Load Case

Analysis > Load Case

This tool is used to group loads and constraints and create different loading combinations. Each load case can be of different analysis type. Solution control parameters and output requests for each load case can be specified.

Description

  1. The loads and constraints are segregated based on structural and thermal analysis types and listed in the load case dialog.
  2. Move the loads or constraints to the right list to include them in the load case.
  3. Contact and connectors can be included in the load case by using the advanced list option.
  4. The right side list will have options Add, Modify and Delete, which are used to control the behavior of loads in Abaqus. Add and Delete is used to write OP=NEW in Abaqus deck for the corresponding load. Modify is used to write OP=MOD in Abaqus deck.

  5. The load case tree view will show the load cases in the order by which it was created and the solver will execute the analysis in the same order.
    • The load case order can be changed by Move Up / Move Down options available when we right click the corresponding load case in load case tree.
  6. Subcase ID can be defined for OptiStruct and Nastran solvers only.
  7. The Solution parameters and Output requests of each load case can be setup individually by using the Create Solver Settings option available at the right click option of each load case.

  8. The load / constraint magnitude can be varied for each load case for the following loads / constraints.
    Load / Constraint Solver Supported Cards
    Pressure magnitude Abaqus *Dload / *Dsload
    Body force > Centrifugal force magnitude Permas $INERTIA ROTATION
    Surface interaction > Friction magnitude Abaqus *Change friction
    Pretension Force Abaqus *Cload
    OptiStruct PTFORCE
    Pretension Constraint Abaqus *Boundary
    OptiStruct PTADJUST
    Contact Abaqus *Model change,Type=Contact pair,Add/Remove
    OptiStruct MODCHG, CONTACT

  9. Also load case specific load parameters can be defined using Load Step Manager or by modifying (double click load and editing the parameters) the load parameters within load case browser.

Following loads and constraints can be modified with respect to loadcase in Load case browser. The parameters which can be varied are shown below and this is supported only for Abaqus, OptiStruct and Permas.

Supported Loads/Constraints Parameters that can be varied
Pressure Magnitude, Amplitude table
Temperature Uniform Temperature
Force Fx,Fy,Fz
Moment Mx,My,Mz
Body Force Centrifugal Force - Magnitude
Fixed Constraint Displacement : X,Y,Z; Rotation : X,Y,Z
Enforced Constraint Displacement : X,Y,Z; Rotation : X,Y,Z
Surface Interaction Friction Coefficient, Amplitude table
Contact Add / Remove
Solid Pretension Force, Adjustment Length
Flux Uniform Heat Flux, Amplitude Table
Convection Uniform Sink Temperature, Uniform Film Coefficient, Amplitude Table
Radiation Uniform Temperature, Uniform Emissivity, Amplitude Table