Mesh Tie Constraints

A surface-based tie constraint can be used to make the translational and rotational motion as well as all other active degrees of freedom equal for a pair of surfaces. By default, as discussed below, nodes are tied only where the surfaces are close to one another. One surface in the constraint is designated to be the secondary surface; the other surface is the main surface. A name must be assigned to this constraint and might be used in postprocessing with Abaqus/CAE.

TIE, NAME=name
secondary_surface_name, main_surface_name

Interaction module: Create Constraint: Tie

Either element-based or node-based surfaces can be used as the secondary surface. Any surface type (element-based, node-based, or analytical) can be used as the main surface. You can define an element-based surface to contain either the element facets or the element edges (also referred to as an edge-based surface). You should not assume that a constraint over element faces also constrains their edges. If you want to constrain the element edges, a separate constraint must be defined over these edges.

You might need to take some surface restrictions into consideration depending on which tie formulation is used and whether the analysis is conducted in Abaqus/Standard or Abaqus/Explicit. Two tie formulations are available: the surface-to-surface formulation, which is used by default in Abaqus/Standard, and the more traditional node-to-surface formulation, which is used by default in Abaqus/Explicit; these formulations are discussed in more detail later in this section. Table 1 and Table 2 provide comparisons of surface restrictions for the different formulations and analysis codes.

The surface-to-surface formulation generally avoids stress noise at tied interfaces. As indicated in Table 1 and Table 2, only a few surface restrictions apply to the surface-to-surface formulation: this formulation reverts to the node-to-surface formulation if a node-based surface is used. The surface-to-surface formulation does not allow for a mixture of rigid and deformable portions of a surface, and the main surface must not contain T-intersections. Any nodes shared between the secondary and main surfaces are not tied with the surface-to-surface formulation. The same comments apply to both Abaqus/Standard and Abaqus/Explicit in these tables for the surface-to-surface formulation.

With the more traditional node-to-surface formulation additional surface restrictions apply in Abaqus/Standard but fewer restrictions apply in Abaqus/Explicit in comparison to the surface-to-surface formulation. Relatively stringent restrictions on main surface connectivity for the node-to-surface tie formulation in Abaqus/Standard are indicated in Table 2: the main surface must be simply connected and must not contain complex intersections such as T-intersections (see About Contact Pairs in Abaqus/Standard for examples of surfaces with various connectivity characteristics).

Differences with the node-to-surface formulation in Abaqus/Explicit are apparent in Table 1: partially rigid surfaces can be used and the treatment of shared portions of main and secondary surfaces is unique to this case. Nodes and faces that are shared between the main and secondary surfaces are eliminated automatically from the main surface in this case if the paired surfaces are either both element-based or both node-based, enabling the possibility of tying multiple secondary surfaces (defined over various regions of the model) to a common main surface defined over the entire model. This is a convenient way to define tie constraints in large models, as it eliminates the need for defining specialized main surfaces for each surface pairing; however, you must still take care that secondary surfaces do not include portions of the opposing surface to which they should be tied (for example, no tie constraints are generated if the main and secondary surfaces are identical). In the node-to-surface formulation in Abaqus/Explicit all facets attached to nodes that are common between main and secondary surfaces are excluded from being tied to secondary nodes. Sometimes when meshes are transitioned from one type of element to another type or from one element size to another element size, common nodes might exist at the interface of the two regions. Typically, a tie constraint is defined at the interface of the two zones to stitch the two meshes together. In a situation like this, common nodes might get tied to a neighboring facet on the interface and might cause undesirable mesh distortion because of the tie adjustment. One possible way to avoid the undesirable mesh distortion is to specify a very small position tolerance for the tie pair. Another situation that might arise when common nodes occur between the main and secondary surfaces at the interface of mesh transition zones is that secondary nodes in the vicinity of the common node might not get tied. This happens because of the exclusion of main facets attached to the common nodes. Therefore, care must be taken to ensure that elements in different mesh zones do not share common nodes at the interface. For all such common nodes, duplicate nodes occupying the same physical location should be defined.

SURFACE, NAME=secondary_surface_name
SURFACE, NAME=main_surface_name

By default, Abaqus uses a position tolerance criterion to determine the constrained nodes based on the distance between the secondary nodes and the main surface. Alternatively, you can specify a node set containing the secondary nodes to be constrained regardless of their distance to the main surface.

By default, Abaqus will constrain the rotational degrees of freedom when they exist on both secondary and main surfaces (see Figure 4).

Figure 4. Surface-based tie algorithm.

You can specify that the rotational degrees of freedom should not be tied.

