Controls dialog box (LS-DYNA)

General options

Name	Description
Name	Defines the name of the modeling object.
Label	Specifies a unique numerical identifier for the modeling object.

Bulk Viscosity tab options

Name	Description
*CONTROL_BULK_VISCOSITY	Select this option to globally reset the default values of the bulk viscosity coefficients. This can be helpful in certain shock wave propagation solutions.
Quadratic viscosity coefficient (Q1)	Specifies the default quadratic viscosity coefficient.
Linear viscosity coefficient (Q2)	Specifies the default linear viscosity coefficient.
Bulk viscosity type (TYPE) internal energy	Specifies the default type for bulk viscosity.(-2) Computed for shell: The internal energy dissipated by the viscosity in the shell elements is computed and included in the overall energy balance.(-1) Not computed for solid: The internal energy is not computed in shell elements.(+1) Always computed for solid: Internal energy is always computed and included in the overall energy balance for solid elements.(+2) Always computed for plane strain and axisymmetric: Internal energy is always computed and included in the overall energy balance for wo-dimensional plane strain and axisymmetric solid elements only.
Bulk viscosity type for beam (BTYPE)	Specifies the default type for bulk viscosity for beam elements.(0) Bulk viscosity turned off: Turns bulk viscosity off for beam elements.(1) Bulk viscosity turned on for beam types 1 and 11: Turns bulk viscosity on for beam types 1 and 11. The energy contribution is not included in the overall energy balance.(2) Same as (1) with energy contribution included: Turns bulk viscosity on for beam types 1 and 11. The energy contribution is not included in the overall energy balance.

