Coupled Damage-Plasticity Microplane Damage Output

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

Comments

  • WenlongWenlong CanonsburgMember
    edited March 26

    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 ----------------------------

     

  • gigihmprayogogigihmprayogo Member
    edited March 26

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

  • WenlongWenlong CanonsburgMember
    edited March 27

    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 ----------------------------

     

  • gigihmprayogogigihmprayogo Member
    edited March 28

    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.

  • WenlongWenlong CanonsburgMember
    edited March 28

    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

     

  • gigihmprayogogigihmprayogo Member
    edited March 28

    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

  • DrDalyODrDalyO youtube.com/drdalyoMember
    edited May 16

    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

  • gigihmprayogogigihmprayogo Member
    edited May 17

    @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

  • gigihmprayogogigihmprayogo Member
    edited June 22

    @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

    image

  • @Wenlong I 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.

Sign In or Register to comment.