Subscribe Now Subscribe Today
Research Article

Investigation and Analysis of Weld Induced Residual Stresses in Two Dissimilar Pipes by Finite Element Modeling

S. Nadimi, R.J. Khoushehmehr, B. Rohani and A. Mostafapour
Facebook Twitter Digg Reddit Linkedin StumbleUpon E-mail

In the present study, Manual Metal Arc Welding (MMAW) of austenitic stainless steel to carbon steel were studied. The Schaeffler diagram were used in determining suitable filler metal for this process and then the finite element analysis of residual stresses in butt welding of two dissimilar pipes is performed with the commercial software ANSYS, which includes moving heat source, material deposit, temperature dependant material properties, metal plasticity and elasticity, transient heat transfer and mechanical analysis. The residual stresses distribution and magnitude in the hoop and axial directions in the inner and outer surfaces of two dissimilar pipes were obtained. Welding simulation considered as a sequentially coupled thermo-mechanical analysis and the element birth and death technique was employed for simulation of filler metal deposition.

Related Articles in ASCI
Similar Articles in this Journal
Search in Google Scholar
View Citation
Report Citation

  How to cite this article:

S. Nadimi, R.J. Khoushehmehr, B. Rohani and A. Mostafapour, 2008. Investigation and Analysis of Weld Induced Residual Stresses in Two Dissimilar Pipes by Finite Element Modeling. Journal of Applied Sciences, 8: 1014-1020.

DOI: 10.3923/jas.2008.1014.1020



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 of pipes.

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 al.

(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.


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):

Fig. 1a: The microstructure of weld metal without filler wire

Fig. 1b: 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 for cracking.

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.

Fig. 2: 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.

Fig. 3a: Comparison of FEM with experimental results for axial residual stresses

Fig. 3b: 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.

Fig. 4: Geometry and finite element model used in this study

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.

Fig. 5a: Temperature distribution at t = 5 sec

Fig. 5b: 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 steel one.

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., 2000).

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).

Table 1: Temperature dependent thermal, physical and mechanical properties of 304 L austenitic stainless steel

Table 2: Temperature dependent thermal, physical and mechanical properties of 309 L filler wire

Table 3: Temperature dependent thermal, physical and mechanical properties of ASTM A36 carbon steel

Fig. 6a: Hoop residual stresses in outer surface

Fig. 6b: Axial residual stresses in outer surface


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.

Fig. 6c: Hoop residual stresses in inner surface

Fig. 6d: 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.
1:  Abid, M. and M. Siddique, 2005. Numerical simulation to study the effect of tack welds and root gap on welding deformations and residual stresses of a pipe-flange joint. Int. J. Pressure Vessels Pip., 82: 860-871.
Direct Link  |  

2:  Bonifaz, E.A., 2000. Finite element analysis of heat flow in single-pass arc welds. Weld. Res. Supplement, pp: 121-125.

3:  Chao, Y. and X. Qi, 2000. Advances in Computational and Engineering Science. Vol. 2, Tech Science Press: Paledale, USA., pp: 1206-1211.

4:  Deng, D. and H. Murakawa, 2006. Numerical simulation of temperature field and residual stresses in multi-pass welds in stainless steel pipe and comparison with experimental measurements. Comput. Mater. Sci., 37: 269-277.
Direct Link  |  

5:  Dubois, D., J. Devaux and J.B. Leblond, 1984. Numerical simulation of a welding operation: Calculation of residual stresses and hydrogen diffusion. Proceedings of the ASME 5th International Conference on Pressure Vessel Technology, Materials and Manufacturing, II, September 1984, San Francisco, CA., USA., pp: 1210-1238.

6:  Fricke, S., E. Keim and J. Schmidt, 2001. Numerical weld modeling: A method for calculating weld-induced residual stresses Nucl. Eng. Des., 206: 139-150.
CrossRef  |  Direct Link  |  

7:  Chang, P.H. and T.L. Teng, 2004. Numerical and experimental investigations on the residual stresses of the butt-welded joints. Comput. Mater. Sci., 29: 511-522.
CrossRef  |  Direct Link  |  

8:  Josefson, B.L., 1993. Prediction of residual stresses and distortions in welded structures. ASME. J. Offshore Mech. Arct. Eng., 115: 52-57.
CrossRef  |  Direct Link  |  

9:  Junek, L., M. Slovacek, V. Magula and V. Ochodek, 1999. Residual stress simulation incorporating weld HAZ microstructure. ASME. PVP-Fracture, Fatigue Weld Residual Stress, 393: 179-192.

10:  Karlsson, R.I. and B.L. Josefson, 1990. Three-dimensional finite element analysis of temperatures and stresses in a single-pass butt-welded pipe. ASME. J. Pressure Vessel Technol., 112: 76-84.
CrossRef  |  Direct Link  |  

11:  Kou, S., 2003. Welding Metallurgy. 1st Edn., John Wiley and Sons, Hobokon, New Jersey, ISBN: 0-471-43491-4, pp: 480.

12:  Lindgren, L.E. and L. Karlsson, 1998. Deformations and stresses in welding of shell structures. Int. J. Numer. Methods Eng., 25: 635-655.
CrossRef  |  Direct Link  |  

13:  Masubuchi, K., 1980. Analysis of Welded Structures. 1st Edn., Pergamon Press, New York, pp: 600.

14:  Murthy, Y.V.L.N., G.V. Rao and P.K. Iyer, 1996. Numerical simulation of welding and quenching processes using transient thermal and thermo-elasto-plastic formulations. Comput. Struct., 60: 131-154.
CrossRef  |  Direct Link  |  

15:  Price, J.W.H., A. Paradowska, S. Joshi and T. Finlayson, 2006. Residual stresses measurement by neutron diffraction and theoretical estimation in a single weld bead. Int. J. Pressure Vessels Pip., 83: 381-387.
Direct Link  |  

16:  Sarkani, S., V. Tritchkov and G. Michaelov, 2000. An efficient approach for computing residual stresses in welded joints. Finite Elements Anal. Des., 35: 247-268.
Direct Link  |  

17:  Sedek, P., J. Brozda, L. Wang and P.J. Withers, 2003. Residual stress relief in MAG welded joints of dissimilar steels. Int. J. Pressure Vessels Pip., 80: 705-713.
Direct Link  |  

18:  Sun, Z. and R. Karppi, 1996. Application of electron beam welding for the joining of dissimilar metals: An overview. J. Mater. Process. Technol., 59: 257-267.
CrossRef  |  Direct Link  |  

19:  Teng, T.L. and P.H. Chang, 1998. Three-dimensional thermomechanical analysis of circumferentially welded thin-walled pipes. Int. J. Pressure Vessels Pip., 75: 237-247.
CrossRef  |  Direct Link  |  

20:  Teng, T.L., P.H. Chang and H.C. Ko, 2000. Finite element analysis of circular patch welds. Int. J. Pressure Vessels Pip., 77: 643-650.
CrossRef  |  Direct Link  |  

21:  Zhu, X.K. and Y.J. Chao, 2002. Effects of temperature-dependent material properties on welding simulation. Comput. Struct., 80: 967-976.
Direct Link  |  

©  2021 Science Alert. All Rights Reserved