Contact tab options

*CONTROL_CONTACT	Select this option to specify options for surface-based contact solutions.
Card 1
Scale factor for sliding interface penalties (SLSFAC)	Defines the scale factor for sliding interface penalties,
Scale factor for rigid wall penalties (RWPNAL)	Defines the scale factor for rigid wall penalties, which treat nodal points interacting with rigid walls.
Initial penetration check (ISLCHK)	Controls whether LS-DYNA checks for initial penetration check in contact surfaces:(1) No checking: LS-DYNA does not check for initial penetration.(2) Full check: LS-DYNA performs a full check for penetration.
Shell thickness to be considered (SHLTHK)	Controls whether LS-DYNA considers shell thickness in surface-to-surface and node-to-surface contact solutions.(0) Not considered: LS-DYNA does not consider shell thickness.(1) Considered but rigid bodies excluded: LS-DYNA considers shell thickness but excludes rigid bodies.(2) Considered including rigid bodies: LS-DYNA considers shell thickness and includes rigid bodies.
Penalty stiffness value option (PENOPT)	Controls how LS-DYNA calculates the penalty stiffness value.(1) Minimum of master segment and slave node: Uses the minimum of the master segment and slave node values.(2) Use master segment stiffness: Uses the master segment stiffness value.(3) Use slave node value: Uses the slave node stiffness value.(4) Use slave node value, area or mass weighted: Uses the slave node stiffness value, area or mass weighted.(5) Same as (4) but inversely proportional to shell thickness: Uses the slave node stiffness value, area or mass weighted, but inversely proportional to the shell thickness values.
Shell thickness changes in single surface contact (THKCHG)	Controls whether LS-DYNA considers shell thickness changes in single surface contact solutions:No consideration: LS-DYNA does not consider shell thickness changes.Include shell thickness changes: LS-DYNA includes shell thickness changes.
Automatic orientation during initialization (ORIEN)	Controls whether LS-DYNA automatically reorients contact interface segments during initialization:Active for automated (part) input only: Only reorients segments listed with the *PART keyword.Active for manual (segment) and automated (part) input only: Both manually and automatically defined segments can be reoriented.Inactive for non-forming contact: Turns reorientation off for non-forming contact problems.Inactive for forming contact: Turns reorientation off for forming contact problems (*CONTACT_FORMING and *CONTACT_DRAWBEAD types).
Treatment of mass of eroded nodes (ENMASS)	Controls how LS-DYNA treats the mass of eroded nodes in contact. This option affects all contact types where nodes are removed after surrounding elements fail. Generally, the removal of eroded nodes makes the calculation more stable; however, in problems where erosion is important, the reduction of mass will lead to incorrect results.Remove eroding nodes from the calculation: LS-DYNA removes eroded nodes from the contact solution.Eroding nodes of solid elements are retained: LS-DYNA does not remove the eroded nodes of solid elements.Eroding nodes of solid and shell elements are retained: LS-DYNA does not remove the eroded nodes of either solid or shell elements.
Card 2
Storage per contact interface control-user subroutine (USRCTR)	Specifies the amount of storage per contact interface for a user-supplied interface control subroutine, see Appendix F in the LS-DYNA Keyword User’s Manual for more information.
Storage per contact interface friction-user subroutine (USRFRC)	Specifies the amount of storage per contact interface for a user-supplied interface friction control subroutine, see Appendix F in the LS-DYNA Keyword User’s Manual for more information.
Number of cycles between contact searching (NSBCS)	Specifies the number of cycles between contact searching using three-dimensional bucket searches.
Flag for intermittent searching (INTERM)	Controls whether LS-DYNA performs intermittent searches (with the legacy surface-to-surface contact algorithm) using the interval specified in the Number of cycles between contact searching (NSBCS) box.Off: Turns intermittent searches off.On: Turns intermittent searches on.
Maximum penetration check multiplier (XPENE)	Specifies the multiplier that LS-DYNA uses for the contact surface maximum penetration check.
Flag for using actual shell thickness in single surface types (SSTHK)	Controls whether LS-DYNA uses actual shell thickness values in single surface contact solutions that use logic types 4, 13, 15 and 26.
Time step size override for eroding contact (ECDT)	Controls the time step size override for eroding contact.
Bypass projection of slave nodes to master in tied contacts (TIEDPRJ)	Controls whether LS-DYNA bypasses the projection of slave nodes to master surface in the following types of contact: *CONTACT_TIED_NODES_TO_SURFACE , CONTACT_TIED_SHELL_EDGE_TO_SURFACE, CONTACT_TIED_SURFACE_TO_SURFACE**Eliminate gaps by projection nodes: LS-DYNA projects the slave nodes.Bypass projection: LS-DYNA bypasses the projection of slave nodes.
Card 3
Default static coefficient of friction (SFRIC)	Specifies the default static coefficient of friction.For more information, see *CONTACT in the LS-DYNA Keyword User’s Manual.
Default dynamic coefficient of friction (DFRIC)	Specifies the default dynamic coefficient of friction.For more information, see *CONTACT in the LS-DYNA Keyword User’s Manual.
Default exponential decay coefficient (EDC)	Specifies the default coefficient of exponential decay.For more information, see *CONTACT in the LS-DYNA Keyword User’s Manual.
Default viscous friction coefficient (VFC)	Specifies the default coefficient of viscous friction.For more information, see *CONTACT in the LS-DYNA Keyword User’s Manual.
Default contact thickness (TH)	Specifies the default thickness value for contact.For more information, see *CONTACT in the LS-DYNA Keyword User’s Manual.
Default thickness scale factor (TH_SF)	Specifies the default thickness scale factor.For more information, see *CONTACT in the LS-DYNA Keyword User’s Manual.
