非线性解析概要-Abaqus 6.9 Nonlinearity

8 8. Nonlinearity This chapter discusses nonlinear structural analysis in Abaqus. The differences between linear and nonlinear analyses are summarized below. Linear analysis All the analyses discussed so far have been linear: there is a linear relationship between the applied loads and the response of the system. For example, if a linear spring extends statically by 1 m under a load of 10 N, it will extend by 2 m when a load of 20 N is applied. This means that in a linear Abaqus/Standard analysis the flexibility of the structure need only be calculated once (by assembling the stiffness matrix and inverting it). The linear response of the structure to other load cases can be found by multiplying the new vector of loads by the inverted stiffness matrix. Furthermore, the structure's response to various load cases can be scaled by constants and/or superimposed on one another to determine its response to a completely new load case, provided that the new load case is the sum (or multiple) of previous ones. This principle of superposition of load cases assumes that the same boundary conditions are used for all the load cases. Abaqus/Standard uses the principle of superposition of load cases in linear dynamics simulations, which are discussed in Chapter 7, “Linear Dynamics.” Nonlinear analysis A nonlinear structural problem is one in which the structure's stiffness changes as it deforms. All physical structures are nonlinear. Linear analysis is a convenient approximation that is often adequate for design purposes. It is obviously inadequate for many structural simulations including manufacturing processes, such as forging or stamping; crash analyses; and analyses of rubber components, such as tires or engine mounts. A simple example is a spring with a nonlinear stiffening response (see Figure 8–1). Figure 8–1 Linear and nonlinear spring characteristics. Since the stiffness is now dependent on the displacement, the initial flexibility can no longer be multiplied by the applied load to calculate the spring's displacement for any load. In a nonlinear implicit analysis the stiffness matrix of the structure has to be assembled and inverted many times during the course of the analysis, making it much more expensive to solve than a linear implicit analysis. In an explicit analysis the increased cost of a nonlinear analysis is due to reductions in the stable time increment. The stable time increment is discussed further in Chapter 9, “Nonlinear Explicit Dynamics.” Since the response of a nonlinear system is not a linear function of the magnitude of the applied load, it is not possible to create solutions for different load cases by superposition. Each load case must be defined and solved as a separate analysis. ・ 8.1 Sources of nonlinearity There are three sources of nonlinearity in structural mechanics simulations: ​ Material nonlinearity. ​ Boundary nonlinearity. ​ Geometric nonlinearity. ​ 8.1.1 Material nonlinearity This type of nonlinearity is probably the one that you are most familiar with and is covered in more depth in Chapter 10, “Materials.” Most metals have a fairly linear stress/strain relationship at low strain values; but at higher strains the material yields, at which point the response becomes nonlinear and irreversible (see Figure 8–2). Figure 8–2 Stress-strain curve for an elastic-plastic material under uniaxial tension. Rubber materials can be approximated by a nonlinear, reversible (elastic) response (see Figure 8–3). Figure 8–3 Stress-strain curve for a rubber-type material. Material nonlinearity may be related to factors other than strain. Strain-rate-dependent material data and material failure are both forms of material nonlinearity. Material properties can also be a function of temperature and other predefined fields. ・ 8.1.2 Boundary nonlinearity Boundary nonlinearity occurs if the boundary conditions change during the analysis. Consider the cantilever beam, shown in Figure 8–4, that deflects under an applied load until it hits a “stop.” Figure 8–4 Cantilever beam hitting a stop. The vertical deflection of the tip is linearly related to the load (if the deflection is small) until it contacts the stop. There is then a sudden change in the boundary condition at the tip of the beam, preventing any further vertical deflection, and so the response of the beam is no longer linear. Boundary nonlinearities are extremely discontinuous: when contact occurs during a simulation, there is a large and instantaneous change in the response of the structure. Another example of boundary nonlinearity is blowing a sheet of material into a mold. The sheet expands relatively easily under the applied pressure until it begins to contact the mold. From then on the pressure must be increased to continue forming the sheet because of the change in boundary conditions. Boundary nonlinearity is covered in Chapter 12, “Contact.” ・ 8.1.3 Geometric nonlinearity The third source of nonlinearity is