## Introduction

Nastran and OptiStruct allow loading and boundary conditions to be defined on finite elements. These loads and boundary conditions are commonly applied as distributed loads. Because of their distributed nature, loads and boundary conditions must be carefully applied on individual FE elements. The repetitive nature of FE modeling development creates the overhead of applying loading and boundary conditions for each repetition of new mesh data. New load management aims to simplify this process and solve the problem of redefining loads.

HyperMesh creates a load entity for each load solver keyword. Classic load entities can be defined on set entities by defining the underlying region of FE elements, but they cannot address all of the issues of distributed loads. Some of the limitations of classic load support are:
• Defining distributed values for loads defined on set entities
• Overhead creation and management of load entities on each FE location
• Dependency of FE locations for load creation
• Limitations of supporting complex boundary condition cards with multiple DOF definitions
• Consolidation of loads by common attributes such as SID, Magnitude, etc.
• Interrogation of loads is more powerful
• Applying pressure on Nodes
• Applying traction on axisymmetric elements
• Applying pressure on 1D elements based on element orientation
• Honoring solver recommendations such as Load on Set
• Enhancements to the Solver Browser to handle large numbers of loads
• A uniform way to set up a model (end-to-end) through the browser

## Objectives

Besides providing a simplified common workflow for managing loads, other engineering load objectives include:
• Defining distributed values for loads defined for each FE location in a set
• Adding complete support for all solver cards mapped to classic loads

Loads created from the panel are called classic loads. Although classic load entities are still supported, their use is not encouraged. New load management allows you to create loads from the Solver Browser. Using the "absorbloads" command, classic load entities can be absorbed into engineering entities.

The advanced segregation feature allows you to spawn new engineering loads from existing engineering loads based on value distribution or topology. You can set up a single load with distributed values and run the "absorbentities" command to obtain multiple meaningful and manageable loads of the same magnitude value.

## Realization

A realization command is provided for those who choose to work with classic loads. The "realizefieldloads" command creates classic loads from engineering loads, although it is not the exact reversal of the absorption command.

Load plotting allows for visualization of distributed load values on an FE region. Different plotting types provide different views of the load.
• Vector Plots – display value distribution with the direction of the load
• Advanced Contour Plots – display value distribution with interactive filters
• Contour Plots – display value distribution with respect to the entire model

Load values can be plotted at specific time stamps for curve-based time dependent loads.

Every load and constraint must be organized into one load collector, and therefore are mutually exclusive to a load collector.

Accelerations

Configuration 9 - Acceleration loads allow for an acceleration (length/time2) to be defined on the model.

Accelerations are displayed as a vector with the letter A at the tail end in the modeling window.

Constraints

Configuration 3 - Constraints allow for constrained degrees of freedom to be defined on the model.

Constraints are displayed with a triangle that connects to the node, with the dof numbers that apply to the node beside the triangle in the modeling window.

Fluxes

Configuration 6 - Flux loads are defined as an amount that flows through a unit area per unit time (amount/length2/time). Fluxes are typically used in modeling transport phenomena such as heat transfer, mass transfer, fluid dynamics, and electromagnetism.

Fluxes are displayed as a thick arrow labeled with the word "flux" in the modeling window.

Forces

Configuration 1 - Force loads allow for a concentrated force (mass*length/time2) to be applied to the model.

Forces are displayed as a vector with the letter F at the tail end in the modeling window.

Moments

Configuration 2 - Moment loads allow for a concentrated moment (length*force) to be applied to the model.

Moments are displayed with a double-headed vector with the letter M at the tail end in the modeling window.

Pressures

Configuration 4 - Pressure loads allow for a pressure (force*length2) to be applied to the model.

For most solvers, the pressure load is considered as force/area, therefore the magnitude of the pressure is multiplied by the calculated area of the elements to which it is applied and resolved as concentrated force loads at the associated nodes.

Pressures are displayed as a vector with the letter P at the tail end in the modeling window.

Temperatures

Configuration 5 - Temperature loads allow for a concentrated temperature to be applied to the model.

Temperatures are displayed as a vertical line with the letter T at the top in the modeling window.

Velocities

Configuration 8 - Velocity loads allow for a velocity (length/time) to be applied to the model.

Velocities are displayed as a vector with the letter V at the tail end in the modeling window.