Default local penalty scale factor (PEN_SF)	Specifies the default, local penalty scale factor.For more information, see *CONTACT in the LS-DYNA Keyword User’s Manual.
Card 4
Ignore initial penetrations in automatic contact (IGNORE)	Sets the default for how LS-DYNA handles initial penetrations for automatic contact solutions.(0) Move nodes to eliminate interference: Moves nodes to eliminate initial penetrations.(1) Allow initial penetrations: Allows initial penetrations to exist. With this option, LS-DYNA tracks the initial penetrations.(2) Same as (1) with printing messages: Allows initial penetrations to exist. LS-DYNA prints penetration warning messages.
Calculation of frictional sliding energy (FRCENG)	Controls whether LS-DYNA calculates frictional sliding energy.(0) Do not calculate: LS-DYNA does not calculate frictional sliding energy.(1) Calculate and store as Surface Energy Density in binary INTFOR file: LS-DYNA calculates frictional energy and stores it as Surface Energy Density in the binary INTFOR file.
To visualize stationary rigid wall (SKIPRWG)	Controls whether LS-DYNA displays the stationary rigid wall by default.(0) Generate 4 extra nodes and 1 shell element: LS-DYNA generates four extra nodes and one shell element to help you visualize a stationary, planar rigid wall.(1) Do not generate stationary rigid wall: LS-DYNA does not generate a stationary rigid wall.
*Write beam spot weld slave/master of CONTACT_SPOTWELD in D3HSP file (OUTSEG)	Controls whether LS-DYNA outputs each beam spot weld slave node and its master segment for contact type: *CONTACT_SPOTWELD into the D3HSP file.
Should error termination occur related to spot weld material (SPOTSTP)	Controls whether LS-DYNA terminates a solve with an error if a spot weld node or face, which is related to a MAT_SPOTWELD beam or solid element, respectively, cannot be found on the master surface.**(0) No, continue calculation*: LS-DYNA deletes the spot weld and continues the calculation.(1) Yes, print error message and terminate: LS-DYNA prints and error message and terminates the solve.(2) No, delete unconstrained weld and continue: LS-DYNA deletes the spot weld, prints a message that the deletion has occurred, and continues the calculation.
Delete spot weld attached to shell (SPOTDEL)	If the nodes of a spot weld beam or solid element are attached to a shell element that fails and those nodes are deleted, this option controls whether LS-DYNA deletes the attached spot weld element.
Optional thickness scale factor (SPOTHIN)	Lets you specify an optional thickness scale factor. Specify a value greater than zero, but less than one.Premature failure of spot welds can occur due to contact of the spot welded parts in the vicinity of the spot weld. This contact creates tensile forces in the spot weld. Although this seems physical, the compressive forces generated in the contact are large enough to fail the weld in tension before failure is observed in experimental test. With this option, the thickness of the parts in the vicinity of the weld are automatically scaled, the contact forces do not develop, and the problem is avoided.Note: This option only applies to automatic single surface contact solutions.
Card 5
Symmetry plane default when contact defined by part ID (ISYM)	Specifies the default for the symmetry plane option for automatic segment generation when contact is defined by part IDs.(0) Off: Turns the symmetry plane off.(1) Do not include faces with normal boundary constraints: Excludes faces with normal boundary constraints, such as segments of brick elements on a symmetry plane.
Flag to use one-way node to surface erosion (NSEROD)	Controls whether LS-DYNA uses a one-way or a two-way algorithm for surface erosion.
Flag to add rigid wall gap stiffness (RWGAPS)	Controls whether LS-DYNA adds rigid wall gap stiffness.
Death time for gap stiffness (RWGDTH)	Specifies the time after which LS-DYNA does not add the gap stiffness.
Rigid wall penalty scale factor for implicit calculations (RWKSF)	Specifies the rigid wall penalty scale factor to use for contact with deformable parts during implicit calculations.Note: This value is independent of SLSFAC and RWPNAL. If RWKSF is also specified in *RIGIDWALL_PLANAR, the stiffness is scaled by the product of the two values.Rigid wall penalty scale factor for contact with deformable parts during implicit calculations.
Invoke the covariant formulation of Konyukhov and Schweizerhof (ICOV)	Specifies whether to use the covariant formulation of Konyukhov and Schweizerhof with the FORMING contact option.
Spot weld radius scale factor for neighbor segment thinning (SWRADF)	Lets you specify an optional scale factor to apply to spot weld radii for neighbor segment thinning.If you do not specify a scale factor, LS-DYNA does not thin neighbor segments.If you do specify a scale factor, LS-DYNA scales the radius of beam spot welds by this value while searching for close neighbor segments to thin.
Offsetting thermal contact surfaces for thick shells (ITHOFF)	Controls whether LS-DYNA offsets thermal contact surfaces for thick thermal shells.(0) No offset: LS-DYNA does not offset thermal contact surfaces.(1) Apply offsets, heat transfer between the outer contact surfaces: LS-DYNA applies offsets so that contact heat transfer is always between the outer surfaces of the contact segments (shells).
Card 6
Assuming edge shape for shells when measuring penetration (SHLEDG)	Controls the edge shape that LS-DYNA assumes for shell elements when measuring penetration.(0) Round: LS-DYNA assumes that the shell element edges are round.(1) Square: LS-DYNA assumes that the shell element edges are square and are flush with the nodes.
Method for calculating the penalty stiffness (PSTIFF)	Specifies the method that LS-DYNA uses to calculate the penalty stiffness for segment-based contact.Based on material density: LS-DYNA uses the material density and segment dimensions to calculate the stiffness.Based on nodal masses: LS-DYNA uses the nodal masses to calculate the penalty stiffness.

