Mesh Tie Constraints

Defining a Tie Constraint for a Pair of Surfaces

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.

Input File Usage

TIE, NAME=name
secondary_surface_name, main_surface_name

Defining the Surfaces to Be Constrained

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.

Table 1. Comparison of characteristics for surface-based tie formulations.
Tie formulation	Optimized stress accuracy	Node-based surfaces allowed	Mixture of rigid and deformable subregions allowed	Treatment of nodes/facets shared between main and secondary surfaces
Surface-to-surface (Abaqus/Standard or Abaqus/Explicit)	Yes	Reverts to node-to-surface formulation	No	Eliminated from secondary surface
Node-to-surface in Abaqus/Standard	No	Yes	No	Eliminated from secondary surface
Node-to-surface in Abaqus/Explicit	No	Yes	Yes	Eliminated from main surface

Table 2. Comparison of element-based surface characteristics allowed for surface-based tie formulations.
Tie formulation	Surface Characteristics (Yes=allowed, No=not allowed)
Tie formulation	Double-sided	Discontinuous	T-intersection	Edge-based
Surface-to-surface (Abaqus/Standard or Abaqus/Explicit)	Main: YesSecondary: Yes	Main: YesSecondary: Yes	Main: NoSecondary: Yes	Main: YesSecondary: Yes
Node-to-surface in Abaqus/Standard	Main: YesSecondary: Yes	Main: YesSecondary: Yes	Main: NoSecondary: Yes	Main: YesSecondary: Yes
Node-to-surface in Abaqus/Explicit	Main: YesSecondary: Yes	Main: YesSecondary: Yes	Main: YesSecondary: Yes	Main: YesSecondary: Yes

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.

Input File Usage

Use the SURFACE option to define the secondary and main surfaces used in the constraint (see About Surfaces):

SURFACE, NAME=secondary_surface_name
SURFACE, NAME=main_surface_name

Specifying the Subset of Secondary Nodes to Be Constrained

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.

Using the Position Tolerance Criterion

The default position tolerance criterion ensures that nodes are tied only where the secondary and main surfaces are close to one another in the initial configuration. For example, consider the case shown in Figure 1. Surfaces Comp1_surf and Comp2_surf are defined to cover all exposed faces of Component 1 and Component 2, respectively. These two surfaces can be used as the secondary and main surfaces in a tie constraint to tie the two components in the desired region, because only the nodes at the initial interface between the two surfaces are tied.

The default value of the position tolerance, $d_{t o l}$ , typically results in desired tie constraints with little effort. Details regarding the calculation of distances between surfaces and default values of the position tolerances are provided below. You can modify the position tolerance if desired.

Input File Usage

Use the following option to use the default position tolerance:

TIE

Use the following option to specify a position tolerance:

TIE, POSITION TOLERANCE=distance

Calculating the Distance between Surfaces

The following factors influence the calculation of the distance between surfaces for a particular secondary node:

Shell thickness. By default, calculations of distances between surfaces account for shell thickness and offset effects for element-based secondary or main surfaces: the distance is measured from the actual top or bottom side of the surface, whichever is closer to the other surface. Alternatively, you can specify that surface thicknesses and offsets should be ignored, which also has implications for nodal position adjustments for resolving initial gaps (discussed later).
Input File Usage
Use the following option to ignore surface thicknesses and offsets in the distance calculations:
```
TIE, NO THICKNESS
```
Whether the surface-to-surface or node-to-surface constraint formulation (discussed below) is used. If a position tolerance is in effect, a constraint is generated at a secondary node for either formulation if the distance between the surfaces, as calculated at the secondary node, does not exceed $d_{t o l}$ . The distance between surfaces at a secondary node is based on a closest-point projection to the main surface for the node-to-surface constraint formulation and is computed along the normal direction to the secondary surface for the surface-to-surface constraint formulation. Additional secondary nodes might be tied if the surface-to-surface constraint formulation is used along with an element-based secondary surface and a main surface that is not node-based. The following addendum to the position tolerance criterion applies in such cases: if the distance between the surfaces is within $d_{t o l}$ over a significant portion of a secondary face (or segment in two dimensions) that forms an angle of less than 30° with the main surface, all secondary nodes attached to such a face (or segment) are considered to satisfy the position tolerance.
The types of surfaces involved (element-based, node-based, or analytical).

