General Mechanical

General Mechanical

problem with eigenvalue buckling beam as line body model

    • Masri
      Subscriber

      hello there,
       I have a problem with modelling a simply supportd beam due to calculate eigen value 
      actually the problem is with the boundary conditions .... beam is defind as line body ... the first end is  defined through Remote Displacement 
      (Displacement X Y and Z are 0 , Rotation X is 0 ,Rotation Z and Y are free) the second end is defined too through Remote displacement 
      (Displacement X is Free ,Y and Z are 0 , Rotation X is 0 ,Rotation Z and Y are free)....
      but unfortunately the defomation form appears not logic .... could anyone help me to define the probelm please ....

    • Masri
      Subscriber

      this is how appears the defomation shape

    • Wenlong
      Ansys Employee

      Hi Masri,


      Does the solver show you warning "not enough constraints appear to be applied to prevent rigid body motion“? Your beam can rotate freely in the z and y direction and that may cause an issue. 


      Regards,


      Wenlong

    • Masri
      Subscriber

      Hi Wenlong,


      THnx for ur replying

       yes i have got this message as Warning,,,, but that is the real situation that i want to represent... beside when i prevent the beam from rotation around Y and Z  axis then it produces momentum at the ends and this is not the same Euler situation that i need to study ....


    • Wenlong
      Ansys Employee

      Hi Masri,


       


      Thanks for clarifying. I just run a  model with similar geometry as yours and the same boundary condition as yours and it is able to run. Could you please share more of the information like the geometry settings and so on? 







      Regards,


      Wenlong

    • Masri
      Subscriber

      thanks Wenlong for ur Attention....these are pics of my modell 





    • Masri
      Subscriber

      and this is the file that i have created 



      https://drive.google.com/open?id=1oNm2puF7MqgCbyJKo3v2seasId3DHyBn


       


      Regard
      Masri,

    • Wenlong
      Ansys Employee

      Hi Masri,


      Based on the image you shared, can you please try changing the force to 1N in the static structural analysis? It is likely that the beam has no longer small deformation when you apply such a large load. 


      Usually what we do is apply a unit load in the static structural module, and the buckling load will be whatever the load amplifier is in the eigenvalue buckling analysis.


      Regards,


      Wenlong

    • Masri
      Subscriber

      Hi Wnlong,

      I have changned the force from 100,000 N to 1 N ..... The load the load amplifier changed from 13.44 to (13.44 X 10^5) .I dont think that is related with the load amplitude ..... I think there is a problem with a boundry conditions but i cant define it ..... could u please show the ansys file that i uploaded to help me defining the problem?


      Regards,
      MAsri

    • Wenlong
      Ansys Employee

      Hi Masri,


      Sorry due to the company policy I cannot download any attachments from the student community. So we can only communicate through images. It looks to me that all your BCs are the same as mine... Do you mind showing more information about the analysis settings and the geometry information? What is in that construction geometry?


      Thanks,


      Regards,


      Wenlong

    • Masri
      Subscriber

      Hi Wenlong,
      Thanks for the clarification
      the geometry is an I cross section that is draw with space claim .... CS is an IPE 330 (Eurocode profil)



    • Wenlong
      Ansys Employee

      Hi Masri,


      Thanks for replying. When I try higher natural frequency I see your behavior too (I apologize for not capturing it the first time, plus, my remote displacement location was wrong, it was not set to the end of the beam).


      I think the reason could be the mesh size being too big and not able to capture the wavelength in high-frequency mode. Could you please try using a very refined mesh 5mm?



      Regards,


      Wenlong

    • Masri
      Subscriber

      Hi Wenlong,

      I have tried to make element size 5 mm and this is the result


    • Masri
      Subscriber

      I tried another case by deleting the remote Displacement at ends (where the force apply) to make it free and another end as a fixed support >>>> it worked and i had a logic deformation shape like this 



       


      but this is not the case that i have to study ...

      Regards, 
      Masri 


       

    • Wenlong
      Ansys Employee

      Hi Masri,


       


      Please try to set the max mode to find to 10 (a large number), I think if you only request 2, the second one will give you the highest frequency? (I will double-check and follow up with you on that).


       


      Regards,


      Wenlong

    • Masri
      Subscriber

      Hi Wenlong,

      I have tried that and Nothing had changed .... the sams Deformation shape also besides there is  just tow modes.... i dont know why....this is the results 






         


       

    • Wenlong
      Ansys Employee

      Hi Masri,


      It is under "Analysis settings". Please also keep your mesh small around 5mm. 


    • Masri
      Subscriber

      Hi  Wenlong, 

      I am so grateful to you that you have really solved my problem ..... a higher number of modes gives indeed a correctly answer .....

      i have remarked ur comment as a solution 
       Regards
      Masri

    • Wenlong
      Ansys Employee

      Hi Masri,


      You are welcome. Sorry it takes so many iterations


      Regards,


      Wenlong

Viewing 18 reply threads
  • You must be logged in to reply to this topic.