Specifies control parameters that can improve the accuracy of the calculation.
Card
OSU = 1. Global flag for objective stress updates. Required for parts that undergo large rotations. When set to 1 the flag is on.
INN = 4. Invariant node numbering for shell and solid elements. When set to 4 the flag is on for both shell and solid elements.
Set global control parameters for the Arbitrary Lagrange-Eulerian (ALE) and Eulerian calculations.
Card
DCT = Continuum Treatment from the ALE Controls section of the Analysis Settings (Defaults to 1):
= 1 if the Continuum Treatment is set to Lagrangian.
= 2 if the Continuum Treatment is set to Eulerian.
= 3 if the Continuum Treatment is set to Arbitrary Lagrangian Eulerian.
= 4 if the Continuum Treatment is set to Eulerian Ambiant.
NDV = Cycles Between Advection from the ALE Controls section of the Analysis Settings (Default to 1).
METH = Advection Method from the ALE Controls section of the Analysis Settings (Default to 1):
= 1 if the Advection Method is set to Donor cell + Half-Index-Shift METH.
= 2 if the Advection Method is set to Van Leer + Half-Index-Shift.
Sets the bulk viscosity coefficients globally.
Card
Q1 = 1.5. Quadratic Artificial Viscosity.
Q2 = 0.06. Linear Artificial Viscosity.
TYPE = -2. Internal energy dissipated by the viscosity in the shell elements is computed and included in the overall energy balance.
Specifies the defaults for computations of contact surfaces.
Card 1
SLSFAC = 0 (uses the default = 0.1). Scale factor for sliding interface penalties.
RWPNAL = 0. Scale factor for rigid wall penalties. When equal to 0 the constrain method is used and nodal points which belong to rigid bodies are not considered.
ISLCHK = 1. Initial penetration check in contact surfaces. When set to 1 there is no checking.
SHLTHK = 1 (default). Shell thickness considered in surface to surface and node to surface contact types. When set to 1, thickness is considered but rigid bodies are excluded.
PENOPT = 1 (default). Penalty stiffness value option.
THKCHG = 0 (default).
ORIEN = 2. Automatic reorientation for contact segments during initialization. When set to 2 it is active for manual (segment) and automated (part) input.
ENMASS = 0. This parameter regulates the treatment of the mass for eroded nodes in contact. When set to 0 eroding nodes are removed from the calculation.
Card 2
USRSTR = 0. Storage per contact interface for user supplied interface control subroutine. When set to 0 no input data is read and no interface storage is permitted in the user subroutine.
Default values are used for all other parameters.
Card3
SFRIC = 0. Default static coefficient of friction.
Default values are used for all other parameters.
Card4
IGNORE = 2. Specifies whether to ignore initial penetrations in the *CONTACT_AUTOMATIC options. When set to 2 initial penetrations are allowed to exist by tracking them. Also, warning messages are printed with the original and the recommended coordinates of each slave node.
FRCENG = 1. Calculate frictional energy in contact. Convert mechanical frictional energy to heat when doing a coupled thermal-mechanical problem.
SKIPRWG = 0 (default).
OUTSEG = 1. Yes, output each beam spot weld slave node and its master segment for *CONTACT_SPOTWELD into D3HSP file.
SPOTSTP = 0 (default).
SPOTDEL = 1.Yes, delete the attached spot weld element if the nodes of a spot weld beam or solid element are attached to a shell element that fails and the nodes are deleted.
SPOTHIN = 0.5. This factor can be used to scale the thickness of parts within the vicinity of the spot weld. This factor helps avert premature weld failures due to contact of the welded parts with the weld itself. Should be greater than zero and less than one.
Specifies the controls for energy dissipation options.
Card
HGEN = 2. Hourglass energy is computed and included in the energy balance. Results are reported in ASCII files GLSTAT and MATSUM.
RWEN = 2 (default).
SLNTEN = 2. Sliding interface energy dissipation is computed and included in the energy balance. Results are reported in ASCII files GLSTAT and SLEOUT.