Energy tab options

Name	Description
*CONTROL_ENERGY	Select this option to specify controls for energy dissipation options.
Hourglass energy option	Controls whether the software calculates hourglass energy.Select Not computed if you do not want to calculate hourglass energy.Select Computed to calculate hourglass energy. This option requires additional storage and may increase the solve time. LS-DYNA reports hourglass energies in the GLSTAT and MATSUM ASCII files.
Stonewall energy dissipation option	Controls whether the software computes Stonewall energy dissipation.Select Not computed if you do not want to calculate the energy dissipation.Select Computed to calculate the energy dissipation. LS-DYNA reports hourglass energies in the GLSTAT ASCII file.
Sliding interface energy dissipation option	Controls whether the software computes the energy dissipation at a sliding interface.Select Not computed if you do not want to calculate the energy dissipation.Select Computed to calculate hourglass energy to calculate the energy dissipation. LS-DYNA reports hourglass energies in the GLSTAT and SLEOUT ASCII files.
Rayleigh energy dissipation option	Controls whether the software computes the Rayleigh damping energy dissipation.Select Not computed if you do not want to calculate the energy dissipation.Select Computed to calculate hourglass energy to calculate the energy dissipation. LS-DYNA reports hourglass energies in the GLSTAT ASCII file.

Hourglass tab options

Name	Description
*CONTROL_HOURGLASS	Select *CONTROL_HOURGLASS to redefine the default values of the hourglass control type and coefficient. Hourglass control is viscosity or stiffness that is added to quadrilateral shell elements and hexahedral solid elements that use reduced integration. Without hourglass control, these elements would have zero energy deformation modes, which could grow large and destroy the solution.
Hourglass Viscosity Type	Lets you specify the default hourglass viscosity type. This option corresponds to the IHQ variable for the *CONTROL_HOURGLASS keyword.
Hourglass Coefficient	Lets you specify a value for the default hourglass coefficient. This option corresponds to the QH variable for the *CONTROL_HOURGLASS command. Specifying a value that exceeds 0.15 may cause instabilities.

