김경종
24 KiB
Specifying individual contact interactions
Alternatively, you can define the general contact domain directly by specifying the individual contact surface pairings. Self-contact will be modeled only if the two surfaces specified in a pair overlap (or are identical) and will be modeled only in the overlapping region.
Multiple surface pairings can be included in the contact domain. At least one surface in each pair must be either an element-based surface or an analytical rigid surface.
Input File Usage: Use both of the following options to specify individual contact interactions:
*CONTACT
*CONTACT INCLUSIONS
surface_1, surface_2
At least one data line must be specified when the ALL EXTERIOR parameter is omitted. Either or both of the data line entries can be left blank, but each data line must contain at least a comma; an error message will be issued for empty data lines. If the first surface name is omitted, the default unnamed, all-inclusive, automatically generated surface is assumed. If the second surface name is omitted or is the same as the first surface name, contact between the first surface and itself is assumed. Leaving both data line entries blank is equivalent to using the ALL EXTERIOR parameter.
Abaqus/CAE Usage: Interaction module: Create Interaction: General contact (Explicit): Included surface pairs: Selected surface pairs: Edit, select the surfaces in the columns on the left, and click the arrows in the middle to transfer them to the list of included pairs
Examples
The following input specifies that contact should be enforced between the default all-inclusive, automatically generated surface and surface_2, including self-contact in any overlap regions:
*CONTACT
*CONTACT INCLUSIONS
, surface_2
Either of the following methods can be used to define self-contact for surface_1:
*CONTACT
*CONTACT INCLUSIONS
surface_1,
or
*CONTACT
*CONTACT INCLUSIONS
surface_1, surface_1
The following input can be used to introduce a node-based surface containing point masses to the contact domain as well as specify self-contact for the default all-inclusive, automatically generated surface:
*CONTACT
*CONTACT INCLUSIONS
,
, node_based_surf
Specifying contact exclusions
You can refine the contact domain definition by specifying the regions of the model to exclude from contact.
The primary motivation for specifying contact exclusions is to avoid physically unreasonable contact interactions. For example, a finite element model may contain multiple forming tools, but not all of the tools participate in the forming process simultaneously; you can specify contact exclusions to prevent certain tools from participating in the contact model in certain steps.
You do not need to be concerned with specifying contact exclusions for parts of the model that are not likely to interact, since these exclusions typically will have minimal effect on computational performance.
Contact will be ignored for all the surface pairings specified, even if these interactions are specified directly or indirectly in the contact inclusions definition.
Multiple surface pairings can be excluded from the contact domain. At least one surface in each pair must be either an element-based surface or an analytical rigid surface. Keep in mind that surfaces can be defined to span multiple unattached bodies, so self-contact exclusions are not limited to exclusions of single-body contact.
You cannot exclude only one side of shell-like surfaces. If a side label (SPOS or SNEG) is used in defining an element-based shell-like surface and that surface is excluded from contact, Abaqus/Explicit will exclude all faces associated with these elements.
Input File Usage: Use both of the following options to specify contact exclusions:
*CONTACT
*CONTACT EXCLUSIONS
surface_1, surface_2
Either or both of the data line entries can be left blank. If the first surface name is omitted, the default unnamed, all-inclusive, automatically generated surface is assumed. If the second surface name is omitted or is the same as the first surface name, contact between the first surface and itself is excluded from the contact domain.
Abaqus/CAE Usage: Interaction module: Create Interaction: General contact (Explicit): Excluded surface pairs: Edit, select the surfaces in the columns on the left, and click the arrows in the middle to transfer them to the list of excluded pairs
Automatically generated contact exclusions
Abaqus/Explicit automatically generates contact exclusions for general contact in some situations.
• Contact exclusions are generated automatically for interactions that are defined with the contact pair algorithm or surface-based tie constraints to avoid redundant (and possibly inconsistent) enforcement of these interaction constraints. For example, if a contact pair is defined for surface_1 and surface_2 and “automatic” general contact is defined for the entire model, Abaqus/Explicit would generate a contact exclusion for general contact between surface_1 and surface_2, so that interactions between these surfaces would be modeled only with the contact pair algorithm. These automatically generated contact exclusions are in effect only during the steps in which the contact pair algorithm or surface-based tie constraint interactions are active.
• Abaqus/Explicit automatically generates contact exclusions for self-contact of each rigid body in the model, because it is not possible for a rigid body to contact itself.
• When you specify pure master-slave contact surface weighting for a particular general contact surface pair, contact exclusions are generated automatically for the master-slave orientation opposite to that specified (see “Contact formulation for general contact in Abaqus/Explicit,” Section 38.2.1, for more information on this type of contact exclusion).
• The general contact algorithm, unlike the contact pair algorithm, activates and deactivates contact faces and contact edges in the contact domain based on the failure status of the underlying elements. See “Modeling surface erosion” below for details.
Examples
The following input specifies that the contact domain is based on self-contact of an all-inclusive, automatically generated surface but that contact (including self-contact in any overlap regions) should be ignored between the all-inclusive, automatically generated surface and surface_2:
*CONTACT
*CONTACT INCLUSIONS, ALL EXTERIOR
*CONTACT EXCLUSIONS
, surface_2
Either of the following methods can be used to exclude self-contact for surface_1 from the contact domain:
*CONTACT EXCLUSIONS surface_1,
or
*CONTACT EXCLUSIONS
surface_1, surface_1
Modeling surface erosion
General contact allows the use of element-based surfaces to model surface erosion for analyses. If an appropriate “interior” surface is defined, the surface topology will evolve to match the exterior of elements that have not failed. Alternatively, if only one of the bodies can erode, a node-based surface can be used to model surface erosion; this approach can be used with either the general contact or contact pair algorithms. However, even if only one body can erode, it is recommended to define an element-based surface for the eroding body to avoid the usual limitations of node-based surfaces (see “Node-based surface definition,” Section 2.3.3).
The general contact algorithm modifies the list of contact faces and contact edges that are active in the contact domain based on the failure status of the underlying elements (element failure is discussed in “Dynamic failure models,” Section 23.2.8). General contact considers a face only if its underlying element has not failed and it is not coincident with a face from an adjacent element that has not failed; thus, exterior faces are initially active, and interior faces are initially inactive. Once an element fails, its faces are removed from the contact domain, and any interior faces that have been exposed are activated. A contact edge is removed when all the elements that contain the edge have failed. New contact edges are not created as elements erode. Based on this algorithm, the active contact domain evolves during the analysis as elements fail (see Figure 36.4.1–2 for an example of an eroding solid).
text_image
surface topology before the shaded elements have failed newly exposed faces surface topology after failure
Figure 36.4.1–2 Topology of an eroding contact surface.
You can control whether contact nodes remain in the contact domain after all the surrounding elements have failed. By default, these nodes remain in the contact domain and act as free-floating point masses that can experience contact with faces that are still part of the contact domain. You can specify that nodes of element-based surfaces should erode (i.e., be removed from the contact domain) once all contact faces and contact edges to which they are attached have eroded. Further discussion of this technique, including reasons for and against nodal erosion, can be found in “Contact controls for general contact in Abaqus/Explicit,” Section 36.4.5.
Erosion of surfaces specified on solid elements
For a solid element mesh consisting of elements that may fail, every face that can potentially be involved in contact (both exterior and interior faces) should be included in the contact domain. The general contact algorithm will activate and deactivate faces as necessary when elements fail.
For example, you define an element set ELERODE that contains all the solid elements in the model that refer to a material failure model. First, you must create a surface SURFERODE containing all of the interior and exterior faces of these elements. You could define this surface using the automatic free surface and interior surface generation methods in Abaqus/Explicit. Assuming all the elements in ELERODE are of type C3D8R, you could alternatively define the surface by specifying the faces S1 through S6 directly. See “Creating surfaces on solid, continuum shell, and cohesive elements” in “Element-based surface definition,” Section 2.3.2, for a discussion of these three methods.
Next, you must construct the contact domain. Defining “automatic” general contact for the entire model is not sufficient because the contact domain created when this method is used does not include any interior faces. Therefore, you must define the pairwise interactions with the erodable surface explicitly in the contact inclusions definition, as outlined in Table 36.4.1–1 and Table 36.4.1–2.
Table 36.4.1–1 Contact inclusions definitions.
| Contact inclusions | Input file syntax |
| Self-contact for the default all-inclusive surface specifies contact between every exterior face in the model | , |
| Contact between the default all-inclusive surface and SURFERODE specifies contact between every exterior face and SURFERODE | , SURFERODE |
| Self-contact for SURFERODE specifies self-contact between the eroding bodies | SURFERODE, |
Table 36.4.1–2 Contact inclusions definitions in Abaqus/CAE.
| Contact inclusions | Abaqus/CAE syntax |
| Self-contact for the default all-inclusive surface specifies contact between every exterior face in the model | First Surface: (All*); Second Surface: (Self) |
| Contact inclusions | Abaqus/CAE syntax |
| Contact between the default all-inclusive surface and SURFERODE specifies contact between every exterior face and SURFERODE | First Surface: (All*); Second Surface: SURFERODE |
| Self-contact for SURFERODE specifies self-contact between the eroding bodies | First Surface: SURFERODE; Second Surface: (Self) |
Alternatively, you could create a more concise definition of the same contact domain by first defining a surface named SURFALL that includes all exterior faces in the entire model and all interior faces of element set ELERODE. In this case, since all faces (exterior and interior) in the contact domain are defined in one surface, there is no need to define contact explicitly between the exterior and interior faces. It would be adequate to specify only self-contact for SURFALL.
Abaqus/Explicit automatically computes a nonzero contact thickness associated with interior faces based on element dimensions, and this default value cannot be changed via a surface property assignment.
Erosion of surfaces specified on structural elements
For structural elements, the general contact algorithm checks the underlying elements of the faces (or “contact edges” on beam and truss elements) for failure. Once the underlying element fails, the face is removed. As with solids, feature edges on structural elements are removed once all of the surrounding faces have failed. A perimeter edge (e.g., on the perimeter of a shell element mesh) is removed once the face it is connected to fails. New perimeter edges are not created to conform to the new perimeter created by the removal of a face.
Memory use
The amount of contact data used to describe the surface topology is proportional to the number of faces included in the contact domain. Including a large number of interior faces in the contact domain can potentially increase memory use significantly compared to analyses in which the contact domain is defined using only exterior faces. Consider creating a surface on a cubic mesh of C3D8R elements with n elements per side. A surface including the exterior faces of the mesh (suitable for modeling contact without element failure) would contain 6 n ^ { 2 } element faces. A surface including both exterior and interior faces of the mesh (suitable for modeling contact with element failure for every element in the mesh) would contain 6 n ^ { 3 } element faces. For large meshes the memory use can increase easily by an order of magnitude when interior element faces are included in the contact domain to model erosion. Therefore, it is recommended to include only those interior element faces in the contact domain that could possibly participate in contact.
Output
The surfaces that compose the general contact domain are available as output in addition to the contact analysis output variables.
General contact domain and component surfaces
Abaqus/Explicit generates the following internal surfaces when a general contact domain is defined:
• General_Contact_Faces_Stepk,
• General_Contact_Edges_Stepk, and
• General_Contact_Nodes_Stepk,
where k is the step number. General_Contact_Nodes_Stepk contains only nodes in the general contact domain that are not included in the other two surfaces. For example, General_Contact_Faces_Step2 would contain all surface faces (interior and exterior) that were initially included in the general contact domain for Step 2. These surfaces contain the contact faces, edges, and nodes that were included in the contact domain at the beginning of the step and are not modified to reflect surface erosion.
Abaqus/Explicit also generates the following internal surfaces associated with “component surfaces”:
• General_Contact_Faces_Stepk_Compm and
• General_Contact_Edges_Stepk_Compm,
where m is the automatically assigned “component number.” Each feature edge component surface, General_Contact_Edges_Stepk_Compm, has a subset of face edges (satisfying the feature edge criteria) of the corresponding face component surface, General_Contact_Faces_k_Compk. The face component surfaces have no nodes in common with each other.
Internal surfaces can be viewed using display groups in the Visualization module of Abaqus/CAE (see the Abaqus/CAE User’s Guide). The internal surface names used by Abaqus/Explicit should not appear in the input file.
General contact output variables
You can write the contact surface variables associated with general contact interactions to the Abaqus output database (.odb) file (see “Surface output in Abaqus/Standard and Abaqus/Explicit” in “Output to the output database,” Section 4.1.3, for more information). The available variables are contact pressure, normal contact force, frictional force, and whole surface resultant quantities (i.e., force, moment, center of pressure, and total area in contact).
Field output
The generic variables CSTRESS and CFORCE are valid field output requests for general contact in Abaqus/Explicit. If CSTRESS is requested for the general contact domain, the variable CPRESS (contact pressure) is available in the output database and can be contoured in Abaqus/CAE. If CFORCE is requested for the general contact domain, the variables CNORMF (normal contact force) and CSHEARF (shear contact force) are available in the output database and can be plotted as vectors in a symbol plot in Abaqus/CAE.
For general contact CPRESS is calculated as the magnitude of the net contact normal force (the CNORMF vector) per unit area (it is an unsigned value). This convention for reporting contact pressure
is different from the convention used for contact pairs. The direction of action of the net contact pressure for general contact can be determined by examining a plot of CNORMF.
CNORMF and CSHEARF are resultant force quantities. If a double-sided surface is contacted on both sides, the resultant force is a vector sum of the force from each side of the surface (for example, the contact normal force will be zero for a double-sided surface that is pinched with equal and opposite forces on each side of the surface).
Displacement field output (U) for the entire model is written to the output database automatically when any of the contact field output variables are requested.
Several output variables associated with quantities computed at slave nodes or edge nodes are also available, with generic output variable names CDISP, CSLIPR, and CTANDIR. These output variables are not available for Eulerian-Lagrangian contact or contact involving particles. If these generic output variables names are requested, the specific output variables written as field output are as follows:
• Contact “displacements” (opening distance and accumulated slips) CDISP: COPEN, CSLIPEQ, CSLIP1, and CSLIP2;
• Contact slip rates CSLIPR: CSLIPRMAG, CSLIPR1, and CSLIPR2;
• Contact tangent directions CTANDIR: CTANDIR1, and CTANDIR2.
COPEN is reported only for slave or edge nodes in contact or very close to being in contact. The accumulated slip variables remain constant when a node is out of contact. The slip rate and tangent direction output variables are reported only for slave or edge nodes in contact. CSLIPEQ represents the total slip length at a slave or edge node while in contact. Incremental contributions to CSLIP1 and CSLIP2 are computed as the scalar product of the incremental relative nodal displacement vector and the respective local tangent direction, \mathbf { t } _ { 1 } (CTANDIR1) or \mathbf { t } _ { 2 } (CTANDIR2).
The algorithm used to establish and evolve local tangent directions for general contact is described in “Local tangent directions for contact” in “Contact formulation for general contact in Abaqus/Explicit,” Section 38.2.1. As local tangent directions for contact evolve across increments, previously accumulated slip components are resolved into the new local system before incremental contributions are added to them.
History output
Several whole surface contact force-derived variables are available as history output. You can specify the surface from which the contact force resultants will be calculated.
Force distributions on the surface due to general contact are used to calculate the surface force resultants; forces due to contact pair interactions are not included and must be output separately. The contact state of a surface is output as a set of force (CFN, CFS, and CFT) and moment (CMN, CMS, and CMT) resultants with respect to the origin. Additional variables give the center of force (XN, XS, and XT) on the surface (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). The last letter of each variable name denotes which contact force distribution on the surface is used to calculate the resultant: the letter N denotes that the normal contact forces are used to derive the resultant quantity; the letter S denotes that the shear contact forces are used to derive the resultant quantity; and the letter T denotes that the sum of the normal and shear contact forces are used to derive the resultant quantity.
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.
The total area in contact at a given time can be requested using output variable CAREA, defined as the sum of all the facets where there is contact force. The contact area reported by CAREA is generally slightly larger than the true contact area for reasonably meshed contact surfaces; therefore, interpretation of CAREA should be done with care. The discrepancy between the CAREA output and the true contact area decreases as the mesh density increases. Using contact inclusions or exclusions to limit CAREA output to smaller contact surfaces may also reduce the discrepancy in some cases. Since the CAREA output is an approximation of the true contact area, deriving force or stress values using this output may not yield accurate values; requesting contact force and stress directly is the most appropriate way to obtain accurate results.
Requesting element output when modeling surface erosion
When modeling the erosion of surfaces, it is useful to request additional element field output of the element status (output variable STATUS). Failed elements (with an element status of zero) can then be excluded from the display group in the Visualization module of Abaqus/CAE so that the active contact surface can be identified and contact results on the active contact surface can be viewed.
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 where surfaces are opened by more than a small amount compared to surface facet dimensions. You can extend the range for which Abaqus/Explicit 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.