LS-DYNA3D Interface

This interface writes global parameter definitions, coordinates, connectivity, property information & boundary conditions in the LS-DYNA3D input deck (keyword format).

Creating the LS-DYNA3D Input File

The translator writes the LS-DYNA3D input deck using the following files:

To create the LS-DYNA3D input file, select the following menu entries from the ICEM CFD/CAE manager:

         Select an existing unstructured domain file

         Give the name of its corresponding boundary condition file (default is configuration/mesh/family_boco)

         Give the name of its corresponding parameter file (default is configuration/mesh/ls_dyna3d.par)

         Give the name of the LS-DYNA3D input file (default is configuration/transfer/ls_dyna3d)

         Specify whether to Ignore Node (0-D) elements (default no).

         Specify whether to Ignore Bar (1-D) elements (default no).

         Specify whether to Ignore Shell (2-D) elements (default no).

The successful execution of the interface generates the LS-DYNA3D input file located in the Transfer Shell. The ICEM CFD/CAE Manager opens a shell window in this directory when the following menu item is selected:

Note: - If you specify Ignore Elements (Node/Bar/Shell) as yes, elements won’t be written to input deck. No keyword would be written which is related to family having all elements ignored. No Boundary Condition will be written to family having all elements ignored. 

Defining parameters for LS-DYNA3D

The next sections describe how to define Default LS-DYNA3D keywords using the Output/ls_dyna3d param menu in the mesh editor (MED).

Default Properties for 3/2/1/0 – D Elements –

 These are the group of properties consisting of keywords *MAT,*SECTION,*ELEMENT,*HOURGLASS,*EOS and *SET. When user will select “Yes” for “Use Default Element properties”, following keywords will be generated automatically. If user has selected “Use Default properties for 3-D elements”, one *PART along with corresponding *MAT and *SECTION will also be generated per 3-D family. Also *ELEMENT keyword will be generated for all 3-D elements.
 
If user wants to override these element properties for a family, define “User Defined 3-D element set” in param menu with required properties. Then through boundary condition menu apply element properties by specifying 3-D element set name defined in Output/ls_dyna3d param menu.
 
*ELEMENT: Default Element Data.
*MAT: Default materials.
*SECTION: Default sections. 
*PART: Default Parts.
*SET: Default Nodal/Segment/Shell/Solid sets for applying loads, contact, etc.
*HOURGLASS: Default Hourglasses.
*EOS: Default Equation of States.
*NODE: Default Node Data. 

Following table shows element types supported by 3-D, 2-D, 1-D and 0-D elements and respective materials. It also specifies whether *SECTION, *HOURGLASS and *EOS properties are applicable or not.

 

Element Type

Materials

SECTION

HOURGLASS

EOS

 

 

 

 

 

3-D Element

 

 

 

Solid

Elastic, Elastic Fluid, Plastic Kinematics, Soil & foam, Viscoelastic, Blatz-Ko Rubber, High Explosive Burn, Null, Elastic plastic hydro, Elastic plastic hydro spall, Isotropic elastic plastic, Soil & foam failure, Johnson-Cook, Power law plasticity, Strain rate dependant plasticity, Rigid, Composite damage, Piecewise linear plasticity, Honeycomb, Mooney-Rivlin rubber, Shape memory, Frazer-Nash rubber, Bamman damage, Closed cell foam, Low density foam, Composite failure model, Viscous foam, Crushable foam, Rate sensitive power law plasticity, Fu chang foam, MTS, Acoustic, Brittle damage, Anisotropic viscoplastic, Finite elastic strain plasticity, Brittle damage, Plasticity compression tension, Modified honeycomb

 

 

 

AA

 

 

 

AA

 

 

 

AA

CFD Solid

Default

AA

AA

AA

Thermal Solid

Isotropic, Orthotropic, Isotropic_TD.

AA

AA

AA

 

Thick Shell

Elastic, Elastic fluid, Plastic Kinematics, Isotropic elastic plastic, Johnson-Cook, Power law plasticity, Strain rate dependant plasticity, Rigid, Composite damage, Piecewise linear plasticity, Laminated glass, Transversely Anisotropic elastic plastic, FLD transversely Anisotropic, Bamman damage, Rate sensitive power law plasticity, Plasticity with damage, Modified piecewise linear plasticity.

 

AA

 

AA

 

NA

 

 

 

2-D Element

 

 

Shell

Elastic, Elastic Fluid, Plastic Kinematics, Blatz-Ko Rubber, Null, Isotropic elastic plastic, Johnson-Cook, Power law plasticity, Strain rate dependant plasticity, Rigid, Composite damage, Piecewise linear plasticity, Honeycomb, Mooney-Rivlin rubber, Resultant Plasticity, Laminated Glass, Transversely Anisotropic elastic plastic, FLD transversely Anisotropic, Bamman Damage, Enhanced composite damage (I), Enhanced Composite damage (II), Composite Failure Model, Rate sensitive power law plasticity, Plasticity with damage, MTS, Plasticity polymer, Anisotropic viscoplastic, Modified piecewise linear plasticity

 

 

AA

 

 

AA

 

 

NA

CFD Shell

Default

AA

AA

NA

Thermal Shell

Isotropic, Orthotropic, Isotropic_TD.

