김경종
25 KiB
Nonmatched surface meshes with second-order heat transfer elements
Inaccurate local results may occur if second-order heat transfer elements are used to model a thermal interface and the meshes do not match across the surfaces. The worst results will be obtained when the midside node of an element on one surface is closest to the corner node of an element on the other surface. If a nonmatching mesh must be used in the model, use first-order elements or use a more refined mesh.
Three-dimensional surfaces with second-order faces and a node-to-surface formulation
Second-order elements not only provide higher accuracy but also capture stress concentrations more effectively and are better for modeling geometric features than first-order elements. Surfaces based on second-order element types work well with the surface-to-surface contact formulation but, in some cases, do not work well with the node-to-surface formulation (see “Contact formulations in Abaqus/Standard,” Section 38.1.1, for a discussion of these contact formulations).
Some second-order element types are not well-suited for underlying the slave surface with the combination of a node-to-surface contact formulation and strict enforcement of “hard” contact conditions, because of the distribution of equivalent nodal forces when a pressure acts on the face of the element. As shown in Figure 39.1.2–6, a constant pressure applied to the face of a second-order element without a midface node produces forces at the corner nodes acting in the opposite sense of the pressure.
text_image
q = \frac{1}{3} pA r = \frac{1}{12} pA
Figure 39.1.2–6 Equivalent nodal loads produced by a constant pressure on the second-order element face in “hard” contact simulations.
Abaqus/Standard bases important decisions for the node-to-surface contact formulation on contact forces acting on individual slave nodes; the ambiguous nature of the nodal forces in second-order elements can cause Abaqus/Standard to make a wrong decision. To circumvent this problem, Abaqus/Standard automatically converts most three-dimensional second-order elements with no
midface node (i.e., serendipity elements) that form a slave surface into elements with a midface node. For the three-dimensional 18-node gasket elements, the midface nodes are also generated automatically if they are not given in the element connectivity. The presence of the midface node results in a distribution of nodal forces that is not ambiguous for the contact algorithm.
The element families C3D20(RH), C3D15(H), S8R5, and M3D8 are converted to the families C3D27(RH), C3D15V(H), S9R5, and M3D9, respectively. Since Abaqus/Standard does not convert second-order coupled temperature-displacement, coupled thermal-electrical-structural, and coupled pore pressure–displacement elements, you should specify a penalty or augmented Lagrange constraint enforcement method to approximate hard pressure-overclosure behavior (see “Contact constraint enforcement methods in Abaqus/Standard,” Section 38.1.2). Abaqus/Standard will interpolate nodal quantities, such as temperature and field variables, at the automatically generated midface nodes when values are prescribed at any of the user-defined nodes. Abaqus/Standard does not convert second-order serendipity elements if the slave surface is used in a tied contact pair.
Second-order tetrahedral elements (C3D10 and C3D10HS) have zero contact force at their corner nodes. This combination of second-order triangular slave facets, a node-to-surface contact formulation, and strict enforcement of “hard” contact conditions is disallowed to avoid a high likelihood of convergence problems and poor predictions of contact pressures that would occur with this combination. To avoid this combination, use at least one of the following alternatives:
• Use the surface-to-surface contact formulation (generally recommended) instead of the node-tosurface contact formulation;
• Use the penalty constraint enforcement method (generally recommended) or augmented Lagrange constraint enforcement method instead of strict enforcement of “hard” contact conditions; or
• Use modified 10-node tetrahedral elements (C3D10M) instead of second-order tetrahedral elements.
Excessive iterations in contact simulations
Abaqus/Standard offers a number of methods to adjust the solver iteration scheme, sometimes resulting in a more efficient analysis with a minimal effect on accuracy.
Converting severe discontinuity iterations in weakly determined contact conditions
By default, Abaqus/Standard continues to iterate until the severe discontinuities associated with changes in contact status are sufficiently small (or no severe discontinuities occur) and the equilibrium (flux) tolerances are satisfied. Alternatively, you can choose a different approach in which Abaqus/Standard continues to iterate until no severe discontinuities occur. These two approaches are discussed in more detail in “Severe discontinuities in Abaqus/Standard” in “Defining an analysis,” Section 6.1.2. The default treatment of severe discontinuity iterations reduces the likelihood of excessive iterations associated with chattering between contact states when the contact conditions are weakly determined. An example of a region with weakly determined contact conditions is near the center of a flat punch that contacts a thin plate supported at its edges.
Controlling the increment size based on penetration distance in unconverged iterations
For most types of contact, if during an iteration the penetration calculated for any contact pair exceeds a specific distance \left( h _ { c r i t } \right) , Abaqus/Standard abandons the increment and tries again with a smaller increment size. There is no critical penetration distance for finite-sliding, surface-to-surface contact (including general contact) and for small-sliding contact in geometrically linear analyses.