RYLEN = 2. Rayleigh energy dissipation is computed and included in the energy balance. Results are reported in ASCII file GLSTAT.
Defines the default values of hourglass control type and coefficient.
Card
IHQ = Default Hourglass from the Hourglass Controls section of the Analysis Settings ( Default to 1 and Standard LS-DYNA Hourglass ):
= 1 if the Default Hourglass is set to Standard LS-DYNA.
= 2 if the Default Hourglass is set to Flanagan-Belytschko Viscous Form.
= 3 if the Default Hourglass is set to Exact Volume Flanagan-Belytschko.
= 4 if the Default Hourglass is set to Flanagan-Belytschko Stiffness Form.
= 5 if the Default Hourglass is set to Exact Volume Flanagan-Belytschko Stiffness Form.
= 6 if the Default Hourglass is set to Belytschko-Bindeman IHQ.
= 7 if the Default Hourglass is set to Belytschko-Bindeman Linear Total Strain.
QH = Default Hourglass Coefficient from the Hourglass Controls section of the Analysis Settings ( Default to 0.1 ).
This keyword controls the printing of various LS-DYNA output text files.
Card
NPOPT is the only parameter that is set. The value is set to 1. With that parameter set, nodal coordinates, element connectivities, rigid wall definitions, nodal SPCs, initial velocities, initial strains,adaptive constraints, and SPR2/SPR3 constraints are not printed.
Controls parallel processing usage for shared memory computers by defining the number of processors and invoking the optional consistency of the global vector assembly.
Card
CONST = 1. Consistency flag disabled for a faster solution
Specify the analysis solution procedure if thermal, coupled thermal analysis, or structural-only is performed.
Card
SOLN
= 0. Structural analysis only, if the Solver Type is set to Program Controlled or Structural Analysis Only.
= 2. Coupled structural thermal analysis, if the Solver Type is set to Coupled Structural Thermal Analysis.
Specifies global parameters for shell element types.
Card
WRPANG = 20 (default). Shell element warpage angle in degrees. If a warpage greater than this angle is found, a warning message is printed.
ESORT = 1, full automatic sorting of triangular shell elements to treat degenerate quadrilateral shell elements as C0 triangular shells.
IRNXX = -1, shell normal update option. When set to -1, fiber directions are recomputed at each cycle.
ISTUPD = 4, shell thickness update option for deformable shells. Membrane strains cause changes in thickness in 3 and 4 node shell elements, however elastic strains are neglected. This option is very important in sheet metal forming or whenever membrane stretching is important. For crash analysis, setting 4 may improve energy conservation and stability.
THEORY = 2 (default). Belytschko-Tsay formulation.
BWC = 1. For this setting, Belytschko-Wong-Chiang warping stiffness is added.
MITER = 1 (default). Plane stress plasticity: iterative with 3 secant iterations.
PROJ = 1, the full projection method is used for the warping stiffness in the Belytschko-Tsay and Belytschko-Wong-Chiang shell elements. This option is required for explicit calculations.
NFAIL1 = 1. Flag to check for highly distorted under-integrated shell elements, print a message, and delete the element.
NFAIL4 = 1. Flag to check for highly distorted fully-integrated shell elements, print a message, and delete the element.
CNTO = 2. Flag to account for shell reference surface offsets in the contact treatment. Offsets are treated using the user defined contact thickness which may be different than the shell thickness used in the element.
Specifies global parameters for solid element types.
Card
ESORT = 1, full automatic sorting of tetrahedron and pentahedron elements to treat degeneracies. Degenerate tetrahedrons will be treated as ELFORM = 10 and pentahedron as ELFORM = 15 solids respectively (see *SECTION_SOLID).
Specifies the termination criteria for the solver.
Card
ENDTIM = End Time in the Step Controls section of the Analysis Settings.
ENDCYC = 10000000(constant) Maximum Time Steps.
DTMIN = 0.001 (constant).
ENDENG = 1000 (constant) Maximum Energy Error.
ENDMAS = 100000 (constant) Maximum Part Scaling.