AA

AA

NA

Airbag

Fabric

AA

AA

NA

 

 

 

 

1-D Element

Hughes – Lui

Elastic, Elastic fluid, Plastic Kinematic, Viscoelastic, Null, Power law, plasticity, Rigid, Piecewise linear plasticity.

AA

NA

NA

Belytschko resultant

Elastic, Elastic fluid, Null, Rigid, Resultant plasticity, Force limited

AA

NA

NA

Truss

Elastic, Elastic fluid, Plastic Kinematic, Null, Rigid.

AA

NA

NA

Belytschko integrated solid

Elastic, Elastic fluid, Plastic Kinematic, Null

AA

NA

NA

Belytschko integrated tubular

Elastic, Elastic fluid, Plastic Kinematic, Null

AA

NA

NA

Discrete

Linear elastic, Nonlinear elastic, Nonlinear plastic, Hydraulic gas damper, Cable, Elastic spring, Elastic 6DOF spring, Inelastic spring, and Inelastic 6DOF spring

AA

NA

NA

Spring and Dampers

Elastic, Viscous, Elastoplastic, Nonlinear elastic, Nonlinear viscous, General nonlinear, Maxwell, Inelastic.

AA

NA

NA

Seatbelt

Default

AA

NA

NA

 

0-D Element

Lumped Mass

NA

NA

NA

NA

SPH Particle

NA

AA

NA

NA

Lumped Inertia

NA

NA

NA

NA

(NA - NOT APPLICABLE, AA – APPLICABLE)

The LS-DYNA3D keywords generated by this section appear in the input deck in the following order:

Default Element (*ELEMENT): -

Elements will be written to the LS-DYNA3D input file when either Default Element properties are applied or user has applied Element properties to a particular family. However, this card allows the part id to be defined, and a brick shell element type to be defined instead of a solid element. If this card is not defined, elements will still be written to the LS-DYNA3D input deck, but the part type will default to part 1, and a default element type (either SHELL or SOLID) will be selected based upon the number of nodes and dimension of the element to be written. If BRICK Shells are required, these cards should be defined. Note that care must be taken in defining the brick shells, because nodes 1-4 in each element must lie on the bottom plane of the brick, and nodes 5-8 must lie on the top surface.

Default elements can be overridden using Output/Bound conds menu. In boundary condition, you can specify element name defined in Output/ls_dyna3d param menu.

Default Materials (*MAT_OPTION): -

When user will select Element Type, corresponding material choice box will be enabled. Select the material from options available
and specify required number of material cards and corresponding values for the same. Material ID will be generated automatically. Default materials can be overridden using Output/Bound conds menu. In boundary condition, you can specify element set name defined in Output/ls_dyna3d param menu.

Default Sections (*SECTION_OPTION): -

In this Section, element formulation, integration rule, nodal thickness and cross sectional properties are defined. The keyword defined in this section are as follows.

*SECTION_BEAM

It will be defined for 1-D families with beam elements.

*SETION_DISCRETE

It will be defined for 1-D families with discrete elements.

*SECTION_SEATBELT

It will be defined for 1-D families with seatbelt elements.

*SECTION_SOLID

It will be defined for all 3-D families.

*SECTION_SHELL

It will be defined for 2-D families with shell elements.

*SECTION_SPH

It will be defined for 1-D families with sph particles as elements.

*SECTION_TSHELL

It will be defined for 2-D families with thick shell elements.

 

Default sections can be overridden using Output/Bound conds menu. In boundary condition, you can specify element set name defined in Output/ls_dyna3d param menu.

Part Definition (*PART)

Define parts i.e. combine material, information, section properties, EOS type, thermal properties and a flag for part adaptivity. Select or Enter values for parameters. Thermal material property ID is taken 0 by default.

Default Sets (*SET): -

A concept of grouping nodes, elements, materials, etc., in sets is employed throughout the LSDYNA3D input deck. In 3D models, element sets can be defined on domains, subfaces, and free subfaces. For element sets defined in 3D, elements, which have an element face which lies along a boundary face, will be grouped in an element set. Only GENERAL option is supported for all options. This card is written by default.

*SET_SHELL_GENERAL - One Set per 2-D family having Shell elements.

*SET_SEGMENT_GENERAL - One Set per 2-D and 3-D family.

*SET_SOLID_GENERA L- One Set per 3-D family.

*SET_BEAM_GENERAL - One Set per 1-D family having Beam elements

*SET_DISCRETE_GENERAL - One Set per 1-D family having Discrete elements

*SET_TSHELL_GENERAL - One Set per 2-D family having Thick Shell elements

*SET_PARTS - One Set per family.

 

*SET_NODE_LIST

 

One Set will be generated per family. It will consist of group of nodes in that family.

It will be generated per family irrespective of whether default element properties

Are defined for the family or not.

  

Default Hourglass (*HOURGLASS): -

Define Hourglass and Bulk Viscosity properties. Using the *PART definition this specification is connected to elements. This keyword is applicable to element types mentioned in the table. This input deck is not generated if none for include option is specified. Unique Hourglass ID is generated automatically.

Default Hourglasses can be overridden using Output/Bound conds menu. In boundary condition, you can specify Hourglass name defined in Output/ls_dyna3d param menu.

Default Equation Of States (*EOS_OPTION): -

LSDYNA has historically referenced equation of state by type identifiers. Below are the identifiers supported by the interface along with their type.

Type

Option

1

*EOS_LINEAR_POLYNOMIAL

2

*EOS_JWL

3

*EOS_SACK_TUESDAY

4

*EOS_GRUNEISEN

6

*EOS_LINEAR_POLYNOMIAL_WITH_ENERGY_LEAK

8

*EOS_TABULATED_COMPACTION

9

*EOS_TABULATED

11

*EOS_TENSOR_PORE_COLLASPE

This keyword is applicable to element types mentioned in the table. This input deck is not generated if none for include option is specified. Unique EOS ID is generated automatically.

Default EOS can be overridden using Output/Bound conds menu. In boundary condition, you can specify EOS name defined in Output/ls_dyna3d param menu.

Node Definition (*NODE)

Nodes will appear in the LS-DYNA3D input deck without any special attention from the user. However, fixed displacements and/or rotations can be applied to nodes and these will appear on the node definitions. For more details see the Fixed Node Displacements and Rotations section in the LSDYNA Boundary condition section defined below.

Note: - *MAT, *ELEMENT, *SECTION, *HOURGLASS and *EOS keywords can be overridden using boundary conditions menu.

The next sections describe how to define Global LS-DYNA3D keywords using the Output/ls_dyna3d param menu in the mesh editor (MED).

The global parameter definitions generated with these sections appear in the input deck in the following order:

*DEFINE: Define Load Curves, Boxes, Coordinates, Vectors and Transformation. 
*INTEGRATION: Define Integration Rules.
*COMPONENT: Define Components.
*DATABASE: Define output files.
*CONTROL_OPTIONS: Define Control parameters.
*LOAD_BLAST: Define Global Blast Load.
*LOAD_BRODE: Define Global Brode Load. 
*LOAD_BODY_OPTIONS: Define Body force loads.
*DAMPING_GLOBAL: Global damping conditions defined.
*DAMPING_RELATIVE: Define Damping Relative to Rigid Body. 
*INITIAL_CFD: Define initial conditions for CFD analysis.
*ALE: Define Input Data for ALE.
*CONSTRAINED_GLOBAL: Apply Global Constraints.
*CONTACT: Define Contact.
*CONTACT_INTERIOR: Define Interior Contact for foam brick elements.
*CONTACT_RIGID_SURFACE: Define Rigid Surface Contact.
*DEFORMABLE_TO_RIGID_AUTO: Define Parameters for Deformable to Rigid.
*TRANSLATE: Translate Other Translator Input Deck.
*USER: Define User Defined Input.
*INCLUDE: Include other input files.

Define Load Curve (*DEFINE_CURVE_OPTION)

First select type of load Curve.

*DEFINE_CURVE: -

Define a curve (e.g. load vs. time) and specify required parameters. Enter / Select values for parameters. Put one pair of points per card. For this card specify Abcissa values and Ordinate values. You can specify any number of points for a curve.

*DEFINE_CURVE_SMOOTH: -

Define a smoothly varying curve using few parameters. This shape is useful for velocity control of tools in metal forming applications. Enter / Select values for parameters.

 

*DEFINE_CURVE_TRIM: -

Define a curve for trimming. Enter / Select values for parameters. It does not require any points.

Define Coordinate System (*DEFINE_COORDINATE_OPTION)

Define a local coordinate system. Select from options whether to define Coordinate System or Coordinate Vector.

*COORDINATE_SYSTEM: -

Define a local coordinate system with three points. Enter / Select the values for parameters. The coordinate of the points must be separated by a reasonable distance and not collinear to avoid numerical inaccuracies.

 

*COORDINATE_VECTOR: -

Define a local coordinate system with two vectors. Enter / Select the values for parameters. These vectors should be separated by a reasonable included angle to avoid numerical inaccuracies.

Define Vector (*DEFINE_VECTOR)

Define a vector by defining the coordinates of two points. The coordinate should differ by a certain margin to avoid numerical inaccuracies.

Define Box (*DEFINE_BOX_OPTION)

Define a box shaped volume. Boxes to limit the geometric extent of certain inputs. It has following options.

*DEFINE_BOX: -

Define a box shaped volume where two diagonally opposite corner points of a box are specified in global coordinates. Enter / Select the values for parameters.

 

*DEFINE_BOX_ADAPTIVE: -

Define a box shaped volume enclosing the elements where the adaptive level is to be specified. If the midpoint falls within the Box, adaptive level is reset. Enter / Select the values for parameters.

 

*DEFINE_BOX_COARSEN: -

Define a specific box shaped volume-indicating elements, which are protected from mesh coarsening. Enter / Select the values for parameters.

 

*DEFINE_BOX_DRAWBEAD: -

Define a specific Box shaped volume around Draw bead. The Box will contain the draw bead nodes and elements between bead and the outer edge of the blanks. Elements directly under the bead are also included.

Define Transformation (*DEFINE_TRANSFORMATION)

Define transformation properties.

Define Integration Rules (*INTEGRATION_OPTION)

Define user defined through the thickness integration rules. Integration rules can be defined for Beam and Shell elements. Multiple integration rules can be created, but Integration Rule ID’s should be unique. Following are the types (Beam and Shell) of integration rules.

*INTEGRATION_BEAM: -

Define integration rules for beam elements. Select / Enter value for the parameters enabled for this option.

 

*INTEGRATION_SHELL: -

Define integration rules for shell elements. Select / Enter value for the parameters enabled for this option.

Define Components (*COMPONENT_OPTION)

This section contains analytical rigid body dummies that can be placed within vehicle and integrated implicitly. This keyword also provides a way of incorporating specialized components and features. Select one of the options for Component options.

*COMPONENT_GEBOD_OPTION: -

Generate a rigid body dummy based on dimensions and mass properties from GEBOD database. OPTION specifies the human subject type. The male and female represent adults while child is genderless. Select / Enter the values for parameters

OPTIONS: - MALE, FEMALE AND CHILD.

*COMPONENT_GEBOD_JOINT_OPTION: -

Alter the joint characteristics of a GEOBD rigid body dummy. Setting a joint parameter value to zero retains the default value set internally. The following options are available

PELVIS, WAIST, LOWER_NECK, UPPER_NECK, LEFT_SHOULDER, RIGHT_SHOULDER, LEFT_ELBOW,

RIGHT_ELBOW, RIGHT_HIP, LEFT_HIP, RIGHT_KNEE, LEFT_KNEE, RIGHT_ANKLE, LEFT_ANKLE.

 

*COMPONENT_HYBRIDIII: -

Define a HYBRID III dummy. The motion of dummy is governed by equations integrated within LS-DYNA separately from the finite element model. Select /Enter the values for parameters

 

*COMPONENT_HYBRIDIII_JOINT_OPTION: -

Alter the joint characteristics of a HYBRIDIII rigid body dummy. Setting a joint parameter value to zero retains the default value set internally. The following options are available

LUMBAR, LOWER_NECK, UPPER_NECK, LEFT_SHOULDER, RIGHT_SHOULDER, LEFT_ELBOW, RIGHT_WRIST, LEFT_WRIST, RIGHT_ELBOW, RIGHT_HIP, LEFT_HIP, RIGHT_KNEE, LEFT_KNEE, RIGHT_ANKLE, LEFT_ANKLE.

Define Database files (*DATABASE_OPTION)

Database options are necessary to obtain output files containing results information. For the ASCII files following are the options. To write LSDYNA input deck, include option is selected.

File Name

Description

ABSTAT

Airbag Statistics

AVSFLT

AVS Database

BNDOUT

Boundary condition forces and energy

DEFGEO

Deformed Geometry file

DEFORC

Discrete Elements

ELOUT

Element Data

GCEOUT

Geometric contact entities

GLSTAT

Global Data

JNTFORC

Joint Force File

MATSUM

Material Energies

MOVIE

Movie file

MPGS

MPGS file

NCFORC

Nodal Interface Forces

NODFOR

Nodal Force Groups

NODOUT

Nodal Point Data

RBDOUT

Rigid Body Data

RCFORC

Resultant Interface Forces

RWFORC

Wall Forces

SBTOUT

Seat belt Output File

SECFORC

Cross Section Forces

SLEOUT

Sliding Interface Energy

SPCFORC

SPC reaction forces

SPHOUT

SPH Data File

SSSTAT

Subsystem data

SWFORC

Nodal Constraint reaction forces

TPRINT

Thermal output from a coupled structural/thermal or thermal only analysis

TRHIST

Tracer particle history information

Specify the time interval between outputs for each option.

Define Extended Database (*DATABASE_EXTENT_OPTION)

Define extended database file. For each option, Enter / Select the values for parameters. It has following database options: -

AVS, MOVIE, MPEG, SSSTAT.

Define Database Format (*DATABASE_FORMAT)

Define the Output Format for binary files. Select appropriate values for the options.

Define Database for Tracer particle (*DATABASE_TRACER)

Tracer particle will save a history of either a material point or a spatial point into an ASCII file TRHIST. The option *DATABASE_TRHIST must be active. Select / Enter values for the parameters.

*DATABASE_CROSS_SECTION: -

Define a cross section for resultant forces written to ASCII file SECFORC.

*DATABASE_BINARY_OPTION: -

Define binary output files.

*DATABASE_HISTORY_OPTION: -

Control which gives nodes or elements are output into binary history file.

*DATABASE_NODAL_FORCES_GROUP: -

Define a nodal force group for output into ASCII file NODFOR and binary file XTFILE.

Define Control Parameters (*CONTROL_OPTION)

Options available in *CONTROL section allow the resetting of default global parameters such as hourglass type, the contact penalty scale factor, shell element formulation, numerical damping and termination time. Control cards can also be used to change activation solution options such as mass scaling, adaptive remeshing and an implicit solution.

*CONTROL_ACCURACY: -

Define parameters that can improve the accuracy of the calculation.

 

*CONTROL_ADAPSTEP: -

Define control parameters for contact interface force updating during each adaptive cycle.

 

*CONTROL_ADAPTIVE: -

Activate adaptive meshing. The parts which are adaptively meshed are defined by *PART. It defines various parameters required for adaptive remeshing.

 

*CONTROL_ALE: -

Set default control parameters for the Arbitrary Lagrange-Eulerian and Eulerian calculations.

 

*CONTROL_BULK_VISCOSITY: -

Reset the default values of the Bulk Viscosity Coefficients Globally. This may be advisable for shock wave propagation and some materials.

 

*CONTROL_CFD_AUTO: -

Set the time step control options for the Navier – Stokes flow solver. *CONTROL_CFD_GENERAL is used in conjunction with this keyword to control the flow solver time – integration options.

 

*CONTROL_CFD_GENERAL: -

Set the solver parameters for the Navier – Stokes flow solver. *CONTROL_CFD_OPTION where option = Momentum, Transport and Pressure are used in conjunction with this keyword to control flow solver options.

 

*CONTROL_CFD_MOMENT: -

Set the solver parameters to be used for the momentum equations in the Navier – Stokes flow solver.

 

*CONTROL_CFD_PRESSURE: -

Set the pressure solver parameters to be used for the incompressible Navier – Stokes equation.

 

*CONTROL_CFD_TRANSPORT: -

Activate the calculation of transport variables and associated solver parameters to be used for the auxiliary scalar transport equations.

*CONTROL_CFD_TURBULENCE: -

Activate a turbulence model and set the associated model parameters.

 

*CONTROL_COARSEN: -

Adaptively de-refine (coarsen) a shell mesh by selectively merging four adjacent elements into one. Adaptive constraints added and removed as necessary.

 

*CONTROL_CONTACT: -

Change the defaults for computation with contact surfaces.

 

*CONTROL_COUPLING: -

Change the defaults for MADYMO3D/CAL3D coupling.

 

*CONTROL_CPU: -

Control CPU Time. The CPU time limit applies to the current phase of analysis.

 

*CONTROL_DYNAMIC_RELAXATION: -

Define the control parameters for dynamic relaxation. Important for stress initialization

 

*CONTROL_ENERGY: -

Provide the controls for energy dissipation options.

*CONTROL_HOURGLASS_936: -

Set the default values of the hourglass control option 936 to override default values. The modification in the hourglass control form version 936 was to ensure that all the components of the hourglass force vector are orthogonal to rigid body rotation.

 

*CONTROL_IMPLICIT_AUTO: -

Define parameters for automatic time step control during implicit analysis. Define following variables for this card.

*CONTROL_IMPLICIT_DYNAMIC: -

Activate implicit dynamic analysis and define time integration constants.

 

*CONTROL_IMPLICIT_EIGENVALUE: -

Activate implicit eigenvalue analysis and define associated input parameters.

 

*CONTROL_IMPLICIT_GENERAL: -

Define control parameters for analysis.

 

*CONTROL_IMPLICIT_SOLUTION: -

Define these control cards for an implicit calculation. These cards specify whether a linear or non-linear solution is desired.

 

*CONTROL_IMPLICIT_SOLVER: -

Define the control parameters for implicit analysis linear equation solver.

 

*CONTROL_IMPLICIT_STABILIZATION: -

Define the parameters for artificial stabilization during multi step implicit springback analysis.

 

*CONTROL_NONLOCAL: -

Allocate the additional memory (percentage increase of memory) allocated for *MAT_NONLOCAL option, over that required initially.

 

*CONTROL_OUTPUT: -

Set the miscellaneous output parameters. This keyword does not control the information such as stress and strain tensors.

*CONTROL_PARALLEL: -

Control the parallel processing usage for shared memory computers by defining number of processor and invoking the optional consistency of the global vector assembly.

 

*CONTROL_REMESHING: -

Control the element size for three-dimensional adaptivity for solid elements. This commands control the size of elements on the surface of the solid part.

 

*CONTROL_RIGID: -

Special control options related to rigid bodies and the rigid flexible bodies.

 

*CONTROL_SHELL: -

Provide control parameters for computing shell response.

 

*CONTROL_SOLID: -

Provide control parameters for solid element response. Specify Automatic sorting of Tetrahedron and Pentahedron elements required or not.

 

*CONTROL_SOLUTION: -

To specify the analysis solution procedure if thermal only or coupled thermal analysis is specified.

 

*CONTROL_SPH: -

Provide control parameters for computing SPH particles.

*CONTROL_TERMINATION: -

Provide control parameters required for terminating a job.

*CONTROL_THERMAL_NONLINEAR: -

Set the parameters for a nonlinear thermal or coupled structural/thermal analysis. The control card *CONTROL_SOLUTION is also required.

*CONTROL_THERMAL_SOLVER: -

Set the parameters for thermal solution in thermal only or coupled structural analysis. The control card *CONTROL_SOLUTION is also required.

*CONTROL_THERMAL_TIMESTEP: -

Set the time step controls for thermal solution in thermal only or coupled structural/thermal analysis. The control cards *CONTROL_SOLUTION and *CONTROL_THERMAL_SOLVER are also required.

*CONTROL_ TIMESTEP: -

Set the structural time step size control using different options.

 

*CONTROL_ SUBCYCLE: -

This keyword activates control time step subcycling.

 

Define Global Load Conditions (*LOAD_BLAST & *LOAD_BRODE)

Define global forces (load) applied to materials.

*LOAD_BLAST: -

Define an airblast function for the application of pressure loads due to explosives in conventional weapons. The implementation is based on a report by Randers - Pehrson and Bannister where it is mentioned that this model is adequate for use in engineering studies of vehicle responses due to blast from land mines. Enter the values for parameters. A minimum of two load curves, even if unreferenced, must be present in the model.

 

*LOAD_BRODE: -

Define Brode function for the application of pressure loads due to explosion. Enter the values for following parameters. Both load curves must be specified for the variable yield option.

 

*LOAD_BODY_OPTIONS: -

Define body force loads due to a prescribed base acceleration or angular velocity using global axes directions. Options are as follows

X, Y, Z, RX, RY, RZ and PARTS.

