–The first six modes are rigid-body modes. These are marked with “(probable rigid-body mode).” If there is a mode close to a rigid-body mode but not marked, you may deactivate it later in the ADAMS program.

–If a mode is marked with “Infinity. Possible mass singularity. Ignored,” check your model carefully. There might be a problem with the Interface points.

–The first few modes are equal to the free-free eigenmodes of the component. You might want to verify this by doing a modal analysis: Set analysis option to ANTYPE,MODAL with MODOPT,LANB (Block Lanczos); activate the lumped mass approach with LUMPM,ON.

•Review the normal modes (load step 1) and the constraint modes (load step 2) in the General Postprocessor.

•Verify the transfer by doing a modal analysis of the component in ADAMS with all interface degrees of freedom fixed. Compare the results with the normal modes calculated in Mechanical APDL (load step 1).

12.5. Running the ADAMS Simulation

After you have verified that the .MNF file contains accurate information, you are ready to run an ADAMS simulation with a flexible component. Import the .MNF file into your ADAMS model and attach it to

the rigid bodies using joints. To keep any numerical imbalance between inertia and external loads small, make sure you simulate your ADAMS model with high accuracy.

For general information about the ADAMS program and how to import flexible bodies, refer to the ADAMS manuals (provided by Mechanical Dynamics, Inc.), especially the documentation provided for the ADAMS/Flex product.

12.6. Transferring Loads from ADAMS

There are two ways to transfer loads and/or deformations from ADAMS to Mechanical APDL:

•If the component is assumed to be rigid in ADAMS, you can transfer joint and external forces, accelerations, and rotational velocity acting on the component as described in Transferring Loads on a Rigid Body (p. 321).

•If the component is flexible, you can transfer the deformed shape of the component using the MSR toolkit from ADAMS. This type of transfer is not supported by the ANSYS-ADAMS Interface. See Transferring the Loads of a Flexible Body (p. 324) for more information on this transfer method.

12.6.1. Transferring Loads on a Rigid Body

If you model your component as a rigid body in ADAMS, you can use the Export FEA Loads feature in ADAMS to export the loads to a file. This file can then be imported into Mechanical APDL for a subsequent stress analysis.

If you model your component as a flexible body, ADAMS allows you to use the Export FEA Loads feature to transfer the loads, but the loads will be incomplete. Therefore, this load transfer procedure should generally not be used for flexible bodies. The transfer of loads may work, however, if the flexible bodies experience only small dynamic effects. If this is not the case, you may want to change the component temporarily to a rigid body (using the Modify utility in ADAMS) and run another simulation before you transfer the loads.

vk.com/club152685050Rigid-Body Dynamics and the| vkANSYS.com/id446425943-ADAMS Interface

12.6.1.1. Exporting Loads in ADAMS

After performing an ADAMS simulation, you can export loads on a specific component at specific times. In ADAMS, select File> Export> FEA Loads to access the ADAMS Export FEA Loads dialog box.

Figure 12.3: ADAMS Export FEA Loads Dialog Box

Complete the following steps in this dialog box.

1.File Type: Select FEA Loads

2.File Format: Select ANSYS

3.File Name: Specify a name for the load file. The default extension is .LOD.

4.Specify whether you want to export loads on a rigid body or a flexible body.

•Rigid body: You must define a marker on the body that has the same position and orientation relative to the body as the global origin does in the Mechanical APDL model.

•Flexible body: The marker is set automatically since this information is known from the .MNF file.

5.Click on “Add Load Points to Nodes Table.”

•If you chose a rigid body, you can input the node IDs of the nodes where the loads have to be applied in Mechanical APDL.

•If you chose a flexible body, ADAMS automatically inputs the correct node IDs.

6.Output at times: Specify at what time steps you want to export the loads.

7.Finally, ADAMS will ask you about the units. The units for export must be the same as those chosen for building the Mechanical APDL model. If they are not the same, change them temporarily to the Mechanical APDL units or scale the loads in the load file later.

Every time step in ADAMS is treated as a load step in Mechanical APDL. In ADAMS versions up to 11.0.0, ADAMS writes the LSWRITE command before the load commands. Therefore, if you are using ADAMS version 11.0.0 or earlier, you must use a text editor to move the LSWRITE command to the end of each time step in the .LOD file.

The following loads will be included in the load file:

Joint forces (F command)

External forces (F command)

Accelerations and rotational velocities (ACEL, OMEGA, DOMEGA commands)

12.6.1.2. Importing Loads

After exporting the load file from ADAMS, you can use the ANSYS-ADAMS Interface to import the load file and initiate a static structural analysis. To access the Import from ADAMS dialog box, pick:

Main Menu> Solution> ADAMS Connection> Import fr ADAMS

Figure 12.4: Import from ADAMS Dialog Box

Complete the following steps in the dialog box:

1.Import file from ADAMS: Enter the name of the load file that was exported from ADAMS.

2.Import option: Theoretically, external forces and inertia forces are in equilibrium. Due to numerical errors or due to mass discrepancies between ADAMS and Mechanical APDL, this is insufficient to prevent a rigidbody motion of the component. Hence, you must constrain the component against rigid-body motion

in order to do a static structural analysis. The ANSYS-ADAMS Interface offers two import options to achieve this.

•Import loads only. The program applies inertia loads and external forces to the structure according to the load file. For this option, you must manually add constraints to the Mechanical APDL model that

are compatible with the constraints used in the ADAMS model (if possible), or use common engineering sense to prevent rigid-body motion.

•Add weak springs: The program adds weak springs (COMBIN14 elements) to the corners of the bounding box of the component. (For more information, see the WSPRINGS command documentation). The weak springs prevent rigid-body motion without influencing the stress results. (See Adding Weak Springs (p. 326) for more information on how the program adds weak springs to the model.)

3.Import button: When you pick the Import button, one load step file is written per time step exported from ADAMS; existing load step files are deleted. If you chose the “Import loads only” option, you will have to start the static solution manually by issuing the SOLVE command for each load step. If you chose