## Abaqus Cards

Loads or constraints that are to be used as history data (under *STEP) should be collected into load collectors with the HISTORY card image. These load collectors also need to be added to the corresponding load steps (*STEP). In contrast, loads or constraints for model data should be collected into load collectors with INITIAL_CONDITION card image. They will automatically be written out in the model portion of the Abaqus input deck.
Note: All loads and boundary conditions on sets can be expanded to individual nodes and elements by selecting the Expand load on sets option in the File Options dialog, which is invoked upon importing a solver deck. If a **HMLOAD_SETS_EXPAND comment is found in the input file, all loads and boundary conditions on sets are expanded to individual nodes and elements.
*BASE MOTION Constraint Defines scale factor and DOF for dynamic loads.
*BOUNDARY (electric potential, dof 9) Flux Specifies flux boundary conditions for piezoelectric analysis.
*BOUNDARY (structural) Constraint Creates structural boundary conditions.

*BOUNDARY

(temperature, dof 11)

Temperatures Specifies temperature boundary conditions.
*CECHARGE Flux Specifies concentrated electric charges for piezoelectric analysis.
*CECURRENT Flux Specifies concentrated current in electric conduction.
*CFLUX Flux Specify concentrated fluxes in heat transfer or mass diffusion analyses.
*COUPLING Constraint Define a surface-based coupling constraint
*DECHARGE Pressure Distributes electric charges for piezoelectric analysis.
*DFLUX Pressure Specify distributed fluxes in heat transfer or mass diffusion analyses.
*DISTRIBUTING Constraint Define a distributing coupling constraint
*DISTRIBUTING COUPLING Elements Specify nodes and weighting for distributing coupling elements
*FILM Pressure Define film coefficients and associated sink temperatures.
*KINEMATIC Multi-point Constraints Define a kinematic coupling constraint
*KINEMATIC COUPLING Multi-point Constraints Constrain all or specific degrees of freedom of a set of nodes to the rigid body motion of a reference node
*MPC Multi-point Constraints Define multi-point constraints
*TEMPERATURE Temperature Specifies predefined temperature field.

## ANSYS Cards

BF Flux Defines a nodal body force load.
BF_FLUE Flux
BF_HGEN Flux
BF_TEMP Temperatures
BFE_FLUE Flux Defines an element body force load.
BFE_HGEN Flux
BFE_TEMP Flux
CE_STRUCT Equation
CE_THERM Equation
CE_MAG Equation
CE_ELEC Equation
ConvBulkTe Pressure
ConvFilmCo Pressure
D_A Constraint Vector magnetic potential.
D_CONSTRNT Constraint Defines DOF constraints at nodes.
D_MAG Constraint Scalar magnetic potential.
D_PRES Constraint
D_TEMP Temperature
D_VOLT Constraint
F_FLOW Flux Specifies force loads at nodes.
F_HEAT Flux
FLOTRAN Pressure Specifies "FLOTRAN data settings" as the subsequent status topic.
Note: FLOTRAN surface load label “FSI [fluid-structure interaction flag]” is available under pressure load.

You must use DOF1 to add value for this label.

FORCE Force Selects the element nodal force type for output.
FORCE2 Moment
FSI Pressure
HFLUX Pressure
IC_A Constraint
IC_CONSTRN Constraint Specifies initial conditions at nodes.
IC_MAG Constraint
IC_PRES Constraint
IC_TEMP Temperature
IC_VOLT Constraint
PRESSURE Pressure
RDSF_EMI Pressure
RDSF_ENCL Pressure
SFE
• Pressure
• Convection
• Heatflux
Note: Structural, thermal and Fluid labels are covered.
SFE
• Structural
• Thermal
• Fluid
• Structural label: PRES
• Thermal label: CONV, HLFUX
• Fluid label: FSI

