User login

You are here

Simulation of wave propagation in ABAQUS/CAE

Hi, I am working on modeling wave propagation in ABAQUS/CAE.

I am not expert on ABAQUS and trying to figure out how it works.

I have a 2D Shell steel plate (1 centimeter by 1 centimeter) and try to obtain wave speed at any points of plate.

I put the material properties in and used ABAQUS/Explicit analysis.

Time steps are 1E-009 seconds and there are 2 steps (impulsed at the first step and propagates at the second step).

The load pluged at the amplitude with equaily spaced for 0.1 micro seconds (so it becomes impulse load).

The mesh was generated with element length of 0.0001 meter (so it becomes 10000 elements).

After the analysis, I checked the displacement of certain nodes and found arrival time.

The wave speeds were calculated based on the distance from the pulsed point and arrival time.

However, the wave speeds are not matched with theoretical value which is cL = √{E(1 − v)/ρ(1 − 2v)(1 + v)}.

Any idea that I did something wrong?

I can provide any other infomation on my input.

Thank you in advance. 

Using E = 200 GPa, nu = 0.3 we have c_L = 5860 m/s.   The impluse has a wavelength of ~ 2*c_L*dt = 2*5860*1.0e-7 = 1.17e-3 m.  The mesh size is h = 1.0e-4 m.  At 10 elements per wavelength that's a good mesh even for shock loading.

You can look at the book on Wave motion by Karl F. Graff for the special wave speeds that you can get under plane stress (strain) conditions.  For instance, in the absence of dispersion, the sound speed in a thin plate under plane stress is

c = sqrt[E/rho(1-nu^2)]

as you can see on p. 82 of the Cambridge handbook of physics formulas by G. Woan.

-- Biswajit

Thank you for your help, Dr. Banerjee.

 

 Hi,

I am a freshman to iMechanica and i hope to get some help,I'm going to simulate wave propagation on thin steel beam using Abaqus.

but,unfortunately, i don't know how i can do it,so i will appriciate if some one guides me or suggests some reference that training is given.

Thanks,

Wave propagation problems are similar to any other dynamic analysis. However, increment size and meshing is highly dependent on the type of wave you want to capture. As Dr. Banerjee explained, the mesh and time increment size should be such that the wavelength (or frequency) being targeted is being captured during the analysis.

 Analogous to this, let me put it this way: Suppose you want to trace a sine curve by straight lines. Then if one uses 4 points only, then sine curve will be plotted as two triangular regions. As you increase the number of points, the obtaine curve start approching the sine curve in appearance.

As a rule of thumb, the element size and increment size should be such that it describes wave sufficientely; i.e.:

  1. Time increment size be sufficent enough to capture the smallest natural period of interest.
  2. Element size should be small enough to capture wave length.
  3. element size should not be so small that in one increment, the wave  crosses the element.

These are basic guidelines, you can refer to the book mentioned by Dr. Banerjee (or any other numerical analysis book where wave propagation problems are discussed).

If anyone has further information, please share it. :)

------

The world started with 0, is progressing with 0, but doesn't want 0.

ramdas chennamsetti's picture

Hi,

Nice thread. To simulate wave propagation, CFL and Blake's criteria are to be satisfied.

Calculate the minimum wavelength. Take the mesh size (deltaX) as wavelength/n, where 'n' = 10 to 15 (in general).

Critical time increment = tcr = deltaX/Vmax, where Vmax is the maximum wave speed. Time increment for time marching is taken as 0.75*tcr.

Best regards,

- Ramadas

hi, 

Maybe the problem is about the output resolution. You should have the history output of displacements with enough frequency to catch the output accurately. tell more about how you get the displacements and how you calculate the wave speed. tihs may help for solution of the problem.

 

for example, if you have a 1 m beam and the calculated speed of sound is 1000 m/s, than it will take 0.001 seconds for wave to arrive to the end of the beam. if your output frequency is less than 1000 Hz (that is 1/0.001) then you can not catch the wave when it hits the end. In this case one would need to have at least 5 kHz of output. In abaqus of course having such a high resolution field output would result in a huge outputfile, and this would also significantly increase the solution time ( because writing field output is so expensive). then the logical way is to use history output option to get high frequency output at some certain nodes or elements. then in postprocessor, plot displacement vs time in the first and last nodes of the beam. the length between the nodes divided by the difference between the peak times of the nodes should give you the exact speed of sound.

 

regards,

 

fatih 

Hi,Thanks for your helps,they were useful for me.

my problem is simulation Lamb waves and Excitation (A0 / S0 mode).                                                                                                              yeah, Maybe the problem depend on output resolution,
but at first i want to know which kind of load  i should use for generating lamb wave in module of load in Abaqus,i saw some ways but i am not sure about detail of them.
for instance,applying a harmonic normal force to small regions of the top and bottom surfaces or apply a shear force on the surface of model are some of them. I'm waiting for your guidance,

 Best Regards,

 

 

Please anyone giv eprocedure how to perform Hyper velocity Impact of Composites using AUTODYN

Hi, guys! A lot of good info in this thread.

I am currently trying to model a 2D plate with a point load/pressure on one of the ends and fixed BC on the other end. I obtain nice results and plots with ABAQUS, but when I measure the wave velocity and compare it with the theoretical speed, I see that it is very dependent on the so-called CFL (Courant) number, given by

CFL = c * delta_t / delta_x,

where delta_x is the element size. According theory it is required that CFL < 1 to obtain a stable solution. I have also heard that is should be as close to 1 obtain the most correct solution. The problem is that I obtain a stable solution if I use CFL = 1.5. I would expect the solution to diverge over time. So to my question: does anyone know if it is most correct to use the formula for c_L given in the first post or c = sqrt(E/rho) to calculate CFL?

 Or does someone have another tip to obtain a stability limit at CFL = 1? I have also noticed that choosing plane stress or strain elements affects the stability limit. Which element type is best to choose you think?

Regards,

Master student at NTNU 

i am frehser to abaqus and interested simulate ocean wvaes. please send me jounals or screen shots of the procedure.. my email id is krishnaprasadvn@rocketmail.com.

thanks in adv

krishnaprasad

Hi

I ve completed smulation of a beam with S0 lamb wave and I wanna compare my results with the theoretical one and experimental as well. I am trying to plot dispersion cureve for the lamb wave. Could you please advise as to how I would use Abaqus outputs for plotting this curve ?

Cheers

Subscribe to Comments for "Simulation of wave propagation in ABAQUS/CAE"

Recent comments

More comments

Syndicate

Subscribe to Syndicate