 

*LOAD_SSA: -

The Sub-Sea Analysis capability allows a simple way of loading the structure to account for the effects of the primary explosion and the subsequent bubble oscillations.

 

*LOAD_SUPERPLASTIC_FORMING: -

Perform Super plastic Forming analyses. This option can be applied to both solid and shell elements. The pressure loading controlled by load curve is scaled to maintain a constant maximum strain rate.

Define Damping: -

*DAMPING_GLOBAL: -

Define mass weighted nodal damping that applies globally to the nodes of deformable bodies and to the mass center of the rigid bodies.

 

*DAMPING_RELATIVE: -

Apply damping relative to the motion of a rigid body.

Define Global Initial condition (*INITIAL_CFD)

Define initial conditions for all nodal variables in the incompressible CFD solver.

Define Elements Set (*ELEMENT, *MAT, *SECTION)

Any number of named 3D, 2D, 1D and 0D elements (with corresponding materials and sections) can be created as required. The element set names can be associated with a family in the Boundary Conditions menu.

Following default values are provided for each of the element.

Element Type: - Select from the options provided.

Material Type: - Select from the options provided.

Define Section parameters.

Define Hourglasses (*HOURGLASS)

Any number of named Hourglasses can be created as required. The names can be associated with a family in the Boundary Conditions menu.

Define EOSes (*EOS)

Any number of named EOSes can be created as required. The names can be associated with a family in the Boundary Conditions menu.

Define ALE (*ALE)

This keyword *ALE provides a way of defining input data pertaining to the Arbitrary-Lagrange-Eulerian capability. Various options available with this keyword are as follows.

Define Global Constraints (*CONSTRAINED_GLOBAL)

Define a global boundary constraint plane. Specify translational and rotational constraints.

Define Contact (*CONTACT_OPTION): -

Define a contact interface. Select one of the options.

Define Interior Contact (*CONTACT_INTERIOR)

Define Interior Contact for foam brick elements. Specify part set Id for this option. Only one part set id can be specified.

Define Rigid Surface Contact (*CONTACT_RIGID_SURFACE)

Define rigid surface Contact. The purpose of rigid surface contact is to model large rigid surfaces, i.e. road surfaces, with nodal points and segments that require little storage and are written out at the beginning of binary databases.

Define Deformable to Rigid (*DEFORMABLE_TO_RIGID_AUTO)

Define a set of parts to be switched to rigid or deformable at some stage in the calculation.

Define Translate (*_OPTIONS) TRANSLATE

Define a set of parts to be switched to rigid or deformable at some stage in the calculation.

Define User Defined Input (*USER_OPTIONS)

Define user-defined input and allocate storage for user defined subroutines for the contact algorithms. Available options include

CONTROL & FRICTION.

Include Options (*INCLUDE_OPTIONS)

This keyword provides a means of reading independent input files containing model data. Generally this keyword is used without any option; however, two options are available

STAMPED_PART & TRANSFORM.

 

Defining boundary conditions for LS-DYNA3D

The next sections describe how to define LS-DYNA3D commands (*LOAD, *BOUNDARY, etc.) using the Output/Bound conds menu in the mesh editor (MED).

The parameter definitions generated with these sections appear in the input deck in the following order:

*ELEMENT: Overriding elements (elements, materials & sections) for a family.
*HOURGLASS: Overriding Hourglasses for a family.
*EOS: Overriding EOSes for a family.
*BOUNDARY: Defining types of boundary condition.
*LOAD: Applying different loads condition.
*INITIAL: Define Initial conditions.
*INTERFACE: Define Interface.
*DAMPING: Define Damping.
*CONSTRAINED: Define Constraints.
*AIRBAG: Define Airbag.
*ALE: Define ALE.
*DEFORMABLE_TO_RIGID: Specify When convert to Rigid.
*RIGIDWALL: Define Rigid wall parameters.
*TERMINATION_BODY: Define Termination parameters for Rigid Body.
 

One window will display name of each family along with Create new menu under Boundary condition menu. After clicking you will see selection window, select one of the boundary condition. Now you can edit parameters related to that boundary condition.

Fixed Node Displacements and Rotations (*NODE):

In 2D, fixed nodal displacements and rotations can be defined on subfaces, free subfaces, or edges and in 3D, on domains, subfaces, or edges. Select an entity then set the parameters.

These constraints are cumulative. If, for example, two separate BOUND cards are used which apply to the same node and which constrain displacements in X and Y respectively, the code for the affected node will be output automatically as 4 (constrained not to move in/about X, Y).

 

Define Elements (*ELEMENT, *MAT, *SECTION): -

 

Here you can override default elements, materials and sections for the family. You have to specify element name from list of elements defined in Output/ls_dyna3d param menu.

 

Define Hourglass (*HOURGLASS): -

 

Here you can override default Hourglass for the family. You have to specify hourglass name from list of hourglasses defined in Output/ls_dyna3d param menu.

 

Define EOS (*EOS): -

 

Here you can override default EOS for the family. You have to specify EOS name from list of EOSes defined in Output/ls_dyna3d param menu.

 

Define Boundary Type (*BOUNDARY_OPTIONS): -

Different types of boundary condition can be applied to specific families. You have to select type of Boundary condition and depending upon boundary type, respective input boxes will be enabled. You have to either select from choices or enter values in input boxes.