The default value of \hslash _ { c r i t } is the radius of a sphere that circumscribes a characteristic surface element face. When calculating the default value, Abaqus/Standard uses only the slave surface of the contact pair. The value of h _ { c r i t } for each contact pair in the model is printed in the data (.dat) file. While the default value of h _ { c r i t } should prove to be sufficient for the majority of contact simulations, in some cases it may be necessary to change the default value for a given contact pair. These cases include:
• Models in which the master surface is highly curved. The default value of h _ { c r i t } may sometimes lead to situations as shown in Figure 39.1.2–7. During the iterative solution process a slave node initially at point a may move to point b, penetrating the master surface with overclosure h less than h _ { c r i t } . Abaqus/Standard may attempt to move the slave node to point c on the master surface. To avoid this situation, specify a smaller value for h _ { c r i t } to force Abaqus/Standard to abandon the increment and to try a smaller increment size.
text_image
a S b M S → Slave node M → Master surface a-b-c → Trajectory of slave node h h_crit b c M
Figure 39.1.2–7 Effect of the critical penetration distance on a highly curved master surface.
• Models in which Abaqus/Standard cannot calculate a reasonable h _ { c r i t } because a node-based surface is used. If there are other contact pairs in the model with surfaces, Abaqus/Standard uses the average dimension of all of the slave surface element faces. If there are no other contact pairs, Abaqus/Standard uses a characteristic element dimension of the entire model.
• Models in which the contact face dimensions in a slave surface vary greatly.
• Models in which the slave surface mesh is very refined compared with the typical surface dimensions so that overclosures much larger than the default h _ { c r i t } can be resolved easily.
• Models in which contact pairs with softened contact allow significant penetration (see “Contact pressure-overclosure relationships,” Section 37.1.2).
Input File Usage: *CONTACT PAIR, HCRIT=
Abaqus/CAE Usage: You cannot adjust the default value of h _ { c r i t } in Abaqus/CAE.
Difficulties interpreting the results of contact simulations
Although an analysis involving contact runs to completion, the results may seem unrealistic. This is sometimes due to modeling errors and sometimes due to the specialized output format of certain contact formulations. In addition to degrading contact output, the factors discussed below also tend to degrade convergence behavior, so avoiding these factors may improve convergence behavior.
Oscillating contact pressures when using second-order elements in “hard” contact simulations
Nonuniform contact pressure distributions are likely to occur when very different mesh densities are used on the two deformable surfaces making up a contact interaction. The nonuniformity can be particularly pronounced when “hard” contact is modeled and both surfaces are modeled with second-order elements, including modified, second-order tetrahedral elements. In such cases oscillations and “spikes” in the contact pressure may occur. Smoother contact pressures may be obtained for surfaces modeled with second-order elements by using penalty-type contact constraint enforcement (see “Contact constraint enforcement methods in Abaqus/Standard,” Section 38.1.2).
Inaccurate contact stresses when using second-order axisymmetric elements at the symmetry axis
For second-order axisymmetric elements the contact area is zero at a node lying on the symmetry axis . To avoid numerical singularity problems caused by a zero contact area, Abaqus/Standard calculates the contact area as if the node were a small distance from the symmetry axis. This may result in inaccurate local contact stresses calculated for nodes located on the symmetry axis.
Self-contact
Contact of a surface with itself (self-contact) is provided for cases in which the original geometry is very different from the (deformed) geometry at which contact takes place. It would then be difficult for you to predict which parts of the surface will come into contact with each other. Where possible, it is always computationally more economical to declare parts of the surface as master and parts as slave. The same unpredictability makes it impossible to determine a priori which side will be the master and which side the slave. Therefore, Abaqus/Standard uses a symmetric contact model: every single node of the surface can be a slave node and can simultaneously belong to master segments with respect to all other nodes.
Because each surface is acting as both a slave and a master, the results of symmetric contact analyses can be confusing and inconsistent. These difficulties are discussed more fully in “Using symmetric master-slave contact pairs to improve contact modeling” in “Defining contact pairs in Abaqus/Standard,” Section 36.3.1.
