김경종
23 KiB
natural_image
Two gray geometric shapes composed of triangles and diagonal lines, arranged in a 2x2 grid (no text or symbols)
Figure 36.3.1–6 Example of a 3D surface with two faces sharing a single node.
• Surfaces with T-intersections: In some cases a contact surface cannot have more than two surface faces sharing a common master node in two dimensions or a common master edge in three dimensions. For example, Figure 36.3.1–7 shows examples of surfaces with T-intersections, in which three faces share a common node in two dimensions or a common edge in three dimensions. While more than two surface faces can share a common slave node in two dimensions or a common edge in three dimensions for node-to-surface formulations, the slave faces must be single-sided, which precludes the most common T-intersection cases for node-to-surface formulations.
natural_image
Simple geometric diagram with a vertical line and horizontal lines forming a Y-shape (no text or symbols)
T-intersection in 2D
natural_image
Geometric pattern composed of intersecting triangles and parallelograms (no text or symbols)
T-intersection in 3D
Figure 36.3.1–7 Examples of surfaces with T-intersections.
Analytical rigid surfaces
Analytical rigid surfaces are often effective for efficiently modeling curved, rigid geometries, as discussed in “Analytical rigid surface definition,” Section 2.3.4. For rare cases in which a very large number (thousands) of segments would be necessary to define an analytical rigid surface, better performance can be achieved with an element-based rigid surface (see “Element-based surface definition,” Section 2.3.2).
Three-dimensional beam and truss surfaces
Abaqus/Standard cannot use three-dimensional beams or trusses to form a master surface because the elements do not have enough information to create unique surface normals. However, these elements can
be used to define a slave surface. Two-dimensional beams and trusses can be used to form both master and slave surfaces.
Edge-based surfaces
Edge-based surfaces (“Element-based surface definition,” Section 2.3.2) on three-dimensional shell elements cannot be used in a contact analysis in Abaqus/Standard.
Limitations of node-based surfaces
Use node-based surfaces with caution when the contact property definition includes user-defined softened contact properties or thermal or electrical interactions because the contact constitutive behavior (which relies on accurate calculation of contact pressure, heat flux, or electric current) will not be enforced correctly unless the precise surface area is associated with each node. For details, see “Contact pressureoverclosure relationships,” Section 37.1.2; “Thermal contact properties,” Section 37.2.1; or “Electrical contact properties,” Section 37.3.1.
Removing and reactivating contact pairs
You can temporarily remove contact pairs from a simulation, which may result in significant computational savings by eliminating unnecessary contact searches and updates of surface orientations during the simulation. Removal and reactivation of contact pairs is commonly used in complicated forming processes where multiple tools need to interact with the workpiece at different stages in the analysis.
You cannot remove tied contact pairs from a simulation (see “Defining tied contact in Abaqus/Standard,” Section 36.3.7).
Removing contact pairs
Removal of contact pairs is a useful technique for uncoupling components of an assembly until they should be brought together (such as tooling in manufacturing process simulations). Significant computational expense may be saved by removing a contact pair and introducing it at the proper time, thus eliminating the need to monitor the contact conditions except when they are relevant.
Input File Usage: *MODEL CHANGE, TYPE=CONTACT PAIR, REMOVE
slave_surface, master_surface
Repeat the data line as needed.
Abaqus/CAE Usage: Use one of the following options:
Interaction module: Create Interaction: surface-to-surface contact or self-contact interaction editor: toggle off Active in this step
Interaction module: interaction manager: select interaction, Deactivate
Removal of contact forces associated with closed contact pairs
If the surfaces are in contact when a contact pair is removed, Abaqus/Standard stores the corresponding contact forces (or heat fluxes if thermal interactions are present, or electrical currents if it is a
coupled-thermal electrical analysis) for every node on each surface. Abaqus/Standard automatically ramps these forces (or heat fluxes or electrical currents) linearly down to zero magnitude during the removal step. Abaqus/Standard always removes the contact constraints for mechanical surface interactions instantaneously.
Care must be taken in removing contact pairs in transient procedures. In transient heat transfer, fully coupled temperature-displacement, or fully coupled thermal-electrical-structural analysis if the fluxes are high and the step is long, this ramping down may have the effect of cooling down or heating up the rest of the body. In dynamic analysis if the forces are high and the step is long, kinetic energy can be imparted to the remaining portion of the model. This problem can be avoided by removing the contact pairs in a very short transient step prior to the rest of the analysis. This step can be done in a single increment.
Using an allowable contact interference to deactivate contact pairs
A contact pair with mechanical contact interactions can be deactivated during an analysis by assigning a very large allowable contact interference to the contact pairs (see “Modeling contact interference fits in Abaqus/Standard,” Section 36.3.4). This method has the disadvantage of not reducing the computational cost of the analysis because the contact algorithm will still calculate the contact conditions for the contact pair in each increment.
