开源线弹性静力小变形UEL子程序分享

https://github.com/bibekanandadatta/Abaqus-UEL-Elasticity

CPE4 C3D8 C3D20 CPE6 CPE8

uel_mech

global_parameters.forerror_logging.forlinear_algebra.forlagrange_element.forgauss_quadrature.forsolid_mechanics.forpost_processing.formode.for

include 'global_parameters.for'     ! global parameters moduleinclude 'error_logging.for'         ! error/ debugging moduleinclude 'linear_algebra.for'        ! linear algebra moduleinclude 'lagrange_element.for'      ! Lagrange element moduleinclude 'gauss_quadrature.for'      ! Guassian quadrature moduleinclude 'solid_mechanics.for'       ! solid mechanics moduleinclude 'post_processing.for'       ! post-processing moduleinclude 'mode.for'

compile_fortran += ['/Qmkl:sequential']

! **********************************************************************! ****************** ABAQUS USER ELEMENT SUBROUTINE ********************! **********************************************************************! make sure to have the correct directory      include 'global_parameters.for'     ! global parameters module      include 'error_logging.for'         ! error/ debugging module      include 'linear_algebra.for'        ! linear algebra module      include 'lagrange_element.for'      ! Lagrange element module      include 'gauss_quadrature.for'      ! Guassian quadrature module      include 'solid_mechanics.for'       ! solid mechanics module      include 'post_processing.for'       ! post-processing module      include 'mode.for'      SUBROUTINE UEL(RHS,AMATRX,SVARS,ENERGY,NDOFEL,NRHS,NSVARS,     & PROPS,NPROPS,COORDS,MCRD,NNODE,Uall,DUall,Vel,Accn,JTYPE,TIME,     & DTIME,KSTEP,KINC,JELEM,PARAMS,NDLOAD,JDLTYP,ADLMAG,PREDEF,     & NPREDF,LFLAGS,MLVARX,DDLMAG,MDLOAD,PNEWDT,JPROPS,NJPROPS,PERIOD)      ! This subroutine is called by Abaqus with above arguments      ! for each user elements defined in an Abaqus model. Users are      ! responsible for programming the element tangent/ stiffness      ! matrix and residual vectors which will be then assembled and      ! solved by Abaqus after applying the boundary conditions.      use global_parameters      use error_logging      use user_element      use post_processing      INCLUDE 'ABA_PARAM.INC'      DIMENSION RHS(MLVARX,*),AMATRX(NDOFEL,NDOFEL),PROPS(*),     & SVARS(*),ENERGY(8),COORDS(MCRD,NNODE),UAll(NDOFEL),     & DUAll(MLVARX,*),Vel(NDOFEL),Accn(NDOFEL),TIME(2),PARAMS(*),     & JDLTYP(MDLOAD,*),ADLMAG(MDLOAD,*),DDLMAG(MDLOAD,*),     & PREDEF(2,NPREDF,NNODE),LFLAGS(*),JPROPS(*)      ! user coding to define RHS, AMATRX, SVARS, ENERGY, and PNEWDT      integer, intent(in)   :: NDOFEL, NRHS, NSVARS, NPROPS, MCRD      integer, intent(in)   :: NNODE, JTYPE, KSTEP, KINC, JELEM      integer, intent(in)   :: NDLOAD, JDLTYP, NPREDF, LFLAGS      integer, intent(in)   :: MLVARX, MDLOAD, JPROPS, NJPROPS      real(wp), intent(in)  :: PROPS, COORDS, DUall, Uall, Vel, Accn      real(wp), intent(in)  :: TIME, DTIME, PARAMS, ADLMAG, PREDEF      real(wp), intent(in)  :: DDLMAG, PERIOD      real(wp), intent(out)           :: RHS, AMATRX      real(wp), intent(out), optional :: SVARS, ENERGY, PNEWDT      character(len=8)      :: abqProcedure      integer               :: nDim, nStress      character(len=2)      :: analysis      logical               :: nlgeom      integer               :: nInt, nPostVars      integer               :: lenJobName,lenOutDir      character(len=256)    :: outDir      character(len=256)    :: jobName      character(len=512)    :: errFile, dbgFile      type(logger)          :: msg      ! initialize the output variables to be defined for Abaqus subroutine      energy        = zero      amatrx        = zero      rhs(:,nrhs)   = zero      ! Open an error and debug file for the current job.      ! See Abaqus documentation for Fortran unit number.      ! File unit numbers are defined in the error_logging module.      