The application interacts with motion simulation software such as Dynamic Designer™ from MSC, and MotionWorks from Solid Dynamics. This is not the motion feature that is built into the Mechanical application. For information on the motion features built into the Mechanical application, see the Rigid Dynamics Analysis and Transient Structural Analysis sections.
Motion simulation software allows you to define and analyze the motion in an assembly of bodies. One set of computed results from the motion simulation is forces and moments at the joints between the bodies in the assembly. For the procedure on inserting these load, see Inserting Motion Loads. These loads are available for static structural analyses.
Single Body Capability
is intended to work only with a single body from an assembly. If more than one body is unsuppressed in the Model during Import, you will receive an error message stating that only one body should be unsuppressed.
Frame Loads File
The application reads a text file produced by the motion simulation software. This file contains the load information for a single frame (time step) in the motion simulation. To study multiple frames, create multiple environment objects for the Model and import each frame to a separate environment. The frame loads file includes joint forces and inertial forces which "balance" the joint forces and gravity.
Inertial State
If the part of interest is a moving part in the assembly, the frame loads file gives the inertial state of the body. This includes gravitational acceleration, translational velocity and acceleration, and rotational velocity and acceleration. Of these inertial "loads" only the rotational velocity is applied in the environment. The remaining loads are accounted for by solving with inertia relief (see below).
If the part of interest is grounded (not allowed to move) in the motion simulation, corresponding supports need to be added in the environment before solving.
Joint Loads
For each joint in the motion simulation, the frame loads file reports the force data - moment, force, and 3D location - for the frame. Features are also identified so that the load can be applied to the appropriate faces, edges, or vertices within the application. These features are identified by the user in the motion simulation software before exporting the frame loads file. For all non-zero moments and forces, a corresponding "Moment" and "Remote Force" are attached to the face(s), edge(s) or vertex(ices) identified in the frame loads file.
The Remote Force takes into account the moment arm of the force applied to the joint.
Solving with Inertia Relief
Inertia relief is enabled when solving an environment with motion loads. Inertia relief balances the applied forces and moments by computing the equivalent translational and rotational velocities and accelerations. Inertia relief gives a more accurate balance than simply applying the inertia loads computed in the motion simulation.
If Weak Springs are enabled, the computed reaction forces in the weak springs should be negligible.
This option will automatically be turned on if you import any motion loads.
Note: Material properties have to be manually set to match density used in motion analysis.
Modifying Parts with Motion Loads
If you modify a part having a motion load, you should rerun the solution in the motion simulator software (for example, Dynamic Designer) and re-export the loads to the Mechanical application. Then, in the Mechanical application, you must update the geometry, delete the load (from the Environment object) and re-insert the motion load.
Modifying Loads
You can modify loads that have been inserted, but you should only do so with great care. Modifying loads in the Mechanical application after importing from the motion simulation software will nullify the original loading conditions set in the motion simulation software. Therefore, you need to examine your results in the Mechanical application carefully.
Inserting Motion Loads
You must make sure the files and data are up to date and consistent when analyzing motion loads. Use the following procedure to ensure that the correct loads are applied for a given time frame.
To insert motion loads after solving the motion simulation:
Advance the motion simulation to the frame of interest.
Export the frame loads file from the motion software.
Attach the desired geometry.
Choose any structural New Analysis type except Rigid Dynamics and Random Vibration.
Suppress all bodies except the one of interest.
Click the environment object in the tree, then right-click and select .
Select the Frame Load file that you exported from Dynamic Designer.
Click . If more than one body is unsuppressed in the Model corresponding to the environment object, you will receive an error message at the time of solution stating that only one body should be unsuppressed.
View the results.
The exported loads depend on the part geometry, the part material properties, and the part's location relative to the coordinate system in the part document. When any of these factors change, you must solve the motion simulation again by repeating the full procedure. Verify that material properties such as density are consistent in the motion simulation and in the material properties.
Insert Motion Loads is intended to work with a single body only. Results with grounded bodies (bodies not in motion in the mechanism) are not currently supported.
If an assembly feature (such as a hole) is added after Dynamic Designer generates its Joint attachments for FEA, the attachments may become invalid. These attachments can be verified by opening the Properties dialog box for a Joint and selecting the FEA tab. An invalid attachment will have a red "X" through the icon. To correct this problem, manually redefine the joint attachments using the FEA tab in the Joint Properties dialog.
A .log file is created when motion loads are imported. This troubleshooting file has the same name (with an .log extension) and file location as the load file. If the .log file already exists, it is overwritten by the new file.