ANSYS Interface

Solver ANSYS
Type of mesh unstructured mesh
Dimension 2D and 3D

T U

(Return)

The interface writes the command deck or batch file according to the ANSYS 5.7 specifications. The ANSYS batch file created with this translator contains the following sections:

Creating the ANSYS Input File

The translator writes the ANSYS batch file using the following files: The steps for generating the fbc & par files are described in the subsequent sections.
Note:  The solver parameter file should be generated by loading ANSYS params menu, setting the solver parameter values and pressing <Accept> button, before using the write input menu.

To create the ANSYS batch input file, select the following menu entries from the ICEM CFD/CAE manager:

After successful execution of the translator, the ANSYS batch file is located in the project directory.

Defining solver parameters for ANSYS

The next sections describe how to define ANSYS commands using Output/Edit parameters menu.

Select Mesh order:
1. Low order / Linear (default)
2. High order / Quadratic

Note:  For meshes to have quadratic elements such as ANSYS element 95 (for Structural analysis) or element 119 (for HF Electromagnetic analysis), first perform the function "Linear-> Quadratic" on the mesh in order to create the higher order elements.

Set ANSYS Analysis Options:
1. Select ANSYS Product
Currently the following products are available:

  • Structural Analysis (ST - default)
  • High Frequency Electromagnetic Analysis (EH)
  • Flotran CFD Analysis (FL)
  • Thermal Analysis (TH)

  • 2. Select Analysis type (ANTYPE)
    The default anlysis type is None, for which the solution preprocessor (/SOLU) and subsequent commands are not output.
    The options for various analyses as follows:

    Structural analysis

    STATIC
  • Equation solvers(EQSLV): Direct(SPARSE), Pre-conditioned Conjugate Gradient iterative(PCG)
  • Include or exclude large deformation effects(NLGEOM)
  • Specifiy the number of substeps(NSUBST)

  • MODAL
  • Mode extraction methods(MODOPT): Block Lanczos(LANB)
  • Number of modes to expand and write(MXPAND)
  • Thermal analysis
    STATIC
  • Equation solvers(EQSLV): Incomplete Cholesky Conjugate Gradient iterative(ICCG)
  • Include or exclude large deformation effects(NLGEOM)
  • Specifiy the number of substeps(NSUBST)
  • 3. Set number of processors (/CONFIG,NPROC)
    4. Select Exit option for ANSYS batch job (/EXIT)
    If set to "Yes", the /EXIT command with the selected sub-option is written at the end of the ANSYS batch input file. If "No"(default), the exit command is not written.

    Set Flotran Options:
    1. Specify fluid families:
    Select from All, None or specify with "Create new" option. The elements of all the specified fluid familes will be automatically assigned material id 1.
    2. Set solution algorithms(FLDATA1):
    Set On(TRUE) or Off(FALSE) flags for the Flotran solution algorithms. If the dafault setting is changed, the FLDATA1 command appears in the Ansys batch file.
    3. Set convergence monitors for the DoF's(FLDATA3)
    4. Set output & Storage controls(FLDATA5)
    The FLDATA5 commands appear as per the logic for (2).
    5. Set convergence monitor output controls(FLDATA6)
    6. Define fluid properties(FLDATA7-FLDATA11):
    Any number of fluid properties can be created as required. The values required for FLDATA8-FLDATA11 can be entered for all properties other than Air properties.
    7. Set property variation flags(FLDATA13)
    If a property has been defined in (6) and is set as varying, the FLDATA13 command appears in the Ansys batch file.
    8-11. Specify reference properties(FLDATA14-FLDATA17)

    Define global parameters:
    The global loads supported are: acceleration(ACEL), rotational velocity(OMEGA) and rotational acceleration(DOMEGA).

    Define Real Constant sets (R/RMORE):
    Any number of named Real Constant sets can be created as required. The names can be associated either with the default elements or later, with a family in the b.c. menu. Id's are generated internally for the named sets, which appear in the batch file. Once a set is created (R), six values can be input for each sub-set. There could be more than one sub-set for a set. The additional sub-sets are written out with RMORE command.

