Use the Ansys-Adams Interface whenever you want to include flexibility of a body in an Adams simulation. Flexibility can be an important aspect in a multibody system, for example, to recognize resonances or to accurately simulate forces and movements of the components. Often, the flexibility of a system is not negligible. A typical example is the model of a piston moving in an engine. The movement of the piston significantly depends on the flexibility of the crankshaft and/or the connecting rod. Because the geometry of a connecting rod can be complex, the Ansys-Adams Interface can be used to account for the connecting rod flexibility.
To use the Ansys-Adams Interface, you first model a flexible component using standard commands. While building the model, you must give special attention to modeling interface points where joints will be defined in Adams. The next step is to use the Ansys-Adams Interface to write a modal neutral file (Jobname.MNF) that contains the flexibility information for the component. This file is written in the format required by Adams/Flex, an add-on module available for Adams. See Exporting to Adams for details on how to use the Ansys-Adams Interface to create the .mnf file. For a complete description of the method used to create the modal neutral file and the information it contains, see The Modal Neutral File.
After performing the dynamic simulation in Adams, you can use the export capabilities of Adams to create an input file containing accelerations and rotational velocities of the rigid part and forces acting in the joints of the component. You can then import the file to perform a stress analysis. See Transferring Loads from Adams for details on how to import the loads and perform a subsequent static structural analysis.
The process for transferring flexible components to Adams and forces back to Mechanical APDL consists of these general steps:
Export to Adams (and create the modal neutral file).
Run the Adams simulation using the modal neutral file.
Transfer resulting loads from Adams to Mechanical APDL and perform a static analysis.
For more information and an example analysis, see Methodology Behind the Ansys-Adams Interface and Example Rigid-Body Dynamic Analysis.
To use the Ansys-Adams Interface, you must first create a complete finite element model in Mechanical APDL.
When building your model, consider that:
The interface is designed to support most element types that have displacement degrees of freedom. Exceptions are axisymmetric elements (for example, PLANE25).
Only linear behavior is allowed in the model. If you specify nonlinear elements, they are treated as linear. For example, if you include nonlinear springs (like COMBIN39), their stiffnesses are calculated based on their initial status and never change.
Material properties can be linear, isotropic or orthotropic, constant or temperature-dependent. You must define both Young's modulus (EX, or stiffness in some form) and density (DENS, or mass in some form) for the analysis. Nonlinear properties are ignored.
Damping is ignored when the interface computes the modal neutral file (Jobname.mnf). Damping of the flexible component can be added later in the Adams program.
The Adams program requires a lumped mass approach (LUMPM,ON). This requirement results in the following special considerations.
For most structures that have a reasonably fine mesh, this approximation is acceptable. If a model has a coarse mesh, the inertia properties may have errors. To determine what the effect will be, start a modal analysis with and without LUMPM,ON and compare the frequencies.
When using SHELL181, set KEYOPT(3) = 2 to activate a more realistic in-plane rotational stiffness. SHELL181 KEYOPT(3) = 2 is also a good choice if the elements are warped.
When using two dimensional elements, the corresponding Adams model must lie in the X-Y-plane. Remember that Adams models are always three dimensional. The 2D flexible component transferred will not have any component in the Z-direction.
Nodes of a plane element only have two degrees of freedom: translations in the X- and Y-direction. Thus, no moment loads (forces, joints) can be applied in the Adams analysis. Likewise, nodes of a solid element only have translational degrees of freedom.
You cannot apply constraints (D command) to the model. Also, make sure that no master degrees of freedom (M command) were defined in an earlier analysis.