1、Lesson content:Viscous RegularizationModeling TechniquesAppendix 2: Cohesive Element Modeling Techniques60 minutesViscous Regularization (1/6)Cohesive elements have the potential to cause numerical difficulties in the following casesStiff cohesive behavior may lead to reduced maximum stable time inc

2、rement in Abaqus/ExplicitPotentially addressed through selective mass scalingUnstable crack propagation may lead to convergence difficulties in Abaqus/StandardPotentially addressed through built-in viscous regularization option specific to cohesive elementsViscous regularizationMaterial models with

3、damage often lead to severe convergence difficulties in Abaqus/StandardViscous regularization helps in such casesHelps make the consistent tangent stiffness of softening material positive for sufficiently small time incrementsSimilar approach used in the concrete damaged plasticity model in Abaqus/S

4、tandardViscous Regularization (2/6)Consistent material tangent stiffnessK0 is the undamaged elastic stiffnessf is a factor that depends on the details of the damage modelViscous regularization ensures that when , “Offending” second term is eliminated when the analysis cuts back drastically Viscous R

5、egularization (3/6)User interface for viscous regularization*COHESIVE SECTION, CONTROLS = control1*SECTION CONTROLS, NAME = control1, VISCOSITY = factorAdd-on transverse shear stiffness may provide additional stability*COHESIVE SECTION*TRANSVERSE SHEAR STIFFNESSOutputEnergy associated with viscous r

6、egularization: ALLCDViscous Regularization (4/6)Example: Multiple delamination problem (Alfano & Crisfield, 2001)Industry standard Alfano-Crisfield nonsymmetric delamination examplesPlies are initially bonded with predefined cracks, then peeled apart in a complex sequence Example done in Abaqus/Stan

7、dard and Abaqus/ExplicitEffect of viscous regularization is investigated10 layers12 layers2 layersInterface elementsInitial cracksa1a2a2LViscous Regularization (5/6)Viscous Regularization (6/6)Effect of viscous regularization on convergence of multiple delamination problem:Significant improvements w

8、ith small regularization factorViscous regularization factorTotal number of increments 0. 375 1.0e-4 171 2.5e-4 153 1.0e-3 164Modeling Techniques (1/28)Model problem: double-cantilever beamAlfano and Crisfield (2001)Pure Mode IDisplacement controlAnalyzed using 1D (B21), 2D (CPE4I), and 3D (C3D8I) e

9、lementsDelamination assumed to occur along a straight lineBeams: Orthotropic materialCohesive layer: Traction-separation with damageInitial cracku- uModeling Techniques (2/28)One-dimensional modelUse tie constraints between the cohesive layer and the beamsRequire distinct parts for the beam and cohe

10、sive zone geometryGeometryModeling Techniques (3/28)One-dimensional model (contd)AssemblyCreate 2 instances of the beam; one of the cohesive zonePosition the parts to leave gaps between them; this will later facilitate picking surfacesModeling Techniques (4/28)One-dimensional model (contd)Tie constr

11、aintsDefine tie constraints between mating surfaces. The cohesive side should be the slave surface (because it is a softer material)This approach is required when quadratic displacement elements are used.beam-topbeam-botcoh-topcoh-botModeling Techniques (5/28)One-dimensional model (contd)Properties:

12、 beamModeling Techniques (6/28)One-dimensional model (contd)Properties: adhesiveModeling Techniques (7/28)One-dimensional model (contd)MeshingFor two-dimensional geometry, use sweep meshable regions for cohesive elementsSweep path must be aligned with thickness directionAssign seeds and meshOnly one

13、 element through the thicknessAssign cohesive element type to the swept region321Modeling Techniques (8/28)One-dimensional model (contd)Meshing (contd)Edit the nodal coordinates of each part instance so that they all have the same 2-coordinateFinal mesh4Toggle this off; otherwise, nodes will project

14、 back to their original positionsModeling Techniques (9/28)Two-dimensional modelAll geometry is 2D and planarProperties, attributes, etc. treated in a similar manner to the 1D case presented earlierModeling options include:Shared nodesTie constraintsSimilar to the 1D modelModeling Techniques (10/28)

15、Two-dimensional model (contd)Shared nodesDefine a finite thickness slit in the beam as shown belowUse the actual overall thickness of the DCBThe center region represents the cohesive layerMesh the part:12Modeling Techniques (11/28)Two-dimensional model (contd)Shared nodes (contd)Edit the coordinates