Reactivating contact pairs
All contact pairs that will be used in a simulation must be created at the start of the analysis; they cannot be created once the simulation has begun. However, contact pairs can be created, removed at the start of the analysis in the first step, and then reactivated at a later point during the simulation.
In Abaqus/CAE you can create contact pairs in any step. If a contact pair is created in a step other than the initial step, Abaqus/CAE automatically deactivates the contact pair in the initial step and reactivates it in the step in which you created it.
Input File Usage: *MODEL CHANGE, TYPE=CONTACT PAIR, ADD
slave_surface, master_surface
Repeat the data line as needed.
Abaqus/CAE Usage: Interaction module: Create Interaction: surface-to-surface contact or
self-contact interaction editor: toggle on Active in this step
Reactivating overclosed contact pairs
When a contact pair is reactivated, the contact constraint becomes active immediately. In mechanical simulations it is possible for the surfaces of a contact pair to move such that they become overclosed while the contact pair is inactive. If this overclosure is too severe when the contact pair is reactivated, Abaqus/Standard may encounter convergence problems as it tries to enforce the suddenly activated contact constraint. To avoid such problems, you can specify a permissible interference value, v, for the contact pair that is larger than the overclosure for the contact pair. Abaqus/Standard will ramp v down to zero during the step. For details on specifying allowable interferences, see “Modeling contact interference fits in Abaqus/Standard,” Section 36.3.4.
Output
Output variables associated with the interaction of contact pairs fall into two categories: nodal variables (sometimes called constraint variables) and whole surface variables. In addition, Abaqus outputs an array of diagnostic information associated with contact interactions, as discussed in “Contact diagnostics in an Abaqus/Standard analysis,” Section 39.1.1.
For more detailed discussions of variables associated with thermal, electrical, and pore fluid analyses, see the sections on the related contact properties in Chapter 37, “Contact Property Models.”
Nodal contact variables
Nodal contact variables can be contoured on contact surfaces in the Visualization module of Abaqus/CAE. Nodal contact variables include contact pressure and force, frictional shear stress and force, relative tangential motion (slip) of the surfaces during contact, clearance between surfaces, heat or fluid flux per unit area, fluid pressure, and electrical current per unit area. Many of the nodal contact variables written to the output database (.odb) file are often available for all contact nodes, regardless of whether they act as slave or master nodes. Other nodal contact variables are available only at nodes acting as slave nodes. Most contact output to the data (.dat) file, results (.fil) file, and the utility subroutine GETVRMAVGATNODE is associated with individual constraints. For contact output to the output database (.odb) file, some filtering is applied to reduce contact output noise.
The contact pressure distribution is of key interest in many Abaqus analyses. You can view the contact pressure on all contact surfaces except for analytical rigid surfaces and discrete rigid surfaces based on rigid-type elements (the latter restriction does not apply to general contact). You can view a contour plot of the contact pressure error indicator next to a contour plot of the contact pressure to gain perspective on local accuracy of the contact pressure solution in regions where the contact pressure solution is of interest (see “Selection of error indicators influencing adaptive remeshing,” Section 12.3.2, for further discussion of error indicator output).
In some cases you may observe the contact pressure extending beyond the actual contact zone due to the following factors:
• The contour plots are constructed by interpolating nodal values, which can cause nonzero values to appear within portions of facets outside of the contact region. For example, this effect is often noticeable at corners, such as when two same-sized, aligned blocks are in contact—if the contact surfaces wrap around the corners, the contact pressure contours will extend slightly around the corners.
To minimize contact stress noise within a region of active contact, Abaqus/Standard computes nodal contact stresses as weighted averages of values associated with active contact constraints in which a node participates. Some filtering is applied to reduce the contact stress values reported for nodes on the fringe of the active contact region (that only weakly participate in contact constraints), but this filtering is not “perfect,” which can result in the contact zone size appearing somewhat exaggerated. Similarly, contact status output will also be affected at nodes that lie on the fringe of the active contact region. In such cases, the contact status may be reported as closed at nodes in the exaggerated region even though it is open.
Due to these factors, trying to infer the contact force distribution from the contact stress distribution can be somewhat misleading. Instead, you can request nodal contact force output, which accurately represents the contact force distribution present in the analysis.
Whole surface variables
Whole surface variables are attributes of an entire slave surface. Available as history output, these variables record the total force and moment due to contact pressure and frictional stress, the center of pressure and frictional stress (defined as the point closest to the centroid of the surface that lies on the line of action of the resultant force for which the resultant moment is minimal), and the total contact area (defined as the sum of all the facets where there is contact force). The last letter of each variable name (except the variable CAREA) denotes which contact force distribution on the surface is used to calculate the resultant:
N Normal contact forces are used to derive the resultant quantity.
S Shear contact forces are used to derive the resultant quantity.
T The sum of the normal and shear contact forces is used to derive the resultant quantity.
For example, CFN is the total force due to contact pressure, CFS is the total force due to frictional stress, and CFT is the total force due to both contact pressure and frictional stress.
Each total moment output variable will not necessarily equal the cross product of the respective center of force vector and resultant force vector. Forces acting on two different nodes of a surface may have components acting in opposite directions, such that these nodal force components generate a net moment but not a net force; therefore, the total moment may not arise entirely from the resultant force. The center of force output variables tend to be most meaningful when the surface nodal forces act in approximately the same direction.
Requesting output
Certain contact variables must be requested as a group. For example, to output the clearance between surfaces (COPEN), you must request the variable CDISP (contact displacements). CDISP outputs both COPEN and CSLIP (tangential motion of the surfaces during contact). A complete listing of available contact pair variables and identifiers is given in “Abaqus/Standard output variable identifiers,” Section 4.2.1.
Output requests can be limited to individual contact pairs or portions of a slave surface. You can:
• request output associated with a given contact pair;
• request output associated with a given slave surface, including contributions from all of the contact pairs to which the slave surface belongs; and
• limit the output by specifying a node set containing a subset of the nodes on the slave surface.
Instructions on forming these output requests are available in the following sections:
• To request output to the data (.dat) file, see “Surface output from Abaqus/Standard” in “Output to the data and results files,” Section 4.1.2.
• To request output to the output database (.odb) file, see “Surface output in Abaqus/Standard and Abaqus/Explicit” in “Output to the output database,” Section 4.1.3.
Differences for small-sliding and finite-sliding contact
For small-sliding contact problems the contact area is calculated in the input file preprocessor from the undeformed shape of the model; thus, it does not change throughout the analysis, and contact pressures for small-sliding contact are calculated according to this invariant contact area. This behavior is different from that in finite-sliding contact problems, where the contact area and contact pressures are calculated according to the deformed shape of the model.
Output of tangential results
Abaqus reports the values of tangential variables (frictional shear stress, viscous shear stress, and relative tangential motion) with respect to the local tangent directions defined on the surfaces. The local tangent directions CTANDIR1 and CTANDIR2 can be output by requesting the generic output variable CTANDIR. The definition of local tangent directions is explained in “Local tangent directions on a surface” in “Contact formulations in Abaqus/Standard,” Section 38.1.1. These directions do not always correspond to the global coordinate system, and they rotate with the contact pair in a geometrically nonlinear analysis.
Abaqus/Standard calculates tangential results at each constraint point by taking the scalar product of the variable’s vector and a local tangent direction, \mathbf { t } _ { 1 } or \mathbf { t } _ { 2 } , associated with the constraint point. The number at the end of a variable’s name indicates whether the variable corresponds to the first or second local tangent direction. For example, CSHEAR1 is the frictional shear stress component in the first local tangent direction, while CSHEAR2 is the frictional shear stress component in the second local tangent direction.
Definition of accumulated incremental relative motion (slip)
Abaqus/Standard defines the incremental relative motion (also known as slip) as the scalar product of the incremental relative nodal displacement vector and a local tangent direction. The incremental relative nodal displacement vector measures the motion of a slave node relative to the motion of the master surface. The incremental slip is accumulated only when the slave node is contacting the master surface. The sums of all such incremental slips during the analysis are reported as CSLIP1 and CSLIP2. Details about the calculation of this quantity can be found in “Small-sliding interaction between bodies,” Section 5.1.1 of the Abaqus Theory Guide; “Finite-sliding interaction between deformable bodies,” Section 5.1.2 of the Abaqus Theory Guide; and “Finite-sliding interaction between a deformable and a rigid body,” Section 5.1.3 of the Abaqus Theory Guide.
Extending the range for which contact opening output is provided for gaps
To reduce computational costs, detailed computations to monitor potential points of interaction are avoided by default where surfaces are separated by a distance greater than the minimum gap distance at which contact forces (or thermal fluxes, etc.) may be transmitted. Therefore, contact opening (COPEN) output is typically not provided for finite-sliding contact where surfaces are opened by more than a small amount compared to surface facet dimensions. You can extend the range in which Abaqus/Standard provides contact opening output; COPEN will be provided up to gap distances equal to a specified
“tracking thickness.” Using this control may increase computational cost due to extra contact tracking computations, especially if you specify a large tracking thickness value.
Input File Usage: *SURFACE INTERACTION, TRACKING THICKNESS=value
Abaqus/CAE Usage: You cannot adjust the default tracking thickness in Abaqus/CAE.
Output for axisymmetric models
In an axisymmetric analysis the total forces and moments transmitted between the contacting bodies as a result of contact pressure and frictional stress are computed in the same manner as in a two-dimensional analysis. Therefore, the component of the total forces along the r-axis is nonzero, and the components of the total moments include contributions from the total forces along the r-axis.
Obtaining the “maximum torque” that can be transmitted about the z-axis in an axisymmetric analysis
When modeling surface-based contact with axisymmetric elements (element types CAX and CGAX), Abaqus/Standard can calculate the maximum torque (output variable CTRQ) that can be transmitted about the z-axis. This capability is often of interest when modeling threaded connectors (see “Axisymmetric analysis of a threaded connection,” Section 1.1.20 of the Abaqus Example Problems Guide). The maximum torque, T, is defined as
T = \iint r ^ {2} p d s d \theta ,
where p is the pressure transmitted across the interface, r is the radius to a point on the interface, and s is the current distance along the interface in the r–z plane. This definition of “torque” effectively assumes a friction coefficient of unity.
Whole model contact-related energy variables
For contact pairs, the same contact-related energy variables are available in Abaqus/Standard as for general contact, as described in “Whole model contact-related energy variables” in “Defining general contact interactions in Abaqus/Standard,” Section 36.2.1.
36.3.2 ASSIGNING SURFACE PROPERTIES FOR CONTACT PAIRS IN Abaqus/Standard
Products: Abaqus/Standard Abaqus/CAE
References
• “Defining contact pairs in Abaqus/Standard,” Section 36.3.1
• *CONTACT PAIR
• “Defining surface-to-surface contact,” Section 15.13.7 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
• “Defining self-contact,” Section 15.13.8 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
Overview
This section describes how to modify the properties associated with surfaces in a contact pair definition.
Accounting for shell and membrane thickness
All of the contact formulations except the finite-sliding, node-to-surface formulation account for initial shell and membrane thicknesses for element-based surfaces by default. The finite-sliding, node-to-surface formulation will not account for surface thickness. Node-based surfaces have no thickness, regardless of which element types are connected to the surface nodes. Accounting for element thicknesses in contact calculations is generally desirable, but you can avoid having thickness considered if it is not desired.
Input File Usage: *CONTACT PAIR, NO THICKNESS
Abaqus/CAE Usage: Interaction module: interaction editor: Sliding formulation: Small sliding or Finite sliding, Discretization method: Surface to surface or Node to surface, toggle on Exclude shell/membrane element thickness
Example
Consider the case of a shell pinched between two rigid surfaces, as shown in Figure 36.3.2–1.
In this example contact pairs using the small-sliding, node-to-surface formulation are defined between the top surface of the shell and the top rigid surface and between the bottom surface of the shell and the bottom rigid surface. Although the shell surfaces are defined at the shell reference location, the contact interactions account for the thickness of the shell and are offset from the reference surface. The penalty constraint enforcement method (see “Contact pressure-overclosure relationships,” Section 37.1.2) is used to avoid overconstraining slave nodes. The following input is used:
* SURFACE, NAME=TOP_RIG_SURF
TOP_RIG_ELS,
* SURFACE, NAME=SHELL_TOP_SURF
text_image
deformable shell rigid solids shell reference surface shell thickness contact interactions
Figure 36.3.2–1 Shell pinched between two rigid bodies.
SHELL_ELS, SPOS
* SURFACE, NAME=SHELL_BOT_SURF
SHELL_ELS, SNEG
* SURFACE, NAME=BOT_RIG_SURF
BOT_RIG_ELS,
* CONTACT PAIR, INTERACTION=INTER_AL, SMALL SLIDING
SHELL_TOP_SURF, TOP_RIG_SURF
SHELL_BOT_SURF, BOT_RIG_SURF
* SURFACE INTERACTION, NAME=INTER_AL
* SURFACE BEHAVIOR, PENALTY
Specifying surface geometry corrections
With the finite element method, curved geometric surfaces are naturally approximated as a faceted group of connected element faces. The use of a faceted surface geometry rather than the true surface geometry can significantly contribute to contact stress inaccuracy in contact pairs, especially when the magnitude of the differences between the faceted and true surface is not small with respect to the deformation of the components in contact. Methods for overcoming convergence and accuracy difficulties associated with faceted surfaces in contact interactions are discussed in “Contact formulations in Abaqus/Standard,” Section 38.1.1, and “Smoothing contact surfaces in Abaqus/Standard,” Section 38.1.3.