28.1 Defining fasteners

You use fasteners to model a point-to-point connection between two or more faces, such as a spot weld, a bolt, or a rivet. You can use the Attachment toolset to create attachments that help you define fasteners; for more information, see “Understanding attachment points and lines,” Section 56.1. You can create point-based fasteners or discrete fasteners.

Point-based fasteners

Point-based fasteners make use of positioning points to create mesh-independent fasteners in Abaqus/Standard and Abaqus/Explicit, as described in “Mesh-independent fasteners,” Section 30.3.4 of the Abaqus Analysis User's Manual. A positioning point can be an attachment point, a reference point, or a node from an orphan mesh. Point-based fasteners modeling spot welds around the edge of a bracket are shown in Figure 28–1. The user first created attachment points at equally spaced intervals around the edge of the bracket. The attachment points were used to define the location of the fastener's positioning points.

Figure 28–1 Point-based fasteners modeling spot welds.

A point-based fastener can connect selected faces with either connectors or rigid (beam) multi-point constraints. If you want to model a rigid connection, you can use rigid connectors or rigid multi-point constraints.

Connectors

If you use connectors to connect the faces, you can model either rigid, elastic, or inelastic connections with failure by using the generality of connector behavior definitions. You can use a rigid connector to model a rigid connection. However, if you are using rigid connectors and Abaqus detects two adjacent point-based fasteners that are sharing nodes, you must avoid overconstraining your model by defining some elasticity in the connector behavior to reduce the stiffness.

You can request output from connectors.

Rigid (beam) multi-point constraints

Rigid multi-point constraints are computationally cheaper than connectors and are less likely to result in an overconstrained model when two adjacent fasteners are sharing nodes. When Abaqus detects two adjacent fasteners that are sharing nodes and using rigid multi-point constraints, it uses a penalty distributing coupling formulation that relaxes, to a small degree, the constraint between the motion of the fastening point and its coupling nodes to avoid the overconstraint.

You cannot request output from multi-point constraints.

A point-based fastener uses distributing coupling constraints to connect the faces regardless of how you mesh the faces. When you submit a job for analysis, Abaqus uses your fastener definition to connect the faces with couplings and connectors. When you open the output database file in the Visualization module, you can display the couplings and connectors; however, outside the Visualization module, symbols are displayed only for the positioning points of the point-based fasteners.

If your model contains many fasteners (more than a thousand), point-based fasteners offer superior performance over discrete fasteners. In addition, you may want to use point-based fasteners if you have a file from a CAD system that defines the coordinates of each positioning point. Point-based fasteners are available only for three-dimensional models. Point-based fasteners are used to model mesh-independent fasteners as described in “Mesh-independent fasteners,” Section 30.3.4 of the Abaqus Analysis User's Manual.

You can use the following two methods to create a point-based fastener, as shown in Figure 28–2:

Select a positioning point and allow Abaqus/CAE to project the point to the closest face along a normal to the surface. The first fastening point is created where the normal intersects the closest face.
Select a positioning point and specify the direction vector along which the point is projected. The first fastening point is created where the vector intersects the closest face.

Figure 28–2 Creating point-based fasteners.

Abaqus creates the second (and subsequent) fastening points when you submit the job for analysis by projecting the first fastening point onto the other surfaces to be connected along the normal to the closest face.

Discrete fasteners

Discrete fasteners make use of attachment lines to create connectors and couplings between selected faces in Abaqus/Standard and Abaqus/Explicit. Figure 28–3 shows a discrete fastener that uses attachment lines and connectors (Beam connection type) to model a spot weld across three surfaces. The user first created attachment lines at the locations of the spot welds. The attachment lines were used to define the location of the discrete fastener.

Figure 28–3 A spot weld across three surfaces modeled with a discrete fastener.

The process of creating an attachment line is similar to the process of creating point-based fasteners. You select a starting point and specify which of the two methods Abaqus/CAE will use to project the point onto the closest face. Figure 28–4 shows the two methods for creating an attachment line that is used to define a discrete fastener.

Figure 28–4 Creating an attachment line that is used to define a discrete fastener.

Abaqus/CAE projects the attachment line along a normal to the closest face. You can use the following two methods to determine the number of faces that are connected by the attachment line:

Specify the number of projections or layers.
Specify the maximum length of the projection.

For each attachment line, Abaqus/CAE determines the fastening points and applies a distributing coupling between each fastening point and its corresponding surface. After you assign a connector section to the attachment line, Abaqus/CAE creates a connector, and the discrete fastener is considered to be fully defined. If your model is complex, Abaqus/CAE can create a chain of attachment lines connecting multiple surfaces that would be time consuming to create manually. In contrast with point-based fasteners, you can view attachment lines and discrete fasteners and their connectors and couplings outside the Visualization module.

If two surfaces are used by two attachment lines and share a common face, Abaqus/CAE merges the two faces into a single face when you submit the model for analysis. This results in better performance by Abaqus/Standard or Abaqus/Explicit, especially when the fasteners connect nodes across faces of a refined orphan mesh.

When you submit a job that contains a model with discrete fasteners for analysis, Abaqus/CAE writes special comment lines to the input file. These special comment lines, which are ignored by the Abaqus solvers, allow Abaqus/CAE to recreate the fully defined discrete fasteners upon import into Abaqus/CAE. For more information, see “Importing interactions, constraints, and fasteners” in “Importing a model from an Abaqus/Standard or an Abaqus/Explicit input file,” Section 10.5.2.

An example of creating discrete fasteners is illustrated in the Python script included in “Buckling of a column with spot welds,” Section 1.2.3 of the Abaqus Example Problems Manual.

Both point-based and discrete fasteners can be modeled using connectors or beam MPCs. If you define connectors that use basic, assembled, or complex connection types, you can request output from your fasteners of connector output variables. However, if you use beam MPCs, no output is available from your fasteners.