related to changes in the geometry of the model during the analysis. Geometric nonlinearity occurs whenever the magnitude of the displacements affects the response of the structure. This may be caused by: ​ Large deflections or rotations. ​ “Snap through.” ​ Initial stresses or load stiffening. For example, consider a cantilever beam loaded vertically at the tip (see Figure 8–5). Figure 8–5 Large deflection of a cantilever beam. If the tip deflection is small, the analysis can be considered as being approximately linear. However, if the tip deflections are large, the shape of the structure and, hence, its stiffness changes. In addition, if the load does not remain perpendicular to the beam, the action of the load on the structure changes significantly. As the cantilever beam deflects, the load can be resolved into a component perpendicular to the beam and a component acting along the length of the beam. Both of these effects contribute to the nonlinear response of the cantilever beam (i.e., the changing of the beam's stiffness as the load it carries increases). One would expect large deflections and rotations to have a significant effect on the way that structures carry loads. However, displacements do not necessarily have to be large relative to the dimensions of the structure for geometric nonlinearity to be important. Consider the “snap through” under applied pressure of a large panel with a shallow curve, as shown in Figure 8–6. Figure 8–6 Snap-through of a large shallow panel. In this example there is a dramatic change in the stiffness of the panel as it deforms. As the panel “snaps through,” the stiffness becomes negative. Thus, although the magnitude of the displacements, relative to the panel's dimensions, is quite small, there is significant geometric nonlinearity in the simulation, which must be taken into consideration. An important difference between the analysis products should be noted here: by default, Abaqus/Standard assumes small deformations, while Abaqus/Explicit assumes large deformations. ・　8. 2 The solution of nonlinear problems The nonlinear load-displacement curve for a structure is shown in Figure 8–7. Figure 8–7 Nonlinear load-displacement curve. The objective of the analysis is to determine this response. Consider the external forces, P, and the internal (nodal) forces, I, acting on a body (see Figure 8–8(a) and Figure 8–8(b), respectively). Figure 8–8 Internal and external loads on a body. The internal loads acting on a node are caused by the stresses in the elements that contain that node. For the body to be in static equilibrium, the net force acting at every node must be zero. Therefore, the basic statement of static equilibrium is that the internal forces, I, and the external forces, P, must balance each other: Abaqus/Standard uses the Newton-Raphson method to obtain solutions for nonlinear problems. In a nonlinear analysis the solution cannot be calculated by solving a single system of equations, as would be done in a linear problem. Instead, the solution is found by applying the specified loads gradually and incrementally working toward the final solution. Therefore, Abaqus/Standard breaks the simulation into a number of load increments and finds the approximate equilibrium configuration at the end of each load increment. It often takes Abaqus/Standard several iterations to determine an acceptable solution to a given load increment. The sum of all of the incremental responses is the approximate solution for the nonlinear analysis. Thus, Abaqus/Standard combines incremental and iterative procedures for solving nonlinear problems. Abaqus/Explicit determines a solution to the dynamic equilibrium equation without iterating by explicitly advancing the kinematic state from the previous increment. Solving a problem explicitly does not require the formation of tangent stiffness matrices. The explicit central-difference operator satisfies the dynamic equilibrium equations at the beginning of the increment, t; the accelerations calculated at time t are used to advance the velocity solution to time and the displacement solution to time . For linear and nonlinear problems alike, explicit methods require a small time increment size that depends solely on the highest natural frequency of the model and is independent of the type and duration of loading. Simulations typically require a large number of increments; however, due to the fact that a global set of equations is not solved in each increment, the cost per increment of an explicit method is much smaller than that of an implicit method. The small increments characteristic of an explicit dynamic method make Abaqus/Explicit well suited for nonlinear analysis. ・　8.2.1 Steps, increments, and iterations This section introduces some new vocabulary for describing the various parts of an analysis. It is important that you clearly understand the difference between an analysis step, a load increment, and an iteration. ​ The load history for a simulation