Analysis of holes and spot weld joints using sub models and superelements

Transcription

1 MASTER S THESIS 2010:179 CIV Analysis of holes and spot weld joints using sub models and superelements Viktor Larsson MASTER OF SCIENCE PROGRAMME Mechanical Engineering Luleå University of Technology Department of Applied Physics and Mechanical Engineering Division of Solid Mechanics 2010:179 CIV ISSN: ISRN: LTU - EX / SE

2 ABSTRACT Components of press hardened boron steel joined by spot welds can show a brittle behavior during certain load cases which may lead to crack initiation. To capture cracks in a FEM simulation, the mesh must be very detailed and if the fully detailed system is modeled it will lead to long and expensive simulations. The approach to solve this is using a global/local method where the part is divided into two models. First a coarse mesh is created of the components excluding the small details and this model is called the global model. The other model is called the local model and contains a fine mesh of the small details. After simulating the global model one step, displacements from the global model are transferred to the local. Then the local model is simulated applying these displacements as boundary conditions during the simulation. In the next step the global model is updated with the reduced stiffness matrix of the local model, which is returned to the global model through a superelement. To develop the method, a simpler model of a component with a hole is used, instead of creating a model of a spot weld. This model is used to develop a routine to capture cracks near the edge of the hole. The routine reduces the stiffness matrix of the local model, to get all the stiffness information of the local model to the nodes shared with the global model, which are called master nodes. This is done through a series of simulations using the definition of the stiffness matrix coefficients to retrieve the reduced stiffness matrix; the stiffness coefficient with index ij, is equal to the force at degree of freedom i, due to the unit displacement of degree of freedom j. In the simulations all boundary degree of freedoms are constrained not to move except one master node s degree of freedom, which is constrained to move a small distance. Also the boundary nodes between this master node and the surrounding ones are constrained to move. Their displacements are linearly interpolated from the surrounding master nodes displacements. The tangential stiffness is obtained by calculating the difference in force, before and after the perturbation of the master node and dividing with the prescribed displacement of the master node. However, the boundary nodes between the master nodes also have a prescribed displacement and therefore they will affect the master nodes. The equivalent force is derived by calculating the work these nodes will perform on the master nodes. The result is that the equivalent force is equal to the reaction force of the master node multiplied with the interpolation constants from the interpolated displacement. These equivalent forces are added to the master node s forces when calculating the tangential stiffness. The function used to import the superelement into the global model treats the superelement linearly and this means that the reaction force from the superelement will not be the correct one. By calculating the difference in the reaction force used and the one that should be used, it can be compensated by applying external forces equal to this difference. The results show that that the routine needs to be further tested and developed before it can be used as a structural mechanics simulation tool for systems with small holes. Especially when the response of the local model is non-linear, the reduction of the stiffness matrix works poorly. The method using LS-DYNA to return the local model properties through a superelement is verified through a script, using an elastic model and decreasing the stiffness in the middle of the simulation.

3 PREFACE This is the report of my master thesis: Analysis of holes and spot weld joints using sub models and superelements. It has been performed at Luleå University of Technology at the division of Solid Mechanics. The thesis is part of a research cooperation within the Faste laboratory, between the division of Solid Mechanics at Luleå University of Technology and Gestamp Hardtech. I am most grateful I ve been given the opportunity to do this project, which has been most interesting and instructive and I hope my work will be useful in future research. I would like to thank Mats Oldenburg, my supervisor and examiner at the division of Solid Mechanics, LTU, for his guidance and support through this project. I would also like to thank Göran Lindkvist at the division of Solid Mechanics, for his aid with all computer-related problems and his support with LS-DYNA. 2

4 INDEX 1 INTRODUCTION Background Recent studies Gestamp Hardtech The Company Scope Restrictions Definitions FRAME OF REFERENCE Fundamentals of the finite element method Coon s Patch Multiscale analysis Static condensation Stiffness calculation in LS-DYNA Boundary nodes Restarts in LS-DYNA Superelements Substructuring Macroelements Direct Matrix Input METHOD Generate mesh Transfer boundary conditions to local model Compute stiffness matrix of local model Return stiffness matrix to global model RESULTS The FEM model The mesh of the local model Applying boundary conditions to the local model Computation of the tangential stiffness matrix of the local model Verification of the theory Verification of the routine Manual to the script Flow chart of the script