Position Tolerance for an Element-Based Main Surface

The default position tolerance for element-based main surfaces is 5% or 10% of the typical main facet diagonal length for the node-to-surface and surface-to-surface tie formulations, respectively. When using an element-based main surface, the distance between surfaces for a particular point on a secondary surface is based on the closest point on the main surface (which might be on the edge of the main surface or within a facet). Figure 2

shows an example with no thickness: nodes 2–14 satisfy the position tolerance criterion for the node-to-surface and surface-to-surface constraint formulations. Significant portions of the end secondary segments (that is, the segment connecting nodes 1 and 2 and the segment connecting nodes 14 and 15) are within the position tolerance shown, so nodes 1 and 15 would also satisfy the position tolerance criterion for the surface-to-surface constraint formulation except for the fact that the angle between the secondary and main surfaces is slightly greater than 30° at those locations.

Position Tolerance for a Node-Based Main Surface

The default position tolerance for a node-based main surface is based on the average distance between nodes in the main surface. The distance between the surfaces for a particular secondary node is based on the closest main node. If this distance is less than the position tolerance, Abaqus will create a tie constraint between the secondary node, the closest main node, and other main nodes in similar proximity to the secondary node. For mismatched meshes across a tied interface, the distance between secondary and main nodes can be much larger than the “normal” distance between the surfaces, which can lead to confusion when using a position tolerance criterion with a node-based main surface. Figure 3 shows how the tolerance region is defined around a node-based main surface. The surface-to-surface constraint formulation reverts to the node-to-surface constraint formulation for a node-based main surface.

Position Tolerance for an Analytical Rigid Main Surface

The default position tolerance for tie constraints between an element-based secondary surface and an analytical rigid main surface is 5% or 10% of the typical secondary facet diagonal length for the node-to-surface and surface-to-surface tied formulations, respectively. The default position tolerance for tie constraints between a node-based secondary surface and an analytical rigid main surface is 5% of the typical distance between secondary nodes. When using an analytical rigid main surface, the distance between surfaces for a particular point on the secondary surface is based on the closest point on the main surface.

Specifying the Constrained Nodes Directly

This method allows you direct control over which secondary nodes are tied.

Input File Usage

TIE, TIED NSET=node_set_label

Unconstrained Nodes in Tie Constraint Pairs

Abaqus does not constrain secondary nodes to the main surface unless they are included in the tied node set or within the tolerance distance from the main surface at the start of the analysis, as discussed above. Any secondary nodes not satisfying these criteria will remain unconstrained for the duration of the simulation; they will never interact with the main surface as part of the tie constraint. In mechanical simulations an unconstrained secondary node can penetrate the main surface freely unless contact is defined between the secondary node and main surface. The general contact algorithms in Abaqus/Standard and Abaqus/Explicit will generate contact exclusions automatically for secondary node–main surface combinations corresponding to constrained nodes of tie constraint pairs, but no such contact exclusions are generated for nodes outside the position tolerance of the constraints. In a thermal, acoustic, electrical, or pore pressure simulation an unconstrained secondary node will not exchange heat, fluid pressure, electrical current, or pore fluid pressure with the main surface.

Determining Which Secondary Nodes Have Been Tied and Which Secondary Nodes Have Not Been Tied

For each tie constraint pair, Abaqus creates a node set comprising secondary nodes that will be tied and a node set comprising secondary nodes that will be left unconstrained.

