the section surface in the direction of each stiffener for a 6 mm thickness model.The observed residual stress distribution is typically characterized by a high tensile stress near the weld bead and a distribution of compressive stress as it moves away from the weld.

Comparison with Test Data
Paik and Yi [36] performed the experiment to obtained test database of the welding-induced residual stresses in a full scale prototype structure.It is concluded that the present finite element analysis model gives very good agreements with test database.

Finite Element Modelling for Predicting the Weld-Induced Distortions
In this section, the finite element model is presented to predict the weld-induced distortions.The thermal buckling analysis method is applied.The validation of the finite element model is made by a comparison with test database obtained from Paik and Yi [36].The MSC/MARC computer program [37] is used for computations in the present study.

Procedure of the Analysis
Figure 12 presents the procedure for the nonlinear finite element analysis to predict the weld-induced distortions comprising 3 steps [42].In step I, the welding FEA.

Transverse Direction for t p = 10mm
Transverse Direction for t p = 12mm World Journal of Engineering and Technology Figure 12.Procedure for the finite element analysis to predict the weld-induced distortions [42].
In step II, shrinkage forces are calculated in association with the weld-induced residual stresses of welding.In step III, thermal buckling analysis is performed to determine the weld-induced distortions.

Material Properties
The mechanical properties of material in Table 2 are used.The yield strength of both plating and stiffeners is 309 MPa.The elastic modulus and Poisson's ratio are 203 GPa and 0.3, respectively.The elastic-perfectly material model without strain-hardening effect is applied.

Thermal Loading and Boundary Conditions
For welding analysis to obtain initial irregularity in thermal buckling analysis, contact analysis is carried out using self-weight and spring elements connected on four vertexes.The spring node constrains all six degrees of freedom to pre-

End
Step Ⅱ. Calculating S.F. (Shrinkage Force) 1) Derived from developed empirical formulae (Regression of Q' vs. S.F.) World Journal of Engineering and Technology vent rigid body motion.In order to simulate the actual welding process situation, the planar state is analyzed to the plane and the contact analysis with the structural element is carried out.The contact friction uses a stick-slip model with excellent convergence.A two-bay (1/2 + 1 + 1/2) model both in the longitudinal and transverse directions is taken as the extent for the analysis as shown in Figure 13.The symmetry condition at all edges is then applied in association with structural continuity.
The thermal loads obtained from steps I and II indicated in Table 5 are applied to individual finite elements.Figure 13(a) shows the boundary conditions.
The imaginary welding temperature (T top and T bot ) loads indicated in Table      presents the computed results of the weld-induced distortions after welding at the plate center in the longitudinal direction.According to the analysis procedure shown in Figure 12, at first welding analysis for initial imperfection was performed.The initial imperfection is assumed to be the deformation that occurs due to welding, and then thermal buckling analysis is performed by applying the shrinkage force as the boundary condition to this model.It is observed that the deflection at the welding line, i.e., on the transverse stiffeners is zero and has the maximum values at the middle of plating between stiffeners.The magnitude of the initial deflection in a thick plate is smaller than that in a thin plate.

Comparison with Test Data
Paik and Yi [36] performed the experiment to obtained test database of the welding-induced distortions in a full scale prototype structure.Figure 16 compares the weld-induced distortions obtained from experiment as well as the computations.It is concluded that the computations are in very good agreement with the experimental results.

Conclusions
The objectives of the present study were to develop finite element modelling techniques to predict weld-induced residual stresses and weld-induced distortions in a stiffened plate structures.The developed techniques were validated using test database obtained from direct measurements from a full scale prototype stiffened plate structures.Based on the results obtained from this study, the following conclusions are drawn.
1) In terms of predicting the weld-induced residual stresses, the modelling of heat source is important.In the present study, a double ellipsoidal shape model was applied to describe the heat source distribution during welding.It was confirmed that the numerical computations applying the proposed model are in good agreement with test data.
2) The procedure for predicting the weld-induced distortions comprises three steps, namely the weld temperature analysis, the shrinkage force computations and the thermal buckling analysis.The proposed procedure was implemented into a commercial computer code.It was confirmed that the numerical computations are in good agreement with test data.
Ships and offshore structures are fabricated by welding and thus weld-induced M. S. Yi et al.DOI: 10.4236/wjet.2018.61010177 World Journal of Engineering and Technology initial imperfections in the form of initial distortions and residual stresses are unavoidable.It is required to predict the weld-induced initial imperfections in magnitude and pattern in association with structural design and construction.

Figure 3 .
Figure3.Definition of geometric parameters for the heat source distribution with a double-ellipsoidal shape[39].

Figure 4
Figure4shows a steel stiffened-plate structure which is extracted from living quarter structures of a very large crude oil carrier (VLCC) class floating, production, storage and offloading (FPSO) unit which is used for the production of oil in deep water.Typically, the longitudinal stiffener spacing (plate breadth) is in

Figure 7 .
Figure 7. Thermal loading and boundary conditions for a quarter model of the structure.

Figure 9 .Figure 10 .
Figure 9. Computed results of welded-induced residual stress.(a) Schematic of moving heat source in the second weld zone with t p = 6 mm.(b) Distribution of equivalent von Mises stresses after 2 nd welding with t p = 6 mm.

Figure 11 comparesFigure 11 .
Figure 11.Comparison between the experiment and the computations.(a) Comparison of residual stresses in the longitudinal direction; (b) Comparison of residual stresses in the transverse direction.
0] World Journal of Engineering and Technology

Figure 15 .
Figure 15.Computed results of the weld-induced distortions of initial imperfection (during welding) and thermal buckling analysis at plate center along the longitudinal direction.(a) Distortions of initial imperfection at the plate center in the longitudinal direction; (b) Distortions of thermal buckling analysis at plate center along the longitudinal direction.

Figure 16 .
Figure 16.Comparison of weld-induced distortions between the experiment and the computations.(a) Final deflection after welding for a plate thickness of t p = 6 mm.(b) Final deflection after welding for a plate thickness of t p = 8 mm.(c) Final deflection after welding for a plate thickness of t p = 10 mm.(d) Final deflection after welding for a plate thickness of t p = 12 mm.
Table 1 indicates the geometric properties of the structures where the
Note: L w indicates the weld bead length (leg length of welding).

b Longi. stiffeners Symmetry Domain of calculation Symmetry Trans. Stiffener Longi. Stiffener
fy World Journal of Engineering and Technology plate thickness is varied as 6, 8, 10 and 12 mm.

Table 2
[40]cates the mechanical properties of material at room temperature.During welding, the material properties greatly change with elevated temperatures as described in Figure 6[40].It is noted that the minimum requirement of the yield strength specified by classification societies is 235 MPa for mild steel which is used for construction of the living quarter structures, but the actual yield strength of 309 MPa is used for the finite element analysis in the present study.

Table 2 .
Mechanical properties of steel at room temperature used for the living quarter structures.
Note: E is the elastic modulus, σ Y is the yield strength, σ u is the ultimate tensile strength, and ν is the Poisson's ratio.

Table 3 .
Welding parameter for leg length.