김경종
23 KiB
35.3.4 MESH-INDEPENDENT FASTENERS
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
References
• “Surfaces: overview,” Section 2.3.1
• “Coupling constraints,” Section 35.3.2
• “Connector elements,” Section 31.1.2
• *FASTENER
• *FASTENER PROPERTY
• “About fasteners,” Section 29.1 of the Abaqus/CAE User’s Guide
Overview
The mesh-independent fastener capability:
• is a convenient method to define a point-to-point connection between two or more surfaces such as a spot weld or rivet connection;
• uses spatial coordinates of fastener locations to define point-to-point connections independent of underlying meshes;
• combines either connector elements or BEAM MPCs with distributing coupling constraints to provide a connection that can be located anywhere between two or more surfaces regardless of the mesh refinement or location of nodes on each surface;
• can be used to connect both deformable and rigid element-based surfaces;
• can model either rigid, elastic, or inelastic connections with failure by using the generality of connector behavior definitions; and
• is available only in three dimensions.
Introduction
Many applications require modeling of point-to-point connections between parts. These connections may be in the form of spot welds, rivets, screws, bolts, or other types of fastening mechanisms. There may be hundreds or even thousands of these connections in a large system model such as an automobile or airframe.
The fastener can be located anywhere between the parts that are to be connected regardless of the mesh. In other words, the location of the fastener can be independent of the location of the nodes on the surfaces to be connected. Instead, the attachment to each of the parts being connected is distributed to several nodes in the surfaces to be connected in the neighborhood of the fastening points. Figure 35.3.4–1 shows a typical one-layer and two-layer fastener configuration. Each layer connects two fastening points using either a connector element or a BEAM MPC. Each fastening point is connected to the surface using
text_image
A Number of layers = 2 B layer 1 Radius of influence C layer 2 Fastening point Number of layers = 1 Fastening point
Figure 35.3.4–1 Typical one-layer and two-layer fastener configuration.
a distributing coupling constraint that couples the displacement and rotation of each fastening point to the average displacement and rotation of the nearby nodes.
The mesh-independent fastener capability in Abaqus is designed to model these connections in a convenient manner. The fastener automatically:
• determines the locations of nodes and orientations of connector elements or BEAM MPCs between two or more surfaces;
• generates distributing coupling constraints to attach the connector elements or BEAM MPCs to each surface in a mesh-independent manner; and
• calculates weights for the distributing coupling constraints that complete the mesh-independent connection.
For an example of the use of mesh-independent fasteners, see “Buckling of a column with spot welds,” Section 1.2.3 of the Abaqus Example Problems Guide. Mesh-independent fasteners are referred to as point-based fasteners by Abaqus/CAE. For more information, see “About fasteners,” Section 29.1 of the Abaqus/CAE User’s Guide. It is also possible to assemble fasteners in Abaqus/CAE using connector elements, coupling constraints, etc. For further details, see “About assembled fasteners,” Section 29.1.3 of the Abaqus/CAE User’s Guide.
Fastener interactions
Fasteners are defined in groups called interactions, which are assigned names. Each interaction defines one or more fasteners. The number of individual fasteners is equal to the number of positioning points used to locate the fasteners. Fastening points on each surface are found by considering the position of the positioning point as discussed in subsequent sections.
Fasteners can be defined using connector elements or BEAM MPCs. BEAM MPCs allow modeling of perfectly rigid connectors between components; while connector elements allow you to model much more complex behavior, such as deformable connectors that include the effects of elasticity, damage, plasticity, and friction.
Input File Usage: *FASTENER, INTERACTION NAME=name
Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Name: name, Type: Point-based
Defining fasteners using BEAM MPCs
For modeling perfectly rigid connections you need not define fasteners using connector elements. Instead, Abaqus can internally generate BEAM MPCs 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 BEAM MPCs with each node in the reference node set becoming the first node of the BEAM MPC. The second node of each BEAM MPC will be generated internally by Abaqus. If multi-layer fasteners are to be defined, Abaqus generates linked sets of BEAM MPCs with each node in the reference node set becoming the first node of the first BEAM MPC 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 BEAM MPCs as the number of layers in the fastener.
Input File Usage: Use the following options:
*FASTENER, INTERACTION NAME=name, REFERENCE NODE SET=node set label *NSET, NSET=node set label
Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: select positioning points: Property: Section: Rigid MPC
Defining fasteners using connector elements
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 35.3.4–2). 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.
flowchart
graph TD
A["1"] -->|100| B["2"]
C["3"] -->|200| D["4"]
style A fill:#000,stroke:#000
style C fill:#000,stroke:#000
style B fill:#000,stroke:#000
style D fill:#000,stroke:#000
single layer fastener modeled with connectors
flowchart
graph TD
A["1"] -->|100| B["2"]
C["4"] -->|200| D["5"]
E["6"] -->|201| F["3"]
style A fill:#000,stroke:#000
style C fill:#000,stroke:#000
style E fill:#000,stroke:#000
style B fill:#000,stroke:#000
style D fill:#000,stroke:#000
style F fill:#000,stroke:#000
multi-layer fastener modeled with connectors
text_image
• nodes ——— connector elements x positioning point location specified by user
Figure 35.3.4–2 Single- and multi-layer fasteners modeled with connector elements.
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.
Connector elements generated by Abaqus
In this approach you do not need to explicitly define the connector elements that connect the fastening points of the fastener. The fastener interaction refers to an empty element set. You must specify a
connector section definition that refers to this element set. In addition, you assign a reference node set containing a list of user-defined nodes to the fastener interaction. The nodes in this reference node set are used as positioning points to locate the fasteners.
If single-layer fasteners are to be modeled, Abaqus generates single connector elements with each node in the reference node set becoming the first node of a connector element. The second node of each connector element will be generated internally by Abaqus. If multi-layer fasteners are to be defined, Abaqus generates linked sets of connector elements with each node in the reference node set becoming the first node of the first connector element 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 connector elements as the number of layers in the fastener. The connector elements are given internally generated element numbers and assigned to the named user-specified element set. You can use this element set to request output for these connector elements. However, this element set should not be included in another element set definition.
| Input File Usage: | Use the following options:*FASTENER, INTERACTION NAME=name, ELSET=element set label,REFERENCE NODE SET=node set labelblank line*NSET, NSET=node set label*CONNECTOR SECTION, ELSET=element set label |
| Abaqus/CAE Usage: | Interaction module: Special→Fasteners→Create: Point-based: select positioning points: Property: Section: Connector section: select connector section |
Example: using connector elements to define single-layer fasteners directly
To define a single-layer fastener directly using connector elements:
• Define two connector elements with user element numbers 100 and 200 and user-defined node numbers 1, 2 and 3, 4, respectively, and include them in an element set. Nodes 1 and 3 act as the positioning points for the two fasteners (see Figure 35.3.4–2).
• Refer to the element set in the fastener interaction and connector section definitions.
• Assign section properties to the fasteners. Suppose in this example that relative displacements between the fastening points are to be allowed. Therefore, the fasteners must be assigned a section that has available components of motion; for example, a CARTESIAN section can be used.
• The relative displacement between the fastening points gives rise to elastic deformations. Hence, the material between the fasteners is modeled as linear elastic with a spring stiffness of 10000 using connector elasticity.
The following input can be used:
*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,
Example: using connector elements to define multi-layer fasteners directly
To define a multi-layer fastener directly using connector elements:
• Define two linked sets of connector elements with each linked set containing exactly two connectors. The first linked set comprises element numbers 100 and 101, with node numbers 1, 2 and 2, 3, respectively. The second linked set comprises element numbers 200 and 201, with node numbers 4, 5 and 5, 6, respectively. Include the connector elements in an element set. Nodes 1 and 4 act as the positioning points for the two fasteners (see Figure 35.3.4–2).
• Refer to the element set in the fastener interaction and connector section definitions
• Assign section properties to the fasteners. Suppose in this example that rigid beam-type behavior between the fastening points is to be modeled; in that case the fasteners must be assigned a BEAM section.
The following input can be used:
*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,
Specifying the positioning points, projection method, and fastening points
Each interaction defines one or more fasteners. The number of individual fasteners is equal to the number of positioning points used to locate the fasteners. Positioning points are nodes defined at the fastener locations and assigned as a reference node set to the interaction.
In general, a positioning point should be located as close to the surfaces being connected as possible. The reference node specifying the positioning point can be one of the nodes on the connected surfaces or can be defined separately. Abaqus determines the actual points where the fastener layers attach to the surfaces that are being connected by first projecting the positioning point onto the closest surface. Abaqus offers the following projection methods to find fastening points on the specified surfaces to form fasteners:
• Face-to-face
• Face-to-edge
• Edge-to-face
• Edge-to-edge
• Connector direction
The choice of method depends on how the surfaces are oriented relative to each other.
Fastening surfaces that are nearly parallel to each other
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 35.3.4–3 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.
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.
Input File Usage:
Use the following option to allow Abaqus to define the projection direction:
*FASTENER, REFERENCE NODE SET=node set label, ATTACHMENT METHOD=FACETOFACE (default)
blank line
text_image
Positioning point Projection direction specified by user First fastening point Positioning point Projection normal for surface Second fastening point
Figure 35.3.4–3 Directed and normal projection to locate the fastening points for the face-to-face projection method.
Use the following option to define the projection direction directly:
*FASTENER, REFERENCE NODE SET=node set label, ATTACHMENT METHOD=FACETOFACE (default)
x-component, y-component, z-component
Abaqus/CAE Usage: Use the following input to allow Abaqus to define the projection direction:
Interaction module: Special→Fasteners→Create: Point-based: select positioning points: Domain tabbed page: Direction vector: Default, Criteria tabbed page: Attachment method: Face-to-Face
Use the following input to define the projection direction directly:
Interaction module: Special→Fasteners→Create: Point-based: select positioning points: Domain tabbed page: Direction vector: Specify, Criteria tabbed page: Attachment method: Face-to-Face
Fastening nearly perpendicular surfaces
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 35.3.4–4 shows attachments for the face-to-edge and edge-to-face projection methods.
Creating the first fastening point on a face
In the face-to-edge projection method Abaqus projects the positioning point onto the closest surface along a directed line segment normal to the surface. The subsequent fastening points are found by searching for the closest points on the remaining specified surfaces. The closest fastening point may fall on the edge or a corner of a surface.
text_image
Subsequent fastening point First fastening point x Positioning point
text_image
First fastening point Positioning point Subsequent fastening point
Figure 35.3.4–4 Face-to-edge and edge-to-face projection methods to locate fastening points for surfaces that form T-intersections.
Input File Usage: *FASTENER, REFERENCE NODE SET=node set label, ATTACHMENT METHOD=FACETOEDGE blank line
Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: select positioning points: Criteria: Attachment method: Face-to-Edge
Creating the first fastening point on an edge
In the edge-to-face projection method, the first fastening point is found by searching for the closest point on the specified surface or surfaces. The closest point may be on the edge or corner of the surface. For subsequent fastening points Abaqus projects the previous fastening point along a directed line segment normal to the surface.
Input File Usage: *FASTENER, REFERENCE NODE SET=node set label, ATTACHMENT METHOD=EDGETOFACE blank line
Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: select positioning points: Criteria: Attachment method: Edge-to-Face
Fastening abutting surfaces
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 35.3.4–5 shows attachments for the edge-to-edge projection method.
text_image
First fastening point Positioning point x Subsequent fastening point
Figure 35.3.4–5 Edge-to-edge projection method to locate fastening points for abutting surfaces.
Input File Usage: *FASTENER, REFERENCE NODE SET=node set label, ATTACHMENT METHOD=EDGETOEDGE blank line
Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: select positioning points: Criteria: Attachment method: Edge-to-Edge
Fastening surfaces that are not parallel
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.
Input File Usage: *FASTENER, ELSET=element set label, ATTACHMENT METHOD=CONNECTORDIRECTION blank line
Abaqus/CAE Usage: Selecting a connector to control the location and direction of the fastener is not supported in Abaqus/CAE.
Specifying the surfaces to be fastened
Once the positioning points have been specified, the surfaces to be fastened can be specified using two different approaches. In the first approach you directly specify the surfaces that are to be connected with a fastener. In the second approach you specify a search zone, and Abaqus automatically identifies the surfaces that are to be connected. However, in the second approach Abaqus does not distinguish between coincident facets. Hence, if coincident facets are to be fastened, you should specify distinct surfaces containing each of the coincident facets and use the first approach. Only element-based surfaces defined on faces can be fastened together (see “Element-based surface definition,” Section 2.3.2, and “Operating on surfaces,” Section 2.3.6).