In addition, Abaqus prints a table in the data (.dat) file listing each secondary node and the main surface nodes to which it will be tied if model definition data are requested (see Controlling the Amount of analysis input file processor Information Written to the Data File). If a constraint cannot be formed for a given secondary node, Abaqus/Standard issues a warning message in the data file.

In Abaqus/Explicit you can also request two nodal field output variables: TIEDSTATUS will help you identify the constrained and unconstrained secondary nodes, and TIEADJUST will help you visualize the adjustment performed at the nodes (see Abaqus/Explicit Output Variable Identifiers). A tied node that participates in more than one tie definition as a secondary node as well as a main node is shown as “tied” regardless of whether it got tied as a secondary node or as a main node.

When creating a model with surface-based tie constraints, it is important to use the information provided by Abaqus to identify any unconstrained nodes and to make any necessary modifications to the model to constrain them.

Constraining the Rotational Degrees of Freedom

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

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

Input File Usage

TIE, NO ROTATION

Constraining the Faces of a Cyclic Symmetric Structure in Abaqus/Standard

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).

Input File Usage

TIE, CYCLIC SYMMETRY

This parameter can be used only with the CYCLIC SYMMETRY MODEL option.

The Surface-Based Tie Constraint Formulation

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.

The “Surface-to-Surface” Approach

The “surface-to-surface” approach minimizes numerical noise for tied interfaces involving mismatched meshes. The surface-to-surface approach enforces constraints in an average sense over a finite region, rather at discrete points as in the traditional node-to-surface approach. The surface-to-surface formulation for surface-based tie constraints is similar to the surface-to-surface contact formulation (see Contact Formulations in Abaqus/Standard); however, a fundamental difference is that each surface-based tie constraint involves only one secondary node (and multiple main nodes), whereas each surface-to-surface contact constraint involves multiple secondary nodes.

The surface-to-surface approach is used by default in Abaqus/Standard with exceptions noted below, and it is optional in Abaqus/Explicit. For the case of infinite acoustic elements tied to shell elements in Abaqus/Standard the added cost of the surface-to-surface approach can be quite significant; therefore, the node-to-surface approach is used by default in this case. If the surface-to-surface approach is “on by default” or explicitly specified, Abaqus automatically reverts to the node-to-surface approach for individual tie constraints in the following circumstances:

if either of the surfaces being tied is node-based;
if the projection along the secondary surface normal direction does not intersect the main surface; or
if single-sided secondary and main surfaces have surface normals in approximately the same direction.

Abaqus/Explicit might automatically add a small amount of artificial mass to the model to maintain numerical stability if the surface-to-surface approach is specified.

The surface-to-surface approach generally involves more main nodes per constraint than the node-to-surface approach, which tends to increase the solver bandwidth in Abaqus/Standard and, therefore, can increase solution cost. In most applications the extra cost is fairly small, but the cost can become significant in some cases. The following factors (especially in combination) can lead to the surface-to-surface approach being quite costly:

A large fraction of tied nodes (degrees of freedom) in the model
The main surface being more refined than the secondary surface
Multiple layers of tied shells, such that the main surface of one tie constraint acts as the secondary surface of another tie constraint

Input File Usage

TIE, TYPE=SURFACE TO SURFACE

The “Node-to-Surface” Approach

The traditional “node-to-surface” approach (which is used by default in Abaqus/Explicit and is optional in Abaqus/Standard) sets the coefficients equal to the interpolation functions at the point where the secondary node projects onto the main surface. This approach is somewhat more efficient and robust for complex surfaces.

For the node-to-surface method of establishing the tie coefficients with an element-based main surface, the point on the surface closest to each secondary node is calculated and used to determine the main nodes that are going to form the constraint (see Figure 5). For example, nodes 202, 203, 302, and 303 are used to constrain node a; nodes 204 and 304 are used to constrain node b; and node 402 is used to constrain node c.

