Mesh-Independent Fasteners

For modeling perfectly rigid connections you need not define fasteners using connector elements. Instead, Abaqus can internally generate BEAMMPCs connecting the fastening points of the fasteners. In this approach you assign a reference node set containing a list of user-defined nodes to the fastener interaction. The nodes in this reference node set will be used as positioning points to locate the fasteners. If single-layer fasteners are to be modeled, Abaqus generates single BEAMMPCs with each node in the reference node set becoming the first node of the BEAMMPC. The second node of each BEAMMPC will be generated internally by Abaqus. If multi-layer fasteners are to be defined, Abaqus generates linked sets of BEAMMPCs with each node in the reference node set becoming the first node of the first BEAMMPC in each linked set. The subsequent nodes in each linked set will be generated internally by Abaqus. For multi-layer fasteners each linked set contains as many BEAMMPCs as the number of layers in the fastener.

FASTENER, INTERACTION NAME=name, 
REFERENCE NODE SET=node set label
NSET, NSET=node set label

Interaction module: SpecialFastenersCreate: Point-based: select positioning points: Property: Section: Rigid MPC

Using connector elements as the basis for a point-to-point connection allows for very complex behavior to be modeled with fasteners. Like other uses of connector elements, the connection can be fully rigid or may allow for unconstrained relative motion in local connector components. In addition, deformable behavior can be specified using a connector behavior definition that can include the effects of elasticity, damping, plasticity, damage, and friction. There are two methods to define fasteners that use connector elements to model the behavior between fastening points. For both methods the fastener interaction refers to an element set containing the connector elements. You must specify a connector section definition that refers to this element set. You should be careful when specifying the connector orientation (if needed) as discussed below in Defining the Fastener Orientation.

Defining the Connector Elements Directly

The most controlled approach to specifying fasteners using connector elements is to define the connector elements explicitly and associate them with an element set. The fastener interaction refers to the element set. Each fastener in the fastener interaction corresponds to one or more connector elements depending on the number of layers of the fastener (see Figure 2).

Figure 2. Single- and multi-layer fasteners modeled with connector elements.

A single connector element is associated with each layer, and the two nodes of the connector element correspond to the fastening points of the two adjacent surfaces. When specifying a multi-layer fastener, the connector elements for each layer should share nodes with the connector elements of adjacent layers.

For a single-layer fastener the positioning point used to locate the fastener and its fastening points is taken as the nodal coordinates of the first node of the connector element. For a multi-layer fastener the positioning point is taken as the first node of the first connector in a linked set of connectors with as many members as layers. Examples of defining a single-layer and multi-layer fastener are included at the end of this section.

Input File Usage

Use the following options:

FASTENER, INTERACTION NAME=name, ELSET=element set label
blank line
ELEMENT, TYPE=CONN3D2, ELSET=element set label
CONNECTOR SECTION,  ELSET=element set label

Abaqus/CAE Usage

For point-based fasteners in Abaqus/CAE, you cannot define the connector elements directly; the connector elements are generated by Abaqus.

FASTENER, INTERACTION NAME=name, ELSET=element set label,
REFERENCE NODE SET=node set label
blank line
NSET, NSET=node set label
CONNECTOR SECTION, ELSET=element set label

Interaction module: SpecialFastenersCreate: Point-based: select positioning points: Property: Section: Connector section: select connector section

FASTENER, INTERACTION NAME=fastinter, ELSET=fastconn, PROPERTY=fastprop
blank line
surface1, surface2
ELEMENT, TYPE=CONN3D2, ELSET=fastconn
100, 1, 2
200, 3, 4
CONNECTOR SECTION, ELSET=fastconn, BEHAVIOR=behav
CARTESIAN, 
CONNECTOR BEHAVIOR, NAME=behav
CONNECTOR ELASTICITY, COMPONENT=1
10000,
CONNECTOR ELASTICITY, COMPONENT=2
10000,
CONNECTOR ELASTICITY, COMPONENT=3
10000,

FASTENER, INTERACTION NAME=fastinter, ELSET=fastconn, PROPERTY=fastprop
blank line
surface1, surface2, surface3
ELEMENT, TYPE=CONN3D2, ELSET=fastconn
100, 1, 2
101, 2, 3
200, 4, 5
201, 5, 6
CONNECTOR SECTION, ELSET=fastconn
BEAM, 

Most commonly the surfaces to be fastened together are nearly parallel to each other; in which case the fastening points are located on element facets away from the periphery of the surfaces. The face-to-face projection method is most appropriate for such situations. It is also the default projection method.

