Recomendados
Más contenido relacionado
La actualidad más candente
La actualidad más candente (20)
Similar a Explore Abaqus-Explicit Techniques.pdf
Similar a Explore Abaqus-Explicit Techniques.pdf (20)
Último
Último (20)
Explore Abaqus-Explicit Techniques.pdf
- 1. 1 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Explore Abaqus/Explicit Techniques Yogesh Parkhi Technical Specialist, SIMULIA India
- 2. 2 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Presentation content Abaqus/Explicit – What? When? Why? Applications of Abaqus/Explicit Defining Abaqus/Explicit procedure Quasi-Static Simulations using Explicit Dynamics Advanced Capabilities in Abaqus/Explicit Arbitrary Lagrangian-Eulerian (ALE) Method SIMULIA Multiphysics – FSI capabilities Managing large models Simplifying the Model Techniques for Reducing CPU Time Tips Summary
- 4. 4 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 What is Explicit Dynamics? Explicit dynamics is a mathematical technique for integrating the equations of motion through time. The dynamic equilibrium equations are written for convenience with the inertial forces isolated from the other forces. These equilibrium equations are completely general. They apply to the behavior of any mechanical system and contain all nonlinearities (large deformations, nonlinear material response, contact). When the first term—the inertial or dynamic force—is small enough, the equations reduce to the static form of equilibrium. I P u M
- 5. 5 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 What is Explicit Dynamics? 1 ( ) ( ) ( ) t t , u M P I The explicit dynamic integration method is also known as the forward Euler or central difference algorithm. Unknown values are obtained from information already known. The lumped mass matrix, M, allows the program to calculate the nodal accelerations easily at any given time, t, using the following expression: where P is the external load vector and I is the internal load vector.
- 6. 6 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 When should Abaqus/Explicit be used? The deciding factor when choosing between Abaqus/Standard and Abaqus/Explicit is often the smoothness of the solution. It may not be possible to obtain an efficient solution with Abaqus/Standard if there are significant discontinuities in the solution. Possible sources of discontinuity in a solution: Impact Buckling or local wrinkling of the material Material degradation or failure, such as cracking of concrete A large three-dimensional model that contains one or more of the discontinuities listed above is a good candidate for Abaqus/Explicit.
- 7. 7 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Why use Abaqus/Explicit? It expands the range of problems you can address Abaqus/Explicit contains many modeling capabilities that do not exist in Abaqus/Standard. For example, Coupled Eulerian-Lagrangian (CEL) analysis, Smoothed Particle Hydrodynamics (SPH), Discrete Element Method (DEM) It is easy to learn The basic input structure and options for an Abaqus/Explicit model are the same as those for an Abaqus/Standard model.
- 9. 9 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Applications of Abaqus/Explicit Abaqus/Explicit provides the capability to analyze the following types of problems: High-speed (short duration) dynamics Drop tests and crash analyses of structural members Large, nonlinear, quasi-static analyses Deep drawing, blow molding, and assembly simulations Extreme deformations, Bulk metal forming, impact and crushing, and fluid flow Courtesy Mechanical Design and Analysis Corporation, 2010 SCC
- 11. 11 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Defining Abaqus/Explicit Procedure An Abaqus/Explicit analysis is performed when the model contains any of the following procedure options: *DYNAMIC, EXPLICIT an explicit dynamics step *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT a coupled thermo-mechanical explicit dynamics step *ANNEAL annealing procedure
- 12. 12 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Defining Abaqus/Explicit Procedure For the majority of Abaqus/Explicit analyses only the total step time needs to be specified. Time increment size is chosen automatically so that it always satisfies the stability limit. *STEP *DYNAMIC, EXPLICIT , ttotal
- 13. 13 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Stable Time Increment Defining Abaqus/Explicit Procedure The explicit procedure integrates through time by using many small time increments. The stability limit can be defined in terms of the highest eigenvalue in the model (max) and the fraction of critical damping () in the highest mode A bounded solution is obtained only when the time increment (Dt) is less than the stable time increment (Dtmin). If Dt Dtmin, the solution will be unstable and oscillations will occur in the model’s response. 2 min max 2 ( 1 ) t .