5 5 DISCUSSION CONCLUSIONS AND FUTURE WORK REFERENCES APPENDIX A APPENDIX B

6 1 INTRODUCTION Simulating crash-tests with computers is done more frequently due to the large expenses in manufacturing prototypes to use in experimental crash-tests. The simulation software uses the finite element method to numerically compute the differential equations in structural problems and produces therefore approximate solutions. When complex structures are simulated in detail, the simulation model must be very detailed to capture the behavior during loading. 1.1 Background Welded joints, like spot welds, are commonly used in the vehicle industry to join components into larger structures. They are known to be difficult to model and can lead to unreliable results during simulation. Dimensioning of these joints is often controlled by the load due to crashes and is therefore a critical parameter to ensure a safety component s properties. Effective simulation of a weld joint s properties is important to do early in the development stage, in order to optimize the properties of the product. Spot welds are very small in relation to the components they join together and the physical properties of the material changes through the spot weld, which makes them very complex to analyze. The most relevant properties to capture in the simulations are the weakening in the heat affected zone and the risk of crack initiation. The weakening is a result of the welding operation. When the material is melted, phase transformations take place outside the weld plug which leads to a reduced initial yield stress. During loading this zone is a critical area, with the highest risk of crack initiation. To be able to capture the crack initiation in a simulation model, the mesh has to be very detailed. Thus, with several spot welds present, the number of finite elements will be very high. This will lead to long simulation times and unacceptable increases in costs. 1.2 Recent studies This thesis is based on an earlier thesis made at Gestamp Hardtech where a sub-model of the spot weld was developed by Löveborn, [1], using a global/local template. In the global/local method a coarse mesh is first created of the components excluding the small details. This is called the global model. Then another model, the local model, is constructed using only a fine mesh of the small detail. They are connected by transferring either nodal displacements or forces from the global to the local model. This sub-model is used in post processing without returning any properties to the global model, in order to evaluate when the weld begins to fail. There is much work done in the field of spot welds but not with the use of macroelements. This technique is most often used in FEM analysis of materials with complex microstructure, where the microstructure is assembled into macroelements by reducing their interior degree of freedoms. For example Wierer, Šejnoha and Zeman used it to analyze complex wound composite tubes [2] and Whitcomb and Woo used it to formulate continuum finite elements for textile composites [3]. 1.3 Gestamp Hardtech The Company Gestamp Hardtech develops press-hardened safety components in hardened boron steel for the vehicle industry including side impact padding, bumpers and body components. Gestamp Hardtech is a competence centre for Gestamp press-hardening group, with manufacturing in Luleå, Sweden, 5

7 Haynrode, Germany, Mason, USA, Kunshan, China and Bilbao, Spain. The development environment consists mainly of the CAD software I-DEAS and the explicit finite element software LS-DYNA. 1.4 Scope In the thesis made by Löveborn, [1], the results are only transferred one way, from the global to the local model, using the results from the global simulation to analyze the effect on the local model. This is called an uncoupled approach by Wierer, Šejnoha and Zeman in [2]. The effects on the global model from the local details are often not considered, because the assumption is made that they are so small they can be neglected. In this thesis a study will be made to see if it is possible to make a two way connection, also transferring information from the local model to the global using a superelement. This is called a coupled approach. It will be done to see if the coupled approach gives more reliable results, while keeping the simulation time within reasonable limits. In the coupled approach, the tangential stiffness of the local model is computed using multipoint constraints and implemented into the global model as a superelement. If the effect on the component is large, it may not be possible to use the sub-model developed earlier without returning any information to the global model. 1.5 Restrictions A simpler model of a hole is used, instead of a spot weld, to develop a method that later also can be used for models with spot welds. The model can then be used to predict failure and crack propagation near the edge of the hole. Another simplification is that only shell elements can be used with the developed routine. Also the routine to calculate the stiffness matrix of the local model is simplified, using LS-DYNA instead of a numerical method. 1.6 Definitions To make the report easier to read, some expressions that are used through the report are briefly explained. FEM finite element method It is the computational method using numerical approximations to calculate problems in solid mechanics. DOF degrees of freedom In Cartesian coordinates an object has six degrees of freedom; three translational and three rotational degrees of freedom in the x-, y- and z-directions. In FEM software, objects can be constrained not to move in chosen DOFs. This resembles the real world where, for example, one side of an object can move freely while the other side is clamped on a wall. Global/local model In global/local analysis the component analyzed is divided into two simulation models. The global model is a coarse mesh of the whole component but excludes small details that are deemed not to affect the overall result too much. The local model contains only a fine mesh of the small details. 6

8 Sub-model A sub-model is a complete model that uses the results from the global simulation to analyze the local model in post-processing. Superelement Superelements are a kind of elements that are composed from other elements. They are called differently depending how they are composed and two types are substructures and macroelements. Substructure When the superelements are large parts of a complete structure they are called substructures. Macroelement Macroelements are superelements that are composed of smaller simpler elements and can be used in a mesh like ordinary elements. Master nodes The boundary nodes in the local model that have corresponding nodes in the global model are called master nodes. Slaved boundary nodes These are the boundary nodes of the local model that are not master nodes and whose displacements have to be interpolated from the surrounding master nodes displacements. 7

