ProductsAbaqus/ExplicitAbaqus/CAE Defining a contact pair interactionThe definition of a contact pair interaction in Abaqus/Explicit consists of specifying:
Defining a contact pair containing two surfacesTo define a contact pair, you must indicate which pairs of surfaces will interact with each other. The order in which the surfaces are specified is important only when a nondefault weighting factor is specified (see Contact surface weighting for details). See Element-based surface definition, Node-based surface definition, and Analytical rigid surface definition for information on defining surfaces for use in contact pairs. Input File Usage CONTACT PAIR surface_1_name, surface_2_name Abaqus/CAE Usage Interaction module: Create Interaction: Surface-to-surface contact (Explicit): select the first surface, click Surface, select the second surface Defining self-contactDefine contact between a single surface and itself by specifying only a single surface or by specifying the same surface twice. Input File Usage Use either of the following options: CONTACT PAIR surface_1, CONTACT PAIR surface_1, surface_1 Abaqus/CAE Usage Interaction module: Create Interaction: Self-contact (Explicit): select the surface or Surface-to-surface contact (Explicit): select the surface, click Surface, select the surface again Limitations with self-contactThe following limitations are enforced for a contact pair with self-contact:
Removing and adding contact pairsRemoval and addition of contact pairs:
Adding contact pairsBy default, the contact pairs specified are added to the list of active contact pairs in the model. Initial penetrations should be avoided for contact pairs introduced after the first step, as large nodal accelerations and severe element distortions can result (see Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit). Redefining a contact pair by deleting it and adding it in the same step can also lead to problems, because the “state” information associated with the slave nodes in contact will be reinitialized. For example, a penalty contact slave node with a penetration past the midsurface of a double-sided master surface would be allowed to pass through the master surface if the contact state were reinitialized. Input File Usage CONTACT PAIR, OP=ADD Abaqus/CAE Usage Interaction module: Create Interaction Removing contact pairsRemoval of contact pairs is a useful technique for simulating complicated forming processes where multiple tools will contact the same workpiece. Removing a contact pair once it is no longer needed eliminates the need to monitor the contact conditions and reduces the cost of the simulation. Input File Usage CONTACT PAIR, OP=DELETE Abaqus/CAE Usage Interaction module: interaction manager: General restrictions on surfaces used in contact pairsThe following general restrictions (in addition to those discussed in Element-based surface definition) apply to all surfaces used in contact pairs:
These restrictions do not apply to surfaces used with the general contact algorithm (About general contact in Abaqus/Explicit). The following restrictions apply to the surfaces forming a kinematic contact pair:
The following restrictions apply to the surfaces forming a penalty contact pair:
Orienting the surface's normalThe orientation of a surface's normal can be critical for the proper detection of contact between two contacting surfaces. At the point of closest proximity the normals of a single-sided master surface forming the contact pair should always point toward the slave surface. If, in the initial configuration of the model, a single-sided master surface's normal points away from its slave surface, Abaqus/Explicit will detect that the slave surface penetrates the master surface. Abaqus/Explicit will attempt to resolve this initial overclosure of the contact pair with strain-free displacements before the start of the simulation (see Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit). Abaqus/Explicit may have difficulty with the simulation if the overclosure is too severe. In most of these cases the analysis will terminate immediately, and an error message about severely distorted elements will be issued. You must give particular attention to checking that analytical rigid surfaces or single-sided surfaces created on shell, membrane, or rigid elements have the proper orientation. Surface orientation errors can often be quickly and easily detected by running a data check analysis (Abaqus/Standard and Abaqus/Explicit execution) and inspecting the deformed configuration in Abaqus/CAE. If large displacements have occurred, they may be due to an incorrect surface orientation. The proper and improper orientation of a rigid and deformable surface is shown in Figure 1. Figure 1. Example of proper and improper surface orientation with a rigid
surface.
It is not necessary for the normals of all of the underlying shell or membrane elements to have a consistent positive orientation for a double-sided surface: if possible, Abaqus/Explicit will define the surface such that its facets have consistent normals, even if the underlying elements do not have consistent normals. The facet normals will be the same as the element normals if the element normals are all consistent; otherwise, an arbitrary positive orientation is chosen for the surface. For double-sided surfaces the positive orientation is significant only with respect to the sign of the contact pressure output variable, CPRESS, as discussed in Element-based surface definition. Defining a continuous surfaceA contact pair surface cannot be made up of two or more disconnected regions. The definition of analytical rigid surfaces automatically ensures that these surfaces are continuous. However, care must be taken to define surfaces formed with elements so that they are continuous across element edges in three-dimensional models or through nodes in two-dimensional models. This continuity requirement has several implications for what constitutes a valid or invalid surface definition. In two dimensions the surface must be either a simple, nonintersecting curve with two terminal ends or a closed loop. Figure 2 shows examples of valid and invalid two-dimensional surfaces for use in contact pairs. Figure 2. Valid and invalid 2D surfaces.
In three dimensions an edge of an element face belonging to a valid surface may be either on the perimeter of the surface or shared by one other face. Two element faces forming a contact pair surface cannot be joined just at a shared node; they must be joined across a common element edge. An element edge cannot be shared by more than two surface facets. Figure 3 illustrates valid and invalid three-dimensional surfaces for use in contact pairs. Figure 3. Valid and invalid 3D surfaces.
The continuity requirement applies to both automatically generated free surfaces and surfaces defined with element face identifiers (see Element-based surface definition). Figure 4 shows an automatically generated free surface resulting from the specification of an element set consisting of two disjointed groups of elements. The resulting surface is not continuous since it is composed of two disjoint open curves. Figure 4. Automatic free surface generation.
Restrictions for two-dimensional contact simulationsThe following restrictions apply when defining a contact simulation for two-dimensional (planar) or axisymmetric problems:
Limitations in contact simulations with three-dimensional beam and truss elementsElement-based surfaces cannot be formed on three-dimensional beam or truss elements, so node-based surfaces must be used to define a surface on these elements. Because a node-based surface must be used, a surface on three-dimensional beam or truss elements must always form the slave surface in a pure master-slave contact pair. Therefore, it is not possible to have two three-dimensional beam or truss structures contact each other. OutputYou can write the contact surface variables associated with the interaction of contact pairs to the Abaqus output database (.odb) file. The surface variables for a mechanical contact analysis include contact pressure and force, frictional shear stress and force, relative tangential motion (slip) of the surfaces during contact, whole surface resultant quantities (i.e., force, moment, center of pressure, and total area in contact), the status of bonded nodes, and the maximum torque transmitted about the z-axis of axisymmetric elements. Additional discussion on requesting contact surface output can be found in Surface output in Abaqus/Standard and Abaqus/Explicit. Output from thermal interactions is discussed in Thermal contact properties. Field outputThe generic variables CSTRESS, CFORCE, FSLIP, and FSLIPR are valid field output requests for Abaqus/Explicit. If CSTRESS is requested for a contact pair, the variables CPRESS (contact pressure), CSHEAR1 (contact traction in the local 1-direction), and, if the contact interaction is three-dimensional, CSHEAR2 (contact traction in the local 2-direction) can be contoured in Abaqus/CAE for each discrete (i.e., non-analytical) surface in a contact pair. Contours of contact pressure (CPRESS) on surfaces used with the contact pair algorithm will be displayed using the convention that a positive pressure represents compressive contact on the positive side of the surface. The positive side of the surface can be determined by drawing the surface normals in the Visualization module of Abaqus/CAE. Following this convention, the sign of CPRESS will be reversed for contact on the negative (back) side of a double-sided surface, so negative values of CPRESS may be seen if contact occurs on the back side of a double-sided surface. If contact from separate contact pairs occurs on both sides of the double-sided surface at the same point, the value of CPRESS is given for each contact pair separately. If CFORCE is requested for a contact pair, the variables CNORMF (normal contact force) and CSHEARF (shear contact force) can be plotted as vectors in a symbol plot in Abaqus/CAE for each discrete (i.e., non-analytical) surface in a contact pair. If FSLIPR is requested, FSLIPR (the magnitude of the slip rate for slave nodes in contact) can be contoured in Abaqus/CAE for each slave surface in a contact pair. In addition, for three-dimensional contact interactions involving an analytical rigid surface and for all two-dimensional contact interactions, components of net slip rate based on local tangent directions (FSLIPR1 and, in three dimensions, FSLIPR2) can also be contoured in Abaqus/CAE for each slave surface in a contact pair if FSLIPR is requested. All of the slip rate variables associated with FSLIPR are zero whenever a slave node is not in contact. If FSLIP is requested, FSLIPEQ (the length of the overall slip path for a slave node while it is in contact) can be contoured in Abaqus/CAE for each slave surface in a contact pair. In addition, for three-dimensional contact interactions involving an analytical rigid surface and for all two-dimensional contact interactions, components of net slip (FSLIP1 and, in three dimensions, FSLIP2) can also be contoured in Abaqus/CAE for each slave surface in a contact pair if FSLIP is requested. These slip variables are equivalent to the slip rate variables integrated over time: FSLIPEQ, FSLIP1, and FSLIP2 are equivalent to FSLIPR, FSLIPR1, and FSLIPR2 integrated over time, respectively. Therefore, these slip variables account only for relative motions that occur while slave nodes are in contact. The algorithm used to establish and evolve local tangent directions for contact pairs is described in Local tangent directions for contact. Unlike general contact, previously accumulated slip components for contact pairs, FSLIP1 and FSLIP2, are not resolved into the new local system before incremental contributions are added to them. 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. History outputSeveral whole surface contact variables are available as history output. These variables record the contact state of a surface 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 pressure (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 (except the variable CAREA) 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. These history output variables will be written twice to the output database once for each surface involved in the contact pair. 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. Detailed history output on the status of bonded surfaces is available from an Abaqus/Explicit simulation. Details can be found in Breakable bonds. Obtaining the maximum torque that can be transmitted about the z-axis in an axisymmetric analysisWhen modeling surface-based contact with axisymmetric (CAX) elements, Abaqus/Explicit can calculate the maximum torque (output variable CTRQ) that can be transmitted about the z-axis. The maximum torque, T, is defined as 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. |