You can prescribe values of basic solution variables, including displacements and
rotations in stress/displacement analysis and temperature in heat transfer or coupled
thermal-stress analysis.
Boundary conditions:
can be used to specify the values of all basic solution variables (displacements,
rotations, warping amplitude, fluid pressures, pore pressures, temperatures, electrical
potentials, normalized concentrations, acoustic pressures, or connector material flow) at
nodes;
can be given as “model” input data (within the initial step in Abaqus/CAE) to define zero-valued boundary conditions;
can be given as “history” input data (within an analysis step) to add, modify, or remove
zero-valued or nonzero boundary conditions; and
can be defined by the user through subroutines DISP for Abaqus/Standard and VDISP for Abaqus/Explicit.
Relative motions in connector elements can be prescribed similar to boundary conditions. See
Connector Actuation for more detailed
information.
Only zero-valued boundary conditions can be prescribed as model data
(i.e., in the initial step in Abaqus/CAE). You can specify the data using either “direct” or “type” format. As described
below, the “type” format is a way of conveniently specifying common types of boundary
conditions in stress/displacement analyses. “Direct” format must be used in all other
analysis types.
For both “direct” and “type” format you specify the region of the model to which the
boundary conditions apply and the degrees of freedom to be restrained. (See Conventions for the degree
of freedom numbers used in Abaqus.)
Boundary conditions prescribed as model data can be modified or removed during analysis
steps.
Any number of data lines can be used to specify boundary conditions, and in
stress/displacement analyses both “direct” and “type” format can be specified with a
single use of the BOUNDARY option.
Category: Mechanical; Displacement/Rotation, Velocity/Angular velocity, or Acceleration/Angular acceleration; select regions and toggle on the degree or degrees of freedom
Category: Electrical/Magnetic; Electric potential; select regions
Category: Other; Temperature, Pore pressure, Mass concentration, Acoustic pressure, or Connector material flow; select regions
If you are specifying a temperature boundary condition for a shell region, you can
enter multiple degrees of freedom, from 11 to 31, inclusive.
Using the “Type” Format in Stress/Displacement Analyses
The type of boundary condition can be specified instead of degrees of freedom. The
following boundary condition “types” are available in both Abaqus/Standard and Abaqus/Explicit:
XSYMM
Symmetry about a plane (degrees of freedom ).
YSYMM
Symmetry about a plane (degrees of freedom ).
ZSYMM
Symmetry about a plane (degrees of freedom ).
ENCASTRE
Fully built-in (degrees of freedom ).
PINNED
Pinned (degrees of freedom ).
The following boundary condition types are available only in Abaqus/Standard:
XASYMM
Antisymmetry about a plane with (degrees of freedom 2, 3, 4 ).
YASYMM
Antisymmetry about a plane with (degrees of freedom 1, 3, 5 ).
ZASYMM
Antisymmetry about a plane with (degrees of freedom 1, 2, 6 ).
Warning:
When boundary conditions are prescribed at a node in an analysis
involving finite rotations, at least two rotation degrees of freedom should be
constrained. Otherwise, the prescribed rotation at the node may not be what you expect.
Therefore, antisymmetry boundary conditions should generally not be used in problems
involving finite rotations.
NOWARP
Prevent warping of an elbow section at a node.
NOOVAL
Prevent ovalization of an elbow section at a node.
NODEFORM
Prevent all cross-sectional deformation (warping, ovalization, and uniform radial
expansion) at a node.
For example, applying a boundary condition of type XSYMM
to node set EDGE indicates that the node set lies on a
plane of symmetry that is normal to the X-axis (which will be the
global X-axis or the local X-axis if a nodal
transformation has been applied at these nodes). This boundary condition is identical to
applying a boundary condition using the direct format to degrees of freedom 1, 5, and 6 in
node set EDGE since symmetry about a plane
X=constant implies , , and .
Once a degree of freedom has been constrained using a “type” boundary condition as model
data, the constraint cannot be modified by using a boundary condition in “direct” format
as model data; modifying a constraint in such a way will only produce an error message in
the data (.dat) file indicating that conflicting boundary conditions
exist in the model data.