call getJobName(jobName,lenJobName)      call getOutDir(outDir,lenOutDir)      errFile = trim(outDir)//'\aaERR_'//trim(jobName)//'.dat'      dbgFile = trim(outDir)//'\aaDBG_'//trim(jobName)//'.dat'      call msg%fopen( errfile=errFile, dbgfile=dbgFile )      ! change the LFLAGS criteria as needed (check Abaqus UEL manual)      if( (lflags(1)  .eq.  1) .or. (lflags(1)  .eq.  2) ) then        abqProcedure = 'STATIC'      else        call msg%ferror(flag=error, src='UEL',     &       msg='Incorrect Abaqus procedure.', ia=lflags(1))        call xit      end if      ! check if the procedure is linear or nonlinear      if (lflags(2)  .eq.  0) then        nlgeom = .false.      else if (lflags(2) .eq. 1) then        nlgeom = .true.      end if      ! check to see if it's a general step or a linear purturbation step      if(lflags(4)  .eq.  1) then        call msg%ferror(flag=error, src='UEL',     &       msg='The step should be a GENERAL step.', ia=lflags(4))        call xit      end if      ! set parameters specific to analysis and element types      if ((jtype .ge. 1).and.(jtype .le. 4)) then         ! three-dimensional analysis        nDim      = 3        analysis  = '3D'        nStress   = 6      else if ((jtype .ge. 5).and.(jtype .le. 8)) then    ! plane strain analysis        nDim      = 2        analysis  = 'PE'        nStress   = 3      else if ((jtype .ge. 9).and.(jtype .le. 12)) then   ! plane stress analysis        nDim      = 2        analysis  = 'PS'        nStress   = 3      else if ((jtype .ge. 13).and.(jtype .le. 16)) then  ! axisymmetric analysis        ! CAUTION: axisymmetric elements are not validated yet        nDim      = 2        analysis  = 'AX'        nStress   = 4      else        call msg%ferror( flag=error, src='UEL',     &       msg='Element is unavailable.', ia=jtype )        call xit      end if      nInt      = jprops(1)      nPostVars = jprops(2)      ! array containing variables for post-processing      if (.not. allocated(globalPostVars)) then        allocate( globalPostVars(numElem,nInt,nPostVars) )         ! print job-related information the first time        call msg%finfo('---------------------------------------')        call msg%finfo('------- Abaqus SMALL STRAIN UEL -------')        call msg%finfo('--------- SOURCE: uel_mech.for --------')        call msg%finfo('---------------------------------------')        call msg%finfo('--- Abaqus Job: ', ch=trim(jobName))        call msg%finfo('---------------------------------------')        call msg%finfo('------- PROCEDURE       = ', ch=abqProcedure)        call msg%finfo('------- ANALYSIS TYPE   = ', ch=analysis)        call msg%finfo('---------- NLGEOM       = ', la=nlgeom)        call msg%finfo('------- MODEL DIMENSION = ', ia=nDim)        call msg%finfo('------- ELEMENT NODES   = ', ia=nNode)        call msg%finfo('---------------------------------------')        call msg%finfo('-------- INTEGRATION SCHEME -----------')        call msg%finfo('----------- NINT   = ', ia=nInt)        call msg%finfo('---------------------------------------')        call msg%finfo('---------- POST-PROCESSING ------------')        call msg%finfo('--- NO OF ELEMENTS            = ',ia=numElem)        call msg%finfo('--- OVERLAY ELEMENT OFFSET    = ',ia=elemOffset)        call msg%finfo('--- NO OF VARIABLES AT INT PT = ',ia=nPostVars)        call msg%finfo('---------------------------------------')      end if       ! call the element subroutine with extended input arguments       call uelMech(RHS,AMATRX,SVARS,ENERGY,NDOFEL,NRHS,NSVARS,     & PROPS,NPROPS,COORDS,MCRD,NNODE,Uall,DUall,Vel,Accn,JTYPE,TIME,     & DTIME,KSTEP,KINC,JELEM,PARAMS,NDLOAD,JDLTYP,ADLMAG,PREDEF,     & NPREDF,LFLAGS,MLVARX,DDLMAG,MDLOAD,PNEWDT,JPROPS,NJPROPS,PERIOD,     & NDIM,ANALYSIS,NSTRESS,NINT)
      END SUBROUTINE UEL

! **********************************************************************! ************** ABAQUS USER OUTPUT VARIABLES SUBROUTINE ***************! **********************************************************************
      SUBROUTINE UVARM(UVAR,DIRECT,T,TIME,DTIME,CMNAME,ORNAME,     & NUVARM,NOEL,NPT,LAYER,KSPT,KSTEP,KINC,NDI,NSHR,COORD,     & JMAC,JMATYP,MATLAYO,LACCFLA)
      ! This subroutine is called by Abaqus at each material point (int pt)      ! to obtain the user defined output variables for standard Abaqus      ! elements. We used an additional layer of standard Abaqus elements      ! with same topology (same number of nodes and int pts) on top of      ! the user elements with an offset in the numbering between the user      ! elements and standard elements. This number is defined in the      ! post_processing module and should match with Abaqus input file.
      use global_parameters      use post_processing
      INCLUDE 'ABA_PARAM.INC'
      CHARACTER*80 CMNAME,ORNAME      CHARACTER*3 FLGRAY(15)      DIMENSION UVAR(NUVARM),DIRECT(3,3),T(3,3),TIME(2)      DIMENSION ARRAY(15),JARRAY(15),JMAC(*),JMATYP(*),COORD(*)
      ! the dimensions of the variables FLGRAY, ARRAY and JARRAY      ! must be set equal to or greater than 15.
      ! explicityly define the type for uvar to avoid issues      real(wp)        :: uvar
      ! assign the stored global variables to the UVAR for Abaqus to process      uvar(1:nuvarm)  = globalPostVars(noel-elemOffset,npt,1:nuvarm)
      END SUBROUTINE UVARM
! **********************************************************************! **********************************************************************

cantilever_U7_CPE4_elem_80_elastic.inpsingle_elem_uniaxial_U3_C3D8_elastic.inpsingle_elem_uniaxial_U4_C3D20_elastic.inpsingle_elem_uniaxial_U5_CPE3_elastic.inpsingle_elem_uniaxial_U6_CPE6_elastic.inpsingle_elem_uniaxial_U7_CPE4_elastic.inpsingle_elem_uniaxial_U8_CPE8_elastic.inp

*Heading** abaqus/ standard input file for uniaxial test of** single CPE8 (U8) type element for uel_mech.for**节点坐标信息*Node1,           0.,           0....****************************************************用户自定义单元信息*User Element,Type1,2*Element, type=U81, 1, 2, 4, 3, 5, 6, 7, 8***************************************************Nset, nset=All, generate 1,  8,  1*Elset, elset=All 1,*Nset, nset=Bottom 1, 2, 5*Elset, elset=Bottom 1,*Nset, nset=Left 1, 3, 8*Elset, elset=Left 1,*Nset, nset=Right, generate 2,  6,  2*Elset, elset=Right 1,*Nset, nset=Top 3, 4, 7*Elset, elset=Top 1,****************************************************给用户自定义单元赋予属性*uel property,elset=all** E, nu, nInt, nPostVars79E9, 0.3, 9, 6**************************************************** same element connectivity as the user element** uses built-in abaqus element to overlay results** negligible young's modulus won't affect the result**嵌套的一层abaqus自带的单元用于可视化*Element, type=CPE8100001, 1, 2, 4, 3, 5, 6, 7, 8*Elset, elset=elDummy 100001*Solid section, elset=elDummy, material=Dummy**给嵌套的一层单元赋予材料属性，无限小的材料属性*Material, name=Dummy*Elastic1.e-20** strain vector (3) and stress vector (3) as user output**UVARM子程序用于可视化*User output variables6****************************************************给左边界和底边界固定住*BoundaryLeft, 1, 1Bottom, 2, 2****************************************************定义幅值曲线*Amplitude, name=LinearRamp0., 0., 1., 1.***************************************************Step, name=Stretch, nlgeom=NO, inc=1000**静力分析步*Static1, 1, 0.001, 1*给右边界施加力*Boundary, amplitude=LinearRampRight, 1, 1, 0.01*Restart, write, frequency=0 *Output, field, frequency=1, time marks=no*node output, nset=Allu,rf** specify the user-defined output for the dummy element set*element output, elset=elDummyuvarm*End Step**************************************************

call abaqus job=cantilever_U7_CPE4_elem_80_elastic user=uel_mech cpus=10 intpause

---------------------------------------------- Abaqus SMALL STRAIN UEL ---------------- SOURCE: uel_mech.for -------------------------------------------------- Abaqus Job: single_elem_uniaxial_U7_CPE4_elastic---------------------------------------------- PROCEDURE       = STATIC------- ANALYSIS TYPE   = PE---------- NLGEOM       = F------- MODEL DIMENSION = 2------- ELEMENT NODES   = 4----------------------------------------------- INTEGRATION SCHEME ---------------------- NINT   = 4------------------------------------------------- POST-PROCESSING --------------- NO OF ELEMENTS            = 50000--- OVERLAY ELEMENT OFFSET    = 100000--- NO OF VARIABLES AT INT PT = 6---------------------------------------