We have an exciting announcement about badges coming in May 2025. Until then, we will temporarily stop issuing new badges for course completions and certifications. However, all completions will be recorded and fulfilled after May 2025.
General Mechanical

General Mechanical

Topics related to Mechanical Enterprise, Motion, Additive Print and more.

how we can apply a follower load or nonconservative force in ansys ?

    • freud farid
      Subscriber

      i need to validate this benchmark "Large deflection of curved cantibver under nonconservative tangential end load" , as show in image bellow , the force R is nonconservative load that mean the force R remains normal to the mid-axis of the beam during deformation

      i need way to apply this kind of force in ansys ? 

    • peteroznewman
      Subscriber

      Here is the Ansys Help entry: 

      https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v231/en/ans_elem/Hlp_E_FOLLW201.html

      Here is an old discussion:

      /forum/forums/topic/how-to-setup-a-follower-force-for-a-cantilever-beam/

    • freud farid
      Subscriber

      this link not open 

      https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v231/en/ans_elem/Hlp_E_FOLLW201.html

      for the discussion , i have already read it , unfortunately It is useless

      There will remain a problem that needs to be answered by Ansys

    • Erik Kostson
      Ansys Employee

       

      Hi By default, Mechanical uses FOLLW201 element to apply a force to a BEAM element.

      Thus, follower effects are considered.

      All the best

      Erik

       

    • peteroznewman
      Subscriber

      First open Ansys Help.

      Copy the URL above and paste it into the Address bar of the browser showing Ansys Help.

      It will open.

    • freud farid
      Subscriber

      hi Erik Kostson

      how you get this information in image ? How can I access to switch between elements availables 

      how i can choose or apply  follw201 element ?

      but I don't get the same results as reference and analytical result

    • Erik Kostson
      Ansys Employee

      Hi

       

      Q: how you get this information in image ?

      Go to Solution in the mechaniacl tree, right mouse button click and choose Worksheet Res. Summary (see below).

      Q: how i can choose or apply  follw201 element ?

      As I said when we apply a force in mechanical on a line body (which is meshed with beam elements), automatically the follw201 elements are created by Mechanical and used, hence follower effects are considered.

      All the best

       

      Erik

      • freud farid
        Subscriber

        It still gives me either  beam188 when i use line sketch or solid186 when i use solid

        I don't know where the problem is ? 

        i find extension in site  for applaying 'follower load' but i didn't know how to apply it
        How do I contact you privately?

    • peteroznewman
      Subscriber

      I tried a standard force applied to a beam 188 mesh, but the follower force is not created by default as can be seen by the Reaction Force.

      I used the Follower Force ACT to create a Follower Force. The Force Reaction shows that it is working.

      • Erik Kostson
        Ansys Employee

         

         

        It is because the native force object inside mech., that generates the folw201 elements in the ds.dat file, uses keyoption(1)=1 – so not to update the direction.

        We need a command to activate the update direction (below the type id is 2 for the follw201 element and typed id 1 for beam188):

        All the best

        Erik

         

         

         

        • freud farid
          Subscriber

          Erik 

          can you share in detail steps to do that ? i need to do this example in follower force for my master project , I desperately need help

    • peteroznewman
      Subscriber

      Erik, I see what your original point was now that I opened the ds.dat input file and found an element type 201 for the follower element and the keyop,3,1,1 to keep the direction from changing!

      /com,*********** Create Remote Point "Remote Force - Remote Point" ***********
      *set,_npilot,74
      _npilot50=_npilot
      et,2,170
      type,2
      real,2
      mat,2
      keyo,2,2,1              ! don't fix pilot node
      keyo,2,4,111111
      tshape,pilo
      en,38,74        ! create pilot node for rigid link
      tshape
      en,39,74,1
      /com,*********** Define Vertex Force Using Follower Elements ***********
      et,3,201
      keyo,3,1,1           ! Keep the direction constant
      keyo,3,2,1           ! Apply Forces only, not moment
      mat,3
      real,3
      type,3
      en,40,1
      r,3
      rmod,3,1,1.0,              ! FX
      mat,4
      real,4
      type,3
      en,41,1
      r,4
      rmod,4,2,1.0,              ! FY
      mat,5
      real,5
      type,3
      en,42,1
      r,5
      rmod,5,3,1.0,              ! FZ
      /gst,on,on
      fini

      In this model, the type ID for the FOLLW201 element is 3 so the Keyops are as shown below.

      Thank you for the help Erik!

      • freud farid
        Subscriber

        thank you for sharing the code , but when i use it not work and give error

        please can you share the result of y displacement ?

        can you show the detail by image how to apply follower load in example above ?

        thank you 

    • Erik Kostson
      Ansys Employee

      All the best Peter.

      Erik

Viewing 9 reply threads
  • The topic ‘how we can apply a follower load or nonconservative force in ansys ?’ is closed to new replies.