김경종
29 KiB
Forming fasteners on user-specified surfaces
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.
| Input File Usage: | *FASTENERfirst data linesurface1, surface2, surface3, etc. |
| Abaqus/CAE Usage: | Interaction module: Special→Fasteners→Create: Point-based: Domain: Approach: Fasten specified surfaces by proximity, select surfaces |
When you select multiple surfaces for a single surface region, Abaqus/CAE combines the multiple surfaces using the single-surface search method, as described in “Forming fasteners on surfaces inside a user-specified search zone” below.
Controlling connectivity of fasteners on user-specified 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 35.3.4–1 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 userspecified surfaces. You can specify that the connectivity of the fastening points be defined by the order in which you specified their associated surfaces.
| Input File Usage: | *FASTENER, UNSORTEDfirst data linesurface1, surface2, surface3, etc. |
If user-specified surfaces are not included on the data lines, the UNSORTED parameter is ignored.
| Abaqus/CAE Usage: | Interaction module: Special→Fasteners→Create: Point-based: Domain: Approach: Fasten in specified order, select surfaces |
Forming fasteners on surfaces inside a user-specified search zone
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,” Section 2.3.6, 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 fastening points closest to the positioning point. If BEAM MPCs 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 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 userspecified 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.
Input File Usage: *FASTENER, SEARCH RADIUS=R, NUMBER OF LAYERS=N first data line
Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: Criteria: Search radius: Specify: R, Maximum layers for projection: Specify: N
Defining the radius of influence
Each fastening point is associated with a group of nodes on the surface in the immediate neighborhood of the fastening point called a region of influence. The motion of the fastening point is then coupled in a weighted sense to the motion of the nodes in this region by a distributed coupling constraint. Several weighting options are available and are discussed in the next section.
To define the region of influence, Abaqus computes an internal radius of influence based on the geometric properties of the fastener, the characteristic length of the connected facets, and the type of weighting function used. The default radius of influence is always chosen to be the largest of the internally computed radius of influence, the physical fastener radius, and the distance of the projection point to the closest node. You can also specify the desired radius of influence. However, Abaqus overrides a user-specified radius of influence that is smaller than the computed default radius of influence. In any case each region of influence will contain a minimum of three nodes.
Input File Usage: *FASTENER, RADIUS OF INFLUENCE=distance blank line
Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: Adjust: Influence radius: Specify: distance
Defining the weighting method
The weighting methods available for the distributed coupling constraints created for a fastener interaction are the same as those available for the surface-based coupling constraints in Abaqus (see “Coupling constraints,” Section 35.3.2). Besides an area-based uniform weighting scheme, various weighting methods are provided that monotonically decrease with radial distance from the fastening point: linear, quadratic, and cubic polynomial weight distributions. By default, Abaqus uses the uniform weighting method. You can modify the default weighting distribution.
The default radius of influence calculated by Abaqus is larger for higher-order weighting methods since the resulting weights for nodes away from the fastening point contribute comparatively little to the motion of the fastening point. Hence, to ensure that there is a sufficient “smearing” effect, it becomes necessary to increase the number of nodes in the region of influence by increasing the size of the default radius of influence. In comparison, for a uniform weighting scheme, surface nodes away from the fastening point contribute significantly to the motion of the fastening point. For this case the default radius of influence chosen can be comparatively small, since even with a small number of nodes in the region of influence, the smearing effect is sufficiently strong. If fewer than three cloud nodes are found, increasing the radius of influence may help in forming the fastener by including more nodes in the cloud of coupling nodes.
| Input File Usage: | Use the following option to specify a uniform weight distribution:*FASTENER, WEIGHTING METHOD=UNIFORMblank lineUse the following option to specify a linear weight distribution:*FASTENER, WEIGHTING METHOD=LINEARblank lineUse the following option to specify a quadratic polynomial weight distribution:*FASTENER, WEIGHTING METHOD=QUADRATICblank lineUse the following option to specify a cubic polynomial weight distribution:*FASTENER, WEIGHTING METHOD=CUBICblank line |
| Abaqus/CAE Usage: | Interaction module: Special→Fasteners→Create: Point-based: Formulation: Weighting method: Uniform, Linear, Quadratic, or Cubic |
Defining the fastener orientation
Each fastener is formulated in a local coordinate system that rotates with the motion of the fastener. By default, Abaqus defines the local system by projecting the global coordinate system onto the surfaces that are being fastened according to the usual convention for surfaces in space (see “Conventions,” Section 1.2.2). Local directions specified in this manner are such that the local z-axis for each fastener is normal to the surface that is closest to the reference node for the fastener.
You can override the default local system by specifying a local coordinate system for the fastener interaction. Generally, the user-defined orientation should be such that the local z-axis of the orientation is approximately normal to the surfaces that are being connected and the local x- and y-axes are approximately tangent to the surfaces that are being connected. By default, Abaqus adjusts the user-defined orientation such that the local z-axis for each fastener is normal to the surface that is closest to the reference node for the fastener. In cases where you wish to define the local directions precisely, you can specify that Abaqus should not adjust them.
Fasteners support only rectangular, cylindrical, and spherical orientation definitions. Additional rotations defined as part of the orientation definition are ignored.
In geometrically nonlinear analysis steps the local directions rotate with the motion of the fastener reference node.
Local coordinate system when connector elements are used
If a connector element is used to model a fastener, the local coordinate system defined on the connector section, \mathbf { T } _ { c o n n e c t o r } , operates on the local coordinate system for the fastener, \mathbf { T } _ { f a s t e n e r } , to determine the final local coordinate system of the connector element, \mathbf { T } _ { c o n n e c t o r f i n a l } . In other words,
\mathbf {T} _ {c o n n e c t o r f i n a l} = \mathbf {T} _ {c o n n e c t o r} * \mathbf {T} _ {f a s t e n e r}.
In the above equations \mathbf { T } _ { c o n n e c t o r } and \mathbf { T } _ { f a s t e n e r } 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 } _ { c o n n e c t o r f i n a l } at all fastener locations unless you specify not to write the orientations to the database; in this case, only \mathbf { T } _ { c o n n e c t o r } 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 } _ { c o n n e c t o r f i n a l } 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 fastenened. 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,” Section 5.1.16 of the Abaqus Verification Guide, for an example of a compounded orientation.
Input File Usage: *FASTENER, ORIENTATION=orientation name, ADJUST ORIENTATION=NO blank line
Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: Adjust: Fastener CSYS: Edit: select local coordinate system, toggle off Adjust CSYS to make local Z-axis normal to closest surface
Clarifications regarding the computation of \mathbf { T } _ { \mathit { f a s t e n e r } }
A few clarifications regarding the default definition of \mathbf { T } _ { f a s t e n e r } are necessary for a precise understanding of the behavior when connector elements are used to model fasteners. The positioning point is always projected on the closest surface to be fastened. Therefore, the choice of coordinates of the reference node relative to the stack of surfaces to be fastened determines which surface is used to compute the local directions. Typically this choice does not matter much in realistic applications because the surfaces to be fastened are more or less parallel to each other in the fastener area.
The projection of the reference node on the closest surface generates a fastening point for the connector element. The local z-axis for each fastener ( \mathbf { T } _ { f a s t e n e r } ) is normal to the surface at this fastening point. The fastening point generated on the closest surface is by default the first fastening point and, therefore, the first connector node. The precise direction into which the local z-axis is pointing is chosen such that the dot product with the unit vector pointing from the first node of the connector to the second node of the connector is positive. As explained above, you can control the connectivity of the fastening points in the connectors by specifying unsorted surfaces. Therefore, you can control the precise direction the local z-axis is pointing along the surface normal by either selecting appropriate coordinates for the reference node and/or by using unsorted surfaces.
The two tangential directions in \mathbf { T } _ { f a s t e n e r } are computed by default according to the usual convention for surfaces in space (see “Conventions,” Section 1.2.2). The global X-axis is projected onto the closest surface at the location of the fastening point to determine the local x-axis in \mathbf { T } _ { f a s t e n e r } . If the global X-axis is within 0.1 degrees of being normal to the surface, the local x-axis in \mathbf { T } _ { f a s t e n e r } is the projection of the global Z-axis on the closest surface. The local y-axis in \mathbf { T } _ { f a s t e n e r } is then at right angles to the local x-axis and z-axis so that the three local axes form a right-handed set.
In the rare cases when the default definition of \mathbf { T } _ { f a s t e n e r } does not suit your application, you can always specify the orientation directly. In this case the following occurs:
- Abaqus first recomputes the local z-axis to align with the facet normal, with the precise direction chosen such that its dot product with the unit vector pointing from the first node of the connector to the second node of the connector is positive.
- Abaqus checks the local x- and y-axes you specified to determine which of these two is closest to the plane of the current facet.
- If the local x-axis is closest, Abaqus recomputes the local y-axis as the normalized cross product of the recomputed z-axis and the specified x-axis. Then Abaqus computes the new local x-axis as the normalized cross product of the recomputed y-axis and the recomputed z-axis.
- If the local y-axis is closest, Abaqus recomputes the local x-axis as the normalized cross product of the specified y-axis and the recomputed z-axis. Then Abaqus computes the new local y-axis as the normalized cross product of the recomputed z-axis and the recomputed x-axis.
Common modeling practices
In most applications the default choice for \mathbf { T } _ { f a s t e n e r } combined with a choice of global system for \mathbf { T } _ { c o n n e c t o r } at both connector nodes would result in a \mathbf { T } _ { c o n n e c t o r f i n a l } that is most suitable. The connection type that you choose depends on several modeling considerations, but very often the
BUSHING connection type offers the best choice. To simplify the discussion, consider that only two surfaces are being fastened, a very common situation as illustrated in the spot weld example in “Connector functions for coupled behavior,” Section 31.2.4. For this common choice, has the local z-axis normal to the closest surface and pointing from the first fastening point (first connector node) toward the second fastening point (second connector node). This choice ensures that for a fastener subjected to a tension load (fastened plates pulled apart) a positive force always develops in the connector along the local z-axis (CTF3) regardless of the choice of coordinates for the positioning point and/or use of unsorted surfaces. Conversely, if a compression load is applied (fastened plates pressed against each other), a negative force develops in the connector.
In most cases, the behavior in the tangential plane defined by the local x- and local y-axes is isotropic; therefore, the precise orientation of these two axes is of less interest to you. The spot weld example in “Connector functions for coupled behavior,” Section 31.2.4, illustrates such a typical case where the (isotropic) magnitude of two in-plane forces ( f _ { 1 } , f _ { 2 } ) and of the two moments ( m _ { 1 } , m _ { 2 } ) are used in the kinetic behavior of the connector element.
If you need to specify anisotropic behavior in the tangential plane, you need to understand precisely how the directions in \mathbf { T } _ { f a s t e n e r } are defined. As explained above, the choice of coordinates for the positioning point relative to the stack of surfaces to be fastened and/or use of unsorted surfaces determines the precise direction of the default local axes. In most cases you have two common modeling choices. In the first case you can specify the coordinates of the positioning points to be exactly on or very close to the surface onto which the first fastening points (connector nodes) are to be placed and use the default sorted surfaces. In this case you do not need to specify the surfaces to be fastened individually. However, in many practical situations imprecise geometry for the surfaces to be fastened and/or inexact coordinates of the fastener reference nodes make the consistent placement of the reference nodes in the vicinity of one particular surface very hard to accomplish. The second modeling technique consists of using sorted surfaces. The exact location of the reference node with respect to the surface stack to be fastened is not that important because the first fastening point is always on the first specified surface. In this case you do have to specify two or more individual surfaces to be fastened. In the rare cases when neither of these modeling techniques suits your application, you can specify the fastener orientation directly to match your needs exactly.
Defining the surface coupling method
There are two methods available to couple the motion of each fastening point to the motion of the associated coupling nodes on the fastened surfaces: the continuum coupling method and the structural coupling method. The continuum coupling method is used by default.
In many cases when the pair of fastened surfaces are close to each other, unrealistic contact interactions may occur between the two surfaces if the continuum coupling method is used. This is particularly the case in shell bending applications. Moreover, in many situations the continuum coupling method can yield an overly stiff response if the two surfaces are pried apart, especially when the fastener radius is small. The structural coupling method can be used to alleviate these issues.
