Repair Weld Simulation of Austenitic Steel Pipe

Transcription

1 Repair Weld Simulation of Austenitic Steel Pipe BÉZI Zoltán 1, a *, SZÁVAI Szabolcs 1,b 1 Bay Zoltán Nonprofit Ltd., Institute for Logistics and Production Engineering, 2 Iglói Str., 3519 Miskolc, Hungary a zoltan.bezi@bayzoltan.hu, b szabolcs.szavai@bayzoltan.hu Keywords: austenitic pipe, repair weld, FEA, isotropic-kinematic model, residual stress Abstract. In this study the repair weld simulation of an austenitic steel pipe is performed to measure the residual stresses caused by the welding. The simulation consists of three work tasks. First the girth welding of the pipe is performed on simplified geometries to decrease the calculation time. The next work task is the simulation of the machining of the repair weld excavation, performed in one simulation step. The last task is the simulation of the repair welding. Residual stress measurements are performed on weld repair to provide validation of the simulation performed on the model. Introduction Repair welds are usually introduced into structures either to remedy initial fabrication defects found in welds by routine inspection, or to rectify in-service degradation of components and thereby extend the life and economic operation of ageing engineering plant. The structural integrity assessment and lifetime prediction for such welded structures require consideration of residual stresses. However, reliable characterization of residual stresses at nonstress-relieved welds is notoriously difficult. Development of more realistic residual stress profiles for structural assessment requires high quality experimental measurements coupled with an understanding of component structural behavior and non-linear modeling of the welding processes responsible [1]. This paper describes a series of residual stress measurements and simulation that were carried out on a stainless steel pipe girth weld of 35mm wall thickness and 180mm outside diameter with center repair. The measurement was compared to results from finite element (FE) weld simulations for these as-welded cases and for deep weld repair. In this study, the MSC.Marc Mentat finite element software was used throughout the investigation. Experimental procedure The material used in this study is Esshete 1250 pipe. The fabrication history of this mock-up (Fig 1.a) is complex, comprising: Rough-machining of pipe sections Solution heat treatment and water quenching Final machining of pipe sections and girth weld preparations Manufacture of pipe girth welds, weld cap dressing Machining of the repair excavations Repair welding, weld cap dressing. The girth welds were made using tungsten inert gas (TIG) process for the root pass and the first fill pass, and manual metal arc (MMA) method for the remaining passes. A total of 23 pass (Fig 2.a) were deposited for mock-up, including 3 capping passes. All the weld passes were deposited in one direction, i.e. increasing circumferential angle.

2 a, Mock-up after repair weld cap dressing b, Central repair welding Fig. 1 Completed mock-up A weaving technique was used for all passes, the width being determined by the joint width and whether more than one pass was required for a given weld layer. In the case of weld layers with multiple pass, including the weld cap, the final passes were deposited on the reference line side of the joint. Detailed process parameter records and bead logs were kept for use in subsequent simulation (Table 1.a). A representative girth weld is shown in Fig 2.a. a, Girth weld bevel b, Repair weld bevel Fig. 2 Weld bevels The repair welds were made using MMA for all 18 passes (Fig 2.b). Where any layer, including the weld cap, required more than one pass, then the final pass was deposited on the reference line side of the joint preparation. During the in-fill welding, a large number of short weld length runs were deposited in order to maintain a constant weld layer height. The intention was to position a central repair at the girth weld centerline. Detailed process parameter records and bead logs were kept for use in subsequent simulations (Table 1.b), and the mock-up was photographed after every repair weld pass. The mock-up was instrumented with thermocouple arrays to record the transient temperature history during welding. The welding and the related mechanical testing were performed at EDF Energy [2].

3 Table 1 Welding parameters a, Girth welding parameters b, Repair welding parameters Finite element analysis The analysis is based on MSC.Marc code, a thermal elastic plastic finite element computational procedure to simulate the welding temperature field and the welding residual stress in medium thick-walled Esshete 1250 pipe. The thermo-mechanical behavior is calculated using a coupled formulation. The welding residual stress and displacement field from the girth welding model is mapped on to the FE-mesh for performing the excavation model and the repair welding thermomechanical analysis. During the welding process, besides the elastic, plastic and thermal strains, the strains due to solid-state phase transformation and creep potentially give some contributions to the total strain. Because Esshete 1250 stainless steel has no solid-state phase transformation during cooling and the heating time is relatively short, it can be expected that the strains due to phase transformation and creep can be neglected in the present simulation. The elastic behavior is modeled using the isotropic Hooke s rule with temperature-dependent Young s modulus. The thermal strain is considered using thermal expansion coefficient. The yield criterion is the Von Mises yield surface. In the present model, the strain hardening is taken into account using the Chaboche s combined hardening law. The Chaboche combined hardening model in MSC.Marc requires at least five parameters (c, y, Q, b, σ y ) which is an acceptable number to be determined from experimental stress vs. strain curves. Using these parameters, the model provides an adequate description of the real elasto-plastic material behavior. The parameters for the Chaboche mixed hardening model implemented in MSC. Marc was derived by EDF Energy (Fig. 3) [2]. All free surfaces of all FE-models are given a convective heat loss with a heat transfer coefficient, h=20w/mk and a radiation heat loss using an emissivity coefficient, ε=0.4. Inactive elements have been activated initially to simulate the addition of filler material. The thermal and mechanical activation of the elements are separated [3]. The criterion for thermal activation is that an element should be inside the volume of the heat source. Mechanical activation of an element is achieved when the temperature in the element has dropped below a threshold value. The chosen threshold value is 1400 C. The heat input model in this work is an elliptic cone. It is very similar to the double ellipsoid presented by Goldak et al, but it has a linear decay of the energy intensity through the thickness. The heat source distribution combines two different ellipses, i.e. one in the front quadrant of the heat source and the other in the rear quadrant [3][4].