- 14. 14 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Stable Time Increment Defining Abaqus/Explicit Procedure The stable time increment can be expressed as Decreasing Le and/or increasing cd will reduce the size of the stable time increment. Decreasing element dimensions reduces Le. Decreasing material density increases cd. Increasing material stiffness increases cd. e d L t c . d E c ,
- 15. 15 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Stable Time Increment Defining Abaqus/Explicit Procedure Example: Compression of a jounce bumper Abaqus/Explicit writes a report to the status (.sta) file during the datacheck phase of the analysis. The initial stable time increments listed do not include damping (bulk viscosity) or mass scaling effects. Initial time increment = 5.09466E-04 Statistics for all elements: Mean = 1.53743E-03 Standard deviation = 3.20027E-04 Most critical elements : Element number Rank Time increment Increment ratio (Instance name) ---------------------------------------------------------- 485 1 5.094664E-04 1.000000E+00 230 2 5.213121E-04 9.772771E-01 224 3 5.219781E-04 9.760302E-01 . . . 185 10 5.687587E-04 8.957514E-01 jounce bumper critical elements
- 16. 16 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Contact in Abaqus/Explicit Defining Abaqus/Explicit Procedure The explicit integration method efficiently solves extremely discontinuous events. Contact is an extremely discontinuous form of nonlinearity. Possible to solve complicated, very general, three-dimensional contact problems with deformable bodies in Abaqus/Explicit. * Gholami, T., J. Lescheticky, and R. Paßmann, “Crashworthiness Simulation of Automobiles with ABAQUS/Explicit,” ABAQUS Users' Conference, Munich, 2003.
- 17. 17 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Contact in Abaqus/Explicit Defining Abaqus/Explicit Procedure The general contact algorithm is usually faster than the contact pair algorithm and is geared toward models with multiple components and complex topology. invoked by using the keywords: *CONTACT *CONTACT INCLUSIONS, ALL EXTERIOR Other features unique to the general contact algorithm include: Contact domains span multiple bodies, including both rigid and deformable bodies Edge-to-edge contact for perimeter edges, geometric feature edges, beams, and trusses Wire crimping
- 19. 19 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Quasi-Static Simulations using Explicit Dynamics Challenging nonlinear quasi-static problems often involve: Very complex contact conditions Very large deformations Mesh distortion possible Applications: Metal forming simulations: Bulk forming (drawing, rolling, extrusion, upsetting, etc.) Sheet metal forming (stretching, drawing) Rolling of a symmetric I-section
- 20. 20 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Quasi-Static Simulations using Explicit Dynamics Two approaches to obtain an economical quasi-static solutions with an explicit dynamics solver Increased load rates Artificially reduce the time scale of the process by increasing the loading rate. Material strain rates calculated in the simulation are artificially high by the same factor applied to increase the loading rate. Mass scaling Mass scaling allows you to model processes in their natural time scale when considering rate- sensitive materials. How much can I increase the load rate or scale the mass? Increased load rates and mass scaling achieve the same effect Increased load rates reduce the time scale of the simulation. Mass scaling increases the size of the stable time increment.
- 21. 21 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Check for Quasi-Static Analyses Quasi-Static Simulations using Explicit Dynamics Examination of the energy content provides measure to evaluate whether the results from an Abaqus/Explicit simulation reflect a quasi-static solution. The kinetic energy of the deforming material should not exceed a small fraction of its internal energy throughout the majority of a quasi-static analysis. A small fraction typically means 1–5%. Not interested in kinetic energy of rigid bodies. Subtract their contribution from global model kinetic energy or restrict energy output to deforming components.
- 22. 22 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Example: Deep drawing of a square box Quasi-Static Simulations using Explicit Dynamics We examine three different punch speeds: 3 m/s 30 m/s 150 m/s The computation cost of each deep drawing simulation is summarized in the following table: Punch speed (m/s) Time increments Normalized CPU time 3 (1) 27929 1.0 30 (10) 2704 0.097 150 (50) 529 0.019 Initial configuration for square box deep drawing
- 23. 23 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Vpunch = 3 m/s Vpunch = 30 m/s Vpunch = 150 m/s Example: Deep drawing of a square box Quasi-Static Simulations using Explicit Dynamics Contours of blank thickness in final formed configuration Excessive punch speeds lead to results that do not correspond to the physics. At 150 m/s unrealistic thinning of the blank is predicted. Results obtained at 30 m/s and 3 m/s are very similar, even though the difference in computation cost is a factor of 10.
- 24. 24 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Example: Deep drawing of a square box Quasi-Static Simulations using Explicit Dynamics Comparison of internal and kinetic energies At a punch speed of 150 m/s the kinetic energy of the blank is a significant fraction of its internal energy. At punch speeds of 3 m/s and 30 m/s the kinetic energy is only a small fraction of the internal energy over the majority of the forming process history.