Load module: Create Boundary Condition: Step: Initial: Symmetry/Antisymmetry/Encastre: select regions and toggle on the boundary condition type
Prescribing Boundary Conditions at Phantom Nodes for Enriched Elements
Phantom nodes for an enriched element can be either colocated with real nodes or located
on an element edge between two real corner nodes (see Modeling Discontinuities as an Enriched Feature Using the Extended Finite Element Method). For phantom
nodes coincident with real nodes, boundary conditions can be specified using the node
numbers of the real nodes.
Alternatively, for phantom nodes with pore pressure degrees of freedom that are located
on an element edge, you can specify the boundary conditions by identifying the phantom
nodes in terms of the two real corner node numbers or by indicating they will be
interpolated from the specified real corner nodes when the enriched element is cracked.
Input File Usage
Use the following option to specify boundary conditions at a phantom node originally
located coincident with the specified real node:
BOUNDARY, PHANTOM=NODEnode number, first degree of freedom, last degree of freedom
Use the following option to specify boundary conditions at a phantom node located at
an element edge:
BOUNDARY, PHANTOM=EDGEfirst corner node number, second corner node number, first degree of freedom, last degree of freedom
Use the following option to indicate that the boundary conditions applied to a
phantom node located at an element edge will be interpolated automatically from the
specified real corner nodes when the enriched element is cracked:
BOUNDARY, PHANTOM=INCLUDEDnode or node set, first degree of freedom, last degree of freedom
Abaqus/CAE Usage
Prescribing boundary conditions at phantom nodes for enriched elements is not
supported in Abaqus/CAE.
Prescribing Boundary Conditions as History Data
Boundary conditions can be prescribed within an analysis step using either “direct” or
“type” format. As with model data boundary conditions, the “type” format can be used only in
stress/displacement analyses; whereas, the “direct” format can be used in analysis types.
When using the “direct” format, boundary conditions can be defined as the total value of a
variable or, in a stress/displacement analysis, as the value of a variable's velocity or
acceleration.
As many boundary conditions as necessary can be defined in a step.
Specify the region of the model to which the boundary conditions apply, the degree or
degrees of freedom to be specified (see Conventions for the degree
of freedom numbers used in Abaqus), and the magnitude of the boundary condition. If the magnitude is omitted, it is the
same as specifying a zero magnitude.
In stress/displacement analysis you can specify a velocity history or an acceleration
history. The default is a displacement history.
Input File Usage
Use either of the following options to prescribe a displacement history:
BOUNDARY or BOUNDARY, TYPE=DISPLACEMENTnode or node set, degree of freedom, , magnitudenode or node set, first degree of freedom, last degree of freedom, magnitude
Use the following option to prescribe a velocity history (the data lines are the
same as above):
Category: Mechanical; Displacement/Rotation; select regions; Distribution: Uniform or select an analytical field or a discrete field; toggle on the degree or degrees of freedom; magnitude
Category: Mechanical; Velocity/Angular velocity or Acceleration/Angular acceleration; select regions; Distribution: Uniform or select an analytical field; toggle on the degree or degrees of freedom; magnitude
Category: Electrical/Magnetic; Electric potential; select regions; Distribution: Uniform or select an analytical field; Method: Specify magnitude; magnitude
Category: Other; Temperature, Pore pressure, Mass concentration, Acoustic pressure, or Connector material flow; select regions; Distribution: Uniform or select an analytical field; Method: Specify magnitude; magnitude
If you are specifying a temperature boundary condition for a shell region, you can
enter multiple degrees of freedom, from 11 to 31, inclusive.
Prescribed Displacement
In Abaqus/Standard you can prescribe jumps in displacements. For example, a displacement-type boundary
condition is used to apply a prescribed displacement magnitude of 0.5 in degree of freedom
1 () to the nodes in node set EDGE. In a
second step these nodes can be moved by another 0.5 length units (to a total displacement
of 1.0) by applying a prescribed displacement magnitude of 1.0 in degree of freedom 1 to
node set EDGE. Specifying a prescribed displacement
magnitude of 0 (or omitting the magnitude) in degree of freedom 1 in the next step would
return the nodes in node set EDGE to their original
locations.
In contrast, Abaqus/Explicit does not admit jumps in displacements and rotations. Displacement boundary conditions
in displacement and rotation degrees of freedom are enforced in an incremental manner
using the slope of the amplitude curve (see below). If no amplitude is specified, Abaqus/Explicit will ignore the user-supplied displacement value and enforce a zero velocity boundary
condition.
The displacement must remain continuous across steps. If amplitude curves are specified,
it is possible, but not valid, to specify a jump in the displacement across a step
boundary when using step time for the amplitude definition. Abaqus/Explicit will ignore such jumps in displacement if they are specified.
Using the “Type” Format in Stress/Displacement Analyses
The type of boundary condition can be specified (as history data) instead of degrees of
freedom in the same manner as discussed above for model data. The boundary condition
“types” that are available as history data are the same as those available as model data.
Once a degree of freedom has been constrained using a “type” boundary condition as
history data, the constraint cannot be modified by using a boundary condition in “direct”
format. The constraint can be redefined only by using a boundary condition in “direct”
format after all previously applied boundary conditions specified using “type” format are
removed.
Use the following option to specify boundary conditions at a phantom node originally
located coincident with the specified real node:
BOUNDARY, PHANTOM=NODEnode number, first degree of freedom, last degree of freedom, magnitude
Use the following option to specify boundary conditions at a phantom node located at
an element edge:
BOUNDARY, PHANTOM=EDGEfirst corner node number, second corner node number, first degree of freedom, last degree of freedom, magnitude
Use the following option to indicate that the boundary conditions applied to a
phantom node located at an element edge will be interpolated automatically from the
specified real corner nodes when the enriched element is cracked:
BOUNDARY, PHANTOM=INCLUDEDnode or node set, first degree of freedom, last degree of freedom, magnitude
Abaqus/CAE Usage
Prescribing boundary conditions at phantom nodes for enriched elements is not
supported in Abaqus/CAE.
Defining Boundary Conditions That Vary with Time
The prescribed magnitude of a basic solution variable, a velocity, or an acceleration can
vary with time during a step according to an amplitude definition (Amplitude Curves).
When an amplitude definition is used with a boundary condition in a dynamic or modal
dynamic analysis, the first and second time derivatives of the constrained variable may be
discontinuous. For example, Abaqus will compute the corresponding velocity and acceleration from a given displacement
boundary condition.
By default, Abaqus/Standard will smooth the amplitude curve so that the derivatives of the specified boundary
condition will be finite. You must ensure that the applied values are correct after
smoothing.
Abaqus/Explicit does not apply default smoothing to discontinuous amplitude curves. To avoid the “noisy”
solution that may result from discontinuities in Abaqus/Explicit, it is better to specify the velocity history of a node. See Amplitude Curves.
Defining Boundary Conditions through User Subroutines
If an amplitude based evolution of a boundary condition is not sufficient, you can define
it yourself in a user subroutine. For this purpose, Abaqus/Standard provides the routine DISP; whereas, Abaqus/Explicit provides the routine VDISP. The region to which the
boundary conditions apply and the constrained degrees of freedom are specified as part of
the boundary condition definition. The actual boundary condition is set within the user
routine based on a number of variables made available in those routines (see DISP and VDISP).
Abaqus/Standard allows for an amplitude and a reference magnitude definition for a user-defined boundary
condition and you may overwrite the amplitude based boundary value within the DISP routine. Whereas, Abaqus/Explicit ignores the reference magnitude, but passes in the amplitude value as an argument to the
user routine VDISP and you may define the
boundary condition to a nonzero value.
By default, all boundary conditions defined in the previous general analysis step remain
unchanged in the subsequent general step or in subsequent consecutive linear perturbation
steps. Boundary conditions do not propagate between linear perturbation steps.
You define the boundary conditions in effect for a given step relative to the preexisting
boundary conditions. At each new step the existing boundary conditions can be modified and
additional boundary conditions can be specified. Alternatively, you can release all
previously applied boundary conditions in a step and specify new ones. In this case any
boundary conditions that are to be retained must be respecified.
If you use a step time amplitude curve when respecifying a boundary condition that is to be
retained from a previous step, the prescribed magnitude of the variable will vary according
to the amplitude definition.
Modifying Boundary Conditions
When you modify an existing boundary condition, the node or node set must be specified in
exactly the same way as previously. For example, if a boundary condition is specified for
a node set in one step and for an individual node contained in the set in another step,
Abaqus issues an error. You must remove the boundary condition and respecify it to change the
way the node or node set is specified.
Input File Usage
Use either of the following options to modify an existing boundary condition or to
specify an additional boundary condition:
Load module: Create Boundary Condition or Boundary Condition Manager: Edit
Removing Boundary Conditions
If you choose to remove any boundary condition in a step, no boundary conditions will be
propagated from the previous general step. Therefore, all boundary conditions that are in
effect during this step must be respecified. The only exception to this rule is during an
eigenvalue buckling prediction procedure, as described in Eigenvalue Buckling Prediction.
Setting a boundary condition to zero is not the same as removing it.
Input File Usage
Use the following option to release all previously applied boundary conditions and
to specify new boundary conditions:
Abaqus/CAE automatically respecifies any boundary conditions (including step time amplitude
curves used in previous steps) that should remain in effect during this step.
Fixing Degrees of Freedom at a Point in an Abaqus/Standard Analysis
In Abaqus/Standard you can “freeze” specified degrees of freedom at their final values from the last general
analysis step. Specifying a zero velocity or zero acceleration boundary condition has the
same effect as fixing the degrees of freedom for displacement or velocity, respectively. In
a one-step inverse procedure, all degrees of freedom are constrained based on the specified
initial configuration for the point.
The
OP=NEW
parameter must be used with the FIXED
parameter if there are any other BOUNDARY options in the same step
that have the
OP=NEW
parameter. Any magnitudes given for the boundary condition are ignored. Except for in a
one-step inverse procedure, the FIXED
parameter is ignored if it is used in the first step of an analysis.
Abaqus/CAE Usage
Load module; Create Boundary Condition; Step: analysis_step; boundary condition; Method: Fixed at Current Position (available only if a previous general analysis step exists)
One-step inverse analysis is not supported in Abaqus/CAE.
Prescribing Boundary Conditions in Linear Perturbation Steps
In a linear perturbation step (General and Perturbation Procedures) the magnitudes
of prescribed boundary conditions should be given as the magnitudes of the perturbations
about the base state. Boundary conditions given within the model definition are always
regarded as part of the base state, even if the first analysis step is a linear perturbation
step. The boundary conditions given in a linear perturbation step will not affect subsequent
steps.
If a perturbation step does not contain a boundary condition definition, degrees of freedom
that are restrained/prescribed in the base state will be restrained in the perturbation step
and will have perturbation magnitudes of zero. To prescribe nonzero perturbation magnitudes,
you have to modify the existing boundary conditions. You can also fix and prescribe
perturbation magnitudes of degrees of freedom that are unrestrained in the base state.
If degrees of freedom that are restrained/prescribed in the base state are released, all
restraints that are to remain must be respecified, remembering that all magnitudes will be
interpreted as perturbations.
Fixing the degrees of freedom at their final values from the last general analysis step
(see previous discussion) has the same effect as modifying the existing boundary conditions
to have zero perturbation magnitudes for all specified degrees of freedom.
The antisymmetric buckling modes of a symmetric structure can be found in an eigenvalue
buckling prediction analysis by specifying the proper boundary conditions (see Eigenvalue Buckling Prediction).
Prescribing Real and Imaginary Values in Boundary Conditions
In steady-state dynamic and matrix generation procedures, a boundary condition can be
prescribed using either a real or an imaginary value (see Direct-Solution Steady-State Dynamic Analysis and Generating Matrices as a Linear Analysis Step). If the real
value is prescribed for a degree of freedom (and the imaginary value is not explicitly
prescribed), the imaginary value is considered to be zero. Similarly, if the imaginary
value is prescribed (and the real value is not explicitly prescribed), the real value is
considered to be zero.
Prescribed Motion in Modal Superposition Procedures
In modal superposition procedures (About Dynamic Analysis Procedures) prescribed
displacements cannot be defined directly using a boundary condition. Instead, the boundary
conditions are grouped into bases in a frequency extraction step. Then, the motion of each
base is prescribed in the modal superposition step. See Natural Frequency Extraction and Transient Modal Dynamic Analysis for details on
this method.
Load module; Create Boundary Condition; Step:modal_dynamic_step, steady-state_dynamic_step, or random_response_step; Category: Mechanical; Types for Selected Step:Displacement base motion or Velocity base motion or Acceleration base motion
Submodeling
When using the submodeling technique, the magnitudes of the boundary conditions in the
submodel can be defined by interpolating the values of the prescribed degrees of freedom
from the file output results of the global model. See Node-Based Submodeling for details.
Prescribing Large Rotations
Sequential finite rotations about different axes of rotation are not additive, which can
make direct specification of such rotations challenging. Abaqus applies rotational boundary conditions by compounding incremental rotations (as described
in Compound rotations). In this process, Abaqus will ignore any jumps in the specified rotation boundary condition, such as when
nondefault amplitudes are used to introduce discontinuities in rotation across step
boundaries. This treatment of rotation boundary conditions in Abaqus is independent of whether the axis of rotation changes or not during the sequence of
rotations. For these and other reasons, it is much simpler to apply finite-rotation boundary
conditions by specifying the rotational velocity versus time. For a discussion of the
rotation degrees of freedom and a multiple step finite rotation example that demonstrates
why velocity-type boundary conditions are preferred for specifying finite-rotation boundary
conditions, see Conventions.
When velocity-type boundary conditions are used to prescribe rotations, the definition is
given in terms of the angular velocity instead of the total rotation. If the angular
velocity is associated with a nondefault amplitude, Abaqus calculates the prescribed increment of rotation as the average of the prescribed angular
velocities at the beginning and the end of each increment, multiplied by the time increment.
In Abaqus/Explicit displacement-type boundary conditions that refer to an amplitude curve are effectively
enforced as velocity boundary conditions using average velocities over time increments as
computed by finite differences of values from the amplitude curve. As with prescribed
displacements (see Prescribed Displacement
above), Abaqus/Explicit does not admit jumps in rotations.
Displacement-type boundary conditions in Abaqus/Standard that constrain just one component of rotation can have essentially no effect on the
solution because the two unconstrained rotational degrees of freedom can combine to override
the constraint.
Example: Using Velocity-Type Boundary Conditions to Prescribe Rotations
For example, if a rotation of about the z-axis is required in a static step, with
no rotation about the x- and y-axes, use a step
time (specified as part of the static step definition) of 1.0, and define a velocity-type
boundary condition to specify zero velocity for degrees of freedom 4 and 5 and a constant
angular velocity of for degree of freedom 6. Since the default variation for a velocity-type
boundary condition in a static procedure is a step, the velocity will be constant over the
step. Alternatively, an amplitude reference could be used to specify the desired variation
over the step.
If, in the next step, the same node should have an additional rotation of radians about the global x-axis, use another static
step with a step time of 1.0 and again define a velocity-type boundary condition to
prescribe zero velocity for degrees of freedom 5 and 6 and a constant angular velocity of for degree of freedom 4.
Prescribing Radial Motion on an Axisymmetric Model
The radial coordinate for any node in an axisymmetric model must be positive. Therefore,
you must make sure that any specified boundary condition does not violate this condition.