4 a, Thermal and mechanical properties b, Chaboche parameters Fig. 3 Material properties During the analysis, a full Newton Raphson iterative solution technique with direct sparse matrix solver is employed for obtaining a solution. During the thermal analysis, the temperature and the temperature-dependent material properties change very rapidly. Thus it is believed that, a full Newton Raphson technique using modified material properties gives more accurate results [5]. The FE-model for the girth welding simulation contains eight noded brick elements and nodes. a, Girth weld model b, Weld passes Fig. 4 Finite element meshing and weld passes of the girth weld model For excavation and repair weld simulation, the FE models are created by 8 nodes hexagonal and 4 nodes tetrahedron elements. Machining of the repair weld excavation, element number is 37118, node number is For repair weld, element number is 68055, node number is The pipe is modeled as simply supported, during both the welding sequences and the cooling sequences. Due to anticipated high temperature and stress gradients near the weld, a relatively fine mesh is used there. Element sizes increase progressively with distance from the weld centre line. The same mesh as used in the repair welding simulation is used in the excavation simulation. See Fig. 4 and Fig 5.

5 a, Excavation and reapair model b, Repair weld passes Fig. 5 Finite element meshing of the excavation and repair model Initial condition mapping tool for moving data between two finite element models is used to map residual stresses fields between the girth weld and the excavation/repair welding analysis. The von Mises stress field before and after the repair welding procedure is shown in Fig. 6. a, Residual stress distribution after girth welding and machining Fig. 6 Residual stress distributions b, Residual stress distribution after repair welding The recorded temperature during the welding experiment together with the computed temperature shows two different passes in Fig. 7. The location of the thermo couple can be seen in Fig. 1.b. Fig. 7 Temperature cycles during welding

6 Fig. 8 compares the predicted and measured through-wall distributions of weld transverse and hoop stress at the centre of the repair. The actual distributions and the stress distributions are linearised to emphasis their membrane and through-wall bending components. The simulations predict a range in membrane and through-wall bending components achieving good agreement. Summary a, Axial stress b, Hoop stress Fig. 8 Residual stresses A 3D finite element model that takes the moving heat source into consideration is used to investigate welding residual stress distributions in a girth and repaired welded austenitic pipe. Meanwhile, an emphasis is focused on examining the welding residual stresses center of the repair weld region, and the simulation results are compared with the measured data. Three-dimensional FE analysis is essential to accurately predict the axial and hoop residual stresses in repair welds of girth welds pipes which change spatially due to the traveling arc and welding start-stop effects. During the repair welding of the austenitic pipe, large and non-uniform residual stresses are generated in the repair weld and HAZ, which may have a great effect on structure integrity of the repair structure. The residual stress simulation shows that accurate predictions of residual stresses in conventional austenitic weld repairs can readily be achieved if appropriate mixed isotropickinematic material hardening is used. Acknowledgement The publication is supported by the TÁMOP A-11/1/KONV project. The project is co-financed by the European Union and the European Social Fund. References [1] P.J. Bouchard, D. George, J.R. Santisteban, G. Bruno, M. Dutta, L. Edwards, E. Kingston, D.J. Smith, Measurement of the residual stresses in a stainless steel pipe girth weld containing long and short repairs, International Journal of Pressure Vessels and Piping 82 (2005) [2] STYLE Deliverable report D-2.2.1: Weld Residual Stress Simulation, 2014 [3] Zhibo Dong, Yanhong Wei, Yanli Xu, Predicting weld solidification cracks in multipass welds of SUS310 stainless steel, Computational Materials Science 38 (2006) [4] M. Fisk, A. Lundback, Simulation and validation of repair welding and heat treatment of an alloy 718 plate, Finite Elements in Analysis and Design 58 (2012) 1-73 [5] MSC.Marc Theory and User Information