Output tab options

*CONTROL_OUTPUT	Select *CONTROL_OUTPUT to control optional output.
Card 1 (Output)
Print suppression during input phase for D3SHSP (NPOPT)	Specifies whether to suppress printing to the d3hsp file during the input phase.(0) No suppression: LS-DYNA does not suppress printing.(1) LS-DYNA does not print nodal coordinates, element connectivity information, rigid wall definitions, nodal SPCs, initial velocities, initial strains, adaptive constraints, and spr2/spr3 constraints.
Print suppression during input phase for echo file (NEECHO)	Controls whether LS-DYNA suppresses printing during input phase for the echo file.(0) Print all data: LS-DYNA prints all data to the echo file.
Update reference node coordinates for beam foundations 12 and 11 (NREFUP)	Controls whether LS-DYNA updates the coordinates of reference nodes for beam formulations 1, 2, and 11.(0) Do not update: LS-DYNA does not update the reference node.(1) Update: LS-DYNA updates the reference node coordinates. If you select this option, each reference node must be unique to the beam element.
Average filter nodal accelerations and time history (IACCOP)	Controls whether LS-DYNA filters nodal acceleration output to the file nodout and the time history database d3thdt.(0) No average: LS-DYNA does not filter the output.(1) Averaged between output intervals” LS-DYNA averages the output between output intervals.(2) Filter accelerations: LS-DYNA internally stores accelerations for each time step and then filters them over each output interval using a filter from General Motors [Sala, Neal, and Wang, 2004] based on a low-pass Butterworth frequency filter. See also [Neal, Lin, and Wang, 2004]. The Time step size for mass scaled solutions option on the Time Step tab must be set to a negative value when you select this option so that the maximum possible number of time steps for an output interval is known, and LS-DYNA can allocate adequate memory.
Output time interval for interface file (OPIFS)	Specifies the output time interval for the interface file written per the *INTERFACE_- COMPONENT_ option.
Flag controlling output of elements based on initial time step size (IPNINT)	Controls the of initial time step sizes for elements that are printed to the d3hsp file.
Problem status report interval steps to D3HSP (IKEDIT)	Specifies the problem interval steps for the problem status report in the d3hsp file.Note: LS-DYNA ignores this option if you use select the Global Data (DATABASE_GLSTAT) option on the General Options tab of the Database dialog box.
Number of time steps interval for flushing I/O buffers (IFLUSH)	Specifies the number of time step intervals after which LS-DYNA should flush the input/output buffers. If LS-DYNA does not empty the buffers and the solve terminates abnormally, the output files may be incomplete. This option does not apply to restart files; LS-DYNA automatically empties the buffers for restart files whenever a restart file is written.
Card 2 (Output)
Default print flag for RDBOUT and MATSUM (IPRTF)	Controls whether LS-DYNA prints data to the rbdout and matsum files by default. This option allows you to reduce the file sizes by eliminating data which is not of interest.
Output eroded internal and kinetic energy to MATSUM (IERODE)	Controls whether LS-DYNA outputs eroded internal, kinetic energy, and extra data into the matsum file. This extra data includes the kinetic energy from nonstructural mass, lumped mass elements, and lumped inertia elements.
Output ten connectivity nodes to D3PLOT (TET10)	Controls whether LS-DYNA outputs ten connectivity nodes or only the four corner nodes of the ten node connectivity into the d3plot database.
Maximum number of each error warning message (MSGMAX)	Specifies the maximum number of each error warning message.
Output digitized curve data (IPCURV)	Controls whether LS-DYNA outputs digitized curve data to the messag and d3hsp files.
Output interval for recorded motions from INTERFACE_SSI_AUX (GMDT)	Specifies the output interval for recorded motions from the *INTERFACE_SSI_AUX keyword.
Output information of 1D seatbelt created for 2D (IP1DBLT)	Controls the output of information to the sbtout file for the 1D (bar-type) seatbelt created for 2D (shell-type) seat belt.(0) Store processed 2D belt information: The analysis results of internally created 1D seat belts are extracted and processed to yield the 2D belt information. The 2D belt information is stored in the sbtout file.(1) Store 1D seatbelts: The analysis results of internally created 1D retractors are stored in the sbtout file. You can use the *DATABASE_CROSS_SECTION keyword to find the belt load information.

