Load Steps

Load step entities are used to define and store load cases for a given analysis. Load steps are defined by selecting the associated load collectors and output blocks which define the load step. Load steps are shown under the Loadstep folder within the Model browser. Some solver interfaces also support the Load Step browser to create and edit load steps.

Load steps have a display state, on or off, which controls the display state of load collectors associated with the load step in the graphics area. The display state of a load step can be controlled using the icon next to the load step entity in the Model browser.

Load steps also have an active and export state. The active state of a load step controls the display state of the load step and the listing of the load step in the Model browser and any of its views. If a load step entity is active, then its display state is available to be turned on or off and it is listed in the Model browser and any of its views. If a load step entity is inactive, then its display state is turned off permanently and it is not listed in the Model browser or any of its views.

The export state of a load step entity controls whether or not that load step is exported when the custom export option is utilized. The all export option is not affected by the export state of a load step. The active and export states of load step entities can be controlled using the Entity State browser.

The data names associated with load steps can be found in the data names section of the HyperMesh Reference Guide.

The following panels can be used to create and edit load steps:

Load Steps

Solver Card Support for Load Steps

The Loadsteps panel generates entities called loadsteps. These loadsteps directly correspond to OptiStruct subcases.

Use the Loadsteps panel to explicitly define load collectors as the referenced static load (LOAD), constraint (SPC), dynamic load (DLOAD), etc. for a subcase. Other OptiStruct input data is automatically generated or may be added to the subcase definition through the edit function.

You can choose the analysis type for the subcase being defined. This will filter the data selectors displayed, so that only those appropriate for the selected analysis type (solution sequence) are displayed. There is also a generic option which will display all selectors.

The following table describes how different OptiStruct Subcase information and I/O Option entries are generated on a subcase level:

Supported Card	Solver Description	Supported Parameters	Notes
ACCELERATION	Control acceleration results output on a subcase level.		Select a subcase (loadstep) and click edit. Check the box next to Output and then the one next to Acceleration.
ANALYSIS	Define a solution sequence for individual subcases.		Select a subcase (loadstep) and click edit. Check the box next to ANALYSIS and then select an analysis type.
CMSMETH	Defines the method, frequency upper limit, and number of modes to be used in component mode synthesis for flexibly-body preparation solution sequence.		Select a component mode synthesis method definition for use in a subcase. Check the box next to CMSMETH and select a load collector with a CMSMETH card image.
CSTRAIN	Control ply strain results output for composites on a subcase level.		Select a subcase (loadstep) and click edit. Check the box next to Output and then the one next to Cstrain.
CSTRESS	Control ply stress results output for composites on a subcase level.		Select a subcase (loadstep) and click edit. Check the box next to Output and then the one next to Cstress.
DESOBJ	Define a subcase specific objective.		Part of the optimization problem setup, created in the Objectives panel.
DESSUB	Define a subcase specific design constraint.		Part of the optimization problem setup, created in the Dconstraints panel.
DISPLACEMENT	Control displacement results output on a subcase level.		Select a subcase (loadstep) and click edit. Check the box next to Output and then the one next to Displacement.
DLOAD	Select dynamic loading information for a subcase.		Check the box next to DLOAD and select a load collector with dynamic loading information (DLOAD, RLOAD1, RLOAD2, TLOAD1, TLOAD2).
EIGVRETRIEVE	Retrieve eigenvalue and eigenvector results from a normal modes analysis from an external data file.		Select a subcase (loadstep) and click edit. Check the box next to EIGVRETRIEVE, choose the number of integer values to be defined, and enter the integer values in the card previewer.
EIGVSAVE	Output eigenvalue and eigenvector results from a normal modes analysis to an external data file.		Select a subcase (loadstep) and click edit. Check the box next to EIGVSAVE, and enter an integer value in the card previewer.
ELFORCE	Control elemental force results output on a subcase level.		Select a subcase (loadstep) and click edit. Check the box next to Output and then the one next to Elforce.
ERP	Control equivalent radiated power output on a subcase level.		Select a subcase (loadstep) and click edit. Check the box next to Output and then the one next to ERP.
ESE	Control element strain energy results output on a subcase level.		Select a subcase (loadstep) and click edit. Check the box next to Output and then the one next to Ese.
EXCLUDE	Select a set of properties to be excluded from a linear buckling analysis.		Select a subcase (loadstep) and click edit. Check the box next to EXCLUDE, then select a SET definition from the card previewer.
FATDEF	Select elements, and associated fatigue properties for fatigue analysis		Check the box next to FATDEF and select a load collector with a FATDEF card image.
FATPARM	Select parameters for fatigue analysis.		Check the box next to FATPARM and select a load collector with a FATPARM card image.
FATSEQ	Select loading sequence for fatigue analysis.		Check the box next to FATSEQ and select a load collector with a FATSEQ card image.
FREQUENCY	Select the set of forcing frequencies to be solved in a frequency response problem.		Check the box next to FREQ and select a load collector containing frequency information (FREQ, FREQ1, FREQ2, FREQ3, FREQ4, FREQ5).
GLOBSUB	Global Model and Transfer Zone Selection		Select a subcase (loadstep) and click edit. Check the box next to GLOBSUB and select loadstep and grid set.
GPFORCE	Control grid point force results output on a subcase level.		Select a subcase (loadstep) and click edit. Check the box next to Output and then the one next to Gpforce.
GPSTRESS	Control grid point stress results output on a subcase level.		Select a subcase (loadstep) and click edit. Check the box next to Output and then the one next to Gpstress.
IC	Select initial conditions for a transient analysis subcase.		Check the box next to IC and select a load collector with initial condition information (TIC).
INVEL	Select multi-body dynamics initial velocity information for a subcase.		Check the box next to INVEL and select a load collector with initial velocity information (INVELB).
LABEL	Provide a label for a subcase.		Select a subcase (loadstep) and click edit. Check the box next to LABEL and enter a label in the card previewer.
LOAD	Select static loading information for a subcase.		Check the box next to LOAD and select a load collector containing static loads (FORCE, MOMENT, PLOAD, PLOAD2, PLOAD4, LOAD), or inertial loading information (GRAV, RFORCE).
MBSIM	Select a multi-body dynamics simulation definition for a subcase.		Check the box next to MBSIM and select the load collector with an MBLIN, MBSEQ or MBSIM card image.
METHOD	Select eigenvalue extraction information for a subcase.		Check the box next to METHOD(STRUCT) or METHOD(FLUID) and select a load collector with an EIGRL card image.
MLOAD	Select multi-body dynamics loading information for a subcase.		Check the box next to MLOAD and select a load collector containing multi-body dynamics loads (GRAV, MBFRC, MBFRCC, MBMNT, MBMNTC, MLOAD).
MODEWEIGHT	Define a multiplier for computed eigenvalues that are to be used in the calculation of the "weighted reciprocal eigenvalue" and "combined compliance index" optimization responses.		Part of the optimization problem setup, created in the Responses panel.
MOTION	Select multi-body dynamics motion information for a subcase.		Check the box next to MOTION and select a load collector containing multi-body dynamics motions (MOTION, MOTNG, MOTNGC).
MPC	Select multi-point constraints for use in a subcase.		Check the box next to MPC and select a load collector containing MPCs.
MPCFORCE	Control MPC force results output on a subcase level.		Select a subcase (loadstep) and click edit. Check the box next to Output and then the one next to Mpcforce.
NLPARM	Select non-linear static analysis settings for use in a subcase.		Check the box next to NLPARM and select a load collector with an NLPARM card image.
NSM	Select non-structural mass input for entire model.		Check the box nex to NSM and select a group with a NSM1 or NSML1 card image or select a load collector with a NSMADD card image. This option is not allowed in the subcase.
OFREQUENCY	Define a set of frequencies for output requests for a subcase.		Select a subcase (loadstep) and click edit. Check the box next to Output and then the one next to Ofrequency.
OLOAD	Request the output of applied loads for a subcase.		Select a subcase (loadstep) and click edit. Check the box next to Output and then the one next to Oload.
OMODES	Define a set of modes for output requests for a normal modes or linear buckling subcase.		Select a subcase (loadstep) and click edit. Check the box next to Output and then the one next to Omodes.
RESVEC	Control the calculation of modal acceleration vectors.		Select a subcase (loadstep) and click edit. Check the box next to RESVEC and choose the desired TYPE and OPTION in the card previewer.
RSPEC	Select response spectra information for use in a subcase.		Check the box next to RSPEC and select a load collector containing response spectra analysis information (RSPEC).
RWALL	Defines a rigid wall of the following types: Infinite Plane, Infinite Cylinder, Sphere and Parallelogram.		Check the box next to RWALL or RWLADD and select a group (RWALL) or a load collector (RWALADD).
SDAMPING	Select damping information for use in a subcase.		Check the box next to SDAMPING and select a load collector containing damping information (TABDMP1).
SOLVTYP	Select the iterative solver.		Select a linear static subcase (loadstep) and click edit. Check the box next to SOLVTYP and then choose a load collector with the SOLVTYP card image.
SPC	Select single-point constraints for use in a subcase.		Check the box next to SPC and select a load collector containing SPCs.
SPCFORCES	Control SPC force results output on a subcase level.		Select a subcase (loadstep) and click edit. Check the box next to Output and then the one next to Spcf.
STATSUB	Select a linear static subcase for linear buckling analysis.		Check the box next to STATSUB and select a static subcase.
STRAIN	Control strain results output on a subcase level.		Select a subcase (loadstep) and click edit. Check the box next to Output and then the one next to Strain.
STRESS	Control stress results output on a subcase level.		Select a subcase (loadstep) and click edit. Check the box next to Output and then the one next to Stress.
SUBCASE	Define a subcase.		Created automatically, when a new subcase is created. The subcase ID matches the ID of the HyperMesh loadstep entity.
SUBCOM	Defines a combination subcase.		Created automatically, when a new load step of type “Combination Subcase Delimiter” is created. The SUBCOM ID matches the ID of the HyperMesh loadstep entity.
SUBMODEL	Subcase-specific Model Selection		Select a subcase (loadstep) and click edit. Check the box next to SUBMODEL and select set ids.
SUBSEQ	Subcase sequence coefficients.		Select a subcom (loadstep) and click edit. Check the box next to SUBSEQ and input the combination coefficients.
SUBTITLE	Provide a subtitle for a loadstep.		Select a subcase (loadstep) and click edit. Check the box next to SUBTITLE and enter a subtitle in the card previewer.
SUPORT1	Select fictitious supports for use in a subcase.		Check the box next to SUPORT1 and select a load collector containing SUPORT1 loads.
TEMP	Select thermal loading information for a subcase.		Check the box next to TEMP and select a load collector containing TEMP loads or a load collector with the TEMPD card image.
TSTEP	Select integration and time step information for a transient analysis subcase.		Check the box next to TSTEP and select a load collector with the TSTEP card image. Set the toggle to either TIME or FOURIER, depending on the type of transient solution desired.
TTERM	Define the termination time of a geometric non-linear subcase		Check the box next to TTERM and input a real value for the termination time.
VELOCITY	Control velocity results output on a subcase level.		Select a subcase (loadstep) and click edit. Check the box next to Output and then the one next to Velocity.
WEIGHT	Define a weighting factor (multiplier) for the compliance of a linear static or inertia relief subcase, which is used in the calculation of the "weighted compliance" and "combined compliance index" optimization responses.		Part of the optimization problem setup, created in the Responses panel.
XHIST	Select time history output for geometric non-linear analysis		Check the box next to XHIST or XHISADD and select a group (XHIST) or a load collector (XHISADD).

A load step corresponds to a *STEP definition in Abaqus model history. Load collectors, output blocks and groups within a load step are exported under the corresponding *STEP block in the Abaqus input deck. It is recommended that all history (*STEP) data be defined from the Step Manager in the Abaqus user profile.

Supported Cards	Solver Description	Supported Parameters	Notes
*ADAPTIVE MESH	Defines an adaptive mesh domain and specifies the frequency and intensity of adaptive meshing for that domain.	EISet AdaptiveMeshOP Controls Frequency MeshSweeps	Defined in the load step card image.
*BUCKLE	Obtain eigenvalue buckling estimates	EigenSolver (None, Subspace, Lanczos)	Defined in the load step card image.
*BULK VISCOSITY	Modify bulk viscosity parameters	b1, b2	Explicit template only. History data.
*COUPLED TEMP-DISPLACEMENT	Analyze problems where the simultaneous solution of the temperature and stress/displacement fields are necessary.	SteadyState Deltmx TimeIncrement TotalTimePeriod Minimum Maximum	Defined in the load step card image.
*DYNAMIC (Explicit)	Dynamic stress/displacement analysis	Time Incrementation Option (None, Direct_User_Control, Element_By_Element, Fixed_Time_Incrementation) Adiabatic Scale Factor ImprovedDtMethod (YES, NO) Time Period	Defined in the load step card image.
*DYNAMIC (Standard)	Dynamic stress/displacement analysis	Subspace Adiabatic Alpha SingularMass Application (TRANSIENT FIDELITY, MODERATE DISSIPATION, QUASI-STATIC) EigenSolver (None, Haftol, Direct, Direct_No_Stop) Initial NoHaf Initial Increment Total Period Minimum Increment Maximum Increment	Defined in the load step card image.
*FILE FORMAT	Specify format for results file output and invoke zero-increment results file output	Options (Binary, ASCII) ZeroIncrement	Defined in the load step card image.
*FREQUENCY	Extract natural frequencies and modal vectors	Option (LANCZOS, SUBSPACE, AMS) Normalization (None, Displacement, Mass) Property Evaluation Nset Frequency SIM Damping Projection (ON, OFF) AcousticCoupling (ON, OFF, PROJECTION) Bias NumberInterval No. Of Eeigen Minimum Frequency Maximum Frequency AMS_CutOff_1 AMS_CutOff_2 AMS_CutOff_3 AMS_Range_Fac ResidualModes	Defined in the load step card image.
*HEAT TRANSFER	Transient or steady-state uncoupled heat transfer analysis	Deltmx End (PERIOD, SS) SteadyState Mxdem Time Increment Time Period Minimum Time Increment Maximum Time Increment	Defined in the load step card image.
*LOAD CASE	Begin a load case definition for multiple load case analysis	Number_of_LoadCase LoadCase_maximum_data_ lines	Defined in the load step card image.
*MODAL DYNAMIC	Dynamic time history analysis using modal superposition	Continue (YES, NO) Time Increment Time Period	Defined in the load step card image.
*MONITOR	Define a degree of freedom to monitor	Value NodeSet Node Frequency	Defined in the load step card image.
*PRINT	Request or suppress output to the message file in an Abaqus/Standard analysis or to the status file in an Abaqus/Explicit analysis	Contact (NO, YES) ModelChange (NO, YES) Frequency Plasticity (NO, YES) Residual (YES, NO) Solve (NO, YES) AdaptiveMesh (NO, YES)	Defined in the load step card image.
*RADIATION_ VIEWFACTOR	Control the calculation of viewfactors during a cavity radiation analysis.	Cavity Blocking (NO, ALL, PARTIAL) Range Cavity TurnOff Vtol Reflection (NO, YES)	Defined in the load step card image; visible in *Heat Transfer analysis procedure
*RESPONSE SPECTRUM	Calculates estimates of peak values of nodal and element responses.	Number_of_Directions SummationMethod (ABS, CQC, DSC, GRP, NRL, SRSS, TENP) Modal_Damping Select_Eigenmode	Defined in the load step card image.
*RESTART WRITE	Save and reuse data and analysis results	Frequency Overlay	Defined in the load step card image.
*STATIC	Static stress/displacement analysis	Adiabatic Direct (Direct, No_Stop) Fully Plastic Riks Stabilize (None, Riks, Stabilize) Long_Term Dataline	Defined in the load step card image.
*STEADY STATE DYNAMICS	Steady-state dynamic response based on harmonic excitation	Direct SubSpace (None, DIRECT, SUBSPACE PROJECTION) SubSpace Projection (ALL FREQUENCIES, CONSTANT, EIGENFREQUENCY, PROPERTY CHANGE, RANGE) Frequency Scale (LOGARITHMIC, LINEAR) Interval (EIGENFREQUENCY, RANGE) Read Only SSD DataLines Modal_Damping	Defined in the load step card image.
*STEP	Begin a step	CONVERT SDI INCREMENT NAME NLGEOM PERTURBATION UNSYMMETRIC AMPLITUDE=STEP, RAMP EXTRAPOLATION=LINEAR, PARABOLIC, NO	Parameters are defined in the load step card image.
*VISCO	Transient, static, stress/displacement analysis with time-dependent material response (creep, swelling, and viscoelasticity)	Cetol Creep Factor Stabilize Initial Time Increment Period Minimum Time Increment Maximum Time Increment	Defined in the load step card image.

Note:

Only load collectors with the HISTORY card image should be added to a load step. Load collectors with INITIAL_CONDITION card images need not be added to any load steps. They will be ignored, if added.

Supported Card	Solver Description	Supported Parameters	Notes
ACEL	Specifies the linear acceleration of the structure.	ACELX, ACELY, ACELZ
ANTYPE	Specifies the analysis type and restart status.	type (STATIC, BUCKLE, MODAL, HARMIC, TRANS, SUBSTR, SPECTR) status (NEW, REST, VTREST) LDSTEP SUBSTEP ANTYPE_Action (CONTINUE, ENDSTEP, RSTCREATE, PERTURB)
CECMOD		NEQN, CONST
CMACEL	Specifies the translational acceleration of an element component.	CM_NAME, CMACEL_X, CMACEL_Y, CMACEL_Z
CMDOMEGA	Specifies the rotational acceleration of an element component about a user-defined rotational axis.	CM_NAME, DOMEGAX, DOMEGAY, DOMEGAZ, X1, Y1, Z1, X2, Y2, Z2
CMOMEGA	Specifies the rotational velocity of an element component about a user-defined rotational axis.	CM_NAME, DOMEGAX, DOMEGAY, DOMEGAZ, X1, Y1, Z1, X2, Y2, Z2, KSPIN
EQSLV	Specifies the type of equation solver.	Lab, TOLER, MULT
LSSOLVE	Reads and solves multiple load steps.	LSMIN, LSMAX, LSINC
NLGEOM	Includes large-deflection effects in a static or full transient analysis.	Key
NSUBST	Specifies the number of substeps to be taken this load step.	NSBSTP, NSBMX, NSBMN, Carry
OMEGA	Specifies the rotational velocity of the structure.	OMEGX, OMEGY, OMEGZ, KSPIN
OUTRES	Controls the solution data written to the database.	Item, FREQ, Cname
TIME	Sets the time for a load step.	time

The Loadsteps panel is available when the Nastran user profile is loaded. It is used to generate Nastran subcase definitions. The panel creates loadstep entities. These loadstep entities directly correspond to Nastran subcase definitions.

Use the Loadsteps panel to explicitly define load collectors as the referenced constraint (SPC), static load (LOAD), multi-point constraint (MPC), fictitious support (SUPORT1), non-linear parameters (NLPARM), eigenvalue extraction data (METHOD), frequency range (FREQ), damping (SDAMPING), dynamic load (DLOAD), thermal loading (TEMP), etc. for a subcase. Other input data is automatically generated (the SUBCASE header) or may be added to the subcase definition through the edit function.

It is recommended to set up a subcase using the Loadstep browser.

Supported Card	Solver Description	Supported Parameters	Notes
NLSTEP	Describes the control parameters for mechanical, thermal and coupled analysis in SOL 400 and for linear contact analysis in SOL 101.	GENERAL, FIXED, ADAPT
SUBCASE		LABEL, ANALYSIS, IC, BCONTACT, TRIM, OUTPUT
SUBCOM	Defines a combination subcase.		Created automatically, when a new load step of type “Combination Subcase Delimiter” is created. The SUBCOM ID matches the ID of the HyperMesh loadstep entity.
SUBSEQ	Subcase sequence coefficients.		Select a subcom (loadstep) and click edit. Check the box next to SUBSEQ and input the combination coefficients.
TSTEPNL	Defines parametric controls and data for nonlinear transient structural or heat transfer analysis.	NDT, DT, NO, KSTEP, MAXITER, CONV, EPSU, EPSP, EPSW, MAXDIV, MAXQN, MAXLS, FSTRESS, MAXBIS, ADJUST MSTEP, RB, MAXR, UTOL, RTOLB, MINITER

Solver Card Support for Load Steps

Supported Card

Solver Description

Supported Parameters

Notes

Supported Card

Solver Description

Supported Parameters

Notes

Supported Card

Solver Description

Supported Parameters

Notes

See Also: