当前位置:首页 >> 机械/仪表 >>

Obtaining a Converged Solution with Abaqus


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


相关文章:
ABAQUS初学者入门导读之一
with ABAQUS Linear and Nonlinear Dynamics with ABAQUS Metal Forming with ABAQUS Metal Inelasticity in ABAQUS Obtaining a Converged Solution with ABAQUS Rubber ...
Abaqus接触分析中出现收敛困难时的常用检查方法(免费)
Abaqus接触分析中出现收敛困难时的常用检查方法(免费)_机械/仪表_工程科技_专业...obtaining a converged contact solution in Abaqus/Standard 2011/05/25 / q"...
Abaqus接触分析中出现收敛困难时的常用检查方法(经典)
1、ABAQUS 接触分析的收敛问题常用检查方法 接触分析收敛不管怎么总还是一个很大...obtaining a converged contact solution in Abaqus/Standard 2011/05/25 / q"...
ABAQUS收敛问题
ABAQUS收敛问题_数学_自然科学_专业资料。[转载][转帖]abaqus 接触分析问题整理...***NOTE: THE SOLUTION APPEARS TO BE DIVERGING. CONVERGENCE IS JUDGED ...
ABAQUS分析收敛控制
Input File Usage: Abaqus/CAE Usage: *CONTROLS, RESET Step module: Other General Solution Controls Edit: toggle on Reset all parameters to their system-...
abaqus分析收敛的个人经验整理
abaqus 分析收敛的个人经验整理 说一下自己在分析收敛方面的一些经验 " X& ?8...( a; `& F. i m4 d- E Q I2 J: ***NOTE: THE SOLUTION APPEARS ...
ABAQUS技巧积累
ABAQUS技巧积累_工学_高等教育_教育专区。ABAQUS是一套功能强大的工程模拟的...if not, please use the solution controls to reset the criterion for zero ...
错误提示及解决方法
Returned solution The solution returned by the stationary solver is not has not converged. to be trusted. It might, however, be useful as initial guess...
使用ANSYS碰到得问题
GUI 方式则按下列步骤进行: 1.选择菜单路径 Main Menu>Solution>Analysis Options,弹出 Modal Analysis 对话框; = n m”,n 和 m 是整数,表示某阶模态被漏掉...
使用ANSYS碰到得问题
GUI 方式则按下列步骤进行: 1.选择菜单路径 Main Menu>Solution>Analysis Options,弹出 Modal Analysis 对话框; = n m”,n 和 m 是整数,表示某阶模态被漏掉...
更多相关标签:
abaqus map solution | converged | hyperconverged | hyper converged | obtaining | unconverged | obtaining ip address | converged revenue |