- 26. 26 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Arbitrary Lagrangian-Eulerian (ALE) Method Motivation In many nonlinear simulations, the material in the structure undergoes very large deformations. These deformations distort the finite element mesh, often to the point where the mesh is unable to provide accurate results or the analysis terminates for numerical reasons. In such simulations it is necessary to use adaptive meshing tools to periodically minimize the distortion in the mesh. without adaptive meshing with adaptive meshing Forming of a steel part
- 27. 27 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Arbitrary Lagrangian-Eulerian (ALE) Method The primary characteristics of the ALE adaptive meshing capability are: A smoother mesh is generated at regular intervals to reduce element distortion and to maintain good element aspect ratios. The same mesh topology is maintained—the number of elements and nodes and their connectivity do not change. The ALE adaptive meshing algorithm in Abaqus/Explicit is not designed to correct discretization errors in finite element meshes.
- 28. 28 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Arbitrary Lagrangian-Eulerian (ALE) Method Example: Axisymmetric forging problem with adaptive meshing Interior nodes adaptively adjust in all directions Nodes along the free boundary move with the material in the direction normal to the material’s surface. They are allowed to adapt (adjust their position) tangent to the free surface. ALE Simulation Deformed meshes at 70% of die travel Lagrangian Simulation
- 29. 29 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Smoothed Particle Hydrodynamics (SPH) analyses Smoothed Particle Hydrodynamics is a very general approach to the simulation of bulk matter in motion. SPH addresses modeling needs in cases where traditional methods (FEM, FDM) fail or are inefficient: Extremely violent fluid flows where mesh or grid-based CFD cannot cope (free surface) Extremely high deformations/obliteration where CEL is inefficient and Lagrangian FEM is difficult Its use can be extended to the simulation of: Fracture of brittle solids Metal forming High (or hyper) velocity impact (HVI) Liquid spraying through a hose Water fall under gravity Turbofan blade bird strike
- 30. 30 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Coupled Eulerian-Lagrangian (CEL) analyses An Eulerian solution is another option for problems involving significant material flow. Coupled Eulerian-Lagrangian (CEL) Approach: An Eulerian mesh and a Lagrangian mesh are assembled in the same model Interactions between Lagrangian bodies and materials in the Eulerian mesh are enforced with a general contact definition Water Drop Simulation Tank Sloshing
- 31. 31 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Discrete Element Method (DEM) DEM is intended for modeling events in which large numbers of discrete particles contact each other New method for analysis of non-continuous media Granular material, material handling, shot peening, etc. Agriculture, pharmaceutical, oil and gas, mining
- 33. 33 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Introduction What is a Large Model? Difficult to define Absolute size changes as computers become more powerful. Rough measures for large models based on number of variables: 1980: Models with >100,000 variables 1990: Models with >1,000,000 variables 2000: Models with >5,000,000 variables Turn-around time is a universal measure This measure includes jobs with relatively few variables and a huge number of increments. Models that take at least 12 hours (overnight) to run are generally considered “large”.
- 34. 34 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Introduction Large models often require: Simplification of the model geometry, physics, element formulation, etc. Intelligent use of system resources: disk space, available processors, memory Minimization of CPU time, number of increments, etc. Several techniques are available to assist in the management of large models: Submodeling Restart
- 35. 35 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Simplifying the Model Geometry simplification When building a complex model, start simple (and small), then add complexity gradually. Making careful choices regarding your geometry and mesh: Take advantage of symmetry axial, planar, quarter, half, cyclic,… Defeature the geometry Avoid small features They result in small elements which in turn reduce the stable time increment. Defeaturing a mechanical component
- 36. 36 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Simplifying the Model Modeling fewer details Consider what you want from the analysis and reduce the level of modeling detail in regions that are less critical to the analysis goals. For example: If you have two parts connected to each other and if you are not interested in detailed stresses of the connection, use connector elements. Use beams or shells instead of solids when appropriate. Focus mesh in regions of interest and use a coarser mesh elsewhere. Simplify the physics. Can a stiff portion of an assembly be replaced with a rigid body or a boundary condition? Do you need all interactions?
