17.3. Modeling

The bar is modeled with a 3-D coarse mesh using 495 SOLID186 elements, as shown in Figure 17.1: Geometry and FE Model of a Metal Bar Impacting a Rigid Wall.

Frictionless contact between the rigid wall and the end of the bar is modeled using TARGE170 and CONTA174 elements.

The CONTA174 elements have the following settings:

The problem uses three separate element-level time-incrementation controls (KEYOPT(7)):

The latter two time-incrementation controls (KEYOPT (7) = 3 and KEYOPT (7) = 4) activate time-step size control to capture all contact status changes.

17.3.1. Impact Scenarios

Three impact scenarios are examined. Each of these scenarios requires its own finite-element model and its own output of results of interest:

  • Rigid Impact

    The bar is modeled as a rigid body using only TARGE170 elements, with automatically constrained boundary conditions for rigid target nodes (KEYOPT (2) = 1). The target elements are located on the exterior surface of the bar which has been premeshed with SOLID186 elements.

    The program builds internal multipoint constraints between the nodes on the exterior surface of the rigid body and a pilot node located at the center of gravity. The pilot node is also shared by a 3-D point mass with rotary inertia (modeled with a MASS21 element).

    The location of the center of gravity, and the mass and moments of inertia properties for MASS21, are estimated by performing a single load step solution with the option for precalculating masses (IRLF,-1).

    For more information, see Modeling Rigid Bodies in a Multibody Analysis in the Multibody Analysis Guide.

    Before obtaining the solution, the underlying SOLID186 mesh is unselected (ESEL,U command).

  • Elastic Impact

    The bar is modeled as a flexible body with linear elastic material properties.

  • Elastoplastic Impact

    The bar is modeled as a flexible body with elastoplastic material properties.


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