10.2. Modeling a Shell-Solid Assembly

The 3-D shell-solid assembly provides a transition from a shell element region to a solid element region. This approach is useful when local modeling requires a full three-dimensional model with a relatively fine mesh, but other parts of the structure can be represented by shell elements (see Figure 10.1: Example of Shell-Solid Assembly). No alignment is required between the solid element mesh and the shell element mesh. The contact surface or edge must be built on the shell element side. The target surface must be built on the solid elements side.

Figure 10.1:  Example of Shell-Solid Assembly

Example of Shell-Solid Assembly

To define a shell-solid assembly using the internal MPC approach, you must set the following key options on the contact elements:

KEYOPT(2) = 2MPC-based approach
KEYOPT(12) = 5 or 6Bonded always or bonded initial
KEYOPT(4) = 1 or 2 Nodal detection for CONTA171, CONTA172, CONTA173, CONTA174 [1]
KEYOPT(4) = 0 or 1Contact normal direction for CONTA175
  1. The surface projection based method for contact detection (KEYOPT(4) = 3) is usually not suitable for modeling shell-solid assemblies.

The following real constants are also used: ICONT, FTOL, PINB, CNOF, PMAX, PMIN, TOLS.

The following key options are ignored: KEYOPT(8), KEYOPT(10), KEYOPT(1) > 0.

In most cases, the program automatically constrains both translational and rotational degrees of freedom for a shell-solid assembly (see Figure 10.2: Shell-Solid Assembly (Original Mesh)). However, you can use KEYOPT(5) of the target element (TARGE170) to explicitly define the type of constraint:

KEYOPT(5) = 0 - Auto constraint type detection (default). Based on the underlying element type, this option automatically identifies the appropriate constraint type and internally sets KEYOPT(5) to the appropriate value: KEYOPT(5) = 1 for a solid-solid assembly; KEYOPT(5) = 2 for a shell-shell assembly; KEYOPT(5) = 3 for a shell-solid assembly.
KEYOPT(5) = 1 - Projected constraint if an intersection is found from the contact normal to the target surface. Only translational DOFs are included in the constraint set.
KEYOPT(5) = 2 - Projected constraint if an intersection is found from the contact normal to the target surface. Both translational and rotational DOFs are included in the constraint set in an uncoupled manner.
KEYOPT(5) = 3 - Force-distributed constraint. Constraint equations are built if an intersection is found from the contact normal to the target surface. Both translational and rotational DOFs are constrained on shell nodes; only translational DOFs are constrained on solid nodes (see Figure 10.3: Shell-Solid Assembly with Force-Distributed Constraint, Normal Projection Option).
KEYOPT(5) = 4 - Force-distributed constraint, all directions. This option acts the same as KEYOPT(5) = 3 if an intersection is found from the contact normal to the target surface. Otherwise, constraint equations are still built as long as contact nodes and target segments are inside the pinball region. (See Figure 10.4: Force-Distributed Constraint - No Intersection (use KEYOPT(5) = 4 or 5) later in this section.)
KEYOPT(5) = 5 - Force-distributed constraint, anywhere inside the pinball region. Constraint equations are always built as long as contact node(s) and target segments are inside the pinball region, regardless of whether an intersection exists between the contact normal and the target surface. (See Figure 10.4: Force-Distributed Constraint - No Intersection (use KEYOPT(5) = 4 or 5) later in this section.)

Figure 10.2:  Shell-Solid Assembly (Original Mesh)

Shell-Solid Assembly (Original Mesh)

Figure 10.3:  Shell-Solid Assembly with Force-Distributed Constraint, Normal Projection Option

Shell-Solid Assembly with Force-Distributed Constraint, Normal Projection Option

For the normal projection only option (KEYOPT(5) = 3 on TARGE170), the program automatically creates an internal set of force-distributed constraints (similar to the RBE3 command) between nodes on the shell edges and nodes on the solid surface. The program uses the pinball region (PINB), initial adjustment zone (ICONT), and influence distance (FTOLN) to determine which nodes on the shell edge will be constrained with which nodes on the solid surface. Each shell node acts as the master node, and associated solid nodes act as slave nodes.

For the bonded always option (KEYOPT(12) = 5), any shell node that lies inside the pinball region (PINB) will be included in the constraint 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 value may be used to prevent any false contact. The default for PINB is 0.25 (25% of the contact depth) for small deformation analysis (NLGEOM,OFF), and 0.5 (50% of the contact depth) for large deformation analysis (NLGEOM,ON). (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 the shell nodes that initially lie inside the adjustment zone (ICONT) are included in the constraint sets. Shell nodes that lie outside ICONT are not constrained with the solid nodes. The default for ICONT is 0.05 (5% of the contact depth).

The influence distance (FTOLN) is used for the normal projection only option (KEYOPT(5) =3 on TARGE170). Each solid node is included in the constraint set if the perpendicular distance from the solid node to any shell edge is smaller than the influence distance. FTOLN defaults to half the thickness of the shell. A positive FTOLN value represents a scaling factor on the shell half-thickness, and a negative value represents an absolute distance value.

A shell-solid assembly can be used in a substructure analysis. However, if a superelement is defined to represent the shell elements, shell thickness is unknown in the use pass. In this case, you must overwrite the default setting of FTOLN (originally a factor of the shell thickness) to account for the zero thickness of the superelement. Input an absolute value for FTOLN (that is, input a negative value) to capture all constrained nodes when the constraint equations are built.

The KEYOPT(5) = 4 option (force-distributed constraint, all directions) can be used for the case when the shell node does not overlap or intersect the contact surface (see figure below). However, if any intersection is detected from the contact normal to the target surface, this option may not be the best choice because it only builds very localized constraints between the shell node and the target segment which is intersected. The same is always true for KEYOPT(5) = 3.

The KEYOPT(5) = 5 option (force-distributed, anywhere inside pinball) is the recommended constraint type because constraint equations are always built between a shell node and all target segments which are inside the pinball region, regardless of the contact normal and contact intersection. Thus, the pinball size is important since a larger pinball will result in a larger constraint set. This option is useful when you wish to completely constrain one contact side to another. The stresses are more evenly distributed at the shell-solid interface for this option than they would be for other constraint types.

Figure 10.4:  Force-Distributed Constraint - No Intersection (use KEYOPT(5) = 4 or 5)

Force-Distributed Constraint - No Intersection (use KEYOPT(5) = 4 or 5)

Keep the following points in mind when modeling shell-solid assemblies:

Figure 10.5:  Shell-Solid Assembly with KEYOPT(5) = 1

Shell-Solid Assembly with KEYOPT(5) = 1

Figure 10.6:  Shell-Solid Assembly with KEYOPT(5) = 2

Shell-Solid Assembly with KEYOPT(5) = 2


Release 18.2 - © ANSYS, Inc. All rights reserved.