- 37. 37 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Simplifying the Model Prototype with rigid bodies Make deformable parts rigid with a rigid body constraint for faster initial runs of the analysis. Once you have verified the model definition, remove the rigid body constraints. Mouse type Portion of mouse that is deformable Relative CPU time rigid prototype 23% 0.35 fully deformable 100% 1 Final deformed shapes Deformable regions in color fully deformable mouse rigid prototype mouse Drop Test Simulation of a Cordless Mouse
- 38. 38 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Techniques for Reducing CPU Time Initial conditions can be used to reduce the length of some analyses You can define initial conditions (stress fields, hardening conditions, velocities,…) rather than modeling the history that lead to the initial conditions. Example: Drop test of a cordless mouse Apply initial velocity conditions consistent with a 1m free fall. V3 Mouse initial velocity *INITIAL CONDITIONS,TYPE=VELOCITY ALL_NODES, 3, 4500
- 39. 39 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Techniques for Reducing CPU Time Static initialization and import Abaqus provides a capability to transfer the deformed mesh and associated material state between an Abaqus/Standard analysis and an Abaqus/Explicit analysis (and vice-versa). Reduce the analysis run time by solving portions of an analysis with Abaqus/Standard. Examples: Simulate a transient event in Abaqus/Explicit after steady-state conditions have been simulated in Abaqus/Standard Simulate springback in Abaqus/Standard after forming analysis in Abaqus/Explicit Steady-state spinning solution in Abaqus/Standard Dynamic blade release analysis in Abaqus/Explicit
- 40. 40 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Techniques for Reducing CPU Time Mass scaling speeds up an analysis by increasing the stable time increment size. Artificially increasing the material density by a factor of f 2 increases the stable time increment by a factor of f. *VARIABLE MASS SCALING, FREQUENCY=1, DT=0.0005, TYPE=BELOW MIN Scale density of elements whose stable time increment is less than .0005 s
- 41. 41 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Techniques for Reducing CPU Time Selective subcycling can reduce the run time for an analysis when a small region of elements in the model controls the stable time increment Subcycling allows for different time increments to be used for different groups of elements Example – Rod impact analysis with selective subcycling With an appropriately chosen subcycling zone, the rod impact analysis runs 2.3x faster than the equivalent analysis without subcycling
- 43. 43 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Postprocessing calculator Tips Review results during a long Abaqus/Explicit analysis to avoid wasting resources running an incorrect model. When reviewing an output database before an analysis is complete, you will need to run the postprocessing calculator to: extrapolate integration point quantities to the nodes or interpolate integration point quantities to the centroid of an element. Execution procedure (at the command line): abaqus oldjob=job-name job=converted-odb-name convert=odb
- 44. 44 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Double-precision execution Tips Analyses that require a large number of increments should be solved with the double-precision executable. Single precision provides accurate results in most cases. Exceptions for which double precision is recommended: analyses of more than 300,000 increments models with hyperelastic materials analyses with multiple revolutions of deformable parts Double-precision execution procedure (at the command line): abaqus job=job-name double
- 45. 45 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 No distortion control With distortion control Element Distortion Control Tips Abaqus/Explicit offers distortion control to prevent solid elements from inverting or distorting excessively. Distortion control is designed to prevent negative element volumes or other excessive distortion from occurring during an analysis. In contrast to the adaptive meshing technique, distortion control does not attempt to maintain a high-quality mesh throughout an analysis. Elements with distortion control can not be included in an adaptive mesh domain. crushable foam indentation *SOLID SECTION, ELSET=BLANK, MATERIAL=FOAM,CONTROLS=DistortionControl *SECTION CONTROLS, NAME=DistortionControl, HOURGLASS=ENHANCED, DISTORTION CONTROL Constraint activates when a rectangular element under uniaxial compression undergoes 90% nominal strain (default).
- 47. 47 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Summary of Abaqus/Explicit Designed to solve highly discontinuous, high-speed dynamic problems efficiently. Very robust contact algorithm that does not add additional degrees of freedom to the model. Does not require as much disk space as Abaqus/Standard for large problems, and it often provides a more efficient solution for very large problems. Contains many capabilities that make it easy to simulate quasi-static problems. Has the capability to effectively solve Fluid-Structure interaction (FSI) problems.
- 48. 48 3DS.COM © Dassault Systèmes | Confidential Information | 10/8/2014 | ref.: 3DS_Document_2013 Next steps … • Register for a Training Class 3ds.com/simulia-training • eSeminar replay: Would be uploaded on SIMULIA Resource Center and SIMULIA Learning Community (SLC), watch out for the email announcement • Join SIMULIA Learning Community 3ds.com/slc • Follow us on social media: @3DS_SIMULIA • Join our SIMULIA Regional User Meeting around globe in 24 locations. For more information visit http://www.3ds.com/events/simulia-regional-user-meetings/