Hi
Maybe you want to take a look at this discussion?
https://www.researchgate.net/post/What_should_be_the_correct_boundary_condition_for_soil_when_accl-time_history_analysis_is_attempted_in_ABAQUS
Sincerely
Claes
Hi claes
thanks for your attention. I visit the page but I can't find any to my problem.the advices were general. I want to know how can I model the soil and it's boundary in ABAQUS, exactly!
Best
Hi
I believe the answer boils down to using a matrix of dynamic stiffness functions on your boundary.
You
- Use analytical functions for the 'green field'
- Exctract data at the cavity of your dig and/or surface of your interface
- Invert the matrix that is output from the above (one inversion per frequency)
- Insert the inverted result as BC to your Abaqus model
- Analyze the response using direct matrix solution
The above can be rather time consuming, so it may be worth your while to see if you can make some shortcuts, e.g. by the use of reciprocity. It all depends on your analysis purpose.
Sincerely
Claes
Hello Azadeh
That's easy first model your parts than for the infinite part assign C3D8 then write input and in the input file change C3D8 to CIN3D8
Be aware that for the infinite part you have to use sweep mesh and the arrow should be outward
Regards
Hamed
Hello Hamed
Thank you for your sugestions.
As you said I do your procedure for CIN3D8 except the sweep mesh! after I run the sample,It's not seem any problem exist!!
Would you please describe why should I do sweep mesh?
I await your response in kind
Hello Azadeh
Well you normally use infinite element for seismic affairs so in these cases the wave direction is very important.
By using sweep mesh you let the seismic wave go freely in that direction.
Regards
Hamed
Thanks alot Hamed
You mean that according to my earthquake direction (X,Y,Z or multicomponent), I should use sweep mesh and then check the arrow of that to be in my earthquake direction?
Hi
Yes exactly. if you are applying the seismic forces in just one direction that would be easy otherwise it would be a bit difficult.
Regards
Hamed
Hi Azadeh
See following link, its can be very useful
https://www.linkedin.com/groups/Abaqus-Use-3D-Infinite-Elements-3958425.S.194473817
Best Regards
Alireza
Hi
I may be wrong here but to the best of my knowledge, infinite ('perfectly' absorbing elements) exist only for acouustic waves (Pressure-waves), while soil involves more wave types.
Aligning the mesh to be normal to the wave direction is good avice but I believe it cannot handle more than some situations as infinite elements handle most situations for the acoustic case.
Therefore, the much more laborious procedure where you use matrices as described above is the general procedure. Than again, if a simple mesh adapations is good enough, then you should use it.
In this spirit, here (see Figure 3) is another approach to model absorbing boundaries. It is simple to make but computationally costly. http://qringtech.com/wp-content/uploads/2014/01/SPIE205933-18.pdf
There exists also the FE code calles Code Aster which uses a 'rubber band mesh' on the boundary to, as best possible, absorb impinging waves. Code Aster has implemented the coupling matrix approach to a French analytical code for layered soils. http://www.code-aster.org/V2/spip.php?rubrique2
Sincerely
Claes
Hello Claes
Thanks for your attention.you mean in the soil problem it's better to use absorbing boundaries than infinite elements?
I really don't know what should I do.
Hi
As far as I understand, a matrix on the boundary is the general method. Physical modelling as shown above using 'absorbing wedges' handle more wave types but leave some reflection. Infinite elements for one wavetype is bettwer than rho*c boundary conditions (rho*c corresponds to diagonal matrix, while the general approach involves a full matrix). The Code Aster 'rubber band' boundary mesh relects but is easy to work with and allow introduction of impinging waves as loads.
The 'best' approach is the one that works for you. What works for you depends on what you want to do and how well you have to do it.
Sincerely
Claes
Hi
Code Aster contains a coupling to a code calles MISS3D which implements the matrix method. Here is PhD thesis on the subject http://www.theses.fr/2013ECAP0006/abes
If you are running a very large model, the matrix method probably is your best bet. I was invoved with a project where we used this approach and still had to use a local supercomputer for the analysis.
Feel free to drop me a mail if you want to try Code Aster instead of Abaqus.
Hope this helps
Claes
Dear Claes.
thank you so much for your responses.
would you please give me your email adress ?
Hi
I advice you to see the document. You will find what you need.
Best regards
http://imechanica.org/files/Pichler_TUHH_final_2222012.pdf
- Badges
- Science topic