In the face-to-face projection method, Abaqus projects each positioning point onto the closest surface along a directed line segment normal to the surface. Alternatively, you can specify the projection direction. Specifying the direction may be useful when two-dimensional drawings are used to identify the positioning point locations and those locations are known precisely in two dimensions but not in a third. For this case the direction specified is typically the normal to the plane of the drawing.

Once the fastening point on the closest surface has been identified, Abaqus determines the points on the other surface or surfaces to be connected by projecting the first fastening point onto the other surfaces along the fastener normal direction, which is typically normal to the closest surface. Figure 3 shows the two ways of locating the projection points. When surfaces to be fastened are not exactly parallel, Abaqus sometimes sets attachment points to be at the closest facet edges or corner on the surface, rather than along the fastener normal direction.

Figure 3. Directed and normal projection to locate the fastening points for the face-to-face projection method.

The location of the positioning point (a node in the reference node set) might not coincide with the locations of the fastening points found by Abaqus. Hence, the coordinates of the node at the positioning point may change from their user-prescribed values when the node is shifted to a fastening point. If the node at the positioning point is part of the connectivity of a user-defined element, this can cause the element whose connectivity includes that node to undergo unacceptable initial distortions. In such situations it is recommended that you define the node at the positioning point separately. In general, you should not specify this node to be one of the nodes of the connected surfaces.

FASTENER, REFERENCE NODE SET=node set label, ATTACHMENT METHOD=FACETOFACE (default)
blank line

FASTENER, REFERENCE NODE SET=node set label, ATTACHMENT METHOD=FACETOFACE (default)
x-component, y-component, z-component

Interaction module: SpecialFastenersCreate: Point-based: select positioning points: Domain tabbed page: Direction vector: Default, Criteria tabbed page: Attachment method: Face-to-Face

Interaction module: SpecialFastenersCreate: Point-based: select positioning points: Domain tabbed page: Direction vector: Specify, Criteria tabbed page: Attachment method: Face-to-Face

When you need to fasten surfaces that are perpendicular or nearly perpendicular to each other; i.e., forming a T-intersection, the face-to-edge or the edge-to-face projection methods are appropriate choices. Figure 4 shows attachments for the face-to-edge and edge-to-face projection methods.

Figure 4. Face-to-edge and edge-to-face projection methods to locate fastening points for surfaces that form T-intersections.

FASTENER, REFERENCE NODE SET=node set label, ATTACHMENT METHOD=FACETOEDGE
blank line

Interaction module: SpecialFastenersCreate: Point-based: select positioning points: Criteria: Attachment method: Face-to-Edge

FASTENER, REFERENCE NODE SET=node set label, ATTACHMENT METHOD=EDGETOFACE
blank line

Interaction module: SpecialFastenersCreate: Point-based: select positioning points: Criteria: Attachment method: Edge-to-Face

When it is desired to form fasteners between surfaces that are butting against each other, the edge-to-edge projection method is appropriate. In this method the first as well as the subsequent fastening points are located by searching for the closest point on the specified surface or surfaces. The fastening points in this method may be located on the edge of a surface. Figure 5 shows attachments for the edge-to-edge projection method.

Figure 5. Edge-to-edge projection method to locate fastening points for abutting surfaces.

FASTENER, REFERENCE NODE SET=node set label, ATTACHMENT METHOD=EDGETOEDGE
blank line

Interaction module: SpecialFastenersCreate: Point-based: select positioning points: Criteria: Attachment method: Edge-to-Edge

When fastening surfaces that are not parallel to one another, you can control the precise location and direction of the fastener. To define the location and direction, prescribe a connector element for each fastener with nodes at a specific location. Abaqus maintains the location and the direction of the connector element.

FASTENER, ELSET=element set label, ATTACHMENT METHOD=CONNECTORDIRECTION
blank line

If you specify multiple surfaces as part of the interaction definition, the surfaces to be fastened are restricted to these surfaces. In general, specifying multiple surfaces is the preferred way of defining fasteners; this method leads to a more precise fastener construct definition. The number of layers of each fastener is one less than the number of surfaces specified. One fastening point is found on each surface.

FASTENER
first data line
surface1, surface2, surface3, etc.

Interaction module: SpecialFastenersCreate: Point-based: Domain: Approach: Fasten specified surfaces by proximity, select surfaces

By default, the connectivity of the fastening points is determined by their relative position along the fastener projection direction. For example, the default connectivity for the two-layer example shown in Figure 1 connects fastening point A to point B (layer 1) and point B to point C (layer 2).

You can control the connectivity of the fastening points when the fasteners are formed on user-specified surfaces. You can specify that the connectivity of the fastening points be defined by the order in which you specified their associated surfaces.

FASTENER, UNSORTED
first data line
surface1, surface2, surface3, etc.

Interaction module: SpecialFastenersCreate: Point-based: Domain: Approach: Fasten in specified order, select surfaces

If you do not specify any surfaces as part of the interaction definition, Abaqus searches for fastening points on all element facets that fall within a sphere of user-specified radius R with its center at the positioning point. If you do not specify the search radius, Abaqus computes a default search radius based on five times the facet thickness (for shell element facets) or the characteristic element length (for other element types) in the vicinity of each positioning point.

To refine the search, you can specify a single surface definition that will limit the facet search to element facets belonging to that surface. In this case you must define a collective surface that includes at least each connected surface. A combined surface can also be used (see Operating on Surfaces for a discussion on combining surfaces).

To refine the search further, you can specify a positive integer value, N, for the number of layers of each fastener. Abaqus searches for the $N+1$ fastening points closest to the positioning point. If BEAMMPCs are used to model the fastener, a warning message is issued if the requisite number of fastening points is not found. However, if connector elements are used to model the fastener and the requisite number of fastening points is not found, Abaqus issues an error message. Thus, when specifying the number of layers, you should ensure that the search radius has been specified such that $N+1$ fastening points can be found.

If multiple surfaces are listed as part of the fastener definition, the number of layers for each fastener is ignored. If a user-specified search radius is used for the multiple surface case, Abaqus searches for fastening points on all facets belonging to each of the listed surfaces that fall within a sphere of user-specified radius R with its center at the positioning point. Facets of the listed multiple surfaces that lie outside this sphere are not included in the search. A maximum of 15 layers can be specified for a particular fastener definition.

You should always examine the fastener definitions that Abaqus created to make sure that they are appropriate for your model.

FASTENER, SEARCH RADIUS=R, NUMBER OF LAYERS=N
first data line

Interaction module: SpecialFastenersCreate: Point-based: Criteria: Search radius: Specify: R, Maximum layers for projection: Specify: N

If a connector element is used to model a fastener, the local coordinate system defined on the connector section, ${\mathbf{T}}_{connector}$, operates on the local coordinate system for the fastener, ${\mathbf{T}}_{fastener}$, to determine the final local coordinate system of the connector element, ${\mathbf{T}}_{connectorfinal}$. In other words,

In the above equations ${\mathbf{T}}_{connector}$ and ${\mathbf{T}}_{fastener}$ are assumed to be orthogonal rotation matrices with the local 1-, 2-, and 3-directions being the first, second, and third rows, respectively. The local coordinate system for a connector element modeling a fastener should be specified with respect to the local coordinate system of the fastener. The orientation displayed in the Visualization module of Abaqus/CAE (Abaqus/Viewer) is ${\mathbf{T}}_{connectorfinal}$ at all fastener locations unless you specify not to write the orientations to the database; in this case, only ${\mathbf{T}}_{connector}$ is displayed. If connector or displacement field output is requested, field output for additional nodal rotation at the connector nodes is generated automatically to ensure that the appropriate connector orientation directions are displayed as the analysis progresses. Otherwise, the orientation ${\mathbf{T}}_{connectorfinal}$ computed at the beginning of the analysis is displayed at all times with the updated orientations used for computation purposes.

For example, suppose you use a HINGE connector and want the released rotational degree of freedom, which is in the connector's local 1-direction, to be normal to the surfaces that are being fastened. If the default local coordinate system is used for the fastener (local 3-direction normal to the surface), the local 1-direction for the connector should be set to (0., 0., 1.); i.e., the local 3-direction of the fastener. When compounded with the local coordinate system for the fastener, the local 1-direction for the connector will be normal to the surface. See Mesh-independent spot welds for an example of a compounded orientation.

FASTENER, ORIENTATION=orientation name, 
ADJUST ORIENTATION=NO
blank line

Interaction module: SpecialFastenersCreate: Point-based: Adjust: Fastener CSYS: Edit: select local coordinate system, toggle off Adjust CSYS to make local Z-axis normal to closest surface

In many cases when the pair of fastened surfaces are close to each other, unrealistic contact interactions may occur between the two surfaces unless an evolving offset associated with bending is introduced in the translational coupling constraints. This offset introduces the influence of cloud node rotational degrees of freedom into the translational coupling constraints. For this coupling method to be active, all rotational degrees of freedom at all coupling nodes must be active (as is the case when shells are fastened together) and all degrees of freedom must be constrained (which is the default; see Defining Fastener Properties below).

Use of this option is independent of whether or not cloud node rotations influence rotational coupling constraints.

FASTENER, COUPLING=STRUCTURAL

Interaction module: SpecialFastenersCreate: Point-based: Formulation: Coupling type: Structural distributing

In Abaqus/Standard you can optionally neglect cloud node rotational degrees of freedom in rotational coupling constraints. In Abaqus/Explicit they are neglected by default. In this case the rotation of the fastening point matches the average “swirling” of the cloud associated with cloud node translations.

If cloud rotations do not participate in rotational coupling constraints, moments at the fastening points are transmitted as a pure force distribution among the cloud nodes. Therefore, when the cloud node arrangement is colinear, the constraint is not capable of transmitting all components of a moment at the reference node. Specifically, the moment component that is parallel to the colinear coupling node arrangement will not be transmitted. When this case arises, Abaqus issues a warning message that identifies the axis about which the element will not transmit a moment.

FASTENER, ROTATIONAL COUPLING=CONTINUUM

Fasteners are assumed to have a circular projection onto the connected surfaces. You are required to specify the radius of the fastener.

FASTENER PROPERTY
r

Interaction module: SpecialFastenersCreate: Point-based: Property: Physical radius: r 

For fasteners modeled with connector elements, translational as well as rotational degrees of freedom can be released by prescribing connector section types that have unconstrained (available) degrees of freedom. For example, a HINGE connector can be used to release the rotational degree of freedom in the connector's local 1-direction.

For fasteners modeled with BEAMMPCs, the moment constraint between the rotation degrees of freedom at the fastening points and the average rotation of the coupling nodes can be released in one, two, or three directions. You can specify the moment constraint directions in the default local coordinate system or a user-defined local coordinate system. The three translational degrees of freedom at the fastening points are always coupled to the average translation of the coupling nodes. You specify the degrees of freedom of the fastening point to be coupled to the average motion of the coupling nodes as part of the fastener property definition.

If no degrees of freedom are specified as part of the fastener property definition, all six degrees of freedom are coupled. If you specify one or more degrees of freedom but not all available translation degrees of freedom, Abaqus issues a warning message and adds all the available translation degrees of freedom to the constraint. If a user-specified local orientation is specified for the fastener interaction, the local degrees of freedom are with respect to the user-defined coordinate system.

FASTENER PROPERTY 
section properties
first dof, last dof

FASTENER PROPERTY 
section properties
1, 5

Interaction module: SpecialFastenersCreate: Point-based: Formulation: toggle off UR1, UR2, or UR3

Fasteners can be used to connect both deformable and rigid element-based surfaces. However, if the fasteners are modeled with BEAMMPCs, potential overconstraints may arise if more than one rigid surface is involved in a given fastener definition. Abaqus automatically attempts to remove these types of overconstraints by allowing at most one rigid surface in any individual fastener definition. A warning message is generated if an overconstraint of this type is detected.

For example, suppose surfaces A and C in Figure 1 are part of the same rigid body, and surface B is deformable. Abaqus automatically removes either surface A or surface C from the fastener definition and only forms the fastener between the deformable surface and the remaining rigid surface. If surface A and surface C belong to two separate rigid bodies, their respective rigid body reference nodes will be joined by an internally generated BEAMMPC.

In another example, suppose all three surfaces in Figure 1 are rigid. In this case no fastener will be formed, and the unique rigid body reference nodes for surfaces A, B, and C will be joined by beam MPCs. Unresolvable overconstraints may arise if inconsistent kinematic constraints (such as displacement boundary conditions) are placed on rigid body reference nodes that have been joined by BEAMMPCs. In this case you must modify the model to resolve the overconstraints. Possible courses of action include removing some of the rigid surfaces from the fastener definitions or removing inconsistent kinematic conditions on the rigid body reference nodes.

The above-described procedure to resolve overconstraints with fasteners and rigid bodies will preserve the kinematics of the original model. In Abaqus/Standard you can bypass the overconstraint checks and prevent automatic model modifications in the model preprocessor (see Overconstraint Checks).

Potential overconstraints exist with rigid fasteners if all the coupling nodes of any associated distributing coupling element are wholly contained within one or more other fastener definitions. This can happen if the spacing between positioning points is small compared to the typical element size in a mesh (which is often the case in automotive models). To avoid overconstraints in this situation, Abaqus uses a penalty formulation for all fastener distributing coupling elements that satisfy the above criteria. The penalty distributing coupling formulation relaxes, to a small degree, the constraint between the motion of the distributing coupling element reference node and its coupling nodes.