Shell tab options

*CONTROL_SHELL	Select *CONTROL_SHELL to select options for computing shell response.
Card 1 (Shell)
Shell element warpage angle (WRPANG)	Specifies the maximum shell element warp angle in degrees. If LS-DYNA detects a shell with a warp value greater than this angle, it prints a warning message.
Automatic sorting of triangular shell elements (ESORT)	Controls the sorting of triangular shell elements to automatically switch degenerate quadrilateral shell formulations to more suitable triangular shell formulations.(0) No sorting: LS-DYNA does not sort the elements.(1) Full sorting, C0 triangular elements: LS-DYNA switches degenerate elements to the C0 triangular shell formulation 4, or to formulation 24 (for quadratic shells).(2) Full sorting, DKT triangular shells: LS-DYNA switches degenerate elements to the DKT triangular shell formulation 17, to shell formulation 24 (for quadratic shells). The DKT formulation is unstable if it is used to model an uncommonly thick, triangular shell.
Shell normal update option (IRNXX)	Controls how shell elements with the Hughes-Liu, Belytschko-Wong-Chiang, and the Belytschko-Tsay shell formulations update.Note: Elements with the Belytschko-Tsay formulation are only affected if you selected the warping stiffness option (BWC=1).
Shell thickness change option (ISTUPD)	Specifies the thickness change option for deformable shell elements.Note: Use the Shell part set ID with no thickness update (PSTUPD) option to apply this setting by part ID.
Default shell formulation (THEORY)	Specifies the default formulation for shell elements. For a complete list of shell formulations, see Remark 2 for *SECTION_SHELL in the LS-DYNA Keywords Reference Manual.
Warping stiffness for Belytshchko-Tsay shells (BWC)	Controls warping stiffness for shell elements with the Belytshchko-Tsay formulation.
Plane stress plasticity option (MITER)	Specifies the plane stress plasticity option for materials 3, 18, 19, and 24.
Projection method for warping stiffness (PROJ)	Specifies the projection method for warping stiffness for shell elements that use the Belytschko-Tsay or Belytschko-Wong-Chiang formulations.Note: This option applies to explicit calculations only because the full projection method is always used if the solution is implicit.
Card 2 (Shell)
Scale factor for rotary shell mass (ROTASCL)	Defines a scale factor for rotary mass of shell elements.Note: This option is not for general use. The rotary inertia for shells is automatically scaled to permit a larger time step size. LS-DYNA does not recommend changing the scale factor to a value other than the default.
Shell through thickness integration rule (INTGRD)	Specifies the default through thickness numerical integration rule for shell and thick shell elements.(0) Gauss integration: Specifies Gauss integration. This is the default integration rule if 1–10 integration points are specified.(1) Lobatto integration: Specifies Lobatto integration. This is the default integration rule if 3–10 integration points are specified. For two-point integration, the Lobatto rule is very inaccurate; Gauss integration is used instead. However, Lobatto integration has an advantage in that the inner and outer integration points are on the shell surfaces.Note: If more than 10 integration points are requested, LS-DYNA uses a trapezoidal rule instead.
Laminated shell theory (LAMSHT)	Specifies whether to use laminated shell theory for thin shell and thick shell materials. This option does not apply to materials that use the Green-Lagrange strain (which occurs if you select options (3), (4), or (5)) and by using the *PART_COMPOSITE or *INTEGRATION_SHELL keywords to define the integration rule.Lamination theory corrects for the assumption of a uniform constant shear strain through the thickness of the shell. Unless this correction is applied, the stiffness of the shell can be grossly incorrect if there are drastic differences in the elastic constants from ply to ply, especially for sandwich type shells. Generally, without this correction the results are too stiff. For discrete Kirchhoff shell elements, which do not consider transverse shear, this option is ignored.
Coordinate system for type 6 shell (CSTYP6)	Specifies the coordinate system to use for type 6 shell elements.(1) Variable local coordinate system: LS-DYNA computes a unique, local system at each in-plane point.(2) Uniform local system: LS-DYNA computes one system that is used throughout the shell element. This involves fewer calculations and is the more efficient method.
Thermal shell option (TSHELL)	Specifies the thermal shell option for thermal and coupled structural thermal analyses.If you specify a value of 0, LS-DYNA does not calculate a temperature gradient through the shell thickness.If you specify a value of 1, LS-DYNA calculates a temperature gradient through the shell thickness.
Check highly distorted under-integrated shells (NFAIL1)	Controls how LS-DYNA handles highly distorted, under-integrated shell elements. Depending on the option you select, LS-DYNA prints a message, deletes the elements, or terminates the analysis. A distorted element is one where a negative Jacobian occurs within the domain of the shell, not just at its integration points.
Check highly distorted fully-integrated shells (NFAIL4)	Controls how LS-DYNA handles highly distorted, fully-integrated shell elements. Depending on the option you select, LS-DYNA prints a message, deletes the elements, or terminates the analysis.
Shell part set ID checked by NFAIL1 and NFAIL4 (PSNFAIL)	Lets you specify which part IDs that LS-DYNA checks with the NFAIL1 and NFAIL4 options. If you do not specify a list of part IDs, LS-DYNA checks all part IDs.
Card 3 (Shell)
Shell part set ID with no thickness update (PSTUPD)	Specifies the optional shell part set ID that identifies which part IDs have or do not have their thickness values updated. By default, the shell thickness update applies to all shell elements in the mesh.
In plane integration rule for the 8 node shell (IRQUAD)	Specifies the in-plane integration rule for shell elements with 8 nodes.

Solid tab options

Name	Description
*CONTROL_SOLID	Select *CONTROL_SOLID to specify options that control the response of solid elements.
Automatic sorting of tetrahedron and pentahedron elements (ESORT)	Controls whether LS-DYNA automatically sorts tetrahedron and pentahedron elements to treat degenerate tetrahedron and pentahedron elements (cohesive elements formulation 19 and 20) as tetrahedron (formulation 10) and pentahedron (formulation 15, cohesive elements formulation 21, 22) solids, respectively.
Calculation method of the deformation gradient ratio (FMATRX)	Specifies the default method that LS-DYNA uses to calculate the deformation gradient matrix.
Number of integration points for quadratic tetrahedron elements (NPTETS)	Specifies whether to use 4 or 5 integration points in quadratic tetrahedral elements.Note: This option applies to type 4, 16, and 17 tetrahedron elements.
Output option for stresses in solid used as spot welds (SWLOCL)	Sets the output option for stresses in solid elements that are used as spot welds with material *MAT_SPOTWELD.

Termination tab options

Name	Description
*CONTROL_TERMINATION	Select *CONTROL_TERMINATION to specify options that control when the software stops the solve.
Termination time (ENDTIM)	Lets you specify the termination time (in seconds, minutes, or hours) for the solve. You must specify a termination time.
Termination cycle (ENDCYC)	Lets you specify a termination cycle. A termination cycle is optional. LS-DYNA uses this value if it reaches the specified cycle before the specified Termination time.
Reduction factor (DTMIN)	Lets you specify a reduction or scale factor for the initial time step size to determine the minimum time step.
Percent change in energy ratio (ENDNEG)	Lets you specify an optional percent change in the energy ratio. When this change occurs, LS-DYNA terminates the solve.
Percent change in total mass (ENDMAS)	Lets you specify an optional percent change in the total mass. When this change occurs, LS-DYNA terminates the solve. This option is only relevant if you used mass scaling to limit the minimum time step size.
Flag for a non-solution run (NOSOL)	Controls whether LS-DYNA terminates normally after initialization for a non-solution run.

