Convergence Problems: Element Behavior
Lecture 6
L6.2
Overview
? Hourglassing in Reduced-Integration Elements ? Checkerboarding ? Ill-Conditioning
O
btaining a Converged Solution with Abaqus
163
Hourglassing in Reduced-Integration Elements
L6.4
Hourglassing in Reduced-Integration Elements
? Full integration vs. reduced-integration elements ? In elastic finite element analysis the strain energy density must be integrated over the element volume to obtain the element stiffness matrix. ? Full integration refers to the minimum Gauss integration order required for exact integration of the strain energy (if the element is not distorted). ? Reduced integration refers to a Gauss integration rule of one order less than full integration. ? The reduced integration method can be used only in quadrilateral and hexahedral elements.
Obtaining a Converged Solution with Abaqus
164
L6.5
Hourglassing in Reduced-Integration Elements
? What is hourglassing? ? The use of the reduced-integration scheme has a drawback: it can result in mesh instability, commonly referred to as “hourglassing.” ? Consider a rectangular plate simply supported along two edges. ? The hourglass mode does not cause any strain and, hence, does not contribute to the energy integral. ? It behaves in a manner that is similar to that of a rigid body mode.
Obtaining a Converged Solution with Abaqus
L6.6
Hourglassing in Reduced-Integration Elements
? The hourglass mode in second-order “serendipity” (8-node) elements (CPS8R, CPE8R) is nonpropagating. ? Neighboring elements cannot share the mode, so the mode cannot occur in a mesh with more than two elements.
? There is no real danger of hourglassing in these elements.
Obtaining a Converged Solution with Abaqus
165
L6.7
Hourglassing in Reduced-Integration Elements
? Hourglass modes of first-order reduced-integration quadrilateral and hexahedral elements can propagate; therefore, hourglassing can be a serious problem in those elements. ? To suppress hourglassing, an artificial “hourglass control” stiffness must be added.
? Abaqus uses hourglass control in all first-order reduced-integration elements.
Obtaining a Converged Solution with Abaqus
L6.8
Hourglassing in Reduced-Integration Elements
? General comments ? Hourglassing is mainly an issue with first-order reduced-integration quad/hex elements. ? Regular triangular and tetrahedral elements in Abaqus always use full integration and, hence, are not susceptible to hourglassing. ? Hourglassing can occur in geometrically linear and geometrically nonlinear problems, including finite-strain problems.
? In geometrically linear problems hourglassing usually does not affect the quality of the calculated stresses.
Obtaining a Converged Solution with Abaqus
166
L6.9
Hourglassing in Reduced-Integration Elements
? In geometrically nonlinear analysis the hourglass modes tend to interact with the strains at the integration points, leading to inaccuracy and/or instability.
? Hourglassing is particularly troublesome for problems involving finite-strain elasticity (hyperelasticity) or very large (incompressible) plastic deformations.
? Fully integrated elements are strongly recommended, whenever feasible, for finite-strain elasticity analysis. ? When hourglassing is creating convergence problems, the simulation will often have many diverging solution cutbacks.
Obtaining a Converged Solution with Abaqus
L6.10
Hourglassing in Reduced-Integration Elements
? When is hourglassing a problem? ? Hourglassing is almost never a problem with the enhanced hourglass control available in Abaqus. ? More robust than other schemes ? No user-set parameters ? Based on enhanced strain methods
Rubber disk rolling against rigid drum
load disk
roll drum
load disk
ALLAE
Comparison of energy histories
Obtaining a Converged Solution with Abaqus
roll drum
Combined hourglass control scheme
ALLIE ALLIE
Enhanced hourglass control scheme
ALLAE
167
L6.11
Hourglassing in Reduced-Integration Elements
? Currently, enhanced hourglass control is not the default scheme for most elements. ? The following table summarizes the hourglass control methods currently available in Abaqus, including the default schemes for most elements:
Abaqus/Standard
Stiffness (default)
Abaqus/Explicit
Relax stiffness (default)
Enhanced strain
Enhanced strain
Stiffness Viscous Combined (stiffness+viscous)
? But…enhanced strain hourglass control is the default for: ? All modified tri and tet elements ? All elements modeled with finite-strain elastic materials (hyperelastic, hyperfoam, and hysteresis)
Obtaining a Converged Solution with Abaqus
L6.12
Hourglassing in Reduced-Integration Elements
? To activate enhanced hourglass control, use the option
*SOLID SECTION, CONTROLS=name, ELSET=elset *SECTION CONTROLS, NAME=name, HOURGLASS=ENHANCED
No user parameters ? Abaqus/CAE usage:
Mesh module: Mesh→Element Type
Obtaining a Converged Solution with Abaqus
168
L6.13
Hourglassing in Reduced-Integration Elements
? Detecting and controlling hourglassing ? Hourglassing can usually be seen in deformed shape plots. ? Example: Coarse and medium meshes of a simply supported beam with a center point load. ? Excessive use of hourglass control energy can be verified by looking at the energy histories. ? Verify that the artificial energy used to control hourglassing is small ( 1 ) relative to the internal energy.
