To define solid-solid or shell-shell assemblies using the internal MPC approach, you must set the following key options on the contact elements:
| KEYOPT(2) = 2 | MPC based approach |
| KEYOPT(12) = 4, 5, or 6 | No separation (see note below), bonded always, or bonded initial |
| KEYOPT(4) = 1, 2, or 3 | Nodal detection or surface projection based method for CONTA172 and CONTA174 |
| KEYOPT(4) = 0 or 1 | Contact normal direction for CONTA175 |
Note: When used with the MPC approach, the no separation option (KEYOPT(12) = 4) is only valid for modeling solid-solid assemblies that represent a slider line or slider plane.
The following key options are ignored: KEYOPT(8) (it is always set to 2 internally), KEYOPT(10).
The following real constants are used: R1, R2, ICONT, PINB, CNOF, TOLS. All other real constants are ignored.
The contact surface must be defined on the deformable bodies, and the target surface must be defined on either deformable or rigid bodies in the contact pair. In order to prevent overconstraint, only asymmetric contact is supported. If symmetric pairs are defined, the program automatically selects one pair and ignores the other pair (acting as KEYOPT(8) = 2). The self-contact pair definition is not supported.
The following topics related to modeling solid-solid and shell-shell assemblies are available:
The nodal detection method (KEYOPT(4) = 1) and the surface projection based method (KEYOPT(4) = 3 or 4) are well suited for contact pairs in which the contact surface normal direction is nearly opposite to the target surface normal direction. These methods, however, should not be used when the projection along the contact normal does not intersect the target surface. KEYOPT(4) = 2 can be used for all cases, regardless of the normal directions. This option is also well suited for the case when the contact normal direction is nearly perpendicular to the target normal direction.
The surface projection based method (KEYOPT(4) = 3 or 4) enforces contact constraints on the overlapping area of contact and target elements in an average sense, rather than on each contact node as the other nodal detection methods do (KEYOPT(4) = 1 and 2). Therefore, each internal constraint equation due to the projection based method can involve multiple contact nodes and target nodes. In general, this method provides much more accurate and smoother stress distributions near the contact interface involving dissimilar meshes than the other contact detection options. This holds true even more so for higher order elements involved in contact. However, the projection based method may significantly increase computational cost when the target element meshes are much more refined than the contact element meshes. To resolve this performance issue, you should flip the contact and target surfaces.
Note: For MPC bonded contact, the program internally switches to the dual shape function option (KEYOPT(4) = 4) if the standard projection option (KEYOPT(4) = 3) is defined.
When the contact node does not exactly lie on the target surface (that is, offsets exist), using the projection based method for a solid-solid assembly may not represent rigid-body rotation correctly. To ensure the correct behavior for rigid-body rotation, you can move the contact nodes onto the target surface by issuing CNCHECK,ADJUST/MORPH at the beginning of the analysis.
For the bonded always option (KEYOPT(12) = 5) and no separation option (KEYOPT(12) = 4), any contact node that lies inside the pinball region (PINB) can be the constrained node in the MPC definition if an intersection with the target surface is detected in the contact normal direction. This holds true at the beginning of deformation, as well as during the deformation process. A relatively small PINB may be used to prevent any false contact. When KEYOPT(12) is set to the bonded always or no separation option, PINB defaults to 0.25 (25% of the contact depth). The default PINB value may differ from what is described here if CNOF is input. See Defining the Pinball Region (PINB) for more information.
For the "bonded initial" option (KEYOPT(12) = 6), only those contact nodes that are initially in contact or have a very small gap but lie inside the adjustment zone (ICONT) are always constrained via internal MPC. Those contact nodes that are initially open will never be constrained, even though they may later penetrate into the target surface during the deformation process. In order to capture contact, you should specify proper ICONT or CNOF values. Use CNCHECK in conjunction with ICONT to move all the contact nodes that are inside the ICONT zone onto the target surface in the initial configuration, without causing any strain. When the "bonded initial" option is set and KEYOPT(5) = 0 or 4, ICONT defaults to 0.05. See Adjusting Initial Contact Conditions for more information on using KEYOPT(5), CNOF, and ICONT.
You can use KEYOPT(4) on the target element (TARGE169 or TARGE170) to control individual degrees of freedom for the constraint. For example, if you are using TARGE170 elements with 3D contact elements, you might specify that only UX, UY, and ROTZ be used in the constraint. You can do this by entering a six digit value for KEYOPT(4). The first to sixth digits represent ROTZ, ROTY, ROTX, UZ, UY, UX, respectively. The number 1 (one) indicates the DOF is active, and the number 0 (zero) indicates the DOF is not active. Therefore, to specify that UX, UY, and ROTZ be used in the constraint, you would enter 100011 as the KEYOPT(4) value.
For a 3D model, you can also use KEYOPT(5) or KEYOPT(6) of the target element (TARGE170) to explicitly define the type of constraint, as described below for solid-solid (KEYOPT(5)), shell-shell (KEYOPT(5)), and 2D/2.5D-3D solid (KEYOPT(6)) assemblies.
For a solid-solid assembly (no rotational DOFs), the KEYOPT(5) = 1, and 2 settings of the target element (TARGE170) are equivalent: a projection constraint type is built if an intersection is found from the contact normal to the target surface. This function works similarly to CEINTF. The contact surface acts as "region A" nodes, and the target surface acts as "region B" elements. Note that when a gap or penetration exists, both the exterior nodes of the target surface (the target nodes) and the interior nodes of underlying elements of the target surface are included in the constraint set.
Use KEYOPT(5) = 3, 4, or 5 of TARGE170 to form a force-distributed constraint type (no rotational DOFs):
For KEYOPT(5) = 3, the constraint equations are built only if an intersection is found from the contact normal to the target surface.
KEYOPT(5) = 4 behaves the same as KEYTOPT(5) = 3 if an intersection is found from the contact normal to the target surface. Otherwise, constraint equations are built as long as contact nodes and target segments are inside the pinball region.
For KEYOPT(5) = 5, the constraint equations are always built as long as contact nodes and target segments are inside the pinball region, regardless of whether an intersection exists between the contact normal and the target surface. KEYOPT(5) = 5 is useful when the contact surface partially overlaps with the target surface or when no projection is found.
Use KEYOPT(5) = 6 of TARGE170 to form a rigid link type constraint (no rotational DOFs) only if an intersection is found from the contact normal to the target surface.
For KEYOPT(5) = 7, behaves the same as KEYTOPT(5) = 3 if an intersection is found from the contact normal to the target surface. Otherwise, constraint equations are built as long as contact nodes and target segments are inside the pinball region.
The default option KEYOPT(5) = 0 internally sets the appropriate constraint type for each contact constraint. The program forms a projection constraint type (as KEYOPT(5) = 1) if the initial gap or penetration is smaller than 0.001*pinball. Otherwise, it forms a force-distributed constraint type (as KEYOPT(5) = 4).
For a shell-shell assembly, set KEYOPT(5) = 1, or 2 for the target element (TARGE170) to build a projection constraint type if an intersection is found from the contact normal to the target surface. This function works similarly to CEINTF. The contact surface acts as "region A" nodes, and the target surface acts as "region B" elements. When KEYOPT(5) = 2, both translational DOFs and rotational DOFs are included in the constraint set in an uncoupled manner. Only the translational DOFs are included in the constraint set if KEYOPT(5) = 1.
Use KEYOPT(5) = 3, 4, 5 of TARGE170 to form the force-distributed constraint type. This function is similar to modeling a shell-solid assembly: both translational DOFs and rotational DOFs of contact nodes and translational DOFs of target nodes are included in the constraint set in a coupled manner.
For KEYOPT(5) = 3, the constraint equations are only built if an intersection is found from the contact normal to the target surface.
KEYOPT(5) = 4 behaves the same as KEYOPT(5) = 3 if an intersection is found from the contact normal to the target surface. Otherwise, constraint equations are built as long as contact nodes and target segments are inside the pinball region.
When KEYOPT(5) = 5, the constraint equations are always built as long as contact nodes and target segments are inside the pinball region, regardless of whether an intersection exists between the contact normal and the target surface.
Use KEYOPT(5) = 6 of TARGE170 to form the rigid surface constraint type only if an intersection is found from the contact normal to the target surface. Both translational DOFs and rotational DOFs of the contact nodes and translational DOFs of the target nodes are included in the constraint set.
When KEYOPT(5) = 7, the rigid surface constraints are always built as long as contact nodes and target segments are inside the pinball region, regardless of whether an intersection exists between the contact normal and the target surface.
The default option KEYOPT(5) = 0 internally sets the appropriate constraint type for each contact constraint. The program forms a projection constraint type (as KEYOPT(5) = 2) if the initial gap or penetration is smaller than 0.001*pinball. Otherwise, it forms a force-distributed constraint type (as KEYOPT(5) = 4).
Note: When consistent target surface normals on shell elements are not feasible, you can use double-sided target surfaces. Define double-sided target surfaces on TARGE170 target elements by setting KEYOPT(8) = 1.
For a 2D or 2.5D to 3D solid assembly, set the contact element type on the 2D/2.5D side to be CONTA175 for bonded MPC, and set the target element on the 3D solid side to be TARGE170 with KEYOPT(6) = 3 which will build a projection constraint type if an intersection is found in the symmetric axis between the contact and target.
In this context, "2D element" refers to a PLANE182 or PLANE183 element with KEYOPT(3) = 1 (Axisymmetric) and "2.5D element" refers to SOLID272 or SOLID273. This type of assembly is limited to:
Cyclic on 3D solid element (CPCYC command with CEOPT = 1)
Linear analysis
Structure degrees of freedom
Note: When comparing 2D/2.5D-3D assemblies to the 3D full model, it is important to apply equivalent boundary conditions and material properties. Modal analysis and any other downstream analysis are not supported.
Keep these important points in mind when determining the type of constraint to use for the assembly:
For the 3D case, if you specify KEYOPT(4) on the target element, only the degrees of freedom that are common to both the KEYOPT(4) degree-of-freedom set and the KEYOPT(5) degree-of-freedom set will be considered in the constraint equations.
When the no separation option (KEYOPT(12) = 4 on the contact element) is used with the MPC approach to model solid-solid assemblies, only the KEYOPT(5) = 0 and 1 options (auto detection or solid-solid constraint) described above are valid. If the auto detection option is set (KEYOPT(5) = 0) and the program finds a shell-shell assembly or shell-solid assembly in this situation (contact nodes contain rotational DOFs), the solution will terminate.
If overconstraint occurs in a bonded shell-shell assembly (for example, contact is defined on both sides of a shell surface) when using the MPC algorithm, you can switch to the penalty method or the augmented Lagrangian method. See Bonded Contact for Shell-Shell Assemblies for more information.
Setting KEYOPT(5) = 2 for a shell-shell assembly constrains the rotational and translational degrees of freedom from both sides. However, the rotational and translational degrees of freedom are decoupled. This option can model situations where one shell edge lines up well with another shell surface. This provides a valid answer which is closer to a matching mesh solution.
If a certain amount of gap or penetration exists in the assembly interface, setting the KEYOPT(5) = 2 constraint option on the target element causes artificial constraints to be added, which can result in an inaccurate solution. In this case, you should use the force-distributed constraint type by setting KEYOPT(5) = 3, 4, or 5. One drawback of using the force-distributed constraint type is that the initial gap or penetration will remain during the solution (similar to setting KEYOPT(9) = 1 on the contact element).
Over-constraint often occurs when the rigid surface constraint (KEYOPT(5) = 6 or 7) is set. These two options may be used to model very localized constraints (such as on points or edges). Spot-welds and seam-welds are good use cases. With KEYOPT(5) = 6, there is only one target element (that is, a maximum 8 target nodes) associated with each contact node. However, with KEYOPT(5) = 7 in general, there is more than one target element and thus many more target nodes are associated with each contact node. The software issues an error when the total number of associated target nodes exceeds 80. You may consider reducing the pinball radius or using other types of constraint (KEYOPT(5) < 7 of target element).
To achieve smooth stress distribution on 2D/2.5D to 3D interfaces, applying similar mesh grid densities on both contact and target sides is recommended.
The MPC approach can be used for multiphysics applications as well as structural applications. The degrees of freedom specified for the contact elements via KEYOPT(1) determine the physics fields that will be considered for contact. See Multiphysics Contact for more information on multiphysics contact capabilities.
If the temperature degree of freedom is active in the model (KEYOPT(1) = 1 or 2), the program builds MPC equations not only for structural degrees of freedom, but also for the temperature DOF. In this case, the real constant TCC is ignored. If only the temperature DOF is set (KEYOPT(1) = 2) and other solution options are defined (ANTYPE,,TRANS, THOPT,QUASI, EQSLV,JCG/ICCG/PCG/SPARSE), the internal MPC approach can support fast thermal transient analysis (see Nonlinear Options in the Thermal Analysis Guide). Internal MPC equations for temperature DOF are built to support heat transfer between the two bonded surfaces.