These APIs are provided for your convenience to help you access solution and material data easily.
c *** subroutine get_ElmInfo(inquire, value) c c description c function to inquire element and solution information c definition c inquire - query argument (string) c value - value of query argument c variables c inquire - value c 'LDSTEP' - load step number c 'ISUBST' - substep step number c 'IEQITR' - current interation number c 'NUMINTG' - number of gauss integration c 'ELEMID' - element number c 'MATID' - material number of current element c 'MATIPT' - integration point number c 'NSVAR' - number of state variable for current material at c gauss intg. c 'NCOMP' - number of vector components, such as stresses c c *** subroutine get_ElmData (inquire, elemId, kIntg, nvect, vect) c c description c function to put solution dependent variables c such as stress, strains at gauss intg. point. c definition c inquire - query argument (string) c elemId - element number c kIntg - guass intg. number c nvect - number of vector to be inquired c vect - vector to be inquired c variables c 'SIG' - stress vector c 'EPTO' - Total strain vector (EPEL+EPPL+EPCR+EPTH) c 'EPPL' - plastic strain vector c 'EPCR' - creep strain vector c 'EPTH' - thermal strain vector c 'ISIG' - initial stress vector c 'PLEQ' - accumulated equivalent plastic strain c 'CREQ' - accumulated equivalent creep strain c 'SVAR' - State variables (define by tb,state) c 'TEMP' - current temperature c 'TREF' - reference temperature c c *** subroutine put_ElmData (inquire, elemId, kIntg, nvect, vect) c description c function to put solution dependent variables c such as stress, strains at gauss intg. point. c !! Use this in caution, it overides ansys database. Usually c !! you should only write user defined state variables, c !! SVAR c definition c inquire - query argument (string) c elemId - element number c kIntg - gauss intg. number c nvect - number of vector to be inquired c Use the 'NCOMP' query to determine the correct c array sizes for tensor quantities c vect - vector to be inquired c c variables c 'SIG ' - stress vector c 'EPTO' - Total strain vector (EPEL+EPPL+EPCR+EPTH) c 'EPPL' - plastic strain vector c 'EPCR' - creep strain vector c 'EPTH' - thermal strain vector c 'ISIG' - Initial stress vector c 'PLEQ' - accumulated equivalent plastic strain c 'CREQ' - accumulated equivalent creep strain c 'SVAR' - State variables (define by tb,state)