9 2 FRAME OF REFERENCE Here fundamental theory is explained needed to develop the routine used to analyze models with holes. The first chapter contains fundamentals of FEM and then the procedure used to create the local model is explained in detail, using Coon s Patch and the global/local method. The technique to reduce the stiffness matrix of the local model is derived and how to do restarts in LS-DYNA is shown. Finally the technique to return the results from the local model to the global model using superelements is explained. 2.1 Fundamentals of the finite element method FEM is a computational technique used to obtain approximate solutions of boundary value problems in engineering. A boundary value problem is a mathematical problem where one or more dependent variables must satisfy a differential equation everywhere in a known domain of independent variables and satisfy specific conditions on the boundary of the domain. The domain is often a physical structure divided into finite elements. The resulting discrete model is called a mesh and the dependent variable of interest is computed at the element corner points, which are called nodes. A rule that usually can be applied if all the boundary conditions are applied correctly is; the more nodes used in the domain, the more accurate solution. A finite element is a discrete volume or surface where specific functions describes, e.g. displacement or temperature inside the element. The function values are determined using the already computed values at the nodes. There are several different types of element formulations and they are developed to be more accurate in certain load cases etc. More detailed information can be found in a book with fundamental FEM theory, like [4] by Hutton. There are different types of elements developed for different geometries of the domain. The most common ones are the three node triangular element, the four node quadrilateral element, the four node tetrahedral element and the hexahedral element consisting of eight nodes, see Figure 1. Figure 1. From left to right; triangular element, quadrilateral element, node tetrahedral element, hexahedral element. In FEM software boundary constraints can be applied to the nodes and material- and damage models can be chosen. The material of the simulation model is determined by material parameters, e.g. density, young s modulus and poisons ratio for an isotropic and elastic material. That is enough for a simple elastic model, but with a more advanced material model more characteristics of the material must be assigned. In FEM-software there are two different time integration algorithms; explicit- and implicit time integration. In the explicit method internal and external forces are summed at each point and a nodal acceleration is computed by dividing with the nodal mass. Then the acceleration is integrated in time to get velocity and displacement. The maximum time step size used with the explicit integration scheme is limited to the shortest time it takes a wave to propagate between two nodes 8

10 in the model. This is called the Courant condition and because of it, explicit time integration requires many but quickly solved time steps. The implicit method assembles the global stiffness matrix, inverts it and multiplies it to the nodal forces to get the displacements. The advantage of this approach is that the time step can be user defined. It is not tied to Courant s criteria but must be small enough for the iterative algorithm to converge. The disadvantage is the numerical effort it takes to assemble, invert and store the stiffness matrix. Implicit simulations therefore often consist of a small number of time steps, each time step demanding a large computational effort. Explicit analysis is well suited for dynamic simulations such as impact and crash analysis, but for long duration analyses the implicit method is a better choice. 2.2 Coon s Patch Coon s patch is used to interpolate a surface between four points and in order to use it curves must be interpolated between the four points, see the lecture material in [5]. A cubic spline is often used to interpolate a curve between two points in space, point A and point B. The cubic spline is created by adapting a parametric cubic polynomial, as can be seen in equation (1), between the two points A and B,. (1) The function has four unknowns; a 1, a 2, a 3 and a 4 and four equations are needed to solve the system of equations. Therefore it is not enough to use only the point coordinates, but the point derivatives have to be used as well. The points next to point A and B are used to calculate the derivative using the central difference method, 3 2. (2) The parametric values at the points have to be defined and usually you use discrete values and in this case the value at point A is set to be μ=0 and at point B: μ=1. These values are put into equation (1) and (2) for the point coordinates and derivatives and give the four equations:... (3) 3 2. The system of equations in equation (3) is expressed in matrix form, (4) To solve for the constants, the matrix in equation (4) is inverted, 9

11 (5) This formulation represents four equations for each dimension and in the three dimensional case it therefore represents twelve equations. When the constants are solved with the matrix calculation in equation (5), they are put into the parametric cubic polynomial in equation (1) which gives the parametric curve between the two points. Coon s Patch is a well used and relatively easy way to define a formulation for an interpolated surface. It is using four curves as boundaries to a closed patch and along these, two parametric variables have to be defined, for example µ and ν, and the curves have to be orthogonal in the parameter space. Figure 2 is an example of a surface patch in parameter space and it can be seen that one parameter is kept constant and the other is varied along each curve. Figure 2. Four curves defining a surface patch. At the four corner points the parameter values have to be defined, P(0,0), P(0,1), P(1,0), P(1,1). (6) Then curves are created between the points and equation (7) defines which curve that spans between which points. P(0, ν) between P(0,0) and P(0,1). P(1, ν) between P(1,0) and P(1,1). (7) P(µ, 0) between P(0,0) and P(1,0). P(µ, 1) between P(0,1) and P(1,1). To get a formulation for the surface, Coon s Patch in equation (8) is used where a linear surface interpolation is made between the curves, μ, μ, 0 1 P μ, 1 P 0, ν 1 μ P 1, ν μ (8) 0,0 1 μ 1 0,1 1 μ 1,0 μ 1 1,1 μ. 10

