Dear fellow scientists,
In the field of wave propagation in elastic half-space, I am trying to model a problem in ABAQUS.
The problem details is:
A harmonic load is applied at the axis of symmetry of a 2D elastic half space and the response of surface nodes at different distances (going as far as 12 meters) are needed.
The problem I have encountered is that for frequencies lower than approximately 50 Hz, the response (e.g. particle velocity, or displacements) is also harmonic at different distances. But for frequencies higher than the mentioned value, the response is neither harmonic nor oscillating with the input frequency, and it more seems like an impulse response. The graphs can be seen in Figures 1 through 4. Figure 1 shows vertical velocity at the location of the input force of 20 Hz, and Figure 2 shows vertical velocity of a surface node 10m far from the source.
Figure 3 shows the same output for 160 Hz input force, and Figure 4 shows the problem.
Figure 5 shows the model geometry.
Material properties:
1. Density=18 kN/m3
2. Elastic modulus=180 MPa
3. Poisson’s ratio=0.25
4. Rayleigh damping parameters: alpha=1.7 beta=5.5e-4
Input force properties:
1. Magnitude=267 N
2. Frequency=20 ~ 160 Hz
3. Applied as either a point load on a node, or pressure load on element face, the results are roughly the same
Model properties:
1. Element dimension and time increment are selected according to published literature and ABAQUS manual, since the shear wave velocity for this material is around 200 m/s, and the highest input frequency is 160 Hz, the Rayleigh wavelength is 0.8 m, the maximum element size is chosen 0.25 m and maximum time increment 0.0005 sec.
NOTE: I have tried smaller mesh (e.g. 0.01 m), and smaller time increment (e.g. 1e-6 sec), but the problem still persisted.
2. Analysis type: Dynamic Explicit, linear bulk viscosity parameter: 0.06 (changed it to 0 but the problem persisted) and Quadratic bulk viscosity parameter: 1.2 (changed it to 0 but the problem persisted)
3. The result types are History output request at different nodes and with time increment equal to analysis time increment.
4. The analysis time is 1~2 sec, no different results.
I know that the FEM analysis cannot cover this range of frequency, but what can we do to make it work for high frequencies?
Some advices:
Well first I have not worked with ABAQUS. From the program description it can be seen, that this is less suitable for dynamic tasks, especially for wave propagation in elastic media.
Furthermore, the results are highly dependent on the related boundary conditions. There is not see which geometric structure has the model and which boundary conditions therein received and which physical boundary conditions, among others stress field, wave form (Love wave, longitudinal wave, shear wave etc) received.
Because it is a coupled system, so it is of great interest, how the input is transmitted to the output.
First, the model should be checked. If that no recipe for success, then another sheet program should be used, a.o. PCGEOFIM.
I wish you success
All the best
Michael Lersow
Dear Dr. Lersow,
ABAQUS programs has been used for many dynamic analysis needless to say for this particular case, the literature is available and they seem to have given good results.
The boundary elements are infinite (CINAX4R).
Thank you for your advice.
Regards
Hi,
If you look on current literature regarding guided wave propagation in the context of Structural Health Monitoring you will see that it is also possible to simulate elastic waves in a frequency range of up to 1MHz. Therefore, another problem must be present in your modelling approach.
Your initial discretization using 4 linear finite elements per wave length is much too coarse. Generally at least 20 elements per wavelength are recommended. In an explicit analysis you should use the automatic time step control as the time step is set according to the CFL condition by Abaqus.
What you could try is to compute the same model in Abaqus/Implicit using quadratic finite elements that are much more accurate than linear ones.
You should also check if the nonlinear geometry option is switched on or off. This also changes the expected behavior. Furthermore it is advisable to use the enhanced hourglass control in the element type settings. This provides more accurate results for wave propagation analysis.
A last suggestion could be to compute an undamped system and see what happens. The mass proportinal damping (alpha) should damp lower frequencies more effectively and stiffness proportional damping (beta) is related to higher frequencies.
As you want to model an elastic half space, how do you account for the infinite boundaries? This can also be an error source.
Otherwise it would be helpful if you could upload your model.
Hope this helps a bit.
Dr. Duczek,
Thank you for your advice. I will check them one by one.
Here is the model .inp file.
Hi Dr. Kianoosh,
Have you solved your problem? I also do some dynamic analysis for engineering problems using the ABAQUS/Dynamic Explicit. I want to know the effect of the linear bulk viscosity parameter and Quadratic bulk viscosity parameter. How can I change these two parameters?
Regards
Darren ZHANG
Dear Dequan,
You can change these parameters when you are defining the step for dynamic Explicit analysis under the "Other" tab, or in the input file under STEP section.
dear Dequan
Quadratic bulk viscosity have effect on fluctuation of results.you can regulate your last results by change this item but it can affects on your results based on waht you simulate.
Dear Kianoosh,
I just changed these two parameters in the 'Other' tab, but I am not sure what is the suitable range of these two parameters.
Best wishes
Dequan
The infinite elements are not the best choice to model unbounded domains at least for dynamic analysis. Try modelling larger area "or" check whether the waves can be reflected back during the analysis time.
- Badges
- Science topic
- Similar topics
- Engineering
- Modeling