Scholarly article on topic 'Welding Process Simulation Model for Temperature and Residual Stress Analysis'

Welding Process Simulation Model for Temperature and Residual Stress Analysis Academic research paper on "Materials engineering"

CC BY-NC-ND
0
0
Share paper
Academic journal
Procedia Materials Science
OECD Field of science
Keywords
{"TIG welding" / "heat flux" / FEA / "transient temperature" / "residual stress."}

Abstract of research paper on Materials engineering, author of scientific article — Harinadh Vemanaboina, Suresh Akella, Ramesh Kumar Buddu

Abstract Welding is widely used in all the fabrication processes for the development of structural components. An accurate and physically suitable heat flux simulation model is to be given as input for analysis of welding processes. The outcome of the heat input is structural deformation and residual stress formation. The temperature and residual stress modelling is one of the complex process which utilise the weld parameters and material properties at higher temperatures. A representation of heat flux model is developed using heat source with constant and uniformly applied condition. Present work is done with cylindrical heat flux model further a realistic model is possible by combining present with other heat flux models, such as Gaussian. The temperature distribution and stress analysis has been carried out with developed model by using the temperature dependent material properties for Stainless steel SS304. This work can be used for selecting process parameters for reducing structural distortion and residual stresses by simulation process. In this paper temperature and residual stresses are discussed.

Academic research paper on topic "Welding Process Simulation Model for Temperature and Residual Stress Analysis"

Available online at www.sciencedirect.com

ScienceDirect PrOCSd ¡0

Materials Science

ELSEVIER Procedia Materials Science 6 (2014) 1539 - 1546

www.elsevier.com/locate/procedia

3rd International Conference on Materials Processing and Characterisation (ICMPC 2014)

Welding Process Simulation Model For Temperature and Residual

Stress Analysis

Harinadh Vemanaboina1* , Suresh Akella1 and Ramesh Kumar Buddu2

1Sreyas Institute of Engineering & Technology, Nagole, Hyderabad-500068, India 2Institute for Plasma Research, Bhat, Gandhinagar-382428, Gujarat, India

Abstract

Welding is widely used in all the fabrication processes for the development of structural components. An accurate and physically suitable heat flux simulation model is to be given as input for analysis of welding processes. The outcome of the heat input is structural deformation and residual stress formation. The temperature and residual stress modelling is one of the complex process which utilise the weld parameters and material properties at higher temperatures. A representation of heat flux model is developed using heat source with constant and uniformly applied condition. Present work is done with cylindrical heat flux model further a realistic model is possible by combining present with other heat flux models, such as Gaussian. The temperature distribution and stress analysis has been carried out with developed model by using the temperature dependent material properties for Stainless steel SS304. This work can be used for selecting process parameters for reducing structural distortion and residual stresses by simulation process. In this paper temperature and residual stresses are discussed.

© 2014ElsevierLtd. This is an openaccessarticleunder the CC BY-NC-ND license (http://creativecommons.Org/licenses/by-nc-nd/3.0/).

Selection and peer review under responsibility of the Gokaraju Rangaraju Institute of Engineering and Technology (GRIET) Keywords: TIG welding, heat flux, FEA, transient temperature, residual stress.

CrossMari

1. Introduction

Welding is a process used in the fabrication of various steel structures for applications from thin sections to thicker sections in various applications like pressure vessels, chemical plants and nuclear reactors. The main problem associated with welding is the presence of residual stresses and deformations developed within the sections

* Corresponding author. Tel.: +91-900-062-3602; fax: 040-2422-7744. E-mail address:harinadh. vh@gmail.com

2211-8128 © 2014 Elsevier Ltd. This is an open access article under the CC BY-NC-ND license (http://creativecommons.org/licenses/by-nc-nd/3.0/).

Selection and peer review under responsibility of the Gokaraju Rangaraju Institute of Engineering and Technology (GRIET) doi:10.1016/j.mspro.2014.07.135

which may cause the failure at the later stages by Masubuchi (1980). During welding process the material exposed with heat flux causes phase change of the metal during melting. The temperature distribution is non uniform like fusion zone with molten metal, heat affected zone and the base metal zone. The molten weld pool movement causes thermal gradients within the material which enhances the residual stresses and deformations within the structure were well addressed by Goldak et.al (1984) and Deng et.al (2008). The heat flux and heat flow conditions are mainly governed by the welding source type mechanism and materials properties at higher temperatures. In welding processes like arc welding with Tungsten Inert gas (TIG) or beam weld processes like Laser beam welding, the estimation of residual stresses is complex due to the various associated entities like thermal gradients due to the coupling mechanism of heat flow, solidification and cooling rate. Approximate analytical calculations of the weld residual stresses and understanding the key influential parameters have been carried out by Akbari et.al (2008), Taljat et.al (1998) and Webster et.al (2002). The heat source is modeled by using the ellipsoidal source approach for arc welding process and Gaussian models for the beam welding process by various researchers. Even though experimental measurements of the weld residual stress are widely applied by researchers, the complete understanding of the cause parameters is complex due to the weld parameters disparity. Analytical approach and modeling are helpful to have clear understanding with the process associated in the welding process for the temperature behavior and stress conditions which are key responsible parameters for the structural deformations as performed by Zhang et.al (2004), Dike et.al (1999) and Shan et.al (2009). The approach used with heat flow within the material and flux distribution is essential considerations for the thermal gradients caused within the weld process in similar to Mollicone et.al (2006). The load is vectorized so that it can be used in analytical FEM analysis or it can be used in FEA packages such as ANSYS or ABAQUS. The present study is focused on the understanding of the heat flux mechanism with heat source used for TIG weld process with developed constant heat source model applied onto the stainless steel, SS304 material by using the temperature dependent properties and finite element approach. The temperature fields at various locations within the weld pool and around the pool geometry (heat affected zone) and base metal condition are analyzed by finite element transient thermal approach. The temperature distribution is estimated which can further give the estimation of the weld deformations and stresses.

2. Formation & simulation of welding process

The heat energy equations are referenced in many including Frewin et.al.(2009). For a isotropic, conductive material with equal coefficient of conductivity kx, ky, kz (W/mK) in all three chosen orthogonal co-ordinates. Equation (1) gives the heat energy in the weld area with temperature, T (K) obtained both in spatial, x, y, z (m) and temporal, t (sec), terms. Q (W/m3 or J/m3s) is the net heat from input and the losses in the form of convection & radiation. Density, p, kg/m3, specific heat capacity, c, give the right hand terms of how much heat is retained with respect to time in the material and how much is taken away with the velocity of welding, v (m/s).The boundary conditions given are T0(x, y, z, 0) throughout the body at time zero or at the starting of the weld, this is an essential boundary condition. In addition the natural boundary conditions have to applied consisting of normal conduction Kn heat

__ryi *4n on

flux q, convection h (T-T0), and the radiation term, OS (T — T0 )

. S2t S2T S2T r«r <m

kx^rx+ky^ry + kz^rz + Q = pc[--v-\ (1)

Together, the boundary conditions are summed up as:

Kn - q + h(T -T0) + os(T4 - T04) = 0 (2)

When symmetric boundary and insulation boundaries are considered as adiabatic, with no heat flowing through the surface, they are obtained by making convection zero, and conduction zero from the surface. Where, Kn is the thermal conductivity normal to the surface in W/mK, h is the convective heat transfer coefficient in W/m2K, e is emissivity of surface radiating, a is the Stefan Boltzmann's constant, which 5.67*10-8, W/m2K4. When it is difficult to use radiation boundary condition, it is combined to convective heat flux by using a modified coefficient, hr, for hot rolled steel plates with an error of about 5% is,

hr = 2.4 * 10"3 £ T1-61 (3)

Radiation inclusion will increase solution time by about three times and hence combined with convection.

2.1 Finite element for simulation

The heat equations (1) can be represented in tensor form so the elemental transient heat equation is obtained and later summed to get the system equation which is analysed with time.

[K(T)m + [C(r)]{rj = {Q(T)} (4)

Where K is a temperature dependent conductivity matrix. C is the temperature dependent capacitance matrix based on specific heat it's product with rate of temperature gives heat. The above equation can be solved numerically, with standard FEM models with Crank Nicholson or Euler time integration models. An initial temperature Tt is assumed K, C and Q are calculated at that temperature and the next temperature T at i+1 is obtained. Again K, C & Q are calculated and temperature at next temperature interval is calculated. The iteration is continued for convergence of temperature or heat flux values. This is a procedure for transient finite element analysis. In the present study the work is done using Ansys.

Assumptions

• Thermal properties, i.e. conductivity, specific heat, density are temperature dependent.

• A combined convection and radiation boundary condition is used on the remaining of the top surface. Heat flux of constant used for fusion welding.

2.2 Finite element model

The finite element model of dimensions 40mm X 150 mm X 10 mm is used. The AISI 304 austenitic stainless steel material is considered for simulations to be carried out. The convection is applied on all the surface of the plate except on the heat applied area. In the present study AISI type 304 stainless steel is used as it is having many advantages such as low thermal conductivity, high resistance of corrosion and high stability at elevated temperatures. Thus SS304 material is widely used in numerous industries, like nuclear industry, chemical plants, aeronautical and specialized pipe industry. It has excellent forming and welding characteristics. The properties of a typical stainless steel sheet are given in Table 1 as per given by Amudala et.al (2012). The temperature dependent thermal properties for AISI 304 stainless steel material are given in Table 2.

Table 1. Mechanical properties of AISI 304 Steel

Tensile strength Yield strength Density Melting point Thermal conductivity % elongation

515 MPa 205 MPa 8000 kg/m3 1400-1450oc 16.2 W/mo K at 100oc 20-40

Table 2. Temperature dependent thermal properties for AISI 304 Austenitic stainless steels.

S.no Temp (K) Thermal conductivity, W/m o K Density, Kg/m3 Specific heat, J/Kg K

1 200 11 8200 350

2 400 15.5 8000 400

3 600 19 7800 440

4 800 22.5 7600 550

5 1000 26 7500 590

6 1200 30 7400 610

7 1400 34.5 7350 640

8 1600 39.5 7300 680

9 1800 44 7200 720

10 2000 47 7200 760

3. Thermal Analysis

The thermal analysis has been carried out with constant heat flux, where the thermal load is applied at a time on the weld area. After the welding processes is completed, the thermal load step is progressively increased up to time=1000 sec to allow the plate to cool down to ambient temperature. In the present work Finite Element Analysis of single-pass butt-welding has been carried out with constant heat flux. For this, a simple Butt-joint welding whose welding parameters are consistent to those of Friedman's model with heat input Q = 1200 W is considered and has been simulated using ANSYS. The present thermal Ansys is conducted using element type SOLID70. This element type has a three-dimensional thermal conduction capability and eight nodes with single degree freedom (temperature) at each node.

Fig 1(a) Geometry of the model Fig 1(b) Mesh model used for analysis

The element is applicable for three dimensional, steady-state or transient thermal analysis. The element can also compensate for mass transport heat flow from a constant velocity field. In this analysis, element SOLID70 is replaced with by a three-dimensional (3-D) structural element SOLID45. The element is defined by eight nodes having three degrees of freedom at each node (translations in the nodal x, y and z directions). The element has plasticity, creep, swelling, stress stiffening, large deflection, and large strain capabilities ANSYS. The geometry and meshed model with tetrahedral shape with volume mesh of size 0.02 were shown in Fig 1(a) and Fig 1(b).

4. Results & Discussion

4.1 Thermal analysis

The temperature distribution was evaluated at various zones i.e. fusion zone, heat affected zone and base plate. The temperature distributions of the weldments are shown in Figs 2 to 4. The 3D temperature distribution is shown in Fig. 2. At time t=0, the weld starts with all the constant heat Q, given as input on the surface of weld region. Fig 2 illustrate the nodal temperature of weldment at time t =15 sec. In Fig.3 show the temperature measurement is study in various zones of the model and to understand the distribution. Fig 3. Shows the temperature versus time distribution graphs in the three regions of Fusion zones, Heat Affected zones & Base plate. The temperature is found to vary from 303 0 K in Base plate and up to 2570 0 K in the fusion zone with the applied heat input parameters in the developed model. Fig 4 shows the temperature distribution in the transverse direction on the surface of the weldment. As the geometry, heat flux & boundary conditions are symmetrically distributed the temperature is also found to be symmetric. It appears like a lecto Kurtic distribution hence the properties of lecto Kurtic normal distribution, of maxima apply where the temperature is more centrally located.