Same load and displacement magnification (1000×)
Obtaining a Converged Solution with Abaqus
L6.14
Hourglassing in Reduced-Integration Elements
? Use the X–Y plotting capability in Abaqus/Viewer to compare the energies graphically.
Internal energy
Internal energy
Artificial energy
Artificial energy
Two elements through the thickness: Ratio of artificial to internal energy is 2 .
Four elements through the thickness: Ratio of artificial to internal energy is 0.1 .
Obtaining a Converged Solution with Abaqus
169
L6.15
Hourglassing in Reduced-Integration Elements
? Example: Engine mount ? Consider two forms of hourglass control: ? Stiffness-based ? Enhanced strain
rubber
steel
Outer rim moves up under load control
1
DISPLACEMENT MAGNIFICATION FACTOR = 1.00
ORIGI
2
3
RESTART FILE = a
STEP 1
INCREMENT 20 .267 TOTAL ACCUMULATED TIME TIME: 13:16:10 DATE: 15-MAY-97
TIME COMPLETED IN THIS STEP ABAQUS VERSION: 5.6-4
Obtaining a Converged Solution with Abaqus
L6.16
Hourglassing in Reduced-Integration Elements
? Results with stiffness hourglass control
1
DISPLACEMENT MAGNIFICATION FACTOR = 1.00 TOTAL ACCUMULATED TIME TIME: 13:16:10 .267
2
3
Nonconvergence at 27
of load
Severe hourglassing occurs
TIME COMPLETED IN THIS STEP ABAQUS VERSION: 5.6-4 .267 DATE: 15-MAY-97
RESTART FILE = a
STEP 1
INCREMENT 20
GNIFICATION FACTOR = STEP 1
1.00
ORIGINAL MESH Obtaining a DISPLACED MESH Converged Solution with Abaqus .267
a
IN THIS STEP
170
INCREMENT 20 .267 TOTAL ACCUMULATED TIME
L6.17
Hourglassing in Reduced-Integration Elements
? Results with enhanced hourglass control
1
DISPLACEMENT MAGNIFICATION FACTOR = 1.00 TOTAL ACCUMULATED TIME TIME: 13:26:19 1.00
2
3
RESTART FILE = a2
TIME COMPLETED IN THIS STEP ABAQUS VERSION: 5.6-4
Deformation at 100 of load; rubber uses default enhanced hourglass control
No hourglassing
1.00 DATE: 15-MAY-97
STEP 1
INCREMENT 13
GNIFICATION FACTOR = STEP 1 1.00
1.00
ORIGINAL MESH Obtaining a DISPLACED MESH Converged Solution with Abaqus 1.00
a2
INCREMENT 13 TOTAL ACCUMULATED TIME TIME: 13:26:19
IN THIS STEP 5.6-4
DATE: 15-MAY-97
L6.18
Hourglassing in Reduced-Integration Elements
? Elastic bending problems and coarse mesh accuracy ? For elastic bending problems, improved coarse mesh accuracy may be obtained using the enhanced hourglass control method. ? The enhanced hourglass control formulation is tuned to give accurate results for regularly shaped elements undergoing elastic bending. ? Where these conditions apply, a coarse mesh may give acceptable results despite the artificial energy being greater than a few percent of the internal energy. ? An independent check of the results should be made to determine if they are acceptable.
