김경종
14 KiB
start of the analysis—e.g., either open or overclosed—will remain unconstrained for the duration of the simulation; they will never interact with the master surface. In mechanical simulations an unconstrained slave node can penetrate the master surface freely. In a thermal, electrical, or pore pressure simulation an unconstrained slave node will not exchange heat, electrical current, or pore fluid with the master surface.
To avoid such unconstrained nodes in tied contact pairs, use the capability for adjusting the surfaces of a contact pair described in “Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs,” Section 36.3.5. This capability moves slave nodes onto the master surface before Abaqus/Standard checks for the initial contact state. It is intended only for nodes that are close to the master surface and is not intended to correct large errors in the mesh geometry.
Checking that slave nodes are constrained
Abaqus/Standard prints a table in the data (.dat) file identifying the predominant slave node and other nodes involved in each constraint. If Abaqus/Standard cannot form a constraint for a given slave node acting as a predominant slave node, either because it is not in contact with the master surface or it cannot “see” the master surface, it will issue a warning message in the data file. For an explanation of when a slave node would not “see” a master surface and how to correct this problem, see “Contact formulations in Abaqus/Standard,” Section 38.1.1. When creating a model with tied contact, it is important to use this information provided by Abaqus/Standard to identify any unconstrained nodes and to make any necessary modifications to the model to constrain them.
36.3.8 EXTENDING MASTER SURFACES AND SLIDE LINES
Product: Abaqus/Standard
References
• “Defining contact pairs in Abaqus/Standard,” Section 36.3.1
• “Common difficulties associated with contact modeling in Abaqus/Standard,” Section 39.1.2
• *CONTACT PAIR
• *SLIDE LINE
Overview
Extending the master surface or a slide line:
• can prevent nodes from “falling off” or getting trapped behind the master surface (or slide line) in finite-sliding problems;
• allows the slave node to find a master surface when the slave node has no intersection with the master surface at the start of the analysis in small- and infinitesimal-sliding problems;
• can avoid numerical roundoff difficulties associated with contact modeling;
• should not be used in lieu of proper contact modeling techniques;
• should not be used to reduce the number of underlying elements of a contact surface;
• applies only at the perimeter of a master surface in three dimensions and at the ends of a master surface in two dimensions; and
• applies only to contact pairs that use a node-to-surface discretization.
Extending the master surface for small-sliding, node-to-surface contact
If a slave node cannot find an intersection with the master surface at the start of the analysis, it will be free to penetrate the master surface because no local tangent plane will be formed. This type of problem, which typically occurs for node-to-surface contact when the slave node is aligned with the end or perimeter of the master surface (which does not wrap around the corner of the rectangular body), is illustrated in Figure 36.3.8–1 and may be caused by numerical roundoff errors when a preprocessor is used to generate the nodal coordinates. There are no extensions to master faces in the interior of a surface. If the master surface in Figure 36.3.8–1 were defined such that it wrapped around the corner of the body, no extensions to the master surface would be required because the slave node would project onto the master surface using the projection method discussed in “Using the small-sliding tracking approach” in “Contact formulations in Abaqus/Standard,” Section 38.1.1. Cases such as that shown in Figure 36.3.8–1 are not problematic for the small-sliding, surface-to-surface formulation because the constraint formulation considers the region of the slave surface near a slave node.
text_image
Slave Node n Master Surface No intersection (e = 0)
text_image
Slave Node n Master Surface Intersection found (e > 0)
Figure 36.3.8–1 Slave node fails to find an intersection with the master surface for small-sliding, node-to-surface contact if e=0.
For node-to-surface contact you can specify the size of the extension zone, e, as a fraction of the end segment or facet edge length (see Figure 36.3.8–2). If e is set to zero, Abaqus will not extend the ends. The value given must lie between 0.0 and 0.2. The default value is 0.1 for node-to-surface contact; surface extensions are not available for surface-to-surface contact.
Input File Usage: *CONTACT PAIR, SMALL SLIDING, EXTENSION ZONE=e
Extending the master surface or slide line in finite-sliding, node-to-surface contact
To prevent slave nodes from “falling off” or getting trapped behind a master surface, an open surface or slide line can be extended beyond its perimeter edges (in three dimensions) or end nodes (in two dimensions) for finite-sliding, node-to-surface contact.
You can specify the size of the extension zone, e, as a fraction of the end segment or facet edge length (see Figure 36.3.8–2). The geometry in the extension zone is extrapolated from the end segment or facet edge. If e is set to zero, Abaqus/Standard will not extend the ends. The value given must lie between 0.0 and 0.2. The default value is 0.1 for node-to-surface contact. Surface extensions are not available for surface-to-surface contact; for finite-sliding, surface-to-surface contact, constraints are located within slave faces, and “falling off” will not occur until nearly the entire slave facet slides off the master surface. Extensions for finite-sliding, node-to-surface contact should be considered only if other modeling techniques to prevent “falling off” are not feasible and when the slave node is expected to travel in the extended zone for a short period of the solution phase or during nonconverged iterations.
Input File Usage: Use either of the following options:
*CONTACT PAIR, EXTENSION ZONE=e*SLIDE LINE, ELSET=element_set_name, EXTENSION ZONE=e
Figure 36.3.8–2 Definition of size of extension zone.