Overconstraining the model
The term overconstraint refers to a situation in which multiple kinematic constraints outnumber the degrees of freedom on which they act. Overconstraints often lead to inaccurate solutions or
failure to obtain a converged solution. Contact conditions strictly enforced with the direct constraint enforcement method (using Lagrange multipliers) are sometimes involved in overconstraints. See “Overconstraint checks,” Section 35.6.1, for a detailed discussion and examples of overconstraints and how Abaqus/Standard will treat overconstraints based on the following classifications:
• Overconstraints detected in the model preprocessor
• Overconstraints detected and resolved during analysis
• Overconstraints detected in the equation solver
Abaqus/Standard will automatically resolve many types of overconstraints; however, many overconstraints involving contact cannot be resolved and will be exposed to the equation solver. The equation solver will often issue “zero pivot” or “numerical singularity” warning messages as a result of overconstraints; when this occurs, Abaqus/Standard will provide a warning message with information that is helpful for determining what contributed to the overconstraint so that you can resolve it. Occasionally overconstraints do not create warning messages; this does not necessarily mean that the overconstraints have not adversely affected the analysis.
Overconstraints involving softened contact
Contact conditions with a softened behavior or enforced with the penalty or augmented Lagrange method will not combine with other constraints to cause “strict overconstraints”; however, “softened overconstraints” can:
• cause zero pivots or ill-conditioning in the equation solver if the stiffness contributions associated with contact are many orders of magnitude higher than the stiffness contributions from typical elements;
• prevent a tight penetration tolerance from being achieved with the augmented Lagrange method; and
• cause oscillations in contact stress solutions, particularly if the contact stiffness is high.
Some types of contact use the penalty or augmented Lagrange method by default to approximate hard pressure-overclosure behavior due to the prevalence of redundant or “competing” contact conditions. For a discussion of available constraint enforcement methods and default behavior, see “Contact constraint enforcement methods in Abaqus/Standard,” Section 38.1.2.
Inaccurate contact forces due to overconstraints
If nodes in a contact pair are overconstrained but the equation solver does find a solution, the contact forces become indeterminate and may become excessively high, particularly in tied contact pairs. Check the time average force (or moment, or flux) reported in the message file, or use Abaqus/CAE to view the diagnostic information interactively (for more information, see Chapter 41, “Viewing diagnostic output,” of the Abaqus/CAE User’s Guide). If it is many orders of magnitude larger than the residual forces (or moments, or fluxes), an overconstraint may have occurred, and there is no guarantee that Abaqus/Standard has found the correct solution. Another sign that the model is overconstrained is that the analysis begins to converge in a single iteration in every increment when the nonlinearities should require
at least several iterations. Overconstraints should be avoided only by changing the contact definition or other constraint type involved.
Overconstraints due to multiple surface interaction definitions at a single node
Automatic resolution of contact overconstraints sometimes depends on whether two contact pairs refer to the same surface interaction definition. For example, consider a case in which two contact pairs have a common master surface and share some slave nodes (perhaps along a common edge of two slave surfaces). Overconstraints will occur at the common slave nodes if the two contact pairs refer to different surface interaction definitions (even if the surface interactions are equivalent); however, Abaqus/Standard automatically avoids these overconstraints if the two contact pairs refer to the same surface interaction definition. (See “Assigning contact properties for contact pairs in Abaqus/Standard,” Section 36.3.3, for a discussion of how to assign surface interaction definitions to contact pairs.)
Discrepancies between contact formulations
The different contact formulations available in Abaqus/Standard (see “Contact formulations in Abaqus/Standard,” Section 38.1.1) allow for a great deal of flexibility when modeling contact simulations. However, two nearly identical simulations that differ only in the contact formulation being used will sometimes generate varying results. This is primarily because of the different ways that contact formulations interpret contact conditions. Certain formulations are better suited to particular situations.
Differences in penetrations
The most observable difference between node-to-surface and surface-to-surface discretization is the amount of penetration that occurs between surfaces. This is because node-to-surface discretization computes penetrations only at slave nodes, while surface-to-surface discretization computes penetrations in an average sense over a finite region. For example, when a slave surface slides across a convex portion of a master surface, the slave surface will tend to ride a bit higher with surface-to-surface discretization than with node-to-surface discretization, as shown in Figure 39.1.2–8 (the opposite is true at a concave portion of a master surface). Figure 39.1.2–9 shows another case in which the two contact discretizations behave fundamentally differently due to the different approaches to computing penetrations. Both discretizations converge to the same behavior as the mesh is refined.
The differences in computed penetrations can sometimes fundamentally affect the results of an analysis. Be aware of this possibility when converting models from one contact formulation to another. Various aspects of preexisting models, such as the friction coefficient or the pressure-overclosure relationship, may have been inadvertently “tuned” to the behavior that occurs with a particular contact formulation.
text_image
Punch Die Holder
Surface-to-surface
natural_image
Curved pipe or duct diagram with color gradient indicating stress or flow direction (no text or symbols)
Node-to-surface
Figure 39.1.2–8 Comparison of contact discretizations in an example with convex curvature in the master surface (forming application).
text_image
master surface Constraints based on "averaged" penetration slave surface Surface-to-surface master surface Constraints based on slave nodes penetration Node-to-surface
Figure 39.1.2–9 Comparison of contact discretizations in an example with a relatively flexible slave surface wrapping around a corner of a master surface.