Continuum coupling method
The default continuum coupling method couples the translation and rotation of each fastening point to the average translation of the group of coupling nodes on each of the fastened surfaces. The constraint
distributes the forces and moments at the fastening point as a coupling node-force distribution only. The force distribution is equivalent to the classic bolt pattern force distribution when the weight factors are interpreted as bolt cross-section areas. For each pair of fastening point and group of coupling nodes, the constraint enforces a rigid beam connection between the fastening point and a point located at the weighted center of position of the coupling nodes. The formulation is discussed in detail in “Distributing coupling constraints,” Section 3.9.8 of the Abaqus Theory Guide.
Input File Usage: *FASTENER, COUPLING=CONTINUUM
Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: Formulation: Coupling type: Continuum distributing
Structural coupling method
The structural coupling method couples the translation and rotation of each fastening point to the translation and the rotation motion of the group of coupling nodes on each of the fastened surfaces. The constraint distributes forces and moments at the fastening point as coupling nodes forces and moments. For this coupling method to be active, all rotation degrees of freedom at all coupling nodes must be active (as would be the case when shells are fastened together) and all degrees of freedom must be constrained (which is the default; see “Defining fastener properties” below).
With respect to translations, for each pair of fastening point and group of coupling nodes, the constraint enforces a rigid beam connection between the fastening point and a moving point that remains at all times in the vicinity of the fastened surface. The location of this moving point is determined by the current curvature of the surface, the current location of the weighted center of position of the coupling nodes, and the fastener projection direction. This choice avoids unrealistic contact interactions between the fastened surfaces when the surfaces are close to each other (typically the case).
With respect to rotations, for each pair of fastening point and group of coupling nodes, the constraint is different along different local directions. Along the projection direction (the twist direction), the constraint is identical to the one enforced via the continuum coupling method (see “Distributing coupling constraints,” Section 3.9.8 of the Abaqus Theory Guide). By contrast, the rotational constraint in the plane perpendicular to the projection direction relates the in-plane fastening point rotations to the in-plane rotations of the coupling nodes in the immediate vicinity of the fastening point. This choice provides a more realistic response when the fastened surfaces are pried apart.
Input File Usage: *FASTENER, COUPLING=STRUCTURAL
Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: Formulation: Coupling type: Structural distributing
Defining fastener properties
Each fastener interaction definition must refer to a property, which defines the geometric section properties of the fastener.
Input File Usage: Use both of the following options:
*FASTENER, PROPERTY=fastener property name
*FASTENER PROPERTY, NAME=fastener property name
Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: Property
Geometric section quantities
Fasteners are assumed to have a circular projection onto the connected surfaces. You are required to specify the radius of the fastener.
Input File Usage: *FASTENER PROPERTY r
Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: Property: Physical radius: r
Releasing degrees of freedom on fasteners using connector elements
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.
Releasing degrees of freedom on fasteners using BEAM MPCs
For fasteners modeled with BEAM MPCs, 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.
Input File Usage: *FASTENER PROPERTY
section properties
first dof, last dof
For example, if the default local coordinate system is used, the following property definition would release the relative rotation constraint of the connected parts about the surface normal:
*FASTENER PROPERTY
section properties
1, 5
The above property definition might be used to approximate a riveted connection.
Abaqus/CAE Usage:
Abaqus/CAE always constrains all translational degrees of freedom in a fastener. Use the following input to remove constraints on the rotational degrees of freedom:
Interaction module: Special→Fasteners→Create: Point-based:
Formulation: toggle off UR1, UR2, or UR3
Overconstraints in fasteners modeled with BEAM MPCs
There are several instances in which a model with fasteners modeled with BEAM MPCs might be overconstrained. Described below are two potential overconstraints that Abaqus automatically attempts to detect and resolve during solver input file processing.
Fasteners and rigid bodies
Fasteners can be used to connect both deformable and rigid element-based surfaces. However, if the fasteners are modeled with BEAM MPCs, 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 35.3.4–1 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 BEAM MPC.
In another example, suppose all three surfaces in Figure 35.3.4–1 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 BEAM MPCs. 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,” Section 35.6.1).
Overlapping fasteners
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.
Output
If fasteners are modeled using connector elements, connector element output variables can be used to request output for fasteners (see “Connector elements,” Section 31.1.2). No fastener output is available if the fasteners are modeled using BEAM MPCs.