General Mechanical

General Mechanical

Coupled Damage-Plasticity Microplane Damage Output

    • gigihmprayogo
      Subscriber

      I am doing reinforced concrete beam column joint analysis using coupled damage-plasticity microplane model. How do i get damage visualisation of homogenized total damage (TOTA), homogenized tension damage (TENS), and homogenized compression damage (COMP) on Workbench


    • Wenlong
      Ansys Employee

      Hi, 


      The microplane damage output is not directly available in Workbench Mechanical. You would need a command snippet to output that.


      "PLESOL, MPDP, TOTA"


      Please refer to PLESOL for more information: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v192/ans_cmd/Hlp_C_PLESOL.html?q=plesol


      And here is an example you can try: 




      ! Graphics power needs to be turned on to view the rebars


      /graphics,power


      ! Enter /post1 module


      /post1


      ! Show result as a png image


      /SHOW,png


      ! Set the frame as the last substep of the 1st step


      set,1,last


      ! Select the SOLID185 elements


      esel,s,ename,185


      /trlcy,elem,0.5     ! Change them to transparent level 0.5 (0 is solid, 1 is completely transparent)


      esel,all


      ! Set view angle


      /view,1,1,1,1


      /angle,1,-0.75


      ! Show the whole section of the reinforcement


      /eshape,1


      ! Plot displacement


      plnsol,u,x


      ! Plot damage


       


      plesol, MDPD, TOTA




       


      Regards,


      Wenlong


       



      Useful Links



       

    • gigihmprayogo
      Subscriber

      @Wenlong, the solution visualisation shows for displacement only, if i check d snippet, it should be shows 2 image right? displacement and damage..


    • Wenlong
      Ansys Employee

      Hmm, what about using these commands:



      It works for me:



      If it still doesn't work, maybe checking the concrete model? Is it possible you are using the Regularized Elastic Damage Microplane Material model? You can find more info about the material model here: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/ans_mat/microplane.html?q=microplane. You can also do a search "output" in that website to find related information.


       


      Regards,


      Wenlong


       



      Useful Links



       

    • gigihmprayogo
      Subscriber

      I already try your latest snippet but it still wont show..I'm using couple damage-plasticity microplane model, using CPT215 element with 2 extra DOF, here the snippet



      Or is there additional step or something that I have to activated?


      when I check at solution information it says:


      *** WARNING ***                         CP =       0.969   TIME= 15:43:50
       The requested MPDP data is not available.  The PLNSOL command is       
       ignored.

    • Wenlong
      Ansys Employee

      Hi,


      Apart from your command snippet, I also have the following to assign the material to concrete, and request all the outputs. You can try putting it below your commands and see.



       


      Regards,


      Wenlong


       

    • gigihmprayogo
      Subscriber

      Thank you, finally it works, here the visualisation



      But another problem comes up =(, when I change the mesh size..the damage wont show, please advice

    • DrDalyO
      Subscriber

      Hi gigihmprayogo,


      Would you mind posting the full command snippits you used in the end? I am also unable to plot the microplane damages TOTA, TENS, COMP, RW using the PELSOL,MPDP command. Error is "The requested MPDP data is not available."


      See the file : Commands

    • gigihmprayogo
      Subscriber

      @DrDalyo, in prep7 snippet, make sure to request all solution: OUTRES,ALL,ALL


      And Here my latest snippet to plot the damage:


      /SHOW,PNG


      !Change White Background


      /RGB,INDEX,100,100,100, 0


      /RGB,INDEX, 80, 80, 80,13


      /RGB,INDEX, 60, 60, 60,14


      /RGB,INDEX, 0, 0, 0,15


       


      ESEL,ALL


      /VIEW,1,1,1,1


      PLNSOL,U,Z


      PLNSOL,MPDP,TOTA


      PLNSOL,MPDP,COMP


      PLNSOL,MPDP,TENS


       


      To test my command and make it simple, I'm modeling cube uniaxial test (on my previous post), and assigning the microplane properties on solid body (same format with your attached snippet). But the damage only show if I used single element, if I mesh the cube, the damage plot wont show..still dont know how to figure it out

    • gigihmprayogo
      Subscriber

      @DrDalyo, if you are still unable to plot the damage, try add command "set,last"  on your post prep command..now i'm able to plot the damage


    • vaibhavtaranekar
      Subscriber
      ArrayI am unable to view the damage at other steps whenever i try to use Set,2,last or any other substep, i don't get any output.n
    • DrDalyO
      Subscriber
      Hi vaibhavtaranekar, I found the same issue as you. It seems like the damage outputs do not work in workbench when there is more than 1 step. Could be we have the commands wrong. A workaround that I used was instead of using steps, just use time. So I created a model that goes to 2s, instead of 1s, and then apply the loading conditions differently at 1s and 2s which basically comes out to the same thing as 2 steps. This method then works, and you can output the damage models at different times. I posted a brand new video on this here!:nn
    • vaibhavtaranekar
      Subscriber
      Looks promising! Thanks for new video!n
Viewing 12 reply threads
  • You must be logged in to reply to this topic.