The Impact Setup facilitates drop test and projectile impact studies. Impact Setup appears in the Subcases branch of the tree when the Analysis Type is defined as Impact Analysis. Input consists simply of the direction of travel, initial velocity, and acceleration. The effective directional natural frequencies of the impacting body and target in the contact state are calculated internally. The critical time step calculations are then automatically carried out based on these responses, providing a precise initial time increment and duration of the analysis. Accurate time step prediction is essential in calculating the magnitude of peak response and maintaining an energy balance during the contact event. Optional user defined time increment and duration may be specified.
Go to the tree and right-click on Analysis; select Solve Impact Analysis-Setup Impact Analysis. The following impact analysis setup appears:
- Projectile Body: Click on the projectile body to differentiate between it and the target body.
- Projectile Translation Vector: You will need to select a sketch line that defines the direction of travel of the projectile. The geometric point of the sketch line on the projectile must be located at a node. You can use Mesh Control to ensure nodes are placed in specific points/vertices/edges. Place the geometric point of the sketch line on the target at the location of the impact.
- Initial Velocity: Define the initial velocity of the projectile. The solver is going to use the initial velocity, acceleration, and the initial separation distance (or drop height) to calculate the projectile velocity at initial impact. Initial Velocity or Acceleration or both must be specified.
- Acceleration: Define your acceleration of the projectile. The solver is going to use the initial velocity, acceleration, and the initial separation distance (or drop height) to calculate the projectile velocity at initial impact. Initial Velocity or Acceleration or both must be specified.
-
Advanced Settings:
- Contact Tolerance: Specifies the contact tolerance used in automatically generating the surface contact. The value set defines the maximum normal activation distance. A recommended value is a distance approximately 10% larger than the largest gap you want to be recognized as contact. The default AUTO setting is based on the model reference dimension multiplied by 1.0E-04. For models with high levels of curvature in contact, it is recommended to explicitly define contact tolerance.
- Large Displacements: Large displacement and follower force effects and differential stiffness. Default is on.
- Number of Modes: Number of natural frequencies calculated to provide a precise time increment and duration of analysis. Default is 30 modes.
- Extraction Method: You can select either the Lanczos or Subspace eigensolver to solve for the natural frequencies. The program picks the best method based on the RAM directive setting (Parameters-Memory Management Directives) and model size.
- Mass Representation: Selecting ON requests the generation of coupled mass matrices for elements with coupled mass capability. Selecting OFF requests the generation of diagonal mass matrices. The AUTO setting will use the coupled mass formulation when rigid elements are specified in the model.
- Dependent Term: Choose one of the following for methods to define the time step size and event duration.
- Auto: This option disables the Time Increment, Max Number of Output Steps, and Duration input fields. The solver calculates the timesteps automatically based on initial velocity/acceleration, the projectile vector, and the initial distance between the projectile and target object.
- Time Increment: Time increment for impact analysis. Calculate the Time Increment from the user-specified Duration and Max Number of Output Steps.
- Duration: Duration of the impact analysis. Calculate the Duration from the user-specified Time Increment and Max Number of Output Steps.
- Max Number of Output Steps: Maximum number of output steps generated. The Max Number of Output Steps is calculated from the user-specified Time Increment and Duration.
The remaining three options make one of the three timestep parameters dependent upon the other two. These options activate two input fields and make the third unavailable. They provide flexibility in defining the interval. Choose the calculated value (Dependent Term) and input the other two
Note: The internally calculated time increment provides very high accuracy. However, the total number of output time steps may be very large for a long duration, soft impact analysis. In such cases, you may want to limit the number of time steps (by increasing the Time Increment or decreasing the Max Number of Output Steps.
When using the Solve option, Autodesk Nastran In-CAD solves the model using the Autodesk Nastran Solver. The progress of the analysis can be seen in the Autodesk Nastran status window that is brought up automatically on a separate tab.
When using the Solve in Editor option, Autodesk Nastran In-CAD will prompt to enter a name for the input file to save to the directory of choice. After clicking Save, the model will automatically load into Autodesk Editor to begin the analysis.