This option is used to prescribe boundary conditions at nodes or to specify the driven nodes in a submodeling analysis. In ABAQUS/Standard it is also used to define primary and secondary bases for modal superposition procedures.
Products: ABAQUS/Standard ABAQUS/Explicit
Type: Model or history data
Level: Model Step
This parameter is relevant only when some of the variables being prescribed have nonzero magnitudes. Set this parameter equal to the name of the amplitude curve defining the magnitude of the prescribed boundary conditions (“Amplitude curves,” Section 19.1.2 of the ABAQUS Analysis User's Manual).
If this parameter is omitted in an ABAQUS/Standard analysis, either the reference magnitude is applied linearly over the step (a RAMP function) or it is applied immediately at the beginning of the step and subsequently held constant (a STEP function). The choice of RAMP or STEP function depends on the value assigned to the AMPLITUDE parameter on the *STEP option (“Procedures: overview,” Section 6.1.1 of the ABAQUS Analysis User's Manual). Two exceptions are displacement or rotation components given with TYPE=DISPLACEMENT, for which the default is always a RAMP function, and displacement or rotation components in a static step given with TYPE=VELOCITY, for which the default is always a STEP function.
If this parameter is omitted in an ABAQUS/Explicit analysis, the reference magnitude is applied immediately at the beginning of the step and subsequently held constant (a STEP function).
In an ABAQUS/Standard dynamic or modal dynamic procedure, amplitude curves specified for TYPE=DISPLACEMENT or TYPE=VELOCITY will be smoothed automatically. In an explicit dynamic analysis using ABAQUS/Explicit, the user must request that such amplitude curves are smoothed. For more information, see “Amplitude curves,” Section 19.1.2 of the ABAQUS Analysis User's Manual.
This parameter applies only to ABAQUS/Standard analyses. It is ignored in all procedures except *STEADY STATE DYNAMICS, DIRECT and *BUCKLE. In these two procedures the parameter can be set equal to 1 (default) or 2.
If this option is used in *STEADY STATE DYNAMICS, DIRECT analysis (“Direct-solution steady-state dynamic analysis,” Section 6.3.4 of the ABAQUS Analysis User's Manual), LOAD CASE=1 defines the real (in-phase) part of the boundary condition and LOAD CASE=2 defines the imaginary (out-of-phase) part of the boundary condition.
If this parameter is used in a *BUCKLE analysis (“Eigenvalue buckling prediction,” Section 6.2.3 of the ABAQUS Analysis User's Manual), LOAD CASE=1 can be used to define boundary conditions for the applied loads and LOAD CASE=2 can be used to define antisymmetry boundary conditions for the buckling modes.
Set OP=MOD (default) to modify existing boundary conditions or to add boundary conditions to degrees of freedom that were previously unconstrained.
Set OP=NEW if all boundary conditions that are currently in effect should be removed. To remove only selected boundary conditions, use OP=NEW and respecify all boundary conditions that are to be retained.
If a boundary condition is removed in a stress/displacement analysis in ABAQUS/Standard, it will be replaced by a concentrated force equal to the reaction force calculated at the restrained degree of freedom at the end of the previous step. If the step is a general nonlinear analysis step, this concentrated force will then be removed according to the AMPLITUDE parameter on the *STEP option. Therefore, if the default amplitudes are used, the concentrated force will be reduced linearly to zero over the period of the step in a static analysis and immediately in a dynamic analysis.
This parameter applies only to ABAQUS/Explicit analyses.
This parameter is relevant only for boundary conditions applied to nodes on the boundary of an adaptive mesh domain. If boundary conditions are applied to nodes in the interior of an adaptive mesh domain, these nodes will always follow the material. ABAQUS/Explicit will create a Lagrangian boundary region automatically for surface-type constraints (symmetry planes, moving boundary planes, and fully clamped boundaries).
Set REGION TYPE=LAGRANGIAN (default) to apply the boundary conditions to a Lagrangian boundary region. The edge of a Lagrangian boundary region will follow the material while allowing adaptive meshing along the edge and in the interior of the region.
Set REGION TYPE=SLIDING to define a sliding boundary region. The edge of a sliding boundary region will slide over the material. Adaptive meshing will occur on the edge and in the interior of the region. Mesh constraints are typically applied on the edge of a sliding boundary region to fix it spatially.
Set REGION TYPE=EULERIAN to apply the boundary conditions to an Eulerian boundary region. This option is used to create a boundary region across which material can flow and is typically used with velocity boundary conditions. Mesh constraints must be used normal to an Eulerian boundary region to allow material to flow through the region. If no mesh constraints are applied, an Eulerian boundary region will behave in the same way as a sliding boundary region.
This parameter applies only to ABAQUS/Standard analyses.
Include this parameter to indicate that the values of the variables being prescribed with this *BOUNDARY option should remain fixed at their current values at the start of the step. If this parameter is used, any magnitudes given on the data lines are ignored.
This parameter is used in a stress/displacement analysis to specify whether the magnitude is in the form of a displacement history, a velocity history, or an acceleration history. In an ABAQUS/Standard analysis TYPE=VELOCITY should normally be used to specify finite rotations.
Set TYPE=DISPLACEMENT (default) to give a displacement history. ABAQUS/Explicit does not admit jumps in displacement. If no amplitude is specified, ABAQUS/Explicit will ignore the user-supplied displacement value and enforce a zero displacement boundary condition. See “Boundary conditions,” Section 19.3.1 of the ABAQUS Analysis User's Manual, for details.
Set TYPE=VELOCITY to give a velocity history. Velocity histories can be specified in static analyses in ABAQUS/Standard, as discussed in “Prescribing large rotations” in “Boundary conditions,” Section 19.3.1 of the ABAQUS Analysis User's Manual. In this case the default variation is STEP.
Set TYPE=ACCELERATION to give an acceleration history. Acceleration histories should not be used in static analysis steps in ABAQUS/Standard.
If amplitude functions are specified as piecewise linear functions in ABAQUS/Explicit and a displacement history is used, there will be a jump in the velocity and a spike in the acceleration at points on the curve where the curve changes slope. This will result in a “noisy” solution. If possible, use *AMPLITUDE, DEFINITION=SMOOTH STEP; *AMPLITUDE, SMOOTH; or *BOUNDARY, TYPE=VELOCITY or TYPE=ACCELERATION. For TYPE=ACCELERATION the value of the initial velocity (given in *INITIAL CONDITIONS, TYPE=VELOCITY) must be specified to obtain the correct displacement history.
This parameter applies only to ABAQUS/Standard analyses.
Include this parameter to indicate that any nonzero magnitudes associated with variables prescribed through this option can be redefined in user subroutine DISP (“DISP,” Section 25.2.4 of the ABAQUS Analysis User's Manual). If this parameter is used, any magnitudes defined by the data lines of the option (and possibly modified by the AMPLITUDE parameter) will be passed into user subroutine DISP and can be redefined in subroutine DISP. Subroutine DISP will be called only for boundary conditions imposed through the option with this parameter on the keyword line. The value of the TYPE parameter is ignored when this option is used.
First line:
Node number or node set label.
Label specifying the type of boundary condition to be applied (see “Boundary conditions,” Section 19.3.1 of the ABAQUS Analysis User's Manual). Only one type specification can be used per line.
Repeat this data line as often as necessary to specify fixed boundary conditions at different nodes and degrees of freedom.
First line:
Node number or node set label.
First degree of freedom constrained. For a definition of the numbering of degrees of freedom in ABAQUS/Standard and ABAQUS/Explicit, see “Conventions,” Section 1.2.2 of the ABAQUS Analysis User's Manual.
Last degree of freedom constrained. This field can be left blank if only one degree of freedom is being constrained.
The following data item is necessary only when nonzero boundary conditions are specified as history data. Any magnitude given will be ignored when the boundary conditions are given as model data.
