Boundary Conditions

You can choose to enter the degrees of freedom to be constrained directly.

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 $X=\mathrm{constant}$ (degrees of freedom $1,5,6=0$).

YSYMM

Symmetry about a plane $Y=\mathrm{constant}$ (degrees of freedom $2,4,6=0$).

ZSYMM

Symmetry about a plane $Z=\mathrm{constant}$ (degrees of freedom $3,4,5=0$).

ENCASTRE

Fully built-in (degrees of freedom $1,2,3,4,5,6=0$).

PINNED

Pinned (degrees of freedom $1,2,3=0$).

The following boundary condition types are available only in Abaqus/Standard:

XASYMM

Antisymmetry about a plane with $X=\mathrm{constant}$ (degrees of freedom 2, 3, 4 $=0$).

YASYMM

Antisymmetry about a plane with $Y=\mathrm{constant}$ (degrees of freedom 1, 3, 5 $=0$).

ZASYMM

Antisymmetry about a plane with $Z=\mathrm{constant}$ (degrees of freedom 1, 2, 6 $=0$).

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.

The NOWARP, NOOVAL, and NODEFORM types apply only to elbow elements (Pipes and Pipebends with Deforming Cross-Sections: Elbow Elements).

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 $u_x=0$, ${\varphi }_y=0$, and ${\varphi }_z=0$.

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.

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.

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.

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 ($u_x$) 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.

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.

You can specify boundary conditions at phantom nodes as history data in the same manner as discussed above for model data (see Modeling Discontinuities as an Enriched Feature Using the Extended Finite Element Method for more information on enriched elements). To specify nonzero boundary conditions, enter the actual magnitude.

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.

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.

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 Structural Matrices). 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.

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.

For example, if a rotation of $6\pi$ 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 $6\pi$ 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.

BOUNDARY, TYPE=VELOCITY
NODE, 4
NODE, 5
NODE, 6, 6, 18.84955592

If, in the next step, the same node should have an additional rotation of $\pi /2$ 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 $\pi /2$ for degree of freedom 4.

BOUNDARY, TYPE=VELOCITY
NODE, 4, 4, 1.570796327
NODE, 5
NODE, 6