Obtaining a Converged Solution with Abaqus
171
L6.19
Hourglassing in Reduced-Integration Elements
? Plastic bending problems ? When plasticity is present, the stiffness-based hourglass control causes elements to be less stiff than in the enhanced control case. ? This may give better results with plastic bending; enhanced hourglass control may cause delayed yielding or excessive springback. ? In using enhanced hourglass control in this case, the usual rule-ofthumb regarding the acceptable level of artificial energy should be followed. ? Recall that C3D10M elements use enhanced hourglass control by default. ? Use alternative hourglass control for problems involving yielding.
Obtaining a Converged Solution with Abaqus
Checkerboarding
172
L6.21
Checkerboarding
? Whereas hourglassing is a behavior where large, oscillating displacements occur without significant stresses, checkerboarding is a behavior where large, oscillating stresses occur without significant displacements. ? Checkerboarding typically occurs for hydrostatic stresses in (almost) incompressible materials that are highly confined. ? It can occur in first- and second-order elements but is most notable in first-order elements. ? It is more likely to occur in regular meshes than in irregular meshes.
Obtaining a Converged Solution with Abaqus
L6.22
Checkerboarding
? Checkerboarding is related to—but is not the same as—volumetric locking. ? Volumetric locking occurs when incompressible material behavior puts more constraints on the deformation field then there are displacement degrees of freedom. ? For example, in a refined, three-dimensional mesh of 8-node hexahedra, there is—on average—1 node with 3 degrees of freedom per element. ? The volume at each integration point must remain fixed. Since full integration uses 8 points per element, we have as many as 8 constraints per element but only 3 degrees of freedom. ? Consequently, the mesh is overconstrained—it locks.
? Volumetric locking can be avoided by using the proper element type; for a more detailed discussion of this topic see the “Element Selection in Abaqus” lecture notes.
Obtaining a Converged Solution with Abaqus
173
L6.23
Checkerboarding
? Checkerboarding does not always manifest itself clearly. ? The displacement field may initially be unaffected, and stress contour plots may not show the checkerboarding because of smoothing of element stresses during postprocessing. ? Discontinuous or “quilt” plots will show the checkerboard pattern, however. ? In linear analyses checkerboarding rarely causes convergence difficulties. ? However, in nonlinear analyses the high hydrostatic stress oscillations can eventually interact with the displacements and cause sudden, usually catastrophic, convergence problems. ? Checkerboarding can be eliminated by introducing some local mesh irregularities.
Obtaining a Converged Solution with Abaqus
L6.24
Checkerboarding
? Example: Rubber bushing ? Consider a cylindrical rubber bushing made of an (almost) incompressible rubber. ? The bushing is modeled with first-order, generalized plane strain elements. ? Both the inner and outer radius of the bushing are fully constrained. ? This constraint severely limits the deformations that can occur in the model. ? A compressive axial load is applied to the bushing through the element reference node.
Obtaining a Converged Solution with Abaqus
174
L6.25
Checkerboarding
? In this model the element indicated in the figure is given a bulk modulus that is one order-of-magnitude smaller than that assigned to the rest of the elements in the mesh. ? This should lead to a smaller hydrostatic pressure in this element.
smaller K
Obtaining a Converged Solution with Abaqus
L6.26
Checkerboarding
? A “quilt” contour plot (without averaging between elements) clearly shows a “checkerboard” pattern with a significant pressure variation.
Quilt (nonaveraged) contour plot of hydrostatic pressure
Obtaining a Converged Solution with Abaqus
175
Ill-Conditioning
L6.28
Ill-Conditioning
? When elements or materials show large stiffness differences, conditioning problems may occur. ? In linear analyses problems typically occur only when the stiffness differences are extreme (factors of 106 or more). ? In such cases the solution of the linear equation system becomes inaccurate. ? In nonlinear analyses problems occur at a much earlier stage.
? The stiffness differences may cause poor convergence or even divergence if the increment size is not very small.