consists of one or more steps. You define the steps, which generally consist of an analysis procedure option, loading options, and output request options. Different loads, boundary conditions, analysis procedure options, and output requests can be used in each step. For example: ​ Step 1: Hold a plate between rigid jaws. ​ Step 2: Add loads to deform the plate. ​ Step 3: Find the natural frequencies of the deformed plate. ​ An increment is part of a step. In nonlinear analyses the total load applied in a step is broken into smaller increments so that the nonlinear solution path can be followed. In Abaqus/Standard you suggest the size of the first increment, and Abaqus/Standard automatically chooses the size of the subsequent increments. In Abaqus/Explicit the default time incrementation is fully automatic and does not require user intervention. Because the explicit method is conditionally stable, there is a stability limit for the time increment. The stable time increment is discussed in Chapter 9, “Nonlinear Explicit Dynamics.” At the end of each increment the structure is in (approximate) equilibrium and results are available for writing to the output database, restart, data, or results files. The increments at which you select results to be written to the output database file are called frames. The issues associated with time incrementation in Abaqus/Standard and Abaqus/Explicit analyses are quite different, since time increments are generally much smaller in Abaqus/Explicit. ​ An iteration is an attempt at finding an equilibrium solution in an increment when solving with an implicit method. If the model is not in equilibrium at the end of the iteration, Abaqus/Standard tries another iteration. With every iteration the solution Abaqus/Standard obtains should be closer to equilibrium; sometimes Abaqus/Standard may need many iterations to obtain an equilibrium solution. When an equilibrium solution has been obtained, the increment is complete. Results can be requested only at the end of an increment. Abaqus/Explicit does not need to iterate to obtain the solution in an increment. ・ 8.2.2 Equilibrium iterations and convergence in Abaqus/Standard The nonlinear response of a structure to a small load increment, , is shown in Figure 8–9. Abaqus/Standard uses the structure's initial stiffness, , which is based on its configuration at , and to calculate a displacement correction, , for the structure. Using , the structure's configuration is updated to . Figure 8–9 First iteration in an increment. Convergence Abaqus/Standard forms a new stiffness, , for the structure, based on its updated configuration, . Abaqus/Standard also calculates , in this updated configuration. The difference between the total applied load, P, and can now be calculated as: where is the force residual for the iteration. If is zero at every degree of freedom in the model, point a in Figure 8–9 would lie on the load-deflection curve, and the structure would be in equilibrium. In a nonlinear problem it is almost impossible to have equal zero, so Abaqus/Standard compares it to a tolerance value. If is less than this force residual tolerance, Abaqus/Standard accepts the structure's updated configuration as the equilibrium solution. By default, this tolerance value is set to 0.5% of an average force in the structure, averaged over time. Abaqus/Standard automatically calculates this spatially and time-averaged force throughout the simulation. If is less than the current tolerance value, P and are in equilibrium, and is a valid equilibrium configuration for the structure under the applied load. However, before Abaqus/Standard accepts the solution, it also checks that the displacement correction, , is small relative to the total incremental displacement, . If is greater than 1% of the incremental displacement, Abaqus/Standard performs another iteration. Both convergence checks must be satisfied before a solution is said to have converged for that load increment. The exception to this rule is the case of a linear increment, which is defined as any increment in which the largest force residual is less than 10–8 times the time-averaged force. Any case that passes such a stringent comparison of the largest force residual with the time-averaged force is considered linear and does not require further iteration. The solution is accepted without any check on the size of the displacement correction. If the solution from an iteration is not converged, Abaqus/Standard performs another iteration to try to bring the internal and external forces into balance. This second iteration uses the stiffness, , calculated at the end of the previous iteration together with to determine another displacement correction, , that brings the system closer to equilibrium (point b in Figure 8–10). Figure 8–10 Second iteration. Abaqus/Standard calculates a new force residual, , using the internal forces from the structure's new configuration, . Again, the largest force residual at any degree of freedom, , is compared against the force residual tolerance, and the displacement correction for the second iteration, , is compared to the increment of displacement, . If necessary, Abaqus/Standard performs further iterations. For each iteration in a nonlinear analysis Abaqus/Standard forms the model's stiffness matrix and solves a system of equations. This means that each iteration is equivalent, in computational cost, to conducting a complete linear analysis. It should now be clear that the computational expense of a nonlinear analysis in Abaqus/Standard can be many times greater than for a linear one. It is possible with Abaqus/Standard to save results at each converged increment. Thus, the amount of output data available from a nonlinear simulation is many times that available from a linear analysis of the same geometry. Consider both of these factors and the types of nonlinear simulations that you want to perform when planning your computer resources. ・ 8.2.3 Automatic incrementation control in Abaqus/Standard Abaqus/Standard automatically adjusts the size of the load increments so that it solves nonlinear problems easily and efficiently. You only need to suggest the size of the first increment in each step of your simulation. Thereafter, Abaqus/Standard automatically adjusts the size of the increments. If you do not provide a suggested initial increment size, Abaqus/Standard will try to apply all of the loads defined in the step in the first increment. In highly nonlinear problems Abaqus/Standard will have to reduce the increment size repeatedly, resulting in wasted CPU time. Generally it is to your advantage to provide a reasonable initial increment size (see “Modifications to the model,” Section 8.4.1, for an example); only in very mildly nonlinear problems can all of the loads in a step be applied in a single increment. The number of iterations needed to find a converged solution for a load increment will vary depending on the degree of nonlinearity in the system. By default, if the solution has not converged within 16 iterations or if the solution appears to diverge, Abaqus/Standard abandons the increment and starts again with the increment size set to 25% of its previous value. An attempt is then made at finding a converged solution with this smaller load increment. If the increment still fails to converge, Abaqus/Standard reduces the increment size again. By default, Abaqus/Standard allows a maximum of five cutbacks of increment size in an increment before stopping the analysis. In Abaqus/Standard you can also specify the maximum number of increments allowed during the step. Abaqus/Standard terminates the analysis with an error message if it needs more increments than this limit to complete the step. The default number of increments for a step is 100; if significant nonlinearity is present in the simulation, the analysis may require many more increments. You specify an upper limit on the number of increments that Abaqus/Standard can use, rather than the number of increments it must use. In a nonlinear analysis a step takes place over a finite period of “time,” although this “time” has no physical meaning unless inertial effects or rate-dependent behavior are important. In Abaqus/Standard you specify the initial time increment, , and the total step time, . The ratio of the initial time increment to the step time specifies the proportion of load applied in the first increment. The initial load increment is given by The choice of initial time increment can be critical in certain nonlinear simulations in Abaqus/Standard, but for most analyses an initial increment size that is 5% to 10% of the total step time is usually sufficient. In static simulations the total step time is usually set to 1.0 for convenience, unless, for example, rate-dependent material effects or dashpots are included in the model. With a total step time of 1.0 the proportion of load applied is always equal to the current step time; i.e., 50% of the total load is applied when the step time is 0.5. Although you must specify the initial increment size in Abaqus/Standard, Abaqus/Standard automatically controls the size of the subsequent increments. This automatic control of the increment size is suitable for the majority of nonlinear simulations performed with Abaqus/Standard, although further controls on the increment size are available. Abaqus/Standard will terminate an analysis if excessive cutbacks caused by convergence problems reduce the increment size below the minimum value. The default minimum allowable time increment, , is 10–5 times the total step time. By default, Abaqus/Standard has no upper limit on the increment size, , other than the total step time. Depending on your Abaqus/Standard simulation, you may want to specify different minimum and/or maximum allowable increment sizes. For example, if you know that your simulation may have trouble obtaining a solution if too large a load increment is applied, perhaps