TIE, NO ROTATION

Interaction module: Create Constraint: Tie: toggle off Tie rotational DOFs if applicable

You can enforce proper constraints on the faces bounding a repetitive sector of a cyclic symmetric structure (see Analysis of Models that Exhibit Cyclic Symmetry). This makes it possible to define a single sector of the cyclic symmetry model together with its axis of cyclic symmetry to define the behavior of the 360° model. Cyclic symmetry models can be used within the following procedures: static; quasi-static; eigenfrequency extraction, based on the Lanczos solver technique; steady-state dynamics, based on modal superposition; and heat transfer. If an eigenfrequency extraction is performed on a cyclic symmetric model, the nodes involved in the cyclic symmetry constraint cannot be used in any other constraint (e.g., multi-point constraints, equations, rigid bodies, couplings, or kinematic couplings).

TIE, CYCLIC SYMMETRY

Interaction module: InteractionCreate: Cyclic symmetry

Abaqus uses the criteria discussed above to determine which secondary nodes will be tied to the main surface. Abaqus then forms constraints between these secondary nodes and the nodes on the main surface. A key aspect in forming the constraint for each secondary node is determining the tie coefficients. These coefficients are used to interpolate quantities from the main nodes to the tie point. Abaqus can use one of two approaches to generate the coefficients: the “surface-to-surface” approach or the “node-to-surface” approach.

If an analysis carried out with Abaqus/Standard is imported into Abaqus/Explicit or vice versa, the tie constraints are not imported and must be redefined. If the imported analysis is essentially a continuation of the original analysis, it is important that the tie constraints are as similar as possible. Hence, you should make sure that the same constraint type is used. If the default approach was used in the original Abaqus/Standard analysis, the surface-to-surface approach should be specified in the Abaqus/Explicit analysis. Similarly, if the default approach was used in the original Abaqus/Explicit analysis, the node-to-surface approach should be specified in the Abaqus/Standard analysis.

By default, with the exceptions mentioned below, Abaqus will automatically reposition the secondary nodes to be tied in the initial configuration without causing strain to resolve gaps such that the surfaces are just touching, accounting for any shell thickness (unless you have specified that thickness should not be accounted for, as discussed above in the context of the position tolerance criterion) but not accounting for beam or membrane thickness. One exception is that no adjustments are made where tied surfaces are closer together than the combined half-shell thickness. All adjustments are performed such that the secondary and main surfaces are never pushed apart; that is, the reference surfaces will only become closer as a result of the adjustments.

It is recommended that you allow the automatic adjustments to occur, especially if neither surface has rotations; in this case a constant offset vector is used, so incorrect behavior of the constraint under rigid body rotation can occur when secondary nodes are not lying exactly on the main surface. Adjustments are not made if the secondary surface belongs to a substructure or when either the secondary or main surface is a beam element-based surface; in the latter cases you should locate the beam element nodes with the desired offset from the other surface.

TIE, ADJUST=YES or NO

Interaction module: Create Constraint: Tie: toggle Adjust secondary surface initial position

The main surface for a tie constraint can be based on three-dimensional beam elements. For this case each secondary node is projected onto the line formed by the nodes of the beam elements in the undeformed configuration to find the projection point. During the subsequent analysis the motion of each secondary node is rigidly constrained to the motion (translation and rotation) of its projection point; that is, each secondary node and its projection point are connected by a rigid beam. Constraining other elements to a beam element-based main surface allows modeling of interactions between the surface of a (complex) beam section and its surroundings, without having to model the beam with continuum and/or shell elements. This feature can be particularly useful for modeling acoustic-structural interactions.

The surface-based tie constraint capability can be used in models where the nodal degrees of freedom on both the secondary and main surfaces include electrical potential, pore pressure, acoustic pressure, and/or temperature. Except for the type of nodal degree of freedom being constrained, Abaqus uses exactly the same formulation for the tie constraint in nonmechanical simulations as it does for mechanical simulations. In general, degrees of freedom common to both surfaces are tied, and any other degrees of freedom are unconstrained. For example, a thermal tie between a solid element and a shell element constrains only degree of freedom 11.

The case of structural-acoustic constraints is the exception to this rule. Here, appropriate relations between the acoustic pressure on the fluid surface and displacements on the solid surface are formed internally (see Acoustic, Shock, and Coupled Acoustic-Structural Analysis). The displacements and/or pressure degrees of freedom on the surfaces are the only ones affected; rotations are ignored by the tie constraint in this case.