 

*BOUNDARY_NON_REFLECTING: -

Non-Reflecting option applies to continuum domains modeled with 3D solid elements, as indefinite domains are usually not modeled. For geomechanical problems this option is important for limiting the size of models.

 

*BOUNDARY_PRESCRIBED_MOTION_OPTION: -

Define an imposed nodal motion (velocity, acceleration or displacement) on a node or set of nodes.

 

*BOUNDARY_SLIDING_PLANE: -

Define a sliding symmetry plane. This option applies to continuum domains modeled with solid elements.

*BOUNDARY_SPC_OPTION: -

Define nodal single point constraint. Do not use this option in r-adaptive problems since Nodal point ID’s Change during Adaptive Steps. Constraints are applied if a value 1 is given for DOFx. If value of zero, means no constraint. Only SET option is supported. *MAT_RIGID should not be defined for the family.

 

*BOUNDARY_SYMMETRY_FAILURE: -

Define a symmetry plane with failure criterion. This option applies to continuum domains modeled with solid elements.

 

*BOUNDARY_TEMPERATURE_NODE: -

Define temperature boundary conditions for a thermal or coupled thermal/structural.

 

Define Load Type (*LOAD_OPTIONS): -

 

This section provides various methods of loading the structure with concentrated point loads, distributed pressure, body force loads and a variety of thermal loadings. You have to select type of load condition and depending upon load type, respective input boxes will be enabled. You have to either select from choices or enter values in input boxes. Some load conditions can be applied to solids, shells or beams only. Following are various load types

*LOAD_BEAM_SET: -

Apply the distributed traction load along any local axis of beam or a set of beams. Enter/Select the following parameters to apply this load condition.

 

*LOAD_DENSITY_DEPTH: -

Define density versus depth for gravity loading. This option has been occasionally used for analyzing underground and submerged structures where the gravitational preload is important. The purpose of this option is to initialize the hydrostatic pressure field at the integration points of the elements. Specify Load Curve ID (defined in ls_dyna3d param) for density vs. depth.

 

*LOAD_HEAT_GENERATION: -

Define solid elements or solid element set with heat generation. Only SET option is supported.

 

*LOAD_MASK: -

Apply distributed pressure load over three-dimensional shell part. The pressure is applied to a subset of elements that are within a fixed global box and lie either outside or inside of a closed curve in a space which is projected onto the surface Specify Load Curve ID defining pressure time history, Vector ID normal to the surface on which applied pressure acts.

*LOAD_NODE_OPTION: -

Apply a concentrated nodal force to a node or set of nodes. Only SET option is supported. In Degree of freedom, follower force and follower moment are not supported.

 

*LOAD_RIGID_BODY: -

Apply a concentrated nodal force to a rigid body. The force is applied at the center of mass or a moment is applied around a global axis. In Degree of freedom, follower force and follower moment options are not supported.

 

*LOAD_SEGMENT_SET: -

Apply the distributed pressure load over each segment in a segment set. If Load Curve ID input is –1,then Brode function is used to determine pressure for the segment set (See*LOAD_ BRODE). If it is –2, then ConWep function is used to determine pressure for segment set (See *LOAD_BLAST).

 

*LOAD_SHELL_OPTION: -

Apply the distributed pressure load over one shell element or shell element set. The numbering of the shell nodal connectivities must follow the right hand rule with positive pressure acting in negative t-direction. Only SET option is supported. If Load Curve ID input is –1,then Brode function is used to determine pressure for the segment set (See *LOAD_BRODE). If it is –2, then ConWep function is used to determine pressure for segment set (See *LOAD_BLAST).

 

*LOAD_THERMAL_OPTION: -

Define nodal sets giving the temperature that remains constant for the duration of the calculation. The reference temperature state is assumed to be a null state with this option. A nodal temperature state read in above and held constant through analysis, dynamically loads the structure. Specify Node set ID containing nodes that are exempted from the imposed temperature. Specify Box ID (all nodes in Box, which belongs to NSID) is initialized. Only CONSTANT, LOAD_CURVE and VARIABLE options are supported.

 

Initial Boundary Conditions (*INITIAL_OPTIONS):

*INITIAL provides a way of initializing velocities and detonation points. After selecting Initial condition, a window will appear showing all parameters. After selecting type of Initial condition, corresponding input boxes will be enabled for selection. You have to either select from choices or enter values in input boxes. In this version EID is taken as ESID. Types of initial conditions are as follows

*INITIAL_DETONATIONS: -

Define points to initiate the location of high explosive detonations in Part ID’s, which use material. *MAT_EXPLOSIVE_BURN card must be defined.

 

*INITIAL_MOMENTUM: -

Define initial momentum to be deposited in solid elements. This option is to crudely simulate an impulsive type of loading.

*INITIAL_TEMPERATUE_OPTION: -

Define initial nodal point temperatures using nodal set ID’s. These initial temperatures are used in thermal only analysis or a coupled thermal/structural analysis. Only SET option is supported.

 

*INITIAL_VELOCITY: -

Define initial nodal point translational velocities using Nodal Set ID’s. Specify Node Set ID for nodes that are exempted from imposed from the imposed velocities. Specify the Box ID defined already in ls_dyna3D param containing all nodes initialized using NSID. Nodes outside the box are not initialized.

 

*INITIAL_VELOCITY_NODE: -

Define initial nodal point translational velocities for Node. This may also be used for sets in which some nodes have other Velocities.