12 2.3 Multiscale analysis Complex structures can often be simplified using multiscale analysis which can reduce the simulation time. First the whole system, called the global model, is analyzed discarding small details that are deemed to not affect the overall behavior of the system and a coarser mesh can then be used. In the next step the small details, called local models, are analyzed separately with a fine mesh using the results from the global simulation as boundary conditions. This can be done in several steps but if the analysis consists of two steps it is called global/local analysis in FEM literature, explained by Felippa in [6]. The boundary conditions applied on the local model from the global simulation results can be of two different kinds; either displacement- or force boundary conditions. If the displacement method is used, displacements are interpolated from the global solution. If the force method is used, internal forces or stresses from the global solution are converted to nodal forces acting on the boundary nodes of the local model. 2.4 Static condensation Static condensation is the process of eliminating the internal degrees of freedom of a substructure, meaning that the stiffness matrices of a substructure are reduced and the master nodes will include the information of the whole model. This is explained in detail by Raghu in [7]. Equation (9) shows the relation between displacement and force,. (9) First equation (9) is partitioned into two sets, m (master) set whose DOFs are to be kept in the reduction process, and the s (slave) set that are reduced,. (10) Then the slave set can be reduced through some matrix calculations. The lower partition of equation (10) is. (11) In equation (11) is isolated,. (12) The upper partition of equation (10) is. (13) Substituting equation (12) into equation (13) gives. (14) Equation (14) can be expressed as. (15) 11

13 This can be rewritten to its final form. (16) The condensed substructure stiffness matrix in equation (16) is equal to. The associated load vector in equation (16) is equal to (17). (18) When using static condensation in FEM applications the inverse of isn t calculated but other matrix solution methods are used, such as partial factorization and forward reduction. This is due to the large amount of computer power that is needed to compute a matrix inverse. 2.5 Stiffness calculation in LS-DYNA Another way to compute the stiffness matrix is using the formal definition of the stiffness coefficient in equation (19). K ij =force at DOF i due to unit displacement at DOF j. (19) The stiffness matrix of the local model is obtained by perturbing the master DOFs, one at a time, while keeping the others fixed. Each perturbation gives a set of forces at the boundary DOFs that constitute one column in the stiffness matrix, corresponding to the perturbed DOF. This can be considered as a numerical application of the direct stiffness method for calculating stiffness matrices. There is a function in LS-DYNA that uses this technique. It is the card control implicit modes, see the LS-DYNA keyword user s manual in [8], but it can only be used in linear problems. To be able to remove interior DOFs in non-linear problems, a routine has to be developed. To use these methods in non-linear FEM the difference in force, f and displacement, between two time steps must be used to compute the current (tangential) stiffness matrix. Equation (20) shows the perturbation of to get the first column in the stiffness matrix. f f / 0 f f /. (20) 0 f f / 2.6 Boundary nodes If there are nodes on the boundary in the local model whose DOFs cannot be retained a special approach to remove their DOFs is needed, explained by Whitcomb and Woo in [3]. They cannot be removed with the direct stiffness approach because it would yield an incorrect result. These nodes have to be removed using interpolation constraints. This is called the enhanced direct stiffness method, which considers the work done by the boundary nodal forces during displacement due to the interpolation constraints. It is derived below with subscript m meaning master DOFs to be retained in the reduced stiffness matrix, subscript s meaning boundary nodes that are slaved to the master DOFs and will be reduced from the stiffness matrix, u is the displacement and f the force corresponding to u. The work done by the boundary nodal forces in a linear elastic model is 12

14 ; m=1, number of master DOFs; s=1, number of slaved DOFs. (21) are slaved to with interpolation constants T expressed in equation (22), T. (22) The interpolation equation (22) is inserted into equation (21) expressing the work, T. (23) The stiffness matrix can be expressed as. (24) But for linear models U=W, which gives. (25) The stiffness relation in equation (25) is inserted into equation (23) that expresses the work done by the nodes,. (26) Now the work done by the boundary forces is set equal to the work done by equivalent forces at the master DOFs,. (27) Then the interpolation relation in equation (22) is inserted into equation (27), T. (28) Equation (28) shows that the equivalent nodal forces are T. (29) The expression for the forces in equation (29) is inserted in the third and fourth terms of the stiffness relation in equation (26),. (30) From the Maxwell-Betti reciprocity theorem the terms in equation (30) are equal and also the first two terms in equation (26) are equal due to the same theorem. Therefore equation (26) can be expressed as. (31) 13

15 Equation (31) expresses the stiffness matrix in only the partial derivatives of the equivalent slaved boundary nodal forces working on the master nodes and the master nodal forces, with respect to the displacement of the master node. 2.7 Restarts in LS-DYNA There is a restart capability in LS-DYNA allowing analyses to be broken down in stages, see [8]. After each simulation a restart dump file is created containing all information needed to continue the analysis. This is useful for many reasons; it makes it possible to post-process the output databases to discover incorrect simulations in an early stage or finding problems with the model. It can also be used to modify the analysis; changing boundary conditions, deleting elements, adding or removing contact surfaces and much more. There are three different types of restarts in LS-DYNA. A simple restart is when no modifications are made to the model and is used to continue an analysis made earlier. In a small restart, minor modifications to the model can be made; boundary conditions can be added, elements or parts can be deleted and termination time or output frequencies can be changed. These changes are written into a restart input file to be read along with the restart dump file. The third option is to do a full restart if many modifications to the model have to be done. Then the full model information needs to be added to the restart input file, but the new nodal coordinates don t need to be updated because the deformation state is extracted from the restart dump file. An extra keyword; stress initialization, needs to be added to the input file and it s used to choose which parts to be initialized. To do a simple restart of stage nn, LS-DYNA R=d3dumpnn is written on the command line, for a small and full restart i=restart input file is added. To update the stiffness- and mass matrix of the superelement in the global model a full restart has to be done. 2.8 Superelements Superelements is a combination of several elements and when assembled may be considered as one element. There are two different views regarding superelements; bottom up or top down explained by Felippa in [6]. In the bottom up view the superelement is built from simpler elements and used as building blocks like ordinary elements, while the top down view thinks of superelements as large parts of a complete structure. A superelement built from simpler elements, using the bottom up view, is called a macroelement and if it is instead a complex assembly of elements building a part of a structure, using the top down view, it is called a substructure. 2.9 Substructuring Substructuring was invented by the aerospace industry in the early 1960s to be able to break down complex systems to smaller components, to make it possible to analyze the system with the limited computer power they had. It is now most often used in two different contexts. One is when there are different groups in a company specialized in different components of a system. Substructuring makes it possible for each group to work on refining, improving or verifying the simulation model of their part (the interface between the parts must stay reasonably unchanged). Another area of usage is if there are several identical (or nearly identical) units in a structure which makes it possible to use one model for those units and save computational time. 14

16 2.10 Macroelements Macroelements were invented in the mid 1960s for user convenience, after they are assembled they are easier to use. They can be used, for example, to model complex materials that are not homogenous but have periodic patterns. Then only a part of the microstructure needs to be meshed and a macroelement can be constructed from that part. A larger part of the material can then be meshed from several macroelements Direct Matrix Input When the reduced stiffness matrix of the local model has been calculated, it must be implemented into the global model. It is done writing the stiffness matrix into a file of DMIG format compatible with NASTRAN, see [9], which is read by a Direct Matrix Input keyword which exists in LS-DYNA, see [8]. This element consisting only of the stiffness- and mass matrix is called a superelement. It is assumed that LS-DYNA treats the superelement as a linear element, which means that the imported stiffness is treated as an elastic stiffness, shown in Figure 3. F Tangential stiffness F (u r ) Tangential stiffness treated as elastic K t u r u r u Figure 3. The figure shows a sketch of the relation between deformation and force of a material. If the local tangential stiffness matrix is calculated at a point where the displacements are u r, then the reaction forces applied to the global model from the local model will be -K t u. That will lead to a drastic change in displacement because the FEM program will update the displacements in the next time step as if the stiffness of the superelement always had been K t. To compensate for that change in reaction force, an outer load of magnitude F (u r ) + K t u r must be applied to the nodes in the global model to balance this change. Then the reaction forces affecting the nodes due to the stiffness of the local model will be -F (u r ) - K t (u-u r ), which are the forces that would have been applied, if the stiffness of the superelement had been treated as a tangential stiffness. 15

17 3 METHOD In this chapter the process of developing the routine is described, dividing the work in different steps shown in Figure 4. Every step has been preceded by literature studies and the final product is the program written in FORTRAN and Python. Figure 4. A flowchart of the process to create the final program. 3.1 Generate mesh It is decided to generate the mesh with a program created in FORTRAN and to replace four elements in the global model with the superelement containing the local model. Then the decision is made to use Coon s patch as the interpolation method, to create the local mesh. That is because it is a basic method and the resulting mesh follows the rest of the structure nicely, due to the continuity of the first derivative in the corner points. The hole can then be created using the middle node as center, either using coon s patch to interpolate points along the edge of the hole or projecting a circle on the surface. The idea to project a circle is discarded, to simplify the program as the routines to interpolate points using Coon s patch already are written. Due to the hole the geometry cannot be divided into areas closed by four edges which is the requirement of using Coon s Patch. A different approach has to be made in order to get surface patches with four edges. It is done by dividing the geometry into four or eight surface patches as in Figure 5. Figure 5. The figure shows two different ways to create surface patches defined by four edges of a geometry including a hole. The circles represent master nodes. The curve defining the edge becomes more exact the more nodes you have to interpolate with and therefore the alternative to divide the geometry into eight surface patches is used to get a more exact representation of the hole. 16

