Coupled Damage-Plasticity Microplane Damage Output

gigihmprayogogigihmprayogo Member Posts: 1

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 CanonsburgPosts: 474Member
    edited March 2020

    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 Posts: 15Member
    edited March 2020

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

  • WenlongWenlong CanonsburgPosts: 474Member
    edited March 2020

    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 Posts: 15Member
    edited March 2020

    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 CanonsburgPosts: 474Member
    edited March 2020

    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 Posts: 15Member
    edited March 2020

    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/drdalyoPosts: 6Member
    edited May 2020

    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 Posts: 15Member
    edited May 2020

    @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 Posts: 15Member
    edited June 2020

    @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

  • vaibhavtaranekarvaibhavtaranekar Posts: 66Member

    @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.

  • DrDalyODrDalyO youtube.com/drdalyoPosts: 6Member

    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!:


  • vaibhavtaranekarvaibhavtaranekar Posts: 66Member

    @DrDalyO Looks promising! Thanks for new video!

Sign In or Register to comment.