Input File Usage

TIE, TYPE=NODE TO SURFACE

Choosing the Secondary and Main Surfaces of a Surface-Based Tie Constraint

The choice of secondary and main surfaces can have a significant effect on the accuracy of the solution, in particular if the “node-to-surface” approach is used. The effect is much less (and the accuracy generally better) for the “surface-to-surface” approach. In either case, if both surfaces in a constraint pair are deformable surfaces, the main surface should be chosen as the surface with the coarser mesh for best accuracy.

In Abaqus/Standard a rigid surface cannot act as a secondary surface in a tie constraint. To comply with this rule, the capability to automatically resolve overconstraints in Abaqus/Standard (see Overconstraint Checks) will modify tie constraint definitions in the following cases:

Tie constraints between two surfaces of the same rigid body are removed.
Tie constraints between two surfaces of two rigid bodies are replaced by a BEAM-type connector between the respective rigid body reference nodes.
Tie constraints specified with a purely rigid secondary surface and a purely deformable main surface are modified to reverse the main and secondary assignments unless this is not possible because of other modeling restrictions (in which case an error message is issued).

These methods are not applied if the secondary surface that you specified is partially rigid and partially deformable; Abaqus/Standard issues an error message in such cases.

In acoustic, structural-acoustic, and elastic wave propagation problems care should be exercised when tying meshes of highly dissimilar refinement. If two media have different wave speeds, the optimal meshes for each of the media will have different characteristic element lengths: the faster medium will have larger elements. If surfaces of these meshes are used in a tie constraint, the surface of the finer mesh (of the slower medium) should be designated as the secondary. Nevertheless, in the region near the tied surfaces, the physical wave phenomena in both fast and slow media will typically have length scales characteristic of the slower medium; that is, of the shortest length scale in the physical problem. Therefore, if these phenomena are important, the mesh of the faster medium should be refined to the scale of the slower medium in the vicinity of the contact region.

Adjusting the Surfaces and Considering Offsets

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.

Input File Usage

TIE, ADJUST=YES or NO

Criteria for Adjustment

A secondary node is considered for adjustment if both of the following conditions are met:

The secondary node satisfies whatever criterion is in effect for generating a constraint (either because it satisfies the position tolerance criterion or belongs to the specified node set of constrained secondary nodes, as previously discussed).
The secondary node is more than the combined thickness of the secondary and main surfaces away from its projection point on the main reference surface, accounting for any offset of the element reference surfaces from the respective element midsurfaces.

For an element-based main surface a secondary node will be moved toward the closest point on the main surface; for a node-based main surface a secondary node will be moved toward the closest main node. The corrected position of an adjusted secondary node is determined from the combined effects of shell element thickness and any specified reference surface offset relative to the shell midsurface of either secondary or main surfaces. Figure 6 shows the adjusted secondary node position in an example with two shell element-based surfaces tied together (in this example one of the element reference surfaces is offset from the element midsurface). It is assumed that the surfaces were farther apart than shown in Figure 6 prior to the adjustment; otherwise, the secondary nodes would not have been adjusted.

Adjustments are made only for secondary nodes that are included in the user-specified tied node set or that meet the tolerance criteria described above.

Adjustments for Overlapping Constraints

Nodal adjustments for tie constraints are processed sequentially in the order of the constraint definitions at the start of an analysis. If different constraint or contact definitions involve the same nodes, some adjustments might cause lack of compliance for contact or constraint definitions that were previously processed. These conflicts are less likely to occur in Abaqus/Explicit because the adjustments in Abaqus/Explicit are automatically processed in the chaining order discussed in Overlapping Constraints. These conflicts can be avoided in Abaqus/Standard in some cases by changing the processing order of constraint and contact definitions: nodes in common between different contact or constraint definitions should be processed first as secondary nodes and later as main nodes.

Input File Usage

To change the processing order of constraint and contact definitions, change the order of the definitions in the input file. Constraint and contact definitions are processed in the order in which they appear.

Accounting for an Offset between Tied Surfaces

Abaqus allows a gap to exist between tied surfaces. Such gaps might exist if you prevent nodal adjustments for tied surfaces. A gap between the reference surfaces might remain because of the presence of shell thickness even if nodal adjustments are performed. Figure 7 shows some cases where an offset between the reference surfaces might be desirable for tied surface pairs to account for shell or beam thickness.

Rigid body motion is properly accounted for when the nodes are separated by a finite distance when at least one of the surfaces is based on shell or beam elements; when the main surface is an analytical rigid surface; or, in the case of node-based surfaces, when the nodes on at least one surface have active rotational degrees of freedom.

The nature of the constraint on translational motion between surfaces in Abaqus depends on whether there is an offset between the surfaces and on which surfaces have rotational degrees of freedom, as discussed below.

Neither Surface Has Rotational Degrees of Freedom

If neither surface has rotational degrees of freedom, the global translational degrees of freedom of the secondary node and the closest point on the main surface are constrained to be the same. When an offset exists, the behavior of Abaqus/Standard differs from that of Abaqus/Explicit.

Abaqus/Explicit enforces the constraint through the fixed offset like a PIN-type MPC when the nodes in the MPC are not coincident. Because the fixed offset does not rotate, the surface-based constraint will not represent rigid body rotation correctly. The constraint represents rigid body motion correctly when the offset is zero. This behavior can be ensured by specifying that all tied secondary nodes should be moved onto the main surface. If an offset needs to be maintained, general contact with surface-based cohesive behavior (as explained in Contact Cohesive Behavior) that correctly accounts for rigid body rotation of the offset should be used.

In general, Abaqus/Standard enforces the constraint such that the surface-based constraint represents rigid body rotation correctly; the enforcement of this constraint will introduce nonlinearity in the model. There are, however, two exceptions in which rigid body rotation between the tied surfaces cannot be enforced: (1) when node-based main surfaces are used and (2) when using tie constraints for cyclic symmetry.

Only One Surface Has Rotational Degrees of Freedom

If the secondary surface has rotational degrees of freedom and the main surface does not, the translational motion is constrained at the closest point on the main reference surface. When the reference surfaces are offset, a moment will be applied to each secondary node based on the constraint force times the offset distance. Similarly, if the main surface has rotational degrees of freedom and the secondary surface does not, the translational motion is constrained at each secondary node and a moment will be applied to the relevant nodes on the main surface if an offset exists. In either case the surface-based constraint will behave correctly under rigid body rotation regardless of the amount of offset.

Both Surfaces Have Rotational Degrees of Freedom

If both surfaces have rotational degrees of freedom, are not offset, and the rotations are tied, each secondary node is constrained to the main surface like a TIE-type MPC. If an offset exists between the surfaces, the constraint acts like a BEAM-type MPC between the secondary node and the closest point on the main reference surface.

If the rotations are not tied, Abaqus allows you to choose the location of the translational constraint. It can be enforced at the main reference surface, the secondary reference surface, or anywhere in between. The location of the translational constraint enforcement for surfaces where the rotations are not tied will affect the distribution of moment to each of the surfaces. The most physically reasonable choice is to locate the constraint at the point where the actual top or bottom sides of each surface meet. The constraint then models a perfect adhesive between the surfaces, which transfers shear stress to each surface. Abaqus will choose the location of the translational constraint as follows:

If the main surface is shell element-based, the translational constraint is enforced on the top or bottom side of the main surface.
If the secondary surface is shell element-based and the main surface is not, the translational constraint is enforced at the top or bottom side of the secondary surface.
Otherwise, the translational constraint is enforced at the main reference surface.

