Transient structural using solid65 element

pradi87pradi87 chennai, tamilnaduMember

My goal is to simulate transient structural analysis for a simply supported beam. How to specify solid65 elements for the beam. Is it possible to model the beam without rebars? I need to obtain a crack pattern for the vibration load applied. I already modeled the beam in static structural and modal analysis, I tried to change the elements to Solid65 using APDL command snippets. But it is showing errors. How to solve this problem?


*** WARNING ***                         CP =       0.421   TIME= 12:08:08
 CONCRETE is not a recognized PREP7 command, abbreviation, or macro.    
  This command will be ignored.                                         

 *** ERROR ***                           CP =       0.468   TIME= 12:08:08
 Element type 1 is not the same shape as SOLID65.  Switching to a       
 different shape is not allowed while elements of type 1 exist.          


  • jj77jj77 Member
    edited February 2019

    There is something with the concrete command and the elements you are using. Soldi65 is 8 node HEX element so you need to use that when meshing. There is also a prism option but not sure how to use that (never used this element). For more info see the element reference manual ( Copy and paste that into the ansys help browser,


    CONCRETE as it says is not a command. You mean CONCR.

    This is (see below) how to define the nonlinear CONCR model (sure you can find lots on that on the internet). Obs: this is a nonlinear material model, so of course it can not be used in modal analysis. To use this you would need to use a nonlinear transient dynamic analysis. Untensst is a constant, and somethng one would have defined in the script, otherwise replace the below names wit the actual values.

    Also for an example see the verification manual VM146 that models RC beam with solid65 elements.

  • pradi87pradi87 chennai, tamilnaduMember
    edited February 2019

    Thank you for mentioning. I'm not quite clear about the "choosing 8 node hex element during mesh", you've mentioned. Could you please explain that. I use Ansys workbench 18.1

    And also I need to first simulate it in modal analysis, it is a must for my work. I need to extract the frequency range. So, this means I can't use solid65 for modal in Ansys workbench like that?



  • jj77jj77 Member
    edited February 2019

    Solid65, is hexahedral element with 8 nodes, so one needs to create a structured mesh (e.g., sweep, if you want to know about this close this, by e.g, choosing Is a solution, and post and start a new one), using these elements (8 noded hex. elements).


    For more info about the elements see


    This should be very clear.

    A nonlinear material model (concr), can not be used and is not accounted for in a modal analysis, since that is a linear analysis which assumes linear elastic material and small deflections. Of course you can still run a modal analysis but it will only use the linear properties of the material (that is E-mod., and v).


  • peteroznewmanpeteroznewman Member
    edited February 2019


    In order to get an 8-node element, you have to click on Mesh and in the Details window, on the row that says Element Order, change it from Program Controlled to Linear.  The default element is Quadratic which means a 20-node hex element and you can't fit an 8-node element into that.

    Regards, Peter


  • shw419shw419 Member
    edited July 9

    Hi Pradi.

    I am also modelling concrete models in transient structural. And I got errors when I try to insert Solid 65 command to concrete. Do you mind sharing your workbench files so I could learn what I did wrong?




Sign In or Register to comment.