General Mechanical

General Mechanical

Ansys APDL Programming buckling FEA C Section Cold Formed Steel

    • tanmaynade
      Subscriber

      Hi,


      I am facing issues with my program. Listed below. This is form my masters project. Also in what way can I connect the filleted surfaces shown in fig by a weld or just load or stress transfer connection. The link to the program is 


      https://www.ansysforum.com/forum/ansys-packages/structural/439-apdl-programming-buckling-fea-c-section-cold-formed-steel?view=stream


       




       



       



       

    • Vitaliy_Degtyarev
      Subscriber

      You can find more detailed descriptions of the issues in the jobname.err file in the working directory. When I ran your code, I got a warning about only one element violating shape warning limits. The following description was given:


      Quadrilateral element 41288 has a pair of opposite edges that are      
       77.42 degrees away from being parallel.  This exceeds the warning      
       limit of 70 degrees.


      You can still run the analysis with this warning, but it is better to change the mesh. I usually select lines and divide them as needed using the LESIZE command, after which I mesh my models using mapped meshing (the MSHKEY command). With this method you have more control over the mesh and get a nice mesh with only rectangular and square elements. You may also want to have smaller divisions for the radii.


      If your connections are discrete, you can couple displacements of the nodes that need to be connected using the CP command. If the connections are continuous, you could specify bonded contact between the surfaces.


      Hope this helps.


      Vitaliy


       


       

    • tanmaynade
      Subscriber

      how to do bonded contact

    • Rohith Patchigolla
      Ansys Employee

      Hello Tanmaynade,


      I have created a simple example to create contacts between two blocks in apdl. It is well commented.
      You can understand the basic procedure here and can further apply it to your model. 
       
      Also, please go through the help documentation for more reference on any commands used in the script. 
      fini
      /clear,nostart
      /prep7

      block,0,1,0,1,0,1 !make two blocks touching each other
      block,1,2,0,1,0,1

      et,1,186 !define a solid element type 

      mp,ex,1,100 !define some elastic material properties
      mp,prxy,1,0.3

      esize,0.2 !element size

      vmesh,all !mesh all volumes

      et,2,174 !create contact elements
      keyopt,2,12,5         !bonded contact
      KEYOPT,2,9,1

      r,2 !real number for this contact pair

      et,3,170 !create target elements

      asel,s,,,6 !select contact area
      nsla,s,1 !select nodes attached to this area
      esln !select elements attached to the selected nodes
      type,2 !set contact type number
      real,2 !set real number for contact pair - one real number for each contact pair
      esurf !create contact elements on selected nodes
      allsel,all

      asel,s,,,11 !select target area
      nsla,s,1
      esln
      type,3 !set target element type number
      real,2 !set real number for this contact pair
      esurf !create target elements

      /solu

      antype,0

      nsel,s,loc,x,0 !constrain one end of block 1
      d,all,all
      allsel,all

      nsel,s,loc,x,2 !apply displacement on other end of block 2
      d,all,ux,0.1
      allsel,all

      solve

      /post1
      plnsol,u,x !plot disp x

      You can also do this process via ANSYS Classic GUI using Contact wizard. 



      Hope this helps. 


      Best regards,


      Rohith

    • tanmaynade
      Subscriber

      thanks a lot

    • tanmaynade
      Subscriber

      also, I'm not able to create e proper mesh for my original program some elements get out of shape?


       

    • Rohith Patchigolla
      Ansys Employee

      Hello Tanmaynade,


      Please provide some mesh sizing controls (to refine the mesh at these areas) to get a proper mesh. Also, posting an image of your mesh, where the elements get out of shape would help us provide better suggestions.


      Best regards,


      Rohith 


       

    • Sandeep Medikonda
      Ansys Employee

      Tanmaynade,


       Please create a new discussion for your question. This discussion is closed. Take a moment to review the guidelines on the Student Community.

Viewing 7 reply threads
  • You must be logged in to reply to this topic.