C.5. Accessing Solution and Material Data

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)