Simulation of welding using MSC.Marc. Paper reference number:

Simulation of welding using MSC.Marc Paper reference number: 2001-29 Tor Morten Olsen 1, Henrik Runnemalm 1 and Daniel Berglund 1, 2 1 Volvo Aero Corporation, Trollhettan, Sweden Tor-morten.olsen@volvo.com +46 (0) 520 94202 Henrik.runnemalm@volvo.com +46 (0) 520 94414 2 Luleaa University of Technology, Luleaa, Sweden Daniel.berglund@volvo.com +46 (0) 520 94528 Abstract Simulation of welding requires the user to select between 2D, 3D shell and 3D solid models in different situations. An investigation regarding capability of MSC.Marc in simulation of welding is presented. The investigation focuses on differences between 3D shell- and 3D solid-models.

INTRODUCTION It is desirable to control and govern the residual deformations and stresses, which are generated in the component via different manufacturing process, in this case welding. Predictability of a component s response to the heat input from welding is important when manufacturing high precision components. Today, mainly experimental tests are used to determine the material response caused by different welding methods and parameters. Due to the high pricing on aerospace components, these tests are expensive. One way to workaround these costly tests would be to utilise simulation tools by means of the Finite Element Method (FEM). FEM has proven to be a versatile tool for predicting a component s response to various thermal and mechanical loads. FEM also offers the possibility to examine different aspects of the manufacturing process without having a physical prototype of the product. It is widely used for structural analyses, but due to lack of high temperature material data and sufficient computational power, it is not commonplace to apply FEM to manufacturing processes. The nonlinear nature of manufacturing processes makes the simulation both time consuming and a sophisticated challenge for the engineers. FEM applied on welding has been performed since the early seventies, [ref. 1] The work done in this paper is an extension on previous related work at Volvo Aero Corporation [ref. 2, 3]. The material response, in terms of deformations, during the welding simulation for the shell model and the solid model are presented. The aspect of choosing either a shell or solid model is discussed with respect to simulation accuracy. PROBLEM DEFINITION Two 3mm thick plates made of Inconel 718 were to be welded together. The hatched areas in Figure 1 represent a clamping device which prescribes the boundary conditions of the FE model with no mechanical degrees of freedom. The rest of the plate is unconstrained. Welding direction is left to right and the weld path is identical to the line of symmetry. Protecting gas swept the backface of the weldseam. Process parameters are described in Figure 2 and Table 1. After cooling, the plates were released from the fixturing device and the residual shrink at distance ab, ac and cd were measured for both the shell and the solid model. Shrink is defined as difference before and after welding in deformation between two geometrical points. Table 1 Process parameters that governs heat input to plates Parameter description Value The "a" value of the ellipse, Figure 2 5.4 [mm] The "b" value of the ellipse, Figure 2 3.0 [mm] The "c-front" value of the ellipse, Figure 2 3.0 [mm] The "c-rear" value of the ellipse, Figure 2 4.0 [mm] The velocity of the arc 2.17 [mm/s] Nominal effect from welding machine (P = U I) 735 [W]

150 30 Clamped 20 a 15 b c d 15 Clamped 15 15 Figure 1 Geometry of plates, boundary conditions and measurement points Flux q Figure 2 The shape of the double elliptic heat source. ANALYSIS Analyse input The solid model was made up of 8-noded hexagonal elements, whereas the shell model had 4- noded thick shell elements, MSC.Marc element type number 4 and 75, respectively, [ref. 5]. The solid elements utilised the constant dilatation element formulation. Simulation using the assumed strain formulation was also compared with the standard formulation for solid elements. To introduce the moving heatsource to the analysis, an in-house developed user subroutine is utilised. This allows the weldtorch to be simulated as a moving double ellipsoidal heat source,