16、 of the nodes along the interface3Modeling Techniques (12/28)Two-dimensional model (contd)Tie constraintsCreate two instances of the beams and position them as shown below.Suppress the visibility of the instances to facilitate picking surfaces, etc.Create a finite thickness cohesive layer, position

17、it appropriately in the horizontal direction, define surfaces, etc. After meshing, adjust the coordinates of all the nodes in the cohesive layer so that they lie along the interface between the two beams.12Modeling Techniques (13/28)Three-dimensional modelAll geometry is 3DSolid geometry for beamsSo

18、lid or shell geometry for cohesive layerModeling options includeShared nodesTie constraintsModeling Techniques (14/28)Three-dimensional model (contd)Shared nodesPartition the geometry and define a mesh seam between these two faces1Modeling Techniques (15/28)Three-dimensional model (contd)Shared node

19、s (contd)Mesh the part with solid (continuum) elements.Create a orphan meshMeshCreate Mesh Part32Modeling Techniques (16/28)Create a single zero-thickness solid layer by offsetting from the midplane (selected by angle) of the orphan mesh created in the previous stepTip 2: Use the selection options t

20、ools to facilitate picking. In particular, select from interior entities.Create a set for the new layer so you can easily assign element type and section properties.Tip 1: Remove elements from top region with display groups (select by angle)4Modeling Techniques (17/28)Three-dimensional model (contd)

21、Shared nodes (contd)Assign section properties and the element type to the set created in the previous step5Modeling Techniques (18/28)Three-dimensional model (contd)Tie constraintsThe cohesive region can be defined asSolid (with finite thickness)Edit nodal coordinates of cohesive elements as in prev

22、ious examplesShell geometryMesh geometry then create orphan meshOffset a zero-thickness layer of solid elements from the orphan meshDefine surfaces automatically to facilitate tie constraintsModeling Techniques (19/28)Three-dimensional model (contd)Tie constraints (contd)When defining the tie constr

23、aints, query the mesh stack direction to determine when the “top” and “bottom” surfaces should be usedBrown = top Purple = bottomModeling Techniques (20/28)What if I dont use Abaqus/CAE?In this case do the following in the preprocessor of your choice:Generate the mesh for the structure and cohesive

24、layer (temporarily assigning an arbitrary element type to the cohesive layer)Position the layer of cohesive elements over the interfaceDefine surfaces on the structure and cohesive layerWrite the input fileSurface top-beamSurface bot-beamSurface top-cohSurface bot-cohModeling Techniques (21/28)Edit

25、the input file:Change the element type assigned to the cohesive layerAssign cohesive section properties*element, elset=coh, type=coh2d4*cohesive section, elset=coh, material=cohesive, response=traction separation, stack direction=2, controls=visco 1.0, 0.02 :*material, name=cohesive*elastic, type=tr

26、action 5.7e+14, 5.7e+14, 5.7e+14*damage initiation, criterion=quads 5.7e7, 5.7e7, 5.7e7*damage evolution, type=energy, mixed mode behavior=bk, power=2.284 280.0, 280.0, 280.0Modeling Techniques (22/28)The stack direction defines the thickness direction based on the element isoparametric directions.S

27、et STACK DIRECTION = 1 | 2 | 3 to define the element thickness direction along an isoparametric direction.2D example (extends to 3D):Thickness directionElement connectivity: 101, 102, 202, 201Stack direction = 2Element connectivity: 102, 202, 201, 101Stack direction = 11012012021021210120120210212Mo

28、deling Techniques (23/28)Edit the input file (contd):Define tie constraints between the surfaces*tie, name=top, adjust=yes, position tolerance=0.002top-coh, top-beam*tie, name=bot, adjust=yes, position tolerance=0.002bot-coh, bot-beamSetting adjust=yes will force Abaqus to move the slave (cohesive e

29、lement) nodes onto the master surface. By adjusting both the top and bottom cohesive surfaces in this way, a zero-thickness cohesive layer is produced.The position tolerance should be large enough to contain the slave nodes when measured from the master surface. In this case the overclosure is equal

30、 to 0.0015 on either side of the interface so a position tolerance of 0.002 is sufficient to capture all slave nodes.0.0015Cohesive surface is the slaveModeling Techniques (24/28)ResultsModeling Techniques (25/28)Effect of viscous regularizationViscous regularization factorTotal number of increments 1.e-5 636 2.5e-5