This keyword is written if the simulation is determined to be a thermal one (for example, Coupled Structural Thermal Analysis). See Solver Type from the Solver Controls section of the Analysis Settings.
Card
TS = Auto Time Stepping from Thermal Step Controls (default to 1):
0 if Auto Time Stepping from Thermal Step Controls is set to No. The time step is fixed.
1 if Auto Time Stepping from Thermal Step Controls is set to Yes. The time step is variable (may increase or decrease).
TIP = Time integration parameter from Thermal Step Controls (default to Crank Nicholson Scheme TIP = 0):
0 if Time integration parameter from Thermal Step Controls is set to Crank-Nicholson scheme.
1 if Time integration parameter from Thermal Step Controls is set to Fully Implicit.
ITS = Initial Time Step from Thermal Step Controls.
TMIN = Minimum Time Step from Thermal Step Controls. If TMIN = 0.0, it is set to the structural explicit time step.
TMAX = Maximum Time Step from Thermal Step Controls. If TMAX = 0.0, it is set to 100 * the structural explicit time step.
This keyword is written if the simulation is determined to be a thermal one (for example, Coupled Structural Thermal Analysis). See Solver Type from the Solver Controls section of the Analysis Settings.
Card
ATYPE = Thermal Analysis Type from Thermal Solver Controls (default to 1)
0 if Thermal Analysis Type from Thermal Solver Controls is set to Steady State Analysis.
1 if Thermal Analysis Type from Thermal Solver Controls is set to Transient Analysis.
SOLVER = Solver Type from Thermal Solver Controls (defaults to 1):
1 if Solver Type is set to Symmetric Direct Solver.
2 if Solver Type is set to Nonsymmetric Direct Solver.
3 if Solver Type is set to Diagonal Scaled Conjugate Gradient Iterative.
4 if Solver Type is set to Incomplete Choleski Conjugate Gradient Iterative.
5 if Solver Type is set to Nonsymmetric Diagonal Scaled bi-Conjugate Gradient.
12 if Solver Type is set to Diagonal Scaling Conjugate Gradient Iterative.
13 if Solver Type is set to Symmetric Gauss-Siedel Conjugate Gradient Iterative.
14 if Solver Type is set to SSOR Conjugate Gradient Iterative.
15 if Solver Type is set to ILDLT0 Conjugate Gradient Iterative.
16 if Solver Type is set to Modified ILDLT0 Conjugate Gradient Iterative.
PTYPE = Thermal problem type from Thermal Nonlinear Controls.
0 if Thermal problem type is set to Linear Problem.
1 if Thermal problem type is set to Nonlinear problem Gauss Point Temperature.
2 if Thermal problem type is set to Nonlinear problem Element Average Temperature.
FWORK = Fraction of Work Converted into Heat from Thermal Solver Controls (defaults to 1).
This keyword is written if the simulation is determined to be a thermal one (for example, Coupled Structural Thermal Analysis). See Solver Type from the Solver Controls section of the Analysis Settings.
Card
THLSTL = Line Search from Thermal Nonlinear Controls (defaults to 0.0)
TOL = Temperature Convergence from Thermal Nonlinear Controls (defaults to 0.0).
Specifies conditions for determining the computational time step.
Card
DTINIT = 0 Initial Time Step.
TSSFAC = Time Step Safety Factor from the Step Controls section of the Analysis Settings.
ISDO = 0 (default). Basis of time size calculation for 4-node shell elements.
TSLIMT = 0 Minimum Element Timestep; the default value of 0.0 is used.
DT2MS = the negative value of Time Step Size specified in the Step Controls section of the Analysis Settings, if Automatic Mass Scaling is set to Yes. If Automatic Mass Scaling is set to No the default value of 0.0 is used.
LCTM = 0.
ERODE = 1 (constant).
MS1ST = 0 (default).
Specifies the mass weighted nodal damping applied globally to the nodes of deformable bodies and the center of mass of rigid bodies.
Card
LCID = 0, a constant damping factor will be used as specified in VALDMP.
VALDMP =Magnitude from the Damping Controls section of the Analysis Settings ( defaults to zero if Global Damping is set to No).