Hello and welcome to this video!
When a system is excited by a sudden, non-periodic excitation, transient vibrations will usually arise.
Such oscillations occur at the system's natural frequencies, with the amplitude varying in a manner depending on the type of excitation.
A baseball bat or cricket bat striking a ball, non-destructive testing methods, vibration measurement techniques, and the response of a building during an earthquake are all examples of transient vibrations.
The mode-superposition method is an efficient way to predict a structure's response to these types of loadings.
It can be used to answer questions such as, “What will be the response's peak amplitude?”, “When will it occur?”, and “How long does it take for the response to decay?”
In this session, we’ll look at how to solve such scenarios using mode-superposition transient analyses with Ansys Mechanical.
We begin with a brief lecture then proceed to a workshop example using a baseball bat with an impulsive load.
Ready? Let’s get started.
In many practical situations, dynamic excitation is neither harmonic nor periodic.
Such non-periodic excitations are often referred to as transient excitations that can vary arbitrarily with respect to time, and these must be solved in the time domain instead of the frequency domain.
Simulating the transient response of a structure can be computationally expensive when solving the typical finite element matrices, also known as using the “full method.”
The mode superposition method, on the other hand known as “MSUP” for short, provides a much more efficient approach.
The MSUP Method rearranges the equations of motion to modal coordinates,
so the solver uses the natural frequencies and mode shapes from the modal analysis to calculate the response in the time domain.
We end up with far fewer degrees of freedom, and the equations are uncoupled, so it becomes trivial for the solver to calculate the transient response.
However, we do need to keep in mind some limitations, including the fact that any source of nonlinearities cannot be included,
constant time steps must be used, and the numerical accuracy is influenced by the number of modes we use.
Typically, the ratio of effective mass to total mass should be greater than 0.9 in the Modal Solution to yield accurate results.
Although the MSUP method is applicable to any type of load with a typically short time-history duration, we will use an impulse load for the purpose of this lesson to demonstrate its usage.
Before learning about the impulse response, let us first briefly understand what an impulse load is.
An impulse load can be considered as an excitation whose magnitude increases from zero to a very high value and reduces to zero value again within a very small interval of time.
In analyses involving short-duration excitations like an impulse, shock, and impact loads, it is essential to begin with the time-history of a quantity that describes a motion or force.
It allows the inclusion of most of the typical types of loads like body accelerations such as gravity, discrete forces, including remote and nodal force and moments, as well as distributed pressures.
Since the solution is conducted in generalized coordinates, displacement and acceleration loads are valid only when applied as base excitation at the support location.
Inputs are excitations consisting of loads that are a function of time, and they can be defined as
a) constant over that time b) based upon closed-form mathematical functions like trigonometric or algebraic to simulate the half-sine or sawtooth excitation,
c) the loads can even vary according to the values input in the tabular data which can be entered directly or even imported or copy and pasted.
These values can be step-applied which means that the values applied at the first sub step jump suddenly and stay constant for the rest of the analysis.
For example, to account for the acceleration due to gravity, standard earth gravity is step-applied.
Or they can be ramped, which implies that the values applied at the first sub step increase linearly at each sub step like a triangular waveform as input.
Now let’s now get into our workshop model. For this workshop, we will simulate a hollow aluminum baseball bat being impacted by a ball.
We won’t model the ball impacting the bat, but rather, we will specify an impulse load onto a small patch on the surface of bat.
From literature, it can be found that the force time history is characterized by this ½ of the sine squared function and illustrated by this graph.
The complete time of impact is 7e-4 seconds, or just under 1 millisecond.
We assume a Max force of 5,000 Newtons although this could vary, depending on the speed of the swing among other variables.
Our force equation is now 5000*sin2(omega*t) where omega = frequency*2*pi or 1/period*2*pi
In this case since our impulse is ½ of a sin wave, then the period is actually 2*7e-4 or 1.4 milliseconds.
The resulting equation is shown here. Let’s now get started in Ansys Mechanical.
Drag and Drop a Modal system onto project page.
Right mouse click on geometry and select baseball bat.scdoc
Double click on Model cell to open mechanical.
Change the units to mm, kg, N, s Click on the Materials branch.
Search for Aluminum Alloy,
pick the plus sign to add to the project.