## LS-DYNA Cards

*BOUNDARY_CONVECTION_SET Flux Apply a convection boundary condition on a SEGMENT_SET for a thermal analysis.
*BOUNDARY_CYCLIC Constraint Define nodes in boundary planes for cyclic symmetry. Optional ID applies to each cyclic definition.
*BOUNDARY_PRESCRIBED_MOTION(Accl) Acceleration Define an imposed nodal motion (Acceleration, VAD=1) on a node or a set of nodes.
*BOUNDARY_PRESCRIBED_MOTION(Disp) Constraint Define an imposed nodal motion (Displacement, VAD=2) on a node or a set of nodes.
*BOUNDARY_PRESCRIBED_MOTION(Vel) Velocity Define an imposed nodal motion (Velocity, VAD=0) on a node or a set of nodes.
*BOUNDARY_PRESCRIBED_MOTION_RIGID(Accl) Acceleration Accelerations (VAD=1) can also be imposed on rigid bodies. If the local option is active, the motion is prescribed with respect to the local coordinate system for the rigid body.
*BOUNDARY_PRESCRIBED_MOTION_RIGID(Disp) Constraint Displacements (VAD=2, 4) can also be imposed on rigid bodies. If the local option is active, the motion is prescribed with respect to the local coordinate system for the rigid body.
*BOUNDARY_PRESCRIBED_MOTION_RIGID(Vel) Velocity Velocities (VAD=0, 3) can also be imposed on rigid bodies. If the local option is active, the motion is prescribed with respect to the local coordinate system for the rigid body.
*BOUNDARY_RADIATION_SET Flux Defines surface segment sets that transfer energy by radiation to the environment.
*BOUNDARY_SPC Constraint Define nodal single point constraints. Supported OPTION1=NODE, SET. OPTION2=BIRTH_DEATH and OPTION3=ID.
*BOUNDARY_TEMPERATURE Temperature Define temperature boundary conditions for a thermal or coupled thermal/structural analysis. Supported OPTION = NODE, SET.
*INITIAL_TEMPERATURE Temperature Define initial nodal point temperatures using nodal set IDs or node numbers. This may also be used for sets in which some nodes have other velocities. Supported OPTION = NODE, SET.
*INITIAL_VELOCITY Velocity Define initial nodal point velocities using nodal set ID’s. This may also be used for sets in which some nodes have other velocities.
*INITIAL_VELOCITY_NODE Velocity Define initial nodal point velocities for a node.
*INITIAL_VELOCITY_RIGID_BODY Velocity Define the initial translational and rotational velocities at the center of gravity (c.g.) for a rigid body or a nodal rigid body. This input overrides all other velocity input for the rigid body and the nodes which define the rigid body.
*INITIAL_VELOCITY_GENERATION Velocity Define initial velocities for rotating and translating bodies.
*LOAD_BEAM Pressure Apply the distributed traction load along any local axis of a beam or a set of beams.
*LOAD_BODY (ACCELERATION) Acceleration Define body force loads due to a prescribed base acceleration using global axes directions. Supported OPTION = X, Y, Z.
*LOAD_BODY (VELOCITY) Velocity Define body force loads due to a prescribed base angular velocity using global axes directions. Supported OPTION = RX, RY, RZ.
*LOAD_GRAVITY_PART Acceleration Define gravity for individual parts. Supported OPTION = PART, SET.
*LOAD_NODE (FORCES) Force Apply a concentrated nodal force to a node or each node in a set of nodes. Supported OPTION = POINT, SET and DOF = 1, 2, 3, 4 (Follower).
*LOAD_NODE (MOMENTS) Force Apply moments to node or each node in a set of nodes. Supported OPTION = POINT, SET and DOF = 5, 6, 7, 8 (Follower).
*LOAD_RIGID_BODY (FORCES) Force Apply a concentrated nodal force to a rigid body. The force is applied at the center of mass. As an option, local axes can be defined for force directions. Supported DOF = 1, 2, 3, 4 (Follower).
*LOAD_RIGID_BODY (MOMENTS) Force Apply a concentrated nodal force to a rigid body. The moment is applied around a global axis. As an option, local axes can be defined for moment directions. Supported DOF = 5, 6, 7, 8 (Follower).
*LOAD_SEGMENT Pressure Apply the distributed pressure load over one triangular or quadrilateral segment defined by four, six, or eight nodes. Apply the distributed pressure load over each segment in a segment set. Supported OPTION = ID and SET.
*LOAD_SHELL Pressure Apply the distributed pressure load over a single shell element or a shell element set. Supported OPTION1 = ELEMENT, SET and OPTION2 = ID.
*LOAD_THERMAL_CONSTANT Temperature Define the constant temperature that is applied to a given nodal set.
*LOAD_THERMAL_CONSTANT_NODE Temperature Define nodal temperature that remains constant for the duration of the calculation.
*LOAD_THERMAL_LOAD_CURVE Temperature Nodal temperatures will be uniform throughout the model and will vary according to a load curve.
*LOAD_THERMAL_VARIABLE Temperature Define nodal temperature using node set(s) and temperature as a function of time curve(s).
*LOAD_THERMAL_VARIABLE_NODE Temperature Define nodal temperature that is variable during the calculation.

## Nastran Cards

ASET Constraints Defines degrees-of-freedom in the analysis set (a-set)
ASET1 Constraints Defines degrees-of-freedom in the analysis set (a-set)
BNDFIX1 Constraints Defines analysis set (a-set) degrees-of-freedom to be fixed (b-set) during generalized dynamic reduction or component mode synthesis calculations.
BOLTFOR Flux
BSET1 Constraints Defines analysis set (a-set) degrees-of-freedom to be fixed (b-set) during generalized dynamic reduction or component mode synthesis calculations.
CSET1 Constraints Defines analysis set (a-set) degrees-of-freedom to be free (c-set) during generalized dynamic reduction or component modes calculations.
DAREA Constraints Defines scale (area) factors for static and dynamic loads. In dynamic analysis, DAREA is used in conjunction with RLOADi and TLOADi entries.
DEFORM Flux Defines enforced axial deformation for one-dimensional elements for use in statics problems.
FORCE Force Requests the form and type of element force output or particle velocity output in coupled fluid-structural analysis.
MOMENT Moment Defines a static concentrated moment at a grid point by specifying a scale factor and a vector that determines the direction.
OMIT1 Constraints Defines degrees-of-freedom to be excluded (o-set) from the analysis set (a-set).
PLOAD Pressure Defines a uniform static pressure load on a triangular or quadrilateral surface comprised of surface elements and/or the faces of solid elements.
PLOAD1 Pressure Defines concentrated, uniformly distributed, or linearly distributed applied loads to the CBAR or CBEAM elements at user-chosen points along the axis.

The THRU field is supported for feinput only. On export, additional pressure cards for the range specified are written.

The THRU field is supported for feinput only. On export, additional pressure cards for the range specified are written.

Unequal nodal pressures are now supported. The average pressure value is used as the magnitude of the pressure for visualization only. The individual field values, P1-P4, can be viewed or edited using the card editor.

Updating the magnitude of pressure from the Pressures panel will have no effect on PLOAD4 cards defined using unequal nodal pressures.

QBDY1 Flux Defines a uniform heat flux into CHBDYj elements.
QSET1 Constraints Defines generalized degrees-of-freedom (q-set) to be used for generalized dynamic reduction or component mode synthesis.
QVOL Flux Volume Heat Addition - Defines a rate of volumetric heat addition in a conduction element.
SPC Constraints Defines a set of single-point constraints and enforced motion (enforced displacements in static analysis and enforced displacements, velocities or acceleration in dynamic analysis).

Constraints on nodes are supported through SPC cards. PS field in GRID card is not supported. Upon import, any PS entry on the GRID card will be converted into an SPC card.

SPC1 Constraints Defines a set of single-point constraints.

Supported for feinput only. On export, equivalent SPC cards are written. Alternate format with THRU in the fifth field is supported.

SPCD Constraints Defines an enforced displacement value for static analysis and an enforced motion value (displacement, velocity or acceleration) in dynamic analysis.
SUPORT Constraints Defines determinate reaction degrees-of-freedom in a free body.
SUPORT1 Constraints Defines determinate reaction degrees-of-freedom (r-set) in a free body-analysis. SUPORT1 must be requested by the SUPORT1 Case Control command.
TIC(D) Constraints Transient Initial Condition - Defines values for the initial conditions of variables used in structural transient analysis.
TIC(V) Constraints Transient Initial Condition - Defines values for the initial conditions of variables used in structural transient analysis.
TEMP Temperatures Defines temperature at grid points for determination of thermal loading, temperature-dependent material properties, or stress recovery.
TEMPBC Temperatures Defines the temperature boundary conditions for heat transfer analysis.
USET Constraints Defines a degree-of-freedom set.
USET1 Constraints Defines a degrees-of-freedom set.

## OptiStruct Cards

General boundary conditions, such as loads and constraints, should not be collected into specific load collectors. Organizing loads and constraints into a specific load collector may result in an error termination.

ASET Constraints Defines the boundary degrees-of-freedom of a superelement assembly for matrix reduction.
ASET1 Constraints Defines the boundary degrees-of-freedom of a superelement assembly for matrix reduction.
BASELIN   Corrects the acceleration record to avoid displacement shift.
Note: Bulk Data Entry
CDENST4   Defines a current density on the face of solid elements (HEXA, PENTA, TETRA, PYRA) or on the side of shell elements (TRIA3, TRIA6, QUAD4, QUAD8) in Electrical analysis.
Note: Bulk Data Entry
CURRENT   Defines a static point current at a grid or a set of grids, by specifying a vector, in Electrical analysis.
Note: Bulk Data Entry
DEFORM Flux Defines enforced axial deformation for one-dimensional elements for use in statics problems.
DPHASE Constraints Defines the phase lead term $\theta$ in the equation of the dynamic loading function. DPHASE is used in conjunction with RLOAD1 and RLOAD2 entries.
FORCE Force Defines a static force at a grid point or a SET of grid points by specifying a vector.
FORCE1 Force Used to define a static force by specification of a value and two grid points that determine the direction. It can also be used to define the EXCITEID field (Amplitude "A") of dynamic loads in RLOAD1, RLOAD2, TLOAD1 and TLOAD2 Bulk Data Entries. Additionally, the FORCE1 entry can be defined as Follower Loads in Large Displacement Nonlinear Analysis.
INLTVEL   Defines the Inlet velocity for Darcy Flow Analysis.
MBFRC Force Defines a constant force at a grid point by specifying a vector.
MBFRCC Force Defines a curve force at a grid point by specifying a vector.
MBMNT Moment Defines a constant moment at a grid point by specifying a vector.
MBMNTC Moment Defines a curve moment at a grid point by specifying a vector.
MOMENT Moment Defines a static moment at a grid point or a SET of grid points by specifying a vector.
MOMENT1 Moment Defines a static moment by specification of a value and two grid points, which determine the direction. It can also be used to define the EXCITEID field (Amplitude A) of dynamic loads in RLOAD1, RLOAD2, TLOAD1 and TLOAD2 Bulk Data Entries.
MOTNG Constraint Defines a constant grid point motion.
MOTNGC Constraint Defines a grid point motion vs. time by specifying a curve.
NLENRG   Defines parameters for energy variables printout for implicit nonlinear static and implicit nonlinear transient analyses.
Note: Bulk Data Entry
NLPRINT   Controls the printing of certain information to the _nl.out file for nonlinear analysis.
Note: Bulk Data Entry
PLOAD1 Pressure Defines concentrated, uniformly distributed, or linearly distributed applied loads to the CBAR or CBEAM elements or a SET of such elements at user-chosen points along the axis. It can also be used to define the EXCITEID field (Amplitude "A") of dynamic loads in RLOAD1, RLOAD2, TLOAD1 and TLOAD2 Bulk Data Entries.
PLOAD2 Pressure Defines a uniform static pressure load applied to two-dimensional elements, or a SET of such elements.
QBDY1 Flux Defines a uniform heat flux for CHBDYE elements.
QVOL Flux Defines a rate of volumetric heat addition in a conduction element.
SPC Constraint Defines sets of single-point constraints, enforced displacements for static analysis, and thermal boundary conditions for heat transfer analysis.
SPCD Constraint Defines an enforced displacement value for static analysis, an enforced displacement, velocity or acceleration for dynamic analysis and a thermal boundary condition for heat transfer (or transient heat transfer) analysis. It can also be used to define the EXCITEID field (Amplitude "A") of dynamic loads in RLOAD1, RLOAD2, TLOAD1 and TLOAD2 Bulk Data Entries.
SPCP   Defines the flow pressure boundary conditions for Darcy Flow Analysis.
SUPORT Constraint Defines determinate reaction degrees-of-freedom in a free body.
SUPORT1 Constraint Defines determinate reaction degrees-of-freedom in a free body.
TEMP Temperature Defines temperature at grid points or a SET of grid points for determination of Thermal Loading and Stress recovery.
TIC(D) or (V) Constraint Defines values for the initial conditions of variables used in structural transient analysis and explicit analysis. Both displacement and velocity values may be specified at independent degrees-of-freedom.
USET Constraint Defines a set of degrees-of-freedom.
USET1 Constraint Defines a set of degrees-of-freedom.

## PAM-CRASH Cards

ACC3D / Acceleration Imposed accelerations
BOUNC / Constraints Define boundary condition
CONLO / Force(1) Concentrated nodal load
DIS3D / Constraints Imposed displacement
DIS3DM / Constraints Imposed minimum displacement
DIS3DX / Constraints Imposed maximum displacement
INVEL / Velocity Define initial velocity
PREFA / Pressure(1) Pressure on shells
RAC3D / Acceleration Imposed rotational acceleration
RAN3D / Constraints Imposed angular rotations
RDA3D / Acceleration Radial 3D boundary conditions
RDD3D / Constraints
RDV3D / Velocity Radial 3D boundary conditions
RVE3D / Velocity Imposed rotational velocities
RWALL / Rigid wall definition
SECFO_PLANE /
VEL3D / Velocity Imposed velocities

## Permas Cards

$ADDMODES Constraints Definition of static mode shapes to be added to the set of eigenmodes used for transformation to modal space. If static mode shapes will be added directly to nodes or nodesets (SOURCE=INPUT), the$ADDMODES can be created through the Constraints panel.

Click sysid to specify the system regarding to which the modes shall be applied.

Use the DOFTYPE button to select an option: DISP, TEMP, PRES, POTE and MATH.

$ADDMODES Pressure Definition of static mode shapes to be added to the set of eigenmodes used for transformation to modal space. If mode shapes will be applied based on the natural deformation of elements (SOURCE=INPUT) the$ADDMODES keyword needs to be created here.

$CONLOAD Force Definition of concentrated loads at nodal point degrees of freedom.$CONLOAD Moment Definition of concentrated loads at nodal point degrees of freedom.
$DISLOAD PRESS Pressure Definition of pressure loads for elements, where loads are given for elements or element sets. Applicable to shells and solids, but also axisymmetric solid elements. Therefore please apply a pressure on an HM shell element. Face identifiers are written in this case. On import IDS ELNODES or NODES will be resolved into ELGEO (face identifiers).$DISLOAD TEMP Pressure Nodal temperatures defined on elements or element sets.
$DISLOAD TEMPFILM Pressure Surrounding temperatures for convective heat transfer applied on elements or element sets.$DISLOADN TEMP Temperature Nodal temperatures definition applied on nodes or node sets
$DISLOADN TEMPFILM Temperature Surrounding temperatures for convective heat transfer applied on nodes or node sets.$INIVAL Constraints Definition of initial values for nodal point degrees of freedom.

For $INIVAL source parameter INPUT is currently supported to specify the initial values based on nodal points.$INERTIA Pressure Definition of inertia forces acting on entire component or element sets. Available are force distributions due to linear acceleration, constant or accelerated rotation and coriolis acceleration.

Only ACCELERATION and GRAVITY are supported. This card is created in the Pressure panel. Assign to a set of elements, and the set statement displays in the card image. To create the card without a set, create a pressure on a 'dummy' element; the card will be created without a set and can be applied to the whole model.

$INERTIAX Pressure Definition of inertia forces acting on entire axisymmetric component or element sets. Available are force distributions due to linear acceleration and constant rotation. Only ACCELERATION and GRAVITY are supported. This card is created in the Pressure panel. Assign to a set of elements, and the set statement displays in the card image. To create the card without a set, create a pressure on a 'dummy' element; the card will be created without a set and can be applied to the whole model.$MPC GENERAL Equation Multipoint constraint definition.

The equation needs to be placed into a load collector with card image SUPRESS.

By attaching the load collector to a load step with ‘CONSTRAINTS’ attribute set, the $MPCVAL card gets written in the desired$CONSTRAINTS variant.

