김경종
19 KiB
39.2 Resolving contact difficulties in Abaqus/Explicit
• “Contact diagnostics in an Abaqus/Explicit analysis,” Section 39.2.1
• “Common difficulties associated with contact modeling using contact pairs in Abaqus/Explicit,” Section 39.2.2
39.2.1 CONTACT DIAGNOSTICS IN AN Abaqus/Explicit ANALYSIS
Products: Abaqus/Explicit Abaqus/CAE
References
• “Output to the data and results files,” Section 4.1.2
• “Contact interaction analysis: overview,” Section 36.1.1
• *DIAGNOSTICS
• Chapter 41, “Viewing diagnostic output,” of the Abaqus/CAE User’s Guide
Overview
Contact diagnostics in Abaqus/Explicit allow you to get detailed information about the surfaces and progress of contact interactions. Diagnostics are available:
• to review automatic adjustments between two surfaces,
• to reveal potentially problematic initial surface configurations in a model,
• to track excessive penetrations between two contacting surfaces, and
• to review warnings associated with contact between warped surfaces.
Reviewing the adjustments of initially overclosed surfaces
Contacting surfaces that are overclosed in the initial configuration of the model are adjusted automatically by Abaqus/Explicit to remove the overclosures (see “Controlling initial contact status for general contact in Abaqus/Explicit,” Section 36.4.4, and “Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit,” Section 36.5.4). There are three sources of information on the adjustments of overclosed surfaces: the status (.sta) file, the message (.msg) file, and the output database (.odb) file.
Obtaining the adjustments of overclosed surfaces in the status and message files
By default, Abaqus/Explicit writes all nodal adjustments and—for general contact surfaces—contact offsets to the message (.msg) file along with a summary listing of the maximum initial overclosure and the maximum nodal adjustment to the status (.sta) file for the contact pairs defined in the first step of a simulation. You can choose to suppress the information written to the message file and write only the summary information to the status file. The information written to the message and status files is also written to the output database (.odb) for use in Abaqus/CAE.
Input File Usage:
Use the following option to obtain both detailed diagnostic output to the message file and summary diagnostic output to the status file:
*DIAGNOSTICS, CONTACT INITIAL OVERCLOSURE=DETAIL (default)
Use the following option to obtain only summary diagnostic output to the status file (no contact diagnostics will be written to the message file):
*DIAGNOSTICS, CONTACT INITIAL OVERCLOSURE=SUMMARY
Abaqus/CAE Usage:
You cannot control the diagnostic information for contact initial overclosures from within Abaqus/CAE. Use the following option to view the saved diagnostic information:
Visualization module: Tools→Job Diagnostics
Viewing the adjustments of surfaces
In the first step the adjustments of initially overclosed surfaces can be viewed in Abaqus/CAE. Displaced shape plots that show the adjustments to the contact pairs defined in the first step can be plotted for the original field output frame at zero time (this nodal coordinate adjustment may introduce small nonzero strain output for solid elements even when the stresses are zero). In addition, output variable STRAINFREE (see “Abaqus/Explicit output variable identifiers,” Section 4.2.2) contains nodal vectors representing initial strain-free adjustments. By default, STRAINFREE is written to the output database (.odb) file for the original field output frame at zero time if any strain-free adjustments are made by Abaqus/Explicit. A symbol plot of this variable in the Visualization module of Abaqus/CAE shows vectors that represent how individual nodes have been adjusted, and a contour plot of this variable shows the distribution of the adjustment magnitude (you must select the original output frame at zero time in the Visualization module of Abaqus/CAE before choosing the STRAINFREE output variable). In the case of overclosures in steps other than the first, vector plots of nodal displacements and accelerations can be particularly helpful in visualizing the adjustments. Such plots can be viewed in Abaqus/CAE after a data check analysis (see “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2).
Visualizing the precise initial clearances for small-sliding contact pairs
Abaqus/Explicit does not adjust the coordinates of the slave surface when precise initial clearances are specified for small-sliding contact pairs (see “Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit,” Section 36.5.4). Therefore, the specified clearances cannot be seen in a postprocessor such as the Visualization module of Abaqus/CAE. Thus, depending on the initial geometry of the surfaces and the magnitude of the clearances or overclosures, the surfaces may appear open or closed in the postprocessor when they are actually just in contact in the simulation.
Detecting crossed surfaces in a general contact domain
If a slave surface initially penetrates a double-sided master surface by a distance greater than the master surface’s thickness, the severely overclosed slave nodes will see the back side of the master surface as the appropriate contact force direction. These slave nodes in these crossed surfaces effectively become trapped behind the master surface. This issue is discussed in more detail in “Controlling initial contact status for general contact in Abaqus/Explicit,” Section 36.4.4, and “Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit,” Section 36.5.4.
For general contact definitions, diagnostic testing that identifies regions in which surfaces are crossed in the initial configuration is activated by default. When the diagnostic tests are activated, a warning message is issued to the message (.msg) file if two adjacent slave nodes (connected by a facet edge) are detected on opposite sides of a master surface. No such warning is issued for node-based surface nodes on opposite sides of a master surface, because adjacency cannot be determined among the node-based surface nodes. In some cases involving corners of master surfaces this warning message may be issued even though adjacent slave nodes are really on the same side of a master surface. The CPU cost of performing diagnostic testing on large models is potentially significant. You can choose to deactivate the diagnostic testing and avoid the extra CPU cost in such cases.
Input File Usage: Use the following option to deactivate diagnostic testing for initially crossed surfaces:
*DIAGNOSTICS, DETECT CROSSED SURFACES=OFF
Abaqus/CAE Usage: You cannot exclude diagnostic testing for initially crossed surfaces from within Abaqus/CAE. Use the following option to view the saved diagnostic information:
Visualization module: Tools→Job Diagnostics
Excessive penetrations between general contact surfaces
As described in “Contact constraint enforcement methods in Abaqus/Explicit,” Section 38.2.3, the penalty constraint enforcement method used by the general contact algorithm in Abaqus/Explicit allows slight penetrations of one surface into another surface. A “spring” stiffness is applied automatically to the surfaces to resist these penetrations. If the nodes involved in general contact do not have adequate mass, the default “spring” stiffness chosen automatically by Abaqus/Explicit may not be sufficient to prevent large penetrations. Such a situation can arise, for example, when a cloud of massless nodes, fully constrained by a kinematic coupling definition, contacts a fully constrained rigid face with no mass.
By default, if during node-to-face contact, the penetration of a node into its tracked face exceeds 50% of the typical face dimension in the general contact domain, the penetration is regarded as excessive and Abaqus/Explicit issues a diagnostic message to the status (.sta) file. A node set containing deeply penetrated nodes is also written to the output database (.odb) file for use in Abaqus/CAE. You can control the fraction of the typical face dimension used to trigger the diagnostic message.
Input File Usage: Use the following option to control the fraction of the typical element face dimension used to trigger the diagnostic message for deep penetrations:
*DIAGNOSTICS, DEEP PENETRATION FACTOR=value
Abaqus/CAE Usage: You cannot control the diagnostic information for deep penetrations from within Abaqus/CAE. Use the following option to view the saved diagnostic information:
Visualization module: Tools→Job Diagnostics
Warning messages for highly warped surfaces
Calculating the correct contact conditions along a surface that is highly warped is very difficult, and Abaqus/Explicit employs a specialized algorithm to enforce contact between warped surfaces; this specialized algorithm is more expensive than the default contact algorithm (see “Contact controls for contact pairs in Abaqus/Explicit,” Section 36.5.5). By default, Abaqus/Explicit checks for highly warped surfaces every 20 increments.
Abaqus/Explicit writes a warning message in the status (.sta) file the first time that it detects that a surface is highly warped. The message is brief; it states only which surface has a highly warped facet. If additional facets on this surface become highly warped later in the analysis, no additional warning messages are issued.
You can request more detailed diagnostic warning messages, if desired. In this case the message file will contain a warning every time a warped facet is found on a particular surface. The warnings will give the parent element associated with the warped facet (the parent element is the element whose face forms the facet) and the warping angle of the facet.
The computation time and the size of the message file can increase significantly if detailed warnings are requested. You can switch back to the summary warnings in subsequent steps or suppress the warped surface warnings entirely.
If the analysis terminates with a fatal error, the preselected output variables will be added automatically to the output database as field data for the last increment.
| Input File Usage: | Use the following option to request detailed diagnostic warning output for warped surfaces:*DIAGNOSTICS, WARPED SURFACE=DETAILUse the following option to request the default summary diagnostic output for warped surfaces:*DIAGNOSTICS, WARPED SURFACE=SUMMARYUse the following option to suppress diagnostic warning output for warped surfaces entirely:*DIAGNOSTICS, WARPED SURFACE=OFF |
| Abaqus/CAE Usage: | Diagnostic output requests for warped surfaces are not supported in Abaqus/CAE. |
39.2.2 COMMON DIFFICULTIES ASSOCIATED WITH CONTACT MODELING USING CONTACT PAIRS IN Abaqus/Explicit
Products: Abaqus/Explicit Abaqus/CAE
References
• “Defining contact pairs in Abaqus/Explicit,” Section 36.5.1
• *CONSTRAINT CONTROLS
• *CONTACT PAIR
Overview
This section highlights the difficulties that are most commonly encountered when modeling contact interactions with contact pairs in Abaqus/Explicit. Most of these issues are not relevant when the general contact algorithm is used; refer to “Defining general contact interactions in Abaqus/Explicit,” Section 36.4.1, for more information on the issues involved with general contact interactions. Recommendations on how to circumvent these problems are presented.
Defining duplicate nodes on the master surface
When defining three-dimensional surfaces formed by element faces, avoid defining two surface nodes with the same coordinates. Such a definition can give rise to a seam, or crack, in the surface as shown in Figure 39.2.2–1.
natural_image
Abstract geometric pattern with interconnected nodes and curved edges, no text or symbols present
Both vertices have the same coordinates. They are separated to show the crack in the surface.
Figure 39.2.2–1 Example of doubly defined surface node.
If viewed with the default plotting options in Abaqus/CAE, this surface will appear to be a valid, continuous surface; however, a node sliding along this surface can fall through this crack and violate the contact conditions. If this were to happen, Abaqus/Explicit would enforce the contact conditions by applying a large acceleration to the node once overclosure is detected. The large resulting acceleration may create a noisy solution or cause the elements to distort badly.
Use the edge display options in the Visualization module of Abaqus/CAE to identify any unwanted cracks in the surfaces used in the model. The cracks will appear as extra perimeter lines in the interior of the surface. Duplicate nodes can be avoided easily by equivalencing nodes when creating the model in a preprocessor.
Using an inadequate surface definition for the desired contact conditions
Occasionally, surface definitions may not be suitable for modeling the desired contact conditions in a problem. Figure 39.2.2–2 shows a two-dimensional model of a simple connection between two parts.
text_image
surface 1 surface 2 surface 3 contact pair 1 = surface 1, surface 3 contact pair 2 = surface 2, surface 3 Analysis will stop after 1st increment with message that elements are badly distorted
Figure 39.2.2–2 Surface definitions that are inadequate for the desired contact conditions.
The surfaces shown in the figure are inadequate for the desired contact conditions that are also shown. At the start of the simulation, Abaqus/Explicit will detect that some of the nodes on surface 3 are behind surfaces 1 and 2. When the contact conditions are enforced, the motions of the surfaces will likely cause badly distorted elements. One solution to this problem is shown in Figure 39.2.2–3.
text_image
surface 4 surface 5
contact pair = surface 4, surface 5
Figure 39.2.2–3 Surface definitions that are adequate for the desired contact conditions.
The surfaces shown in that figure are suitable for the desired contact definition. Other solutions, such as using a pure master-slave contact pair, exist for this problem and may be more suitable, depending on the details of the intended simulation.
Using poorly discretized surfaces
Several problems are caused by surfaces created on very coarse meshes.
Penetrations with coarsely discretized surfaces when using hard surface behavior
When a coarsely discretized surface is used as the slave surface in a pure master-slave contact pair with hard surface behavior, an inaccurate solution may be produced as a result of the gross penetration of the master surface into the slave surface. This situation is shown in Figure 39.2.2–4. This problem can be minimized if the contact pair can be switched to a balanced master-slave contact pair. However, some contact pairs in Abaqus/Explicit must always use a pure master-slave formulation. In these cases the only solution to gross penetration is to refine the slave surface.
Problems with coarsely discretized rigid surfaces
For rigid surfaces formed by element faces, inaccurate results may be obtained if too few elements are used to represent a curved geometry. When a very coarse mesh is used on a curved geometry, it is possible for slave nodes to get “snagged” on the sharp vertices.
In general, using a reasonable number of element faces to represent a curved surface will not increase the computational time of the simulations. However, a large number of element faces can significantly increase the memory that Abaqus/Explicit will need for the simulation. When a specific
flowchart
graph TD
A["master surface (segments)"] --> B["slave nodes cannot penetrate master segments"]
B --> C["penetration"]
C --> D["slave surface (nodes)"]
D --> E["master node can penetrate slave segment"]
E --> F["gap"]
F --> A
Figure 39.2.2–4 Master surface penetrations into the slave surface due to coarse discretization.
curved surface geometry can be modeled, using an analytical rigid surface may provide a more accurate geometric description while minimizing computational expense; see “Analytical rigid surface definition,” Section 2.3.4.
Penalty contact behavior sensitivity in rigid-to-rigid interactions
The contact penalties are, in general, determined from stable time increment considerations and masses of the nodes involved in contact. To compute a reliable contact penalty when rigid bodies are contacting each other, Abaqus/Explicit accounts in a comprehensive fashion for the inertial properties of the rigid bodies by distributing the mass of the rigid bodies at all nodes that might be involved in contact. Hence, the final contact penalty will depend on the size of the actual rigid surfaces that are included in the contact definitions. Consequently, the contact response (forces, penetrations) will depend somewhat on your choice in defining the contacting surfaces on the rigid bodies. If large penetrations occur, specifying realistic inertial properties for the rigid bodies will help in general to resolve the issue. Alternatively, you can use a scaling factor for the penalties to enforce contact in a more accurate fashion.
Conflicts with boundary conditions
If boundary constraints are applied to contact nodes on both surfaces of a contact pair in the direction that the contact constraints are active, the boundary constraints may override the contact constraints. For kinematic contact, contact force related quantities will be output as the force necessary to resolve the contact constraint in a single increment, causing misleading results for these output quantities if the boundary constraints violate the contact constraints. Contact force output for penalty contact does not show this behavior since the contact force is proportional only to the current penetration and does not depend on the time increment. Boundary constraints are not affected by contact constraints.