Obtaining a Converged Solution with Abaqus
176
L6.29
Ill-Conditioning
? Long, slender or rigid structures ? Large differences in stiffness occur in long, slender structures (such as very long pipes or cables) or very stiff structures (such as a link in a vehicle’s suspension system). ? If such structures undergo large motions in geometrically nonlinear analyses, convergence can be very difficult to obtain. ? Slight changes in nodal positions can cause very large (axial) forces that, in turn, cause incorrect stiffness contributions. ? This makes it very difficult or impossible for the usual finite element displacement method to converge. ? Convergence problems in these simulations usually manifest themselves in very slow or irregular convergence rates or in diverging solutions.
Obtaining a Converged Solution with Abaqus
L6.30
Ill-Conditioning
? Use hybrid beam elements (types B21H, B31H, B31OSH) or hybrid truss elements to model such problems. ? In these hybrid elements the axial and, in the case of hybrid beams, the transverse shear forces in the elements are included as primary variables in the element formulation ? Because the forces are primary variables, they remain reasonably accurate during iteration, and the elements usually converge faster. ? Even though the additional primary variables make these elements more expensive per iteration, they are usually much more efficient because the improved convergence rate reduces the number of iterations.
Obtaining a Converged Solution with Abaqus
177
L6.31
Ill-Conditioning
? Example: Near bottom pipeline pull-in and tow ? Simulating a seabed pipeline installation. ? Drag chains used to offset buoyancy effects. ? Model:
? Pipeline modeled using beam elements.
? Pipeline is very slender. ? One end of the pipeline is winched into an anchor point. ? The other end is built in for the pull-in and free for the tow.
Pipeline dimensions: Length = 1000 ft Outer diameter = 0.75 ft Wall thickness = 0.025 ft
Obtaining a Converged Solution with Abaqus
L6.32
Ill-Conditioning
? Pull-in analysis ? The job with hybrid elements converges significantly faster than the job without hybrid elements.
Element type B33H B33
Number of increments 26 28
Number of cutbacks 2 1
Number of iterations 99 151
Obtaining a Converged Solution with Abaqus
178
L6.33
Ill-Conditioning
? Tow analysis
? The pipeline has no restraint (and is, therefore, singular) until the drag chain extends sufficiently to stabilize the pipeline.
INCREMENT 1 STARTS. ATTEMPT NUMBER 1, TIME INCREMENT 1.000E-02 ***WARNING: SOLVER PROBLEM. NUMERICAL SINGULARITY WHEN PROCESSING NODE 3 D.O.F. 6 RATIO = 7.26788E+15 ***WARNING: THE SYSTEM MATRIX HAS 1 NEGATIVE EIGENVALUES.
? To overcome numerical difficulties in the early stages of the analysis, a small initial stress is applied to the pipeline:
*INITIAL CONDITIONS,TYPE=STRESS BEAMS,1.E-8
Element type B33H B33
Number of increments 26 37
Number of cutbacks 0 2
Number of iterations 182 323
Obtaining a Converged Solution with Abaqus
L6.34
Ill-Conditioning
? Approximately incompressible material behavior ? If the bulk modulus, K, is much larger than the shear modulus, G, large stiffnesses occur inside an element. ? Slight changes in nodal positions can cause very large volumetric strains and, as a result, large hydrostatic stresses. ? The large hydrostatic stresses cause incorrect stiffness contributions, which seriously hamper convergence.
? This effect is particularly seen with hyperelastic materials.
Obtaining a Converged Solution with Abaqus
179
L6.35
Ill-Conditioning
? Use hybrid solid elements (types CPE4H, C3D20H, CAX4H, etc.) in such cases. ? In these elements the hydrostatic pressure (or in some cases the volume change) is included as a primary variable in the element formulation. ? Consequently the hydrostatic stresses (and, thus, the effective stiffness) remain reasonably accurate during the iteration process. ? Although the cost per iteration increases due to the additional degrees of freedom, the overall analysis cost typically is reduced because a smaller number of iterations will be needed. ? An exception is the modified 10-node tetrahedral elements (C3D10MH). ? For these elements the cost per iteration increases significantly.
Obtaining a Converged Solution with Abaqus
180