$PRESCRIBE/ PREVAL Constraints Prescribed degrees of freedom/Nodal point values (implemented as HyperMesh constraints)$SUPPRESS Constraints Suppressed degrees of freedom

/ALE/BCS Constraint Describes the ALE boundary conditions.
/BCS Constraint Defines boundary conditions on node groups for translational and rotational motion.
/BCS/LAGMUL Constraint Defines boundary conditions on node groups using Lagrange multipliers. This keyword is not available for SPMD computation.
/CLOAD Force Defines a concentrated force applied to each node of a prescribed nodal group.
/CLOAD Moment Defines a concentrated moment applied to each node of a prescribed nodal group.
/CONVEC Thermal Describes the free or forced convective flux.
/DFS/DETCORD Pressure Set burning times of explosive material elements along a neutral fiber of detonating cord. Neutral fiber is provided with an ordered group of nodes and numerically built by spline interpolation.
/DFS/DETLINE Pressure Enable explosive material ignition from a detonation line [A,B]. Point A & B - XYZ coordinate.
/DFS/DETLINE/NODE Pressure Enable explosive material ignition from a detonation line [A,B]. Node ID defining Point A & B Coordinates.
/DFS/DETPLAN Pressure

Describes a planar detonation wave. Node identifier for base point P.

/DFS/DETPLAN/NODE Pressure

Describes a planar detonation wave. XYZ coordinate for basis point P.

/DFS/DETPOINT Pressure Locates the detonation point and set lighting time for an explosive material law, XYZ coordinates.
/DFS/DETPOINT/NODE Pressure Locates the detonation point and set lighting time for an explosive material law, node identifier defining ignition coordinates.
/DFS/LASER Pressure Enable to model laser impact taking into account laser-matter interaction.
/DFS/WAV_SHA Pressure Enables you to shape detonation wave to take into account obstacles.
/EBCS/GRADP0 Pressure Describes the elementary boundary condition sets. Keyword: Zero pressure gradient.
/EBCS/INIP Pressure Describes the elementary boundary condition sets. Keyword: Initial pressure.
/EBCS/INIV Velocity Describes the elementary boundary condition sets. Keyword: Initial velocity.
/EBCS/NORMV Velocity Describes the elementary boundary condition sets. Keyword: Imposed normal velocity.
/EBCS/PRES Pressure Describes the elementary boundary condition sets. Keyword: Imposed density and pressure.
/EBCS/VALVIN Pressure Describes the elementary boundary condition sets. Keyword: Inlet valve (Imposed density and pressure).
/EBCS/VALVOUT Pressure Describes the elementary boundary condition sets. Keyword: Outlet valve (Imposed density and pressure).
/EBCS/VEL Velocity Describes the elementary boundary condition sets. Keyword: Imposed velocity.
/GRAV Acceleration Defines gravity load on node group.
/IMPACC Acceleration Defines imposed accelerations on a group of nodes.
/IMPDISP Constraint Defines imposed displacements on a group of nodes.
/IMPDISP/FGEO Constraint Describes the final position of a set of N nodes, input by coordinates.
/IMPFLUX Thermal Defines an imposed thermal surface flux on the specified surfaces or a thermal volumetric flux on the specified bricks.
/IMPTEMP Thermal Defines imposed temperatures on a group of nodes.
/IMPVEL Velocity Defines imposed velocities on a group of nodes.
/IMPVEL/FGEO Velocity Describes the final position of a set of N nodes. The final position is provided by a node number. The node may eventually move.
/INITEMP Thermal Describes the initial nodal temperature.
/INIVEL/AXIS Velocity Initialize both translational and rotational velocities on a group of nodes in a given coordinate system.
/INIVEL/TRA Velocity

Defines initial velocity on a group of nodes.

Initial velocity type: TRA - Translational material velocity.
/INIVEL/ROT Velocity

Defines initial velocity on a group of nodes.

Initial velocity type: ROT - Rotational material velocity.
/INIVEL/T+G Velocity

Defines initial velocity on a group of nodes.

Initial velocity type: T+G - Translational and grid material velocity (only used for ALE material).
/INIVEL/GRID Velocity

Defines initial velocity on a group of nodes.

Initial velocity type: GRID - Grid material velocity (only used for ALE material).
/LOAD/CENTRI Moment Apply a centrifugal force on a set of nodes according a body rotational velocity around the defined direction.
/LOAD/PFLUID Pressure Simulates hydrodynamic fluid pressure on a structure. The fluid pressure is calculated according to the specified fluid velocity, orientation of the structural surface against the fluid vector and the height of the fluid column above the surface of the structure.
/SPHBCS/SLIDE Constraint

Describes the SPH symmetry conditions.

Type: Material is perfectly sliding along the plane.
/SPHBCS/TIED Constraint

Describes the SPH symmetry conditions.

Type: Material cannot slide along the symmetry plane.