Time Step tab options

*CONTROL_TIMESTEP	Select *CONTROL_TIMESTEP to specify options for time steps.
Card 1
Initial time step size (DTINIT)	Specifies the size of the initial time step.
Scale factor for computed time step (TSSFAC)	Specifies a scale factor for the computed time step.
Basis of time size for shell elements (ISDO)	Controls the basis that LS-DYNA uses to calculate the size of time steps for shell elements with four nodes.
Shell element minimum time step (TSLIMT)	When a shell element controls the time step, LS-DYNA modifies element material properties (moduli, not masses) such that the time step does not fall below the assigned time step size. This option only applies to shell elements that use the following material models: *MAT_PLASTIC_KINEMATIC, *MAT_POWER_LAW_PLASTICITY, *MAT_STRAIN_RATE_DEPENDENT_PLASTICITY, and *MAT_PIECE- WISE_LINEAR_PLASTICITY.
Time step size for mass scaled solutions (DT2MS)	Specifies the time step size for solutions with mass scaling.
Load curve ID that limits the maximum time step size (LCTM)	Specifies an optional load curve ID that limits the maximum time step size. This load curve defines the maximum time step size permitted versus time. If the solution time exceeds the final time value defined by the curve, then the computed step size is used. If the time step size from the load curve is exactly zero, the computed time step size is also used.
Erosion flag for solid and t-shell elements (ERODE)	Controls the erosion flag for solid, thermal shell, and SPH elements when the specified TSMIN (*CONTROL_TERMINATION keyword) is reached.
Limit mass scaling to the first step (MS1ST)	Controls how mass scaling is handled during the analysis.(0) No: Mass scaling is considered throughout the analysis. Added mass may increase with time but it never decreases.(1) Yes: Added mass is calculated at the first time step and remains unchanged thereafter.
Card 2
Scale factor for initial time step size (DT2MSF)	Specifies the reduction (or scale) factor for the initial time step size.
Load curve ID by specifying DT2MS (DT2MSLC)	Specifies the ID of the load curve that defines the time step size for mass scaled solutions (DT2MS) as a function of time during the explicit solutions phase. You can use a load curve only to increase the magnitude of DT2MS. Consequently, the magnitude of DT2MS is taken as the maximum of the current value and the value from the load curve.
Flag for selective mass scaling (IMSCL)	Controls whether LS-DYNA selectively scales mass if mass scaling is active for the solution. Selective mass scaling does not scale the rigid body mass and is therefore more accurate.Note: Because selective mass scaling is memory and CPU intensive, you should only apply it to small, finely meshed parts.
Flag for selective mass scaling (RMSCL)	Controls whether only translational inertia are mass scaled or whether both translational and rotational inertia are mass scaled.

MPP_DECOMPOSITION tab options

*CONTROL_MPP_DECOMPOSITION_SHOW	Select *CONTROL_MPP_DECOMPOSITION_SHOW to control the display of the final decomposition.
*CONTROL_MPP_DECOMPOSITION_TRANSFORMATION	Select *CONTROL_MPP_DECOMPOSITION_TRANSFORMATION to specify transformations to apply to modify the decomposition.
TYPE=RXTYPE=RYTYPE=RZ	Lets you select the directions in which to apply a rotational transformation.
Amount of rotation to apply (VAL)	Lets you specify the amount of rotation to apply in the selected directions.
TYPE=SXTYPE=SYTYPE=SZ	Lets you select the directions in which to apply a scaling transformation.
Amount of scaling to apply (VAL)	Lets you specify the amount of scaling to apply in the selected directions.
TYPE=VEC3TYPE=C2RTYPE=S2R****TYPE=S2R	Lets you specify the type of transformation to apply.
Parameter to the transformation (V1–V9)	Lets you specify the value for each parameter to the transformation.For more information, see *CONTROL_MPP_DECOMPOSITION_TRANSFORMATION in the LS-DYNA Keyword User’s Manual, Vol. 1

Learn more

Allocating DBset size

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Controls dialog box (LS-DYNA), Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });