HyperMesh and BatchMesher

Load Steps entityLoadsteps-24

Load Steps entityLoadsteps-24

Previous topic Next topic Expand/collapse all hidden text  

Load Steps entityLoadsteps-24

Previous topic Next topic JavaScript is required for expanding text JavaScript is required for the print function  

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


hmtoggle_arrow1OptiStruct

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).

hmtoggle_arrow1Abaqus

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.

 

hmtoggle_arrow1ANSYS

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

 

hmtoggle_arrow1Marc

Supported Card

Solver Description

Supported Parameters

Notes

FOUNDATION

 

 

 

INITIAL_vel

 

 

 

Init_Disp

 

 

 

Fixed_Acce

 

 

 

Fixed_Pres

 

 

 

hmtoggle_arrow1Nastran

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

 

hmtoggle_arrow1PERMAS

The following cards are supported in the PERMAS interface:

Supported Card

Solver Description

Supported Parameters

Notes

$CONSTRAINTS

Constraint variant bracket header line

NAME

Create a loadstep and open its card image. Set the Analysis Procedure to CONSTRAINTS.

$FREQLOAD

Definition of frequency dependent dynamic loads for use in frequency response analysis.

DOFTYPE

The AnalysisProcedure toggle must be set to LOADING in the card image.

$LOADING

Loading variant bracket header line

NAME

 

$NLLOAD

Define a nonlinear static load history.

TABLE

TIME={LIST/Time and increment}

EXTRA=CONST

DOFTYPE=DISP

The AnalysisProcedure toggle must be set to LOADING in the card image.

To visualize the nonlinear load history curves you can use the Plot NLLOAD tool from the utility page.

$SITUATION

Situation definition header line

NAME

Open the loadstep and set the AnalysisProcedure to SITUATION

$TRANSLOAD

Definition of time dependent dynamic loads for use in transient response analysis.

AMPLITUDE

BOUNDS

DELAY

DOFTYPE

FUNCTION

PHASE

The TRANSLOAD card and FREQLOAD cards are mutually exclusive.

 

 

See Also:

Browsers

HyperMesh Entities & Solver Interfaces

Include Files

Element Property and Material Assignment Rules

Model Setup