General Mechanical

General Mechanical

Having Problem with XFEM while writing APDL commands in Ansys Workbench.

    • Puhan
      Subscriber

      Hello

      I hope you are doing well.


      I am having a problem with XFEM while writing APDL in Ansys Workbench.

    • Puhan
      Subscriber
      Hello
      It has been some days and I could not find almost noting in this forum can anyone makes a discussion on this please, this has already been solved in APDL in Ansys manual I am just trying to replicate the same in Workbench as have to solve some other problems.

      The whole problem is explained above. It is a three-point test. The below is the whole interface as you can see



      The command is written is like following


      "!Commands inserted into this file will be executed just prior to the ANSYS SOLVE command.
      !These commands may supersede command settings set by Workbench.

      !Active UNIT system in Workbench when this object was created:Metric (mm, t, N, s, mV, mA)
      !NOTE:Any data that requires units (such as mass) is assumed to be in the consistent solver unit system.
      !See Solving Units in the help system for more information.


      /PREP7
      !crack-growth criterion

      tb, cgcr, 2, , , STTMAX ! Fracture Behavior: Maximum circumferential stress
      tbdata, 1, 0.5 ! Maximum normal traction: = 0.5 N/mm2

      !Decay of stresses on newly cracked interface

      tb, cgcr, 2, , , RLIN
      tbdata, 1, 0.04, , 0.0

      ! Element component required for XFENRICH command
      esel,s,cent,x,-1,1
      cm, testcmp, elem
      allsel
      ! Define enrichment identification

      xfenrich,ENRICH1,TESTCMP ! Defines parameters associated with crack propagation using XFEM
      xfdata, ENRICH1, LSM, 939, 1042, 0.047123
      xfdata, ENRICH1, LSM, 939, 1043, 0.047123
      xfdata, ENRICH1, LSM, 939, 1045, -0.048062
      xfdata, ENRICH1, LSM, 939, 1044, -0.048062


      /com ******************************************
      /com LISTING OF CRACK INFORMATION
      /com ******************************************
      xflist

      ! Crack-tip element
      esel,s,elem,,939
      cm, crktipelem, elem ! Element set component for CINT command
      allsel,all

      ! Loading - Displacement on two nodes on top
      nsel,s,loc, x, -0.048062, 0.047123
      nsel,r,loc, y, 1.5
      d, all, uy, -0.16 ! Uy = -0.16mm
      d, all, ux, 0

      allsel

      /SOLU

      ! CINT calculations : Defines parameters associated with fracture parameter calculations
      CINT, NEW, 1
      CINT, CXFE, crktipelem ! Crack-tip element
      CINT, TYPE, STTMAX ! Uses STTMAX
      CINT, RSWEEP, 181, -90, 90
      ! CGROW calculations : Defines crack-growth information
      CGROW, NEW, 1
      CGROW, CID, 1
      CGROW, METHOD, XFEM ! Uses XFEM method for the crack propagation
      CGROW, FCOPTION, MTAB, 2 ! Fracture criterion
      SOLVE
      finish"


      So kindly please let me know, I will be grateful to you.

      Can you sir please look into it? Thank you very much.

    • Puhan
      Subscriber
      Sir can you please help? Can we do the same with the command in workbench for XFEM, if no there is an extension I found on the app and I added it in the workbench but I have some questions about that? But can you please at least give the answer to the first question?

      I will be grateful to you.

      With regards
      Biswabhanu Puhan

    • David Weed
      Ansys Employee

      I ran this on my end and discovered the same error regarding the PLANE182 key options. The issue here is that the MAPDL solver has some internal logic by which it forces certain element key options regardless of what you've initially specified. This is done through the ETCON command. You'll see that it's forcing keyopt(1) = 3, which is not supported for XFEM:
      ELEMENT TYPE1 IS PLANE182 WITH PLANE STRAIN OPTION. IT IS ASSOCIATED WITH
      LINEAR MATERIALS ONLY AND POISSON'S RATIO IS NOT GREATER THAN 0.49. KEYOPT(1)=3
      IS SUGGESTED AND HAS BEEN RESET.
      KEYOPT(1-12)=302000000000
      To override this, simply use ETCON,OFF in /PREP7. For instance, I place all of the material information in a command object under the surface body and you can see that etcon,off is set first:
      with this, the simulation ran to completion.



    • Puhan
      Subscriber
      Dear David
      Thank you very much, I will try to implement that.
      Also, can you please clarify if xfem can be used in Ansys in 3D or not?

      Again thank you very much, it will help a lot.
      With regards
      Biswabhanu Puhan
    • David Weed
      Ansys Employee

      XFEM is supported in 3-D; see the help and Example 3.8: Generating a Center Crack in a 3-D XFEM Model (MESH200 Method): https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/ans_frac/Hlp_G_FRACXFEM.html?q=xfem
    • Ali_sh
      Subscriber

      I have a problem with the XFEM command in the workbench too.
      I am trying to solve the same problem that Puhan mentioned earlier. It is not exactly the same I implemented it on the workbench; however, almost the same dimensions and boundary conditions.
      I have attached the data file here too.
      I do not have a problem defining enriched elements and specifying the crack tip. There is no error, and I also transferred the model to APDL and checked the elements there.
      The problem is that the crack will not propagate in my model, although I defined enriched area and pre-crack elements.
      I also tried to run with different radii, and nothing changed (CINT, RADIUS, 0.0005)
      here is my xflist data:
      DISCONTINUITY DATA ASSOCIATED WITH THIS ENRICHMENT NAME:
      ELEMNODEPHI
      12096184.94952E-05
      1209619-4.56814E-05
      1209599-4.58041E-05
      12095984.93726E-05
      I also checked the constrain equations after solution by transferring the model to APDL, and here is the result (CELIST). I do not know why the constraint equations are defined automatically in the enriched area after the solution:

      LIST ALL SETS FOR CONSTRAINT EQUATIONS WITH ANYNODES SELECTED
      MAXIMUM CONSTRAINT EQUATION NUMBER=1409

      Would you please look at the file and help me with that?


    • Ali_sh
      Subscriber
    • Ali_sh
      Subscriber
      Hi
      It is solved.
      I added the following in my commands
      /SOLU
      antype,0
      Bests Ali
Viewing 8 reply threads
  • You must be logged in to reply to this topic.