Autodesk® CFD determines and adjusts the time step size (shown on the Solve dialog) if Intelligent Solution Control is enabled (which it is by default). Click the Estimate button on the Solve dialog to compute an initial time step size. To manually set the time step size, disable Intelligent Solution Control on the Solution Control dialog.
When Intelligent Solution Control is enabled, the time step for user-prescribed motion is calculated and set automatically based on the specified distance and/or velocity.
The time step for flow-driven motion is calculated automatically by initially using a value based on the surrounding flow velocity and/or the initial velocity of the object. As the object accelerates, the time step will automatically decrease to satisfy the basic criterion that an object in motion should not move through more than one element per time step. Adjusting the time step in this way has been shown to balance calculation efficiency with solution accuracy.
Intelligent Solution Control automatically adjusts under-relaxation parameters to remove instabilities from the calculation. Tests have shown that this does not appreciably affect the time accuracy of the solution, and that is improves solution stability.
Motion analyses are always run transient. When a motion is assigned to a part, certain solution settings are automatically set:
We have found that for some Solid Motion analyses, the presence of Mesh Enhancement can cause stability problems during the analysis. Because it is disabled, additional care should be taken when defining the mesh size to ensure that the mesh density is adequate for the flow.
Setting the time step save interval and the number of times steps are left to the user. Be careful not to set a save interval that fills the hard disk with time step results sets.
As an object moves through a fluid, the space that was once occupied by the object is converted to a fluid. With this in mind, it is recommended that when applying slip conditions to a symmetry wall that cuts through a moving solid, that they be applied to the surface of the object that will become a fluid boundary after the solid has moved away. Not applying a slip condition to the surface of the solid (at its starting location) will result in a wall surface within the slip plane.
In most devices with a moving solid, there will be regions of fluid that are isolated from other regions during some point in the movement. An incompressible fluid will not allow pressure waves to travel throughout the medium, and may cause solution instabilities. Additionally, objects that are to move due to flow-induced forces may not move at all. For this reason, the use of compressibility is recommended for flow-induced motion analyses.
Enable Compressible in the Solve dialog. For liquids and gases, this will cause pressure waves to move throughout the device, and will produce a much more realistic solution for flow-induced motion.
If Intelligent Solution Control is not used, then it is recommended to apply convergence controls to pressure on the Solution Controls dialog. Use of a value of 0.25 for pressure helps stability, and will damp out noise from the calculation.
Use the default advection scheme, ADV1. The flux-based advection scheme, ADV3, cannot be used for a motion analysis.
Due to the organization of motion data, it is not generally possible to continue a motion analysis from existing results if changes have been made to the mesh, boundary conditions, or motion parameters. If settings of a motion analysis are modified and the analysis continued from a saved time step, a warning will be given, and the analysis will be prevented from continuing. In particular, Motion changes that cannot be made mid-run include:
To stop a part with a user-prescribed motion from moving part-way through an analysis, either construct a motion table so that after a certain time its displacement does not change (or its velocity is 0). For a flow-driven part, a part can be stopped mid-run by modifying its bounds so that it cannot move from its current location. Alternatively, modify its material density so that it is so heavy that the flow cannot continue to move it.
Obviously, if none of the changes described above are made to the Motion analysis, the solution can be stopped and continued.
There are some parameters, however, that can be changed mid-run, and the analysis made to continue:
For every moving solid, a table is produced that contains a time history of the linear and angular velocity, linear and angular displacement, force and torque. Open this table by clicking Results > Review > Motion Results.
The linear and angular displacement values are relative to the initial position of the object as specified using the Initial Position slider on the Motion task dialog. Pay particular attention to this if the initial position differs from the as-built location in the CAD model.
This data is also written to an external “.csv” file. The file name is the scenario name with the word motion appended to it. For example, the motion file for a scenario called Scenario 1 that contains a moving solid called Product is called Scenario 1_PRODUCT_1_motion.csv. This file is located in the scenario sub-folder of the design study directory structure.
Note that the force and torque values are the net values, and include driving, resistance, collision, contact forces as calculated in the Motion module. The hydraulic force and torque are just the force and torque imparted on the object by the fluid, and do not include any forces specified in the motion definition. The hydraulic values are reported in the Wall dialog.
Related Topics: