If the effects of inertia, damping, and transient loading are significant, then a nonlinear transient analysis should be used. Additionally, “quasi-static” models that undergo buckling or other instable loading conditions will often converge better in a nonlinear transient analysis due to the inertia effects keeping the model stable.
A nonlinear transient analysis requires both dynamic and nonlinear setup steps. Autodesk Inventor Nastran solves both analyses essentially simultaneously, making it one of the most complex yet exciting solution types in FEA.
An important element to having a stable nonlinear transient (NLT) solution is to provide damping in the model. There are two types of damping that can be applied in NLT solutions:
- Global damping value: specified using a PARAM,G followed by a PARAM,W3 which defines the frequency at which to apply the damping (see the Dampings topic in the User’s Guide for more detailed information on damping).
- Material based damping: which is defined on each material card directly. PARAM,W4 is needed to define the frequency at which to apply the material based damping. Note that the units of W3 and W4 are radians per unit time.
The increased flexibility of material based damping (i.e., different damping values can be applied to different areas/materials of the model) makes it the logical choice for NLT analysis.
A note of caution when using damping in a NLT solution is that for models where the velocity/inertia is the main driver of the analysis such as in an impact solution, damping can have a significant effect on the acceleration/velocity/displacement of the model. This is because the solver cannot make a distinction between rigid body motion/velocity, and flexible motion/velocity, so the damping is applied to any part of the structure that has a velocity. For impact analysis it is recommended to use no damping or a small “stability” damping value (i.e., 1.E-6). The Solve Impact Analysis topic in the User’s Guide contains additional information about impact analysis.
Impact Analysis
There are a few guidelines to follow when performing an impact analysis that will have a large effect on solution time and quality of the results.
Understanding the Normal Modes of the Structure
This is a very important and often overlooked stage. You need to know the linear response characteristics of the structure to get some idea of what the actual nonlinear frequencies and mode shapes are going to be. It can never be an exact representation, but it gets you in the right ball park for several key input parameters:
- Frequency range of interest
- Size of time step
- Duration of analysis
Constrain (fully fixed) the area of the model that you expect to make contact with the ground (or other impactor) and run a normal modes solution with ~20 modes. Look at the mode shapes and find the mode you would consider to be the “dominate” response of the structure during/after impact. A look at the modal effective mass table in the *.OUT file may also help determine the critical mode. The frequency of the mode can be used to calculate the key input parameters above:
- Frequency range of interest – This would be the frequency of the dominant mode.
- Size of time step – This can be calculated using 1/f, and then assuming 100 data points per cycle would net: dt = 1/ (100*f).
- Duration of analysis – This largely depends upon the velocity of the impact, the size of the model, and the flexibility of the model. A good estimate is to run the analysis for 2-5 cycles.
Positioning the Model
In most situations it is best to perform a hand calculation to find the velocity at impact and then start the two models near each other. This approach will net shorter analysis times, and better fidelity than starting the two bodies at a physical distance (i.e., as in a drop test). A good method for calculating the small separation distance is to use the equation:
d = v * (2*dt)
where:
d = separation distance
v = velocity
dt = time increment
This separation distance will allow for the solution of 2 time steps before impact.
Multiple Subcases
When pre/post-impact behavior is desired, using multiple subcases is a good way to fine-tune the analysis such that detailed time stepping can be used during impact, and a much coarser time-step can be used after impact.
Automated Impact Analysis (AIA)
Autodesk Inventor Nastran features an automated impact analysis solution type that automatically does the steps mentioned in the above Impact Analysis section. The AIA solution type is activated via the IMPACTGENERATE Case Control card (see the Autodesk Nastran Reference Manual located in the Inventor Nastran install directory for more info on the IMPACTGENERATE card). The solver will automatically execute the following steps to perform the AIA analysis:
- Drop Distance and Final Velocity – Nastran AIA will calculate the distance the object will travel up to the point where contact is made, automatically repositioning the projectile.
- Automated Surface Contact Generation – Nastran AIA seeks contacting mesh surfaces and creates contact between the two bodies.
- Vibration Characteristics – The natural frequencies of both the dropped object and the target are assessed at the point where they are just in contact and the dominant frequencies are identified.
- Impact Duration and Time Steps – Both the impact duration and the time step can be assessed from the characteristic mode being excited in the impact.
- User Input – Define the starting position of the projectile or drop object, the initial velocity, and the acceleration on the Impact Analysis dialog box, as shown in the Solve Impact Analysis topic in the User’s Guide.
- The analysis is solved as a nonlinear transient solution using all the data gathered above.
|
Previous Topic: Flat Walled Tank Exercise |
Next Topic: Ball Impact Exercise |