18 3.2 Transfer boundary conditions to local model As described in the theory section, there are two different ways of transferring boundary conditions to the local model. Either displacements are interpolated from the global solution or internal forces are converted to nodal forces acting on the boundary nodes of the local model. The force method is a little more reliable in some cases but the displacement method is easier to use and it is that method that is chosen to apply boundary conditions on the local model. 3.3 Compute stiffness matrix of local model There are several methods that can be used to compute the stiffness matrix. Static condensation is not used since it may only be applied on linear problems and while there are numerical methods to compute the tangential stiffness it is decided to use LS-DYNA, since it is a simple and reliable method. 3.4 Return stiffness matrix to global model There are two solutions to return the stiffness matrix to the global model using LS-DYNA. The first is to use User Defined Elements, which is a function in LS-DYNA described in the LS-DYNA keyword user s manual in [8]. It is a more general way to tailor an element to be used in a mesh. The other option is to use a function in LS-DYNA called Direct Matrix Input where the stiffness- and mass matrix may be assigned to a superelement in a mesh. That is the method used in this thesis due to its simplicity. 17

19 4 RESULTS First the routine is described in detail and then a simple two step simulation with a superelement is made, where the stiffness is updated half way through. This is done to see how LS-DYNA behaves when updating the superelement and try to verify the assumption that LS-DYNA treats the superelement as an elastic element. During this verification, the function in LS-DYNA is used to reduce the stiffness matrix of the local model and use it as a superelement in the global model. Then the routine developed in this thesis is used to calculate the reduced stiffness matrix, to verify if it will match the one extracted using the function in LS-DYNA. Finally, the script is explained in detail. 4.1 The FEM model In this thesis shell elements are used as 3D quadrilaterals to create the mesh. An elasto-plastic material model is used where the plastic behavior is specified through the change of effective plastic strain due to the change in effective stress. This relation is set in a table with point data and in [8], detailed information of the material model used in LS-DYNA is covered. It is decided to use both time integration schemes in the simulations. In the global simulations an explicit scheme is used, because it is better with dynamic simulations such as crash simulations. In the local simulations however, an implicit scheme is used to increase the accuracy of the solution. The time steps are more time consuming with the implicit method but since the local mesh will be relatively small, it is possible to use this method. 4.2 The mesh of the local model The nodes on the edge of the hole are created by first creating curves between the middle node and the boundary nodes. Along those curves, new nodes are created on the edge of the hole, a distance from the middle node equal to the radius of the hole. To create more nodes along the edge of the hole, a curve has to be interpolated along the edge and it is done using the nodes already created on the edge. The nodes are generated using Coon s Patch in a FORTRAN routine, see Appendix A, and in the same routine the nodes are connected to each other anti clockwise defining elements. The node coordinates and numbering and the element numbering are then written into a file of the LS-DYNA keyword format. A mesh created with Coon s Patch can be seen in Figure 6. Figure 6. A mesh with a small hole created with Coon s Patch. 18

20 4.3 Applying boundary conditions to the local model The local model has eight master nodes, nodes at the same positions as the boundary nodes of the four global elements. In a python script, see Appendix B, the displacements of the master nodes are extracted from the global solution and written to lists that are applied to the master nodes in the local model. There must be boundary conditions applied to all boundary nodes of the local model and the displacements applied to the slaved boundary nodes are interpolated from the master nodes displacements. This is done using a function in LS-DYNA called constrained interpolation, see [8], where each slave node s displacement is connected to the two surrounding master nodes displacements with weighting factors. The DOFs to be controlled by the constraint are then chosen in the same function. Figure 7 shows the deformed local- and global model connected through the displacements of the master nodes and the linear interpolations of the slaved boundary nodes. Figure 7. The figure shows the global and local model together to demonstrate that the local model is connected to the global model via the extracted displacements. 4.4 Computation of the tangential stiffness matrix of the local model In a LS-DYNA keyword file a small displacement is assigned to one master node DOF at a time with the keyword boundary prescribed motion, described in [8]. At the same time the other DOFs of the perturbed node and all DOFs of the other master nodes are constrained not to move with boundary prescribed motion keywords. But the only way to output both moment and forces for all DOFs is to constrain all DOFs with single point constraints using the keyword boundary spc described in [8]. Therefore the boundary prescribed motions are killed after one time step and at the same time single point constrains are birthed on those DOFs. A simulation is carried out for each DOF because if all perturbations were assigned in the same simulation, it would generate a wrong result for a non-linear analysis. Equivalent forces from the slaved boundary nodes are added to the master nodes forces in the stiffness calculation routine to reduce the slaved boundary nodes from the stiffness matrix, before calculating the tangential stiffness. 19

21 4.5 Verification of the theory To see if it is possible to use LS-DYNA to make these kinds of simulations and to verify the assumption that LS-DYNA treats the superelement as an elastic element, a script is created using an elastic model loaded in the z-direction. Four of the elements are removed and the middle node is reduced through static condensation to get the superelement stiffness matrix of the four elements and then imported with Direct Matrix Input. Halfway through, the simulation is stopped and the elastic modulus of both superelement and cylinder is decreased by half. The stiffness is in linear problems linearly dependent of the elastic modulus. The simulation is restarted with the updated elastic modulus and the behavior of the displacements is analyzed. An implicit integration scheme is used with a time step of 1e-3 seconds. The plot in Figure 8 shows how the displacements are updated when performing a simulation with a superelement but without applying balance forces. The graph shows that during the first time step LS-DYNA compensates the change in stiffness by updating the displacement. Figure 8. The graph shows the behavior of the displacement when changing the stiffness of a model with a superelement and not applying any balance forces. Figure 9 shows the displacement behavior when applying balance forces and in the graph no compensation of displacement can be seen. 20

22 Figure 9. The graph shows the behavior of the displacement when changing the stiffness of a model with a superelement and applying balance forces. Figure 10 is a plot from a simulation without a superelement to compare the results. The result shown in the previous graph correlates well with the result in this. Figure 10. The plot is from a simulation of a model without a superelement and where the stiffness is changed halfway through the simulation. 4.6 Verification of the routine A script similar to the one used in the previous paragraph is used, but instead using the developed routine to calculate the reduced stiffness matrix. The FEM model is a plate loaded in the y-direction with applied balance forces and the result is shown in Figure 11 where a decrease in stiffness is apparent. The transition between the two different stiffness cases seems to go smooth. 21

23 Figure 11. The graph shows the stress dependent of the displacement in the y-direction from a simulation where the stiffness is changed halfway through the simulation and where the stiffness calculation routine is used. In Table 1 the calculated stiffness coefficients is compared with the extracted stiffness coefficients using LS-DYNA s static condensation. The coefficients for the translational DOFs correlate rather well except when the coefficients are very small (close to zero). In those cases the calculated coefficients differ with several orders of magnitude. The calculated rotational stiffness coefficients also differ from the coefficients extracted with LS-DYNA. Sometimes there is a small error and sometimes a larger error. 22

24 Table 1. In the table calculated stiffness coefficients are compared to LS-DYNA extracted stiffness coefficients. LS-DYNA stiffness coefficients Calculated stiffness coeficients LS-DYNA stiffness coefficients Calculated stiffness coeficients STIF STIF ,485887E+07-1,486614E ,363126E+04-6,972859E ,081115E+06 5,079661E ,220082E+04 3,005286E ,223857E+06-1,225350E ,804217E+01-3,170000E ,961190E+04 3,954728E ,606890E+02 9,572425E ,813514E+04 7,800278E ,153753E+02 1,866487E ,570049E+04 1,543949E ,372453E-01-2,637073E ,375683E+07 5,370351E ,568988E-11-5,846326E+04 STIF ,248815E-11 2,669592E ,794713E+06 4,789148E ,395178E+02-5,561000E ,379117E+06-8,381899E ,209735E+02 2,426939E ,013864E+06-3,013810E ,455989E+02 4,895719E ,070345E+04-2,076716E+04 STIF ,986593E+04-3,999325E ,712493E+03-3,387124E ,243082E+03-7,507552E ,909003E+03 1,762203E ,070421E+07 1,064430E ,084223E+03-5,000000E ,870746E+07 6,873775E ,470235E+01-4,026862E+01 STIF ,848191E+01-8,025656E ,207678E+06 2,201227E ,201322E+01-1,710529E ,232344E+06 4,229454E ,236575E+04 3,908890E ,296588E+07-4,296903E ,873214E+04-2,039520E ,023668E+02-1,673391E ,449724E-12 8,391000E ,009097E+02-3,296504E ,473746E-14-7,828860E ,354694E+00-2,643389E ,797796E-15-1,560444E ,330816E-09-5,921406E ,714478E+02 4,347983E ,483270E-09 2,516760E ,152544E+08 1,152485E+08 STIF ,220366E+04-3,830139E ,683383E+04 1,468606E ,204233E+01-3,070000E ,187378E+01 1,690675E ,606891E+02 3,195825E ,246869E-01-2,633947E ,134323E-11-5,846328E ,059119E-11 2,669592E ,395509E+02-6,556700E ,791839E+02 1,009005E+02 23