Contact at a single point
Figure 39.1.2–10 shows an example in which a circular rigid body is pushed into a deformable body. In the initial configuration shown, the two bodies touch at a single point, which corresponds to a slave node location. The following scenarios are likely for respective analyses of this model with node-to-surface and surface-to-surface discretization:
text_image
Concentrated load x Rigid body Deformable body
Figure 39.1.2–10 Example with two bodies initially touching at a single point.
• With node-to-surface discretization, the first iteration is performed with one active contact constraint. A converged solution is obtained with a reasonable number of iterations and increments.
• With surface-to-surface discretization, penetrations are computed in an average sense over finite regions of the surface, so a positive gap distance is computed for all potential contact constraints even though the surfaces touch at one of the slave nodes. However, the finite-sliding, surface-to-surface contact formulation detects that the surfaces are initially touching and by default automatically activates localized contact damping in the neighborhood where the gap distance is zero. Without such damping, Abaqus/Standard may not obtain a converged solution due to an unconstrained rigid body mode. This contact damping typically has an insignificant effect on the converged solution, and the damping is completely removed by the end of the step.
If you deactivate the automatic localized damping for the finite-sliding, surface-to-surface formulation—or if you are using the small-sliding, surface-to-surface formulation—you should use one of the techniques discussed above in “Difficulties resolving initial contact conditions” to remove the perceived initial gap between surfaces and prevent rigid body modes in the analysis.
Input File Usage: Use the following option to deactivate automatic localized contact damping at artificial surface gaps for contact pair definitions:
*CONTACT PAIR, MINIMUM DISTANCE=NO
Use the following option to deactivate automatic localized contact damping at artificial surface gaps for general contact definitions:
*CONTACT INITIALIZATION DATA, MINIMUM DISTANCE=NO
Abaqus/CAE Usage: You cannot deactivate automatic localized contact damping at artificial surface gaps in Abaqus/CAE.
Differences in contact normal direction
Node-to-surface discretization uses a contact normal direction based on the master surface normal, whereas surface-to-surface discretization uses a contact normal direction based on the slave surface normal (averaged over a region nearby the slave node). For most active contact definitions the slave and master surfaces are nearly parallel, so the master and slave normals are approximately aligned; in which case this distinction in how the contact normal is determined is not significant. However, in some cases the differences in the contact normal can be significant.
• When modeling large interference fits, surface-to-surface discretization can sometimes cause tangential motion of the slave surface as the overclosures are resolved. This tangential motion may have undesirable effects on an analysis. See “Controlling initial contact status in Abaqus/Standard,” Section 36.2.4, and “Modeling contact interference fits in Abaqus/Standard,” Section 36.3.4, for more details.
• Contact constraints involving geometric edges of surfaces sometimes use a significantly different contact normal depending on which contact discretization approach is used, because the normals for the slave and master surfaces may not directly oppose each other.
• The contact opening distance output variable (COPEN) can vary considerably depending on what type of contact formulation is used if the contact surfaces are not parallel. For node-to-surface discretization, the opening distance that is reported approximates the closest distance to the master surface; for surface-to-surface discretization, the opening distance that is reported corresponds to the distance from the slave surface to the master surface along the slave normal direction. The opening distance for surface-to-surface discretization is undefined if a line emanating from the slave surface in the slave normal direction does not intersect the master surface (as discussed in “Using the small-sliding tracking approach” in “Contact formulations in Abaqus/Standard,” Section 38.1.1, if a small-sliding constraint cannot be formed in such a case for the small-sliding, surface-to-surface formulation, Abaqus/Standard automatically reverts to the node-to-surface approach for individual constraints).
Contact at corners
The finite-sliding, surface-to-surface formulation is often better-suited than other contact formulations for modeling contact near corners. In the example shown in Figure 39.1.2–11, the slave surface is on the “outer” body (i.e., the body with a reentrant corner). With node-to-surface discretization a single constraint acts at the corner slave node in the “average” normal direction of the master surface, which often leads to poor resolution of contact, non-physical response, and even early termination of an analysis. However, surface-to-surface discretization generates two constraints near the corner for the respective faces, as shown in Figure 39.1.2–11, resulting in more stable contact behavior.
natural_image
Diagram showing a grid with arrows indicating direction, no text or symbols present
Surface-to-surface
natural_image
Diagram showing a red grid with a white arrow pointing to a teal square adjacent to it (no text or symbols)
Node-to-surface
Figure 39.1.2–11 Comparison of contact formulations in an example with abutting surfaces having respective interior and exterior corners.