Fig 2. Nodal solution of the plate

Fig 3. Temperature distribution perpendicular to welding direction of the weldment at time=15 sec

0 1.662 3.364 5.M6 6.72S 8.405

,641 2.553 4.206 5.SS7 7.569

Distance (ra)

Fig 4. Temperature distribution in transverse direction

4.2 Residual stresses

The estimate of residual stresses is analyzed in all the regions. Due to the variance in the temperature gradient, the material properties are given in the model for elevated temperatures. A stress acting normal to the direction of weld bead is known as a transverse residual stress. The stresses distributions are shown in the Fig.5 to 7. The temperature near the weld bead and heat affected zone rapidly changes with distance from the heat source. Transverse stress distribution over the plate area of heat input is shown in Fig .5, which shows more stress value in the weld bead area and gradually decreases from center line to the base plate end. It shows a symmetric distribution as similar way seen in temperature profile. The maximum stress value is about 76.90 MPa. The longitudinal stresses along weld bead are about 60 MPa with some peaks at the edges because of boundary conditions. The stress variation along the length in the base plate is about 15 MPa. This is also constant, except for the difference at the edges. The value is less as the temperature at the base plate is less.

Fig 5. Stress in Transverse weld, X-direction of weldment.

1® -¡m-.«SB gm. _Distaiige frn)

Fig 6. Stress in Longitudinal, Y-axis to weld direction in fusion zone.

The transient thermal analysis was useful to have the estimation of the stress distribution with the given heat in terms of weld process parameters. This process simulation can be used to get the approximate idea for the weld structure level of stress prior to the fabrication process with appropriate het flux input parameters.

B .;B3l 386 M .12 .IS

.-8® «a : ass .ass Dîstâriiïé gif

Fig 7. Stress in length along Y-direction of weldment.

5. Conclusion

FEM simulation by adapting a constant heat flux analysis has been carried out on SS 304 steel material for the transient thermal temperature and residual stress analysis. The temperature field at the weld zone was found higher at the given constant heat flux input when compared with the heat affected zone and base plate regions. The stress analysis indicates as residual stress values of higher level at fusion zone are noticed compared to HAZ and Base metal it tends to lower in transverse and along the weld bead. This prediction of analysis with reference to the estimation of stress can be useful to predict the weld residual stress status with the heat input parameters which can be used for experimental application.

Acknowledgements

The authors acknowledge the support from The Board of Research for Fusion Science and Technology (BRFST)

for sanctioning the grant NFP-MAT-A11-02, for creating simulation studies on welding processes for SS material

under National Fusion Programme.

References

Akbari Mousavi. S.A.A, R. Miresmaeili., 2008. Experimental and numerical analyses of residual stress distributions in TIG welding process for 304L stainless steel, Journal of materials processing technology, 208, 383-394.

Amudala Nata Sekhar Babu, et.al. 2012. Finite Element Simulation of Hybrid Welding Process for Welding 304 Austenitic Stainless Steel Plate, IJRET Vol 1, Issue 3, 101-410.

Dean Deng, Hidekazu Murakawa. 2008. "Prediction of welding distortion and residual stress in a thin plate butt-welded joint" Computational Material Science 3,353-365.

Dike.J.J, A.R Ortega and C.H. Cadden, .1999. Finite element modelling and validation of residual stresses in 304L girth welds, in Trends in Welding Research, 5th International Conference, ASM International, Materials Park, Ohio, pp.961-966.

Frewin m r, scott d a, "finite element model of pulsed laser welding", welding j, 1999, 15s - 22s

Goldak.J.A, B. Chakravarti and M. J. Bibby. 1984. A new finite element model for welding heat sources, Metallurgical Transactions B, 15, 229-305.

Masubuchi.K, .1980Aftalysis of Welded Structures. Oxford, Pergamon Press.

Mollicone.P, et al,.2006. Simple thermo-elastic-plastic models for welding distortion simulation. Journal of Material Processing Technology, 176, 77 - 86.

Shan.X, C.M. Davies, T. Wangsdan , N.P. O'Dowd, K.M. Nikbin,.2009. Thermo-mechanical modelling of a single-bead-on-plate element Method, International Journal of Pressure Vessels and Piping 86, 110-121

Taljat.B, B. Radhakrishnan, T. Zacharia, 1998. Numerical analysis of GTA welding process with emphasis on post-solidification phase Transformation effects on residual stresses, Materials Science and Engineering A246 45-54

Webster. P.J. et al, 2002.Measurement and modeling of residual stresses in a TIG weld, Appl. Phys. A 74[ suppl ]. S1421-S1423.

Zhang W, Kim C-H and DebRoy T,.2004. Heat and fluid flow in complex joints during gas metal arc welding: I. Numerical model of fillet Welding J. Appl. Phys. 95 5210-9.