General Mechanical

General Mechanical

transient analysis with infinite element

    • Augusto13
      Subscriber

      I'm trying to simulate an earthquake on the basis of a cubic structure (Figure 1) using the infinite element of ansys, the use of the element is explained in the link below.


      https://www.sharcnet.ca/Software/Ansys/17.2/en-us/help/ans_cmd/Hlp_C_EINFIN.html



                                            Figure 1


      I'm applying example 3 of the link in ansys. My base is fixed. In this way, I decided to apply the remote displacement command to its base, all directions are restricted, except in the direction of the earthquake. I can not solve this mistake:


      The value of UZ at node 1609 is 2052922.18. It is greater than the


        current limit of 1000000 (which can be reset on the NCNV command).


        This generally indicates rigid body motion as a result of an


        unconstrained model. Verify that your model is properly constrained.


       


      is there any other strategy for me to overcome this?


       


      obeservation: I am declaring the name of the infinite element as et, matid + 100, without this I have problems. I'm implementing this way:



                                                         Figure 2

    • Sandeep Medikonda
      Ansys Employee

      Please see this post on how to identify and deal with rigid body motion.


      Please remove any links to sharcnet and use ansys help. It is more up to date and accurate. If you don't know how to access the help, please see this post.


      Regards,
      Sandeep
      Guidelines on the Student Community

    • Augusto13
      Subscriber

      thanks for the tip.


      I found two examples in ansys help for static analysis. It seems to me that the problem is that the infinite element must also be restricting. So, I added this in the APDL commands:


      NSEL, S, LOC, Z, O! select restriction nodes


      D, ALL, UX,,,,, UZ, ROTX, ROTY, ROTZ! Constraints on Z = 0


      NSEL, ALL! restore selection for solve


      With this there is no free body movement. The infinite element is implemented successfully (Fig. 1). However, my transient analysis does not work (Fig. 2),  all displacements are zero.



                                        Figure 1.


       


                                          Figure 2.


       


      It would be interesting if ansys have a test sample for a transient analysis.

    • Augusto13
      Subscriber

      another thing.


      Mr. Sandeep, would you know how I could plot the constraints of FIG 1?

    • Sandeep Medikonda
      Ansys Employee

      Hi Augusto,


      If you intend to graphically display FE Connections, please select the ‘Solution Information’ item and click the graphics tab.


      Please see this article.


      Regards,
      Sandeep
      Guidelines on the Student Community

    • Augusto13
      Subscriber

      Hi Sandeep,


      unfortunately I have not yet succeeded. I am almost convinced that ANSYS does not solve transients problems with INFIN257.


      I found two examples of static analysis: VM290 and VM291


      I succeeded in static analysis. If ANSYS had any examples with transient analysis it would help a lot.


       


      I appreciate any help, I'm very interested in this problem.

    • jj77
      Subscriber
      If you look on the reference for infin257, it can be used for transient analysis. See the help related to , Elements Used to Model the Truncation of an Infinite Structural Domain
    • Augusto13
      Subscriber

       Yes, I know that.


      I did a new analysis on a beam now. I applied a pulse at one end and in the other, I introduced the infinite element (Fig. 1) in order to perceive the absorption. Again the same problem occurred (peaks of displacements at the points located at the finite-infinite interface).


       



       


      including this problem is reported by another user:


      https://studentcommunity.ansys.com/thread/non-linear-analysis-infinite-elements/

    • jj77
      Subscriber

      I am sure these element should work at least for what they were partially/mainly aimed to do that is to be used for absorbing waves, could be elastic, acoustic, EM,ocean,.. in FEA. 


       


      A good benchmark of this, can be found in abaqus, where infinite elements are used to look at different types of elastic waves (P, S , Rayleigh surface waves, in Ultrasonic regimes), and how they are absorbed at infinite boundaries.


      The benchmark is called,  2.2.1 Wave propagation in an infinite medium 


      just search for it. Try to do this one, and surely that it should give similar results (otherwise the setup must be wrong, it can be tricky to use these elements since they are non standard 3D or 2D elements. Also they can be some sensitivity (how effective they work) I would imagine depending how the wave/front travels,and the orientation of the element.


       


       


       


       

    • jj77
      Subscriber

      Did a small test, not saying that it works great for all types of waves.


       


      In order to keep it simple and so I know exactly the waves and the infinite elements are aligned in the best possible way:


       


      Quasi long. wave in a plate (plane strain), also known as the S0 Lamb wave (50 kHz). The wave is excited in the middle of the plate, thus two S0 waves propagate left and right as seen on the top image (red arrow shows force excitation while blue shows the wave vector direction).


      The second image is just before they hit on the left a fixed boundary and on the right an infinite absorbing boundary. Thus we expect reflection on the left but not on the right.


       


      This can be seen as expected in the last image where there is no reflected wave on the right, while there is a reflected wave (left BC) propagating back in to where it came from.


       


      I am sure you can do some better tests, but this is to show how these elements can be used in dynamics and say guided ultrasonic wave propagation.


    • Augusto13
      Subscriber

      Hi jj77


      yea! this behavior is what I expected. Could you send me this file? 

    • jj77
      Subscriber

      Unfortunately not they are deleted. Try to set it up yourself, or even better do another benchmark where the waves are not 1D (like guided waves)

    • Augusto13
      Subscriber

      Yes .. I will try. I will post it here.


      would it be possible to post the commands used in apdl for this example posted above? would help me a lot

    • jj77
      Subscriber

      As I said I do not ahve the file, which was very simple.


      I basically used the model/link that you show on the first image, but the first 2D example on that site (seen in einfin, used to generate infinite el., file is in that example).


      In dynamics of waves one uses at least typically 6 elements per wave-length, and a time step, in implicit that is 1/10 of the excitation period (so here 1/10 of 1/50 000 Hz). Total time is so the waves can travel back and forth.


      then I use , D command for restraint, F command for force and the thing bellow for importing an amplitude time curve (Amp.csv), could be a sine with a couple of cycles. Mytable is an array, reading the Amp.csv file. The array can then be used in the F command to excite the waves. Thus select the nodes you need (use nsel), and then say (for x excitation):   


      F,all,FX, %mytable%


      --


      !Importing Amp.csv


      to_skip=0


      /INQUIRE,numlines,LINES,Amp,csv


      to_read=numlines-to_skip


       


      *DEL,mytable,,NOPR


      *DIM,mytable,TABLE,to_read 


      *TREAD,mytable,Amp,csv,,to_skip


       

    • SriVin
      Subscriber

      How did you solve the issue of wave reflection ?


      Please let me know the details, it would be a great help. I am working on soil structure interaction

Viewing 14 reply threads
  • You must be logged in to reply to this topic.