Sets of Boundary Conditions

In Fidesys, you can create sets of boundary conditions based on already defined constraints, loads, and contract terms. Sets of boundary conditions are used to determine the loading case (corresponding to any step of the analysis strength) when writing an exported file, including for the purpose of performing calculation by another program. Sets of boundary conditions can define the form calculation (static, thermal, dynamic or modal) by setting the value of the analysis type pointer in the creation commands or changes to sets of boundary conditions:

create bcset [ID] [name <'name'>] [after bcset <ID>] [{add | remove} {bc_type} <ID-range | <with name 'name'> >] [analysistype {STATIC | heat | dynamic | modal}] [modal_max_frequency <value>]

modify bcset {ID_list | 'name' | all} [name <'name'>] [after bcset <ID>] [{add | remove} {bc_type} <ID-range | <with name 'name'> >] [analysistype {STATIC | heat | dynamic | modal}]

The keyword after can be used to define the order of writing sets of boundary conditions when exporting a data file calculation model.

In the sets of boundary conditions contained in the export file, it is possible to set parameters specific to the calculation program used. In particular, for the Abaqus program, such parameters can be: *STEP, *STATIC, *DYNAMIC, *FREQUENCY, *HEAT TRANSFER, *MASS SCALING, *RESTART, *OUTPUT, *EL FILE, *NODE FILE, *EL PRINT, *NODE PRINT. If NASTRAN is used, it is possible define the parameters responsible for generating output data: Displacement, Reaction Loads, MPC Forces, SPC Forces, Stress, and Element Strain Energy.

The Abaqus parameters are set using the commands:

modify bcset {ID_list | 'name' | all} [max_step_increments <value>] [nonlinear_geometry <on | OFF>] [perturbation <on | OFF>] [stabilize <on | OFF>] [steadystate <on | OFF>] [modal_max_frequency <value>]

modify bcset {ID_list | 'name' | all} [initial_step_size <value>] [step_period <value>] [min_step_size <value>] [max_step_size <value>] [min_step_temperature_change <value>]

modify bcset {ID_list | 'name' | all} [mass_scaling <on | OFF>] [mass_scaling_dt <value>] [mass_scaling_factor <value>] [mass_scaling_type <'uniform' | 'BELOW_MIN' | 'set_equal_dt'>]

modify bcset {ID_list | 'name' | all} [restart <on | OFF>] [restart_overlay <on | OFF>] [{restart_frequency | restart_num_intervals} <value>]

modify bcset {ID_list | 'name' | all} [output_field <on | OFF>] [output_field_frequency <value>] [output_history <on | OFF>] [output_history_frequency <value>]

modify bcset {ID_list | 'name' | all} [el_file <on | OFF>] [el_file_frequency <value>] [node_file <on | OFF>] [node_file_frequency <value>]

modify bcset {ID_list | 'name' | all} [el_print <on | OFF>] [el_print_frequency <value>] [node_print <on | OFF>] [node_print_frequency <value>]

To set NASTRAN parameters, the following commands are applicable:

modify bcset {ID_list | 'name' | all} {displacement_output <on | OFF> {PLOT | print | punch | punchprint} {group <ALL | none | <ID>>}}

modify bcset {ID_list | 'name' | all} {oload <on | OFF> {PLOT | print | punch | punchprint} {group <ALL | none | <ID>>}}

modify bcset {ID_list | 'name' | all} {mpcforces <on | OFF> {PLOT | print | punch | punchprint} {group <ALL | none | <ID>>}}

modify bcset {ID_list | 'name' | all} {spcforces <on | OFF> {PLOT | print | punch | punchprint} {group <ALL | none | <ID>>}}

modify bcset {ID_list | 'name' | all} {stress <on | OFF> {PLOT | print | punch | punchprint} {group <ALL | none | <ID>>} {CENTER | cubic | sgage | corner} {VONMISES | maxs}}

modify bcset {ID_list | 'name' | all} {element_strain_energy <on | OFF> {PLOT | print | punch | punchprint} {group <ALL | none | <ID>>} {AVERAGE | amplitude | peak}}