To override these default locations, you can specify a constraint ratio for the tie constraint equal to the fractional distance between the main reference surface and the secondary node at which the translational constraint should act. Figure 8 shows an example of the use of a constraint ratio to prescribe the location of the translational constraint between two shell surfaces that are tied together with no rotational constraints. The distance between the main reference surface and the secondary reference surface is b. The prescribed constraint ratio, r, is then used to locate the translational constraint at a distance a from the main reference surface. All distances are measured along the vector between the secondary node and its projection point onto the main reference surface. The constraint behavior is then similar to that of two rigid beams pinned together, as shown.

Input File Usage

TIE, CONSTRAINT RATIO=value

Constraining a Surface to a Three-Dimensional Beam

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.

Use of Tie Constraints in Nonmechanical Simulations

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.

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.

Table 3. Possible secondary-main surface pairings.
Secondary Surface	Main Surface	Degrees of Freedom Tied
Acoustic	Acoustic	Acoustic pressure
Acoustic	Stress	Translations
Stress	Acoustic	Acoustic pressure
Stress	Stress	Translations and/or rotations
Heat-Stress	Stress	Translations and/or rotations
Stress	Heat-Stress	Translations and/or rotations
Heat-Stress	Heat-Stress	Temperature, translations and/or rotations
The following surface pairings are available only in Abaqus/Standard:
Heat transfer	Heat transfer	Temperature
Electrical-Heat	Heat transfer	Temperature
Heat transfer	Electrical-Heat	Temperature
Electrical-Heat	Electrical-Heat	Temperature and electric potential
Pore-Stress	Pore-Stress	Pore pressure and translations
Pore-Stress	Stress	Translations
Stress	Pore-Stress	Translations
Pore-Stress	Pore	Pore pressure
Electrochemical-Heat	Electrochemical-Heat	Temperature, electric potential in the solid, electric potential in the fluid, and ion concentration

If the surfaces involved in the tie constraint contain pore pressure and/or temperature degrees of freedom, you can specify that these degrees of freedom should not be tied.

Input File Usage

TIE, NO PORE
TIE, NO TEMPERATURE

Tie Constraints Versus Tied Contact in Abaqus/Standard

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.

Overlapping Constraints

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.

Overconstrained Secondary Nodes in Abaqus/Standard

If an overconstraint occurs, Abaqus/Standard issues an error message unless the constraints are redundant or nearly redundant, as discussed below. As discussed previously, each tie constraint involves a single secondary node and a set of main nodes with nonzero tie coefficients. Abaqus/Standard considers tie constraints involving the same secondary node to be nearly redundant if at least one node is common among the respective sets of main nodes with nonzero tie coefficients. In such cases, rather than issuing an error message, Abaqus/Standard issues a warning message and only enforces one of the constraints.

The surface-based tie constraint is imposed in Abaqus/Standard by eliminating the degrees of freedom on the secondary surface; therefore, nodes on the secondary surface should not be used to apply boundary conditions, nor should they be used in any subsequent tie, multi-point, equation, or kinematic coupling constraint (see Overconstraint Checks for a more complete discussion of overconstraints in Abaqus/Standard).

Overconstrained Secondary Nodes in Abaqus/Explicit

In contrast, Abaqus/Explicit treats overconstraints with a penalty method, thus enforcing the constraints in an average sense; the computational cost of the analysis might increase in these cases.

In addition, if the secondary surface for a tie constraint definition in Abaqus/Explicit is part of a rigid body while the main surface comprises a deformable element- or node-based surface and the main surface acts as the secondary surface in a subsequent tie constraint definition, the resolution of the resulting constraints can prove to be computationally intensive. It is recommended that, wherever possible, you order the secondary and main surfaces of the constraint definitions to avoid such a situation.

Nullifying the Tie Constraint on Secondary Nodes because of Element Deletion in Abaqus/Explicit

In Abaqus/Explicit tie constraints are nullified as underlying elements of tied surfaces are deleted because of material point failure. The tie constraint between a secondary node and its corresponding main nodes is deleted when either all the elements attached to the secondary node are deleted or the main element to which the secondary node is tied is deleted.

Limitations

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.