Actual magnitude of the variable (displacement, velocity, or acceleration). This magnitude will be modified by an amplitude specification if the AMPLITUDE parameter is used. If this magnitude is a rotation, it must be given in radians. If TYPE=DISPLACEMENT in an ABAQUS/Explicit analysis and no AMPLITUDE specification is provided, this value will be ignored (see “Boundary conditions,” Section 19.3.1 of the ABAQUS Analysis User's Manual). The magnitude can be redefined in user subroutine DISP if the USER parameter is included.
Repeat this data line as often as necessary to specify boundary conditions at different nodes and degrees of freedom.
This parameter is used to define a secondary base and can be used only in a frequency extraction step (“Natural frequency extraction,” Section 6.3.5 of the ABAQUS Analysis User's Manual). Set this parameter equal to the name of a secondary base (“Dynamic analysis procedures: overview,” Section 6.3.1 of the ABAQUS Analysis User's Manual). In subsequent modal superposition steps this base will be excited as specified by the *BASE MOTION option that refers to the same base name. If this parameter is not used in a frequency extraction step, the nodes will be assigned to the primary base.
First line:
Node number or node set label.
First degree of freedom constrained. For a definition of the numbering of degrees of freedom in ABAQUS/Standard, see “Conventions,” Section 1.2.2 of the ABAQUS Analysis User's Manual.
Last degree of freedom constrained. This field can be left blank if only one degree of freedom is being constrained.
Repeat this data line as often as necessary to specify boundary conditions at different nodes and degrees of freedom.
Set this parameter equal to the step number in the global analysis for which the values of the driven variables will be read during this step of the submodel analysis.
Include this parameter to specify that the boundary conditions are the “driven variables” in a submodel analysis. Nodes used in this option must be listed in the *SUBMODEL model definition option.
This parameter can be used only in a static linear perturbation step (“General and linear perturbation procedures,” Section 6.1.2 of the ABAQUS Analysis User's Manual). Set this parameter equal to the increment in the selected step of the global analysis at which the solution will be used to specify the values of the driven variables. By default, ABAQUS/Standard will use the solution at the last increment of the selected step.
Set OP=MOD (default) for existing *BOUNDARY conditions to remain, with this option defining boundary conditions to be added or modified.
Set OP=NEW if all boundary conditions that are currently in effect should be removed. To remove only selected boundary conditions, use OP=NEW and respecify all boundary conditions that are to be retained.
If a boundary condition is removed in a stress/displacement analysis, it will be replaced by a concentrated force equal to the reaction force calculated at the restrained degree of freedom at the end of the previous step. If the step is a general nonlinear analysis step, this concentrated force will then be removed according to the AMPLITUDE parameter on the *STEP option. Therefore, by default the concentrated force will be reduced linearly to zero over the period of the step in a static analysis and immediately in a dynamic analysis.
The OP parameter must be the same for all uses of the *BOUNDARY option in a step.
If the submodel analysis step time is different from the global analysis step time, use the TIMESCALE parameter to adjust the time variable for the driven nodes' amplitude functions. The time variable of each driven node's amplitude function is scaled to match the submodel analysis step time. If this parameter is omitted, the time variable is not scaled.
First line:
Node number or node set label.
First degree of freedom constrained. For a definition of the numbering of degrees of freedom in ABAQUS/Standard and ABAQUS/Explicit, see “Conventions,” Section 1.2.2 of the ABAQUS Analysis User's Manual.
Last degree of freedom constrained. This field can be left blank if only one degree of freedom is being constrained.
Repeat this data line as often as necessary to specify submodel boundary conditions at different nodes and degrees of freedom.
First line:
Node number or node set label.
Thickness of the center zone size around the shell midsurface (given in the units of the model). If this value is omitted, a default value of 10% of the shell thickness specified on the *SUBMODEL option is used. If more than one *SUBMODEL option is used, the default value is 10% of the maximum thickness specified on any of the *SUBMODEL options.
Repeat this data line as often as necessary to specify submodel boundary conditions at different nodes.