36.3.9 CONTACT MODELING IF SUBSTRUCTURES ARE PRESENT
Product: Abaqus/Standard
References
• “Element-based surface definition,” Section 2.3.2
• “Node-based surface definition,” Section 2.3.3
• “Using substructures,” Section 10.1.1
• “Membrane elements,” Section 29.1.1
• “Surface elements,” Section 32.7.1
• “Contact interaction analysis: overview,” Section 36.1.1
• “Defining contact pairs in Abaqus/Standard,” Section 36.3.1
Overview
Contact in Abaqus/Standard involving substructures:
• is not part of the substructure definition;
• requires retaining nodes on the exterior of the substructure;
• requires the definition of a contact surface on the retained nodes; and
• can be between the exterior of one substructure and another surface, the exterior of one substructure and the exterior of another substructure, and the exterior of one substructure and itself.
Defining the contact surface of a substructure
Since a substructure consists only of a group of retained nodal degrees of freedom, it has no surface geometry upon which Abaqus/Standard can define a contact surface. One of the following methods must be used to define the surface geometry of the substructure:
• mesh the exterior of the substructure with surface elements,
• mesh the exterior of the substructure with structural elements,
• use a node-based surface, or
• use contact elements.
Meshing the surface of the substructure with surface or structural elements provides the most flexibility in defining the contact conditions; the surface can be used as either a master or slave surface in the simulation. Using a node-based surface is probably the easiest method to use, but the limitations inherent to node-based surfaces (such as the inability to act as a master surface, the need to define nodal contact areas for exact contact stress recovery, and the lack of visualization of contact stresses) may limit the usefulness of this approach. Contact elements can be a useful method if the model uses matched meshes.
Meshing the surface of the substructure with surface elements
The surface geometry of the body being modeled with a substructure can be designated by defining elements on the retained surface nodes of the substructure. The elements can be used to create an element-based surface (see “Element-based surface definition,” Section 2.3.2), which can then be used as part of a contact pair.
Whenever possible, it is recommended that you use surface elements to mesh the exterior of a substructure. Surface elements will accurately define the surface geometry of the substructure without introducing any additional stiffness to the model; the stiffness of the underlying body is built into the substructure. See “Surface elements,” Section 32.7.1, for more information about surface elements.
Figure 36.3.9–1 shows a simulation where both of the contacting bodies have been modeled with substructures. The nodes retained in the model are indicated in the figure. If this were a three-dimensional model, general surface elements would be used to reconstruct the appropriate surface geometries of the original mesh.
text_image
(a) critical model ⇒ (b) nodes retained for contact resolution
Figure 36.3.9–1 Substructuring in a contact simulation.
Limitations of surface elements
Surface elements cannot be used to overlay substructures in planar models.
Surface elements also cannot be used to overlay a substructure that consists of second-order, three-dimensional elements with midface nodes (C3D27(R)(H) or C3D15V(H)). Surface elements with midface nodes are not currently available in Abaqus/Standard, and the 8-node surface element (SFM3D8) is not well suited for contact modeling.
Meshing the surface of the substructure with structural elements
Although surface elements are generally preferable for use in substructure contact situations, you can also use structural elements to define the surface geometry of a substructure. You can use membrane elements in three-dimensional models and axisymmetric models, and trusses in planar models. Define the elements to have very small thickness or area and define their material property to have a very small elastic modulus so that their contribution to the stiffness of the model is negligible.
If the model in Figure 36.3.9–1 were a planar model, truss elements would be used to connect the nodes and define the surface geometry. The truss elements would have a very small cross-sectional area and refer to a material property with very low stiffness so that they do not add any significant stiffness to the underlying bodies.
Limitations of structural elements
Membrane elements cannot be used to overlay a substructure that consists of second-order, three-dimensional brick elements of type C3D20(R)(H) if the substructure will be used as a slave surface. Normally, Abaqus/Standard automatically converts C3D20(R)(H) brick elements to elements with midface nodes C3D27(R)(H) because this class of elements performs better in contact simulations. Abaqus/Standard also converts any second-order, three-dimensional structural element that does not have a midface node when it is used in a slave surface (see “Three-dimensional surfaces with second-order faces and a node-to-surface formulation” in “Common difficulties associated with contact modeling in Abaqus/Standard,” Section 39.1.2, for details). Therefore, if second-order membrane elements (type M3D8) are used to reconstruct the surface topology of a substructure consisting of C3D20 elements, Abaqus/Standard will convert them to M3D9 elements when the surface is used as a slave surface. The midface nodes that are generated automatically will not correspond to any retained nodes and, thus, will have zero stiffness. The lack of stiffness at these nodes will cause numerical problems during the analysis. Membrane elements can be used if elements of type C3D27(R)(H) have been used on the surface of the substructure.
Using a node-based surface to define the substructure’s surface
If the retained nodes of the substructures are associated with the slave surface of a contact pair, the retained nodes can be included in a node-based surface (see “Node-based surface definition,” Section 2.3.3). In this case it is not necessary to overlay the surface of the substructure with elements.
Using contact elements to define the substructure’s surface
GAP elements (“Gap contact elements,” Section 40.2.1) can be used to define the contact interactions in the model. These elements require that matching nodes be present on the opposite sides of the contact surfaces and allow only for small relative sliding between the surfaces. This latter assumption is usually consistent with the assumption of linear behavior that is built into a substructure.