Click on baseball ball in the tree and change assignment to Aluminum Alloy
Highlight all 4 surfaces of the bat and specify a thickness of 2.5mm
Click on the modal branch Select the surface where the hands will hold the bat
Right mouse click and insert remote displacement Confirm the behavior to be deformable.
This allows the mesh to deform locally, while enforcing the specified displacements on that face in an averaged sense.
Specify zero for all DOFs to hold the remote point of that remote displacement in all 6 DOFs.
Under analysis settings, change the max modes to find to 24. Recall that using too few modes for the transient analysis may result in some inaccuracies due to modal truncation.
Solve the model Left click in the tabular data as shown
Right click and pick Create Mode Shape Results Right click and evaluate all results.
Click on the first mode and animate the results to see the mode shape. Feel free to repeat this for other modes to get a sense of the natural frequencies and mode shapes.
Now let’s setup the MSUP transient In Home tab, pick analysis, then transient structural
In initial conditions, pick modal. This tells mechanical that the modal solution results will be used which is a requirement for the MSUP transient
In Analysis Settings, change number of steps to 2. This will enable some capabilities related to the duration of the loading that will be specified in a moment.
For the first step, set the step end to .0007, this coincides with the end time of the impulse loading.
Set the time step size to 1e-4, which is small enough to resolve the higher frequency transient response. It is also small enough to properly apply the impulse load.
If the time step is too large, the step will not capture the sharp peaks in short duration transient impulse load and the results will be inaccurate.
Under damping controls, specify a damping ratio of 2% Now change the current step number to 2.
Set the step end time to .05 This will be the total duration of the transient simulation
Set the Time step to 1e-4, again to be able to properly resolve the transient response.
If the time step is too large, then we will end up with sampling error, which is evident when a decaying sinusoidal response looks sharp and uneven.
In the output controls set the nodal forces to yes. This will allow us to retrieve the reaction forces
Now let's apply our excitation which is the force the ball imparts onto the bat as mentioned earlier.
Right mouse click on transient, insert force Pick the face on the bat for the geometry selection.
This represents the location of the ball impact, and we have a simplified assumption that the force is evenly distributed over that area.
Change define by to component Change X direction to function
Confirm that the angular measure says radians, since we will be using a trigonometric function, its evaluation depends on the unit setting, which can be change by picking the region as shown.
Now Specify the equation shown here, where the negative sign is needed for the proper sign of the loading.
The graph of the loading shows a continuous sine squared wave, and we don’t wish the loading to continue in the 2nd load step,
so left click on the graph in for the 2nd load step, then right click and pick activate/deactivate at this step to toggle the load off.
In details change number of segments from 200 to 1200. This will graphically improve the resolution of the time history but has no effect on the solution.
Left click and highlight start of curve Then right click and pick zoom to range
Notice we now have the ½ sine squared wave in red in the first load step, but then it is deactivated in the 2nd load step where it is shown dimmed.
Let’s solve the model Insert Deformation Total
Evaluate all results Set the deformation scale to auto scale
Pick the results set icon to have the animation play with all the results Play the animation
We can see how the bat vibrates following the simulated impact with the ball
Insert stress, equivalent stress Evaluate all results
Now highlight the start of curve, Right click and pick zoom to range.
Notice the superposition of higher frequency content on top of the lower frequency response.
Also notice from the graph the peak stress occurs around 5 milliseconds
Highlight the start of the curve again and play the animation We may be interested in the reaction force where the bat is being held, so Insert probe, force reaction,
Change boundary condition to the remote displacement Change axis to X axis
We can also repeat and look at the moment reaction, so insert probe, moment reaction.
Change boundary condition to the remote displacement Change axis to Y axis and evaluate all results
You may notice the reaction forces and moment magnitudes are quite high, but they are very short in their duration and dissipate very quickly.
If you have ever hit a baseball with a bat, you may have noticed the sting these high frequency vibrations can cause in your hands.
I hope this video has clarified why employing the MSUP Transient technique for calculating the transient vibrations of structures is computationally advantageous.
We discussed how to specify transient loads in ANSYS Mechanical and how to post-process the transient response.
I hope you have found this video informative. Thank you for watching and do check out our other courses to discover more useful learning resources.