The internally computed structural-acoustic coupling conditions use surface areas and normal directions associated with the secondary surface elements. The secondary surface for structural-acoustic tie constraints cannot be a node-based surface. In two-dimensional analyses the out-of-plane thickness of the secondary elements is required. Generally, this thickness is the thickness specified on the section definition for the secondary surface elements. However, when beam elements form the secondary surface in a tie constraint pair with acoustic elements, a unit thickness in the out-of-plane direction is assumed for the beams.

In Abaqus/Standard you can define coupling between solid medium and acoustic medium infinite elements along the surfaces that extend to infinity. These surfaces are defined using the edges of the acoustic elements and sides numbered “2” and higher of the solid medium infinite elements. The infinite surfaces of solid medium and acoustic infinite elements can be coupled only through the use of a surface-based tie constraint. As shown in Figure 9, the acoustic infinite elements must be the secondary elements and the edges of the acoustic infinite elements should lie within the specified position tolerance to the solid medium infinite element base facets.

Figure 9. Use of a surface-based tie constraint to prescribe the coupling between solid medium and acoustic medium infinite elements.

If the base facets of acoustic infinite elements are to be coupled to solid medium finite elements, to solid medium infinite elements, or to structural elements, either a surface-based tie constraint or acoustic-structural interaction elements can be used. Surfaces defined on solid medium infinite elements cannot be used in a surface-based tie constraint in Abaqus/Explicit.

Table 3 enumerates all possible cases. For other secondary-main pairings not listed in this table, an error message is issued.

You can specify that certain degrees of freedom should not be tied between the surfaces involved in a tie constraint. These degrees of freedom are pore pressure, solid electric potential, temperature, fluid electric potential, and ion concentration.

TIE, NO PORE
TIE, NO ELECTRIC POTENTIAL
TIE, NO TEMPERATURE
TIE, NO FLUID ELECTRIC POTENTIAL
TIE, NO ION CONCENTRATION

There are the following advantages to using a surface-based tie constraint in Abaqus/Standard instead of defining tied contact as discussed in Defining Tied Contact in Abaqus/Standard:

• Degrees of freedom of the secondary surface nodes will be eliminated.

• The tie constraint is more efficient in terms of the size of the fronts of the operator matrix because fewer main surface nodes are associated with each secondary node.

• Rotational degrees of freedom as well as translational degrees of freedom can be tied.

• Tie constraints are much more general since they allow the use of general surfaces.

• Surface offsets and shell thickness are taken into account.

In a model with multiple tie constraint definitions it is possible that the secondary and main surfaces of different tie constraint definitions might intersect. If two tie constraint definitions have part or all of their main surfaces in common or if the surfaces tied are layered (that is, the main surface of one tie constraint definition acts as the secondary surface of a subsequent tie constraint definition), Abaqus will attempt to chain the constraint definitions together. This will reduce the number of degrees of freedom and lower the computational expense, resulting in faster run times. However, in a model with multiple tie constraint definitions and nodes on the secondary surface of one tie constraint definition are part of the secondary surface of other tie constraint definitions, an overconstraint occurs. In most cases the overconstraint is because of the existence of redundant constraints, and it is safe to eliminate this redundancy. However, the overconstraint might also be due to conflicting constraints, in which case the problem is because of a modeling error that you should correct. Simulation results will vary depending on which constraint is removed to avoid an overconstraint if the overlapping constraints are not identical. It is recommended that, wherever possible, you order the secondary and main surfaces of the constraint definitions to avoid intersecting secondary surfaces. See Adjustments for Overlapping Constraints for a discussion of initial strain-free adjustments for overlapping constraints. When secondary nodes of a tie constraint also participate in other types of constraints, Abaqus will replace these nodes in the other constraints with corresponding main nodes from the tie constraint.

The following limitations exist for tie constraints:

• Surface-based tie constraints cannot be used to connect gasket elements that model thickness-direction behavior only.

• A rigid surface cannot act as a secondary surface in a constraint pair in Abaqus/Standard.

• A secondary node of a tie constraint cannot act as a secondary node of another constraint in Abaqus/Standard.

• Tie constraints cannot be used to tie infinite elements to finite elements in Abaqus/Explicit. To couple infinite and finite elements in Abaqus/Explicit, the elements must share nodes.

• The axisymmetric solid Fourier elements with nonlinear, asymmetric deformation cannot form element-based surfaces; therefore, such surfaces cannot be used in tie constraints.

• In Abaqus/Standard, tie constraints cannot be used to connect nodes included in a node-based surface or nodes included in an element-based surface defined using an element edge identifier if such nodes have more than one temperature degree of freedom.