Dismiss Notice
Join Physics Forums Today!
The friendliest, high quality science and math community on the planet! Everyone who loves science is here!

Aerospace Ansys meshing

  1. Feb 28, 2010 #1
    I'm using anysis to model a 3-d object. i'm using a series of beams. however, when i try to mesh the beams, it says that it's unable to do that. When I add a shell, anysis meshes the model. How do I create a mesh with only beam objects?
     
  2. jcsd
  3. Mar 1, 2010 #2

    minger

    User Avatar
    Science Advisor

    BEAM elements must be meshed on lines, using the LMESH command with the proper TYPE, REAL, and SECN set prior. The following is a full example of a static analysis using beam elements
    Code (Text):

    /prep7

    !--insert materials here
    SECTYPE,1,BEAM,CSOLID
    SECDATA,1.0,8,2

    !--define geometry
    k,,0,0,0
    k,,10,0,0
    l,1,2

    !--mesh the line
    type,1
    real,1
    secn,1
    lmesh,1

    !--boundary conditions
    ksel,s,kp,,1
    nslk
    d,all,ux,0.0,,,,uy,uz,rotx,roty,rotz

    ksel,s,kp,,2
    nslk
    f,all,fx,-100

    allsel,all
    /solu
    antype,static
    save
    solve
    save
    finish

     
    edit: You can use the command /ESHAPE,1 to turn on the element shaping which allows you to "see" what the beams look like. This can be important when you start using orientation nodes and need to see which way unsymmetric elements are facing. Good luck,
     
  4. Mar 1, 2010 #3

    Mech_Engineer

    User Avatar
    Science Advisor
    Gold Member

    When you say a 3-D object, is it a truss structure with lines that are defined in 3-D? Beams can only be meshed to lines; if your object is a volume or surface, you cannot use beam elements to mesh it.
     
  5. Mar 2, 2010 #4
    I'm trying to model a 3-d object (a frame with t-bars) and I thought that defining 3d beams would be the best way. Is there an easier way?
     
  6. Mar 2, 2010 #5

    minger

    User Avatar
    Science Advisor

    That's probably the easiest way. As mentioned though, you need to line mesh. Put keypoints [K,num,x,y,z] at all the intersections. Then draw lines from keypoint to keypoint [L,kp1,kp2]. Then, you define your sectypes as I mentioned above.

    At this point, I'll give the obligatory RTFM for defining beam sections.

    At that point, simply LMESH the lines, apply boundary conditions and solve. From the sound of it, you need to spend a few days and just go through the help, do some test cases, get accustomed to the software.
     
Know someone interested in this topic? Share this thread via Reddit, Google+, Twitter, or Facebook




Similar Discussions: Ansys meshing
  1. Irregular mesh (Replies: 4)

Loading...