 

*INITIAL_VOID_OPTION: -

Define initial voided Part Set ID’s. Only SET option is supported. Void materials cannot be created during calculation. Fluid elements which are evacuated, e.g. by a projectile moving through fluid during the calculation are approximated as fluid elements with very low densities. The constitutive properties of fluid materials used as voids must be identical to those of the materials, which will fill the voided elements during calculation.

 

*INITIAL_VOLUME_FRACTION: -

Define initial volume fraction of different materials in multi-material ALE, or in single material and void, models.

Define Interface (*INTERFACE): -

Define an interface definitions to define surfaces, nodal lines, and nodal points for which the displacement and velocity time histories are saved at some user specified frequency. You have to select type of interface and depending upon type, respective input boxes will be enabled. You have to either select from choices or enter values in input boxes.

*INTERFACE_COMPONENT_OPTION: -

This capability allows the definition of interfaces that isolate critical components. Only SEGMENT option is supported. Interface may consist of a set of four node segments.

*INTERFACE_LINKING_DISCRETE_NODE_OPTION: -

Define an interface for linking discrete nodes to an interface file. This link applies to spring and beam elements only. Interface ID will be generated automatically.

*INTERFACE_LINKING_SEGMENT: -

Define an interface for linking segments to an interface file for the second analysis using L=isf2 on the execution command line. This applies segments on shell and solid elements.

*INTERFACE_LINKING_EDGE: -

Define an interface for linking a series of nodes in shell structure to an interface file for the second analysis using L=isf2 on the execution command line.

*INTERFACE_JOY: -

Define an interface for linking calculations by moving a nodal interface.

Define Damping (*DAMPING): -

Define damping for a family. Select type of damping. After selecting type of damping, respective input boxes will be enabled. You have to either select from choices or enter values in input boxes.

*DAMPING_PART_MASS: -

Define mass weighted damping by Part ID. Parts may be either rigid or deformable. In rigid bodies the damping forces and moments act at the center of mass.

 

*DAMPING_PART_STIFFNESS: -

Assign Rayleigh stiffness damping coefficient by Part ID. Values between 0.01 and 0.25 are recommended. Higher values are strongly discouraged, and values less than 0.01 may have little effect.

 

Define Constraints (*CONSTRAINED_OPTION): -

This keyword provides a way of constraining degrees of freedom to move together in some way. Select one of the options from following available

*CONSTRAINED_ NODE_SET: -

Define nodal constraint set for translational motion in global coordinates. No rotational coupling.

 

*CONSTRAINED_LAGRANGE: -

Couple a Langrangian mesh (slave) of shells, solids or beams to the material points of an Eulerian Mesh (master). The slave part is coupled with the master part.

 

*CONSTRAINED_RIGID_BODY: -

Merge two rigid bodies. One rigid body called slave rigid body, is merged to the other one called a master rigid body.

 

*CONSTRAINED_RIGID_BODY_STOPPERS: -

Rigid body stoppers provide a convenient way of controlling the motion of rigid tooling in metal forming applications.

 

*CONSTRAINED_TIED_NODES_FAILURE: -

Define a tied node set with failure based on plastic strain. The nodes must be coincident.

 

*CONSTRAINED_EXTRA_NODES_SET:-

Define a extra nodes for the rigid body.

 

*CONSTRAINED_SPOTWELD:-

Define mass less spot welds between non-contiguous nodal pairs. This boundary condition can only be applied to families having bar elements.

 

*CONSTRAINED_GENERALIZED_WELD_OPTION:-

Define spot and fillet welds.

Define Contact Entity (*CONTACT_ENTITY): -

Define a contact entity. Geometric contact entities treat the impact between a deformable body defined as a set of slave nodes and a rigid body.

Define GEBOD Contact (*CONTACT_GEOBOD_OPTION): -

Define a contact interaction between segment of a GEOB dummy and parts of a finite element model. Select one of the options available options.

Define 1D Contact (*CONTACT_1D_OPTION): -

Define one dimensional slide lines/contact for rebar in concrete.

Define 2D Contact (*CONTACT_2D_OPTION): -

Define two dimensional slide lines/contact.

Define Airbag (*AIRBAG_OPTION): -

Define an Airbag or control volume. User has to specify parameters set for Airbag in ls_dyna3d/params window. Also specify parameters set for the selected Option, in ls_dyna3d/params window. Then select names for Airbag parameters set and Option parameters set from the given choices. For example if you want *AIRBAG_SIMPLE_AIRBAG_MODEL keyword, define one Airbag parameters set and one Simple Airbag model parameters set. Options supported are as follows –

 

SIMPLE_AIRBAG_MODEL

SIMPLE_PRESSURE_VOLUME

LINEAR_FLUID

WANG_NEFSKE

ADIABATIC_GAS_MODEL

LOAD_CURVE

Define ALE (*ALE)

This keyword *ALE provides a way of defining input data pertaining to the Arbitrary-Lagrange-Eulerian capability. Various options available with this keyword are as follows.

Define Deformable to Rigid (*DEFORMABLE_TO_RIGID): -

Define materials to be switched to rigid at the start of calculation.

Define Rigid Wall (*RIGIDWALL_OPTIONS): -

Define Rigid Wall parameters.

Define Termination Parameters (*TERMINATION_BODY): -

Define Termination parameters for rigid body.