25 4.7 Manual to the script First a LS-DYNA input file of the global model must be created without any information of output of data and termination time. It is moved into an optional working folder together with the FORTRANand Python scripts and a script used to start the simulations. The node identities within four elements from the global model, where the hole should be situated, are written into a list in the Python script but excluding the middle node identity. Into another list the node identities from the four elements together with node identities from the adjacent elements are written. The node identities must be written into the lists, in the same order as in Figure Figure 12. The figure shows in which order the node identity numbers should be written into the lists. The middle node identity is written to a variable and the global LS-DYNA filename is specified in another variable. This is used to extract the node positions from the global model to create the local mesh. Furthermore the variables nmy and nnu must be assigned in the FORTRAN routine to control the number of elements created in the local model. The material model of the local model must be changed to match the one in the global model. When the local mesh has been created, the mass- and stiffness matrices are extracted using static condensation in LS-DYNA. After this, the script consists of three parts. The first part adds small displacements to the master node DOFs, to calculate the reduced stiffness matrix. The next part is the global simulation, which imports the stiffness- and mass matrix using the restart routine. The last part assigns displacements to the master nodes in the local model extracted from the global simulation. To specify how often the global simulation will stop to update the stiffness matrix of the superelement, some values have to be assigned to variables. The total simulation time, the output frequency and an interval will control the update frequency and number of times the three main parts of the script will be looped. The full scripts are in the appendices and in the next section an overview of the script is made through a flow chart. 24

26 4.8 Flow chart of the script 1 A mesh of the local model is created from the master node coordinates extracted from four elements in the global LS-DYNA input file. 2 A simulation is carried out of the local model to get the reduced massand stiffness matrices through static condensation in LS-DYNA The mass-and stiffness matrices are used as a superelement in a global simulation. A simulation of the local model is carried out in LS-DYNA, with applied displacements of the master nodes from the result of the global simulation and interpolated displacements on the other boundary nodes. The forces and deformations are saved to compute the tangential stiffness matrix. LS-DYNA simulations of the local model are initiated where small displacements are assigned to all DOFs of the master nodes in the local model, one simulation per DOF. The forces and moments are written into a text file. The tangential stiffness matrix is calculated from the difference of the forces in this step and from the previous step, divided with the small added displacement. A superelement is created in the global model with the calculated stiffness matrix and the saved mass matrix from step 2. Calculated balance forces are applied on the master nodes. A full restart of the global simulation is started and the displacements of the master nodes are saved. The script restarts at point 4 until the final termination time is reached. 25

27 5 DISCUSSION The routine with LS-DYNA failed when the material started to plasticize and there are several factors that may have introduced errors in the simulation routine. One source of error is the problems to reduce the stiffness matrix. Another source of error may be the inexactness of the stiffness calculation. When perturbing each DOF with a small displacement, the largest displacement used was 1 µm, the difference in forces before and after will be small. However the small assigned displacement has to be small to get an exact stiffness matrix. The largest number of decimals that could be extracted from LS-DYNA, using output files, were six and that led to inexact calculations of the stiffness matrix. Sometimes the change in force was so small that the difference became zero due to the low number of decimals. Another source of error may be the interpolation routine. To get the mass matrix, LS-DYNA s static condensation routine (the control implicit modes keyword) was used and the keyword constrained interpolation was used to interpolate the boundary nodes between the master nodes. But that keyword did not interpolate rotation and due to the use of the resulting mass matrix from the static condensation, the rotations could not be interpolated. If they were to be interpolated through a routine created by the user, a new mass matrix has to be assembled as well. To get hold of the moments, single point constraints had to be used in the simulations and then it is not possible to use the restart routine. The reason for this is that once the rotation DOFs are constrained, they cannot be unconstrained in LS-DYNA. Therefore all displacements, for each time step (or specified frequency), must be added to a vector and each simulation of the local model must start from the beginning. This leads to longer and longer simulations times in each step, to assemble the reduced stiffness matrix of the local model. This routine uses four elements to build the superelement, which leads to eight master nodes with forty-eight DOFs. To assemble the reduced stiffness matrix in each step forty-eight simulation has to be done and the result of this is very long simulation times. 26

28 6 CONCLUSIONS AND FUTURE WORK The verification of the theory shows that is possible to use LS-DYNA for this method to simulate structural components with holes or spot welds. When using the routine to reduce the stiffness matrix the results aren t the ones expected. To be able to use this routine to calculate the tangent stiffness of a model, the routine must be further developed and tested. It was decided to try to use LS-DYNA to assemble the reduced stiffness matrix of the local model for simplicity, only to try the method but not as a long term solution. If LS-DYNA is to be used for this in the future, a way to extract the forces more accurately is a necessity. Also a routine to assemble the mass matrix has to be added to be able to interpolate rotations. Otherwise a new routine, using numerical methods to assemble the reduced stiffness matrix of the local model has to be developed. In the future it would be much more effective to make a specific numerical program that solves the simulations of the local model instead of using LS-DYNA. 27