Contact diagnostics in an Abaqus/Explicit analysis | |||||||||
|
| ||||||||
ProductsAbaqus/ExplicitAbaqus/CAE
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 and Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit). 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: 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) 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 and Abaqus/Explicit execution).
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). 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 and Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit.
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:
Excessive penetrations between general contact surfaces
As described in Contact constraint enforcement methods in Abaqus/Explicit, 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:
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). 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=DETAIL
Use the following option to request the default summary diagnostic output for warped surfaces:
DIAGNOSTICS, WARPED SURFACE=SUMMARY
Use 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.