first described by Goldak et al. [ref. 4]. The doubleellipsoid is defined in Figure 2 and Table 1. The weld path is generated separately in the CAD software I-DEAS. The thermomechanical analysis was performed using the so-called staggered approach. This means that solution of the thermal matrix is done using the geometry matrix of last converged mechanical increment. The error introduced by letting the geometry of the thermal solution lag one step after the mechanical solution is neglectable, as the timesteps in welding analysis are small, often in the order of 10-2 s to 1 10-1 s. The heat flux is inserted at every integration point that is encircled by the ellipsoid at each increment. The energy is applied to the shells as a face flux and as volumetric flux to the solids. When performing the analysis with shell structures, the joining of material is done by activating links as the heatsource moves along the weldpath. Joining of material in the solid model is done by first deactivating elements along the weldpath, then revive these elements as the heatsource encounters them. Another feature is that stresses and strains are to be reset to zero when the material reaches the melting temperature. In the present analyses this was only implemented for the solid elements. For shells then, the stresses from material expansion will therefore impact the remainder of the analysis. Figure 3 shows how stresses differ in solid and shell model as temperatures exceed T melt at some instant during welding. 700 600 500 [MPa] 400 300 Solid model Shell model 200 100 0-20 -15-10 -5 0 5 10 15 20 [mm] Figure 3 Distance from centre of weldpool (x=0) vs. Von Mises stress Large deformation and large plastic strains were accounted for and the additive decomposition of elastic, plastic and thermal strain contributions was utilized for the stress recovery process. The analysis ran using a regular elasto-plastic material model with von Mises yield criteria. The material data included mechanical properties, specific heat and conductivity as functions of temperature. The density is only given as a value at room temperature. The staggered approach will automatically force the FE code to account for density variation as the temperature changes in the material. The thermal conductivity was increased by a magnitude of 10 when T T melt. This accounts for stirring of the liquid weldpool. T melt is set to1570k. For the shell analysis, equal heat input to top and backface was implemented. This gives a constant temperature through thickness. To minimize the errors of introducing constant temperature through the thickness and to account for the protecting gas at the backface, an increased convection was applied on the backface.

Analyse results Simulation of welding is in many respects time consuming. The time spent in modelling is usually more time consuming than the actual runtime. However, in parametric studies the time of a run is essential. The analyses presented in this paper has been run on a SUN Ultra 60 450 MHz workstation. The runtimes for each analysis can be seen in Table 2. The assumed strain and the constant dilatation approach gave the same results for this specific case, but the assumed strain formulation increased the computational demands drastically. Table 2 Solids vs. shells, computational demands Solid model Shell model # elements 12012 480 # nodes 15400 558 nodes dofs 46200 3348 # increments 763 977 # layers NA 11 # solution time ~ 3 days, 15 hours (two proc.) ~ 5 days, 8 hours (two proc. & ass. strain) 2 hours 45 minutes The application of an increased convection induced bending components that forces the shell plate into the preferred displacement mode. The heat input to the solid model corresponds to the elliptic model. Figure 4 shows the temperature contour lines of a small part of the weldseam in the solid model as the torch passes it. Figure 4 Contour lines of temperature distribution [K] in weld seam. Displacement enlarged five times The actual welding of the plates takes 70 seconds. Figure 5 shows the heat absorbed by the plates at an arbitrarily chosen interval between t=35s and t=40s. Figure 5 clearly shows a cyclic flux going into the shell model. This cyclic behaviour arises since the double ellipsoid encircles a varying number of integration points where heat can flow into the structure. The cycle spans 2,4seconds, in which the center of the heatsource travels approximately one element length. At instants t=35s, t=37,4s and t=39,8s the ellipsoid encounters only two integration points that

receives noticeable energy. The average flux input to shell model between t=35s and t=40s is 440W while the solid model receives 650W. The cyclic variation of the flux into the shell model spans between 62% to 76% of the constant flux obtained by the solid model. Heat flux into FEM models 700 600 500 Flux [W] 400 300 Shell model Solid model/domain1 Solid model/domain2 Solid model Total 200 100 0 35.0 36.0 37.0 38.0 39.0 40.0 Time [s] Figure 5 Flux into structures as torch crosses domain boundaries. Domain 1 & 2 corresponds to CPU number. In the case of the solid model the doubleellipsoid always encircles more integration points. The solid model thus receives a higher and constant flux. Between 35 and 40 seconds the weld arc moves across the element domain boundaries. The total flux remains constant, which shows that MSC.Marc handles the transition from one element domain to another (2 CPUs), also with the subroutine running. The flux into the dense meshed solid model is 89% of the nominal effect, 735W. For comparison, an identical solid model, but with only two elements through thickness was inspected with respect to heat flux. The result suggests that two brick elements through thickness are sufficient with respect to amount of heat absorbed by the model. The shell model reaches maximum temperatures in the weldpool between 1690 and 1870 K depending on amount and shape of heat flux absorbed by the model. The shape of the weldpool is also varying with the heat flux absorbed by the shell model. The width of the weldpool at topface changes between 1mm and 4mm. This variation shows the sensivity of the mesh with respect to energy input. The solid model reaches maximum temperatures in weldpool between 1633 and 1643 K. The width of the weldpool at topface is constant and equals 6.0mm. The models have similar displacement modes during welding, but displacements out of plane is smaller for the solid model, decreasing its resultant displacement compared to the shell model, see Figure 7. The resultant displacement is defined as res = ( x 2 + y 2 + z 2 ). This means that four elements through thickness and with the constant dilatation approach is not enough to include correct bending behaviour of the plate. The solid model thus becomes too stiff. Table 3 shows the direction conventions for the shell and the solid model. Table 4 presents the residual deformations predicted by the simulations.

Table 3 Direction conventions in shells and solids Element Welding direction Perpendicular to w. direction (inplane) Shell 11, σ 11 22, σ 22, N/A Thickness direction Solid 33, σ 33, 11, σ 11, 22, σ 22 Table 4 Shrinkage perpendicular to welding direction Shrink at distance ab Shrink at distance cd Shrink at distance ac Shell model 0,23 mm 0,28 mm 0,07 mm Solid model 0,17 mm 0,18 mm 0,14 1 2 Point 1: (50, -5.0) mm Point 2: (70, -5.0) mm Weld path is left to right. Origo is at weld start. Figure 6 Definition of points 1 and 2. Resultant displacements, shell & solid mode l 2.00E-01 Shell, point1 1.50E-01 [mm] 1.00E-01 Solid, point1 Solid, point2 Shell, point2 5.00E-02 0.00E+00 0.00E+00 1.00E+01 2.00E+01 3.00E+01 4.00E+01 5.00E+01 6.00E+01 Time [s] Figure 7 Displacements during welding, res = ( x 2 + y 2 + z 2 ) As mentioned, the resetting of stresses and strains is not currently implemented for shell elements. This results in stress components where the largest, σ 11, is -230 MPa and σ 22 equals -140 MPa when T > T melt. In the solid model, the equivalent stresses at nodes are less than 10 MPa for T > T melt. Since the stresses are reset in the integration points, the projected stresses at the nodes differ from zero. Thus, the implementation of resetting in solid elements is sufficient.

From Figure 8 at t=60s, we have the midplane stress components σ 11 450MPa and σ 22 120MPa in the shell model. Stress components on topface are σ 11 350MPa and σ 22 0MPa (not shown in picture). The stress contribution from bending is approximately 100 MPa parallel to weld and 120 MPa perpendicular to weld. Thus the plate is dominated by pure tensile stresses rather than local bending. This is expected as the plate is thoroughly clamped. Similarly inspection of solid model in Figure 9 yields stress contributions from bending; 30 MPa in welding direction and zero perpendicular to the weld, as σ 11 is constant through thickness. Due to poor bending behaviour in the solid model, the solid model becomes too stiff. This gives smaller displacements and higher stress concentrations during welding compared to the shell model. As can be calculated from Figure 8 and Figure 9, the maximum equivalent stresses as the torch passes are 13% higher in the solid model. This is mainly due to stresses in thickness direction. After the heatsource has passed, the inplane stresses rise much steeper in the solid model. This is partly explained above, as energy is transformed to plate bending in the shell model and mainly to tensile stresses in the solid model. Stresses in shell model 800 600 Temperature/2 [K] 400 σ 11 200 [MPa] 0-200 -400 σ 22 σ 12-600 -800 0 10 20 30 40 50 60 Time[s] Figure 8 Temperature [K] and stresses [MPa] in point 1 (Figure 6), shell model. Middle of plate thickness

Stress components in solid model 800 600 Temperature/2 [K] σ 33 400 [MPa] 200 0 σ 11-200 -400 σ 22 σ 31-600 0 10 20 30 40 50 60 Time[s] Figure 9 Temperature [K] and stresses [MPa] in point 1 (Figure 6), solid model. Middle of plate thickness DISCUSSIONS There is an uncertainty in the loss of energy between welding equipment and what is actually landed in the weld seam. In these analyses the solid model received 88% which is believed to be too high. The shell model received 60% of the nominal effect, which is believed to be closer to reality. The FEM simulations assume a perfectly rigid clamping of the plates in the fixturing device. In a real welding process this might not be the case, as the plates might slide inside the fixture to increase the weld gap. With the observed magnitude of the reaction forces at the interface between plate and fixture this likely happens. When sliding, the weld gap will increase, causing increased weldpool width and thus a larger area where substantial shrink occurs. CONCLUSIONS When using element number 7 in MSC.Marc in conjunction with thermomechanically coupled analysis with plasticity, no additional accuracy was gained using the assumed strain formulation instead of only constant dilatation formulation. The heat source defined by Goldak's ellipsoid is very dependent upon inplane element size. Good consistency regarding measured shrink and computations gives increased control of the components final shape. Both shell and solid models predict global plate deformations at the same magnitude. The shell model is not sufficient for determining local deformations near the weld seam, as the mesh is too coarse and the heat flux shows cyclic variation.

To make FE welding analysis on complex prototypes more commonplace, better hardware/software combinations are desired. Joining multiple processors and adaptive meshing would be a great advance. When sufficient combinations of hardware and software makes FE weld analysis applicable on large models, initial weld testing on real components will be drastically reduced. This will also enable design- and welding engineers to tailor-make desired deformations, residual stresses or a preferred microstructure onto a component though welding. This might be a certain amount of compressive stresses to enhance the fatigue properties of an engine component. One might also be interested in capturing a sequence of manufacturing operations, for example combining welding and heat treatment. The latter combination using MSC.Marc and CFD has proven useful at Volvo Aero Corporation. Finally, in the future, the use of manufacturing simulation makes it possible to run FE analyses with operating loads with correct prestressed components. This will make it easier to reveal potential operating failures. ACKNOWLEDGEMENTS This work is part of the results gained in EU s 5 th frame project MMFSC, contract number GRD1-1999-10248. We would also like to thank MSC.Software Support for subroutine to reset stresses and strains. REFERENCES 1. Thermal stress analysis of metals with temperature dependent mechanical properties. Ueda Y. and Yamakawa T. JWRI, Vol 2, No. 2, 1971. 2. Three-Dimensional Finite Element Simulation of Laser Welded Stainless Steel Plate D. Berglund, L.E. Lindgren and A. Lundbaeck. Accepted for 7 th Int. Conf. On numerical Methods in Industrial Forming Processes, Japan 2001. 3. Welding Simulation using FEM- Joining of Geometries. M. Sc. thesis by Joergen Naeslund. Volvo Aero Corporation & Luleaa Technical University, Sweden. 2000 4. A new finite element model for welding heat sources. J.A Goldak, Chacravarti A. and M. J. Bibby. AIME, Vol. 15B, No.2, 1984. 5. Marc manuals MSC.Marc Volume B Element Library, version 2000. MSC Software Corporation