    Set Element defaults:
    Specify defaults for 2-D & 3-D elements for the ANSYS product & Element order, selected above. Following ANSYS elements are currently supported:
     

    ANSYS Product
    Element Type(s)
    Supported Elements
    Low order (Linear)
    High order (Quadratic)
    2-D
    3-D
    2-D
    3-D
    Structural 
    SHELL/SOLID
    41, 43, 63, 143, 181*
    45, 64, 65, 185(default)
    93*
    92, 95, 1110(default), 187
    HF Emag
    HF
    --
    --
    --
    119, 120, Auto**(default)
    Flotran CFD FLUID 141(default) 142(default) --
    --
    Thermal
    SOLID
    --
    --
    --
    87, 90, Auto**(default)

    * The default ET for these element types is "None", in which case the elements for the specified type of IcemCFD families are not output. However, nodal components are still output if user selects not to ignore 2-D (TRI & QUAD) elements.
    ** These get automatically mapped to the suitable Ansys element depending on elements of the underlying IcemCFD family.

    Following default values are provided for each of the tabulated element:
    1. Real constant set name: Select from the list of Real Constant sets created earlier. ( default - None )
    2. Key options (KOP1-6).
    3. Solution printout flag (INOPR)

    Notes:
    1. The element defaults specified in this section can be overridden by specifying different Element type through the boundary conditions menu.
    2. The 1-D elements for Beams, Spars and Springs & Dampers can be specified through the b.c. menu. The 1-D elements currently supported as follows:
     

     ANSYS 1-D Element Type
    Supported Elements 
    Spars (LINK)
    8, 10, 11
    Beams (BEAM)
    4, 24, 44
    Springs & Dampers (COMBIN)
    7, 14, 37, 39, 40

    Define temperature dependant property data (MPDATA/MPTEMP):
    Any number of Property-Temperature named data sets can be created as required. The names can be later associated with a family in the b.c. menu. Under a given named data set, one can create as many Temperature-Property value pairs as required.

    Note:
    The temperature values keyed in the data points should be in non-descending order.

    Define coupled DOF's (CP):
    The coupled DOF's can be applied to the the nodes of one or more families.

    The CP command is issued as follows:
    CP, NEXT, LAB, fam1.nid1
    CP, HIGH, LAB, fam1.nid2
    ...
    CP, HIGH, LAB, fam1.nidlast
    CP, HIGH, LAB, fam2.nid1
    ...
    CP, HIGH, LAB, fam2.nidlast
    ...
    CP, HIGH, LAB, famn.nid1
    ...
    CP, HIGH, LAB, famn.nidlast

    pre-set variables:

    user defined variables:
    Select the DOF label for CP, LAB, see list below
    Select families, fam1 through famn

    If the ANSYS interface option "output components" is "yes", the CP command is issued in the following steps:
    CMSEL, S, fam1
    CMSEL, A, fam2
    ...
    CMSEL, A, famn
    CP,NEXT,LAB,ALL

    The CP command can be repeated for the same or different labels as many times as required, within the Ansys limitation that the selection of families across all sets is kept mutually exclusive. If not, a warning is issued.

    The DOF labels for CP available within the interface are:

        Analysis type    Label
        -------------    -----
    
        Structural       ALL, UX, UY, UZ, ROTX, ROTY, ROTZ
        Thermal          ALL, TEMP
        Emag-HF          ALL, AX
        Flotran          Not supported
    Note:
    The choice lists for the selection of families appear in the solver parameters menu ONLY IF the boundary condition file is loaded earlier.

    Define constraint equations (CE):
    The constraint equations can be applied either to the the nodes of a single family or to a pair of families that contain periodic nodes.

    The CE command when applied to a single family is issued as follows:
    CE, NEXT, CONST, fam1.nid1, Lab1, C1, fam1.nid1, Lab2, C2, fam1.nid1, Lab3, C3
    CE, HIGH, CONST, fam1.nid1, Lab4, C4, fam1.nid1, Lab5, C5, fam1.nid1, Lab6, C6
    CE, NEXT, CONST, fam1.nid2, Lab1, C1, fam1.nid2, Lab2, C2, fam1.nid2, Lab3, C3
    CE, HIGH, CONST, fam1.nid2, Lab4, C4, fam1.nid2, Lab5 C5, fam1.nid2, Lab6, C6
    ...
    CE, NEXT, CONST, fam1.nidlast, Lab1, C1, fam1.nidlast, Lab2, C2, fam1.nidlast, Lab3, C3
    CE, HIGH, CONST, fam1.nidlast, Lab4, C4, fam1.nidlast , Lab5, C5, fam1.nidlast, Lab6, C6

    If the periodic family is specified, the CE command output appears as follows:
    CE, NEXT, CONST, fam1.nid1, Lab1, C1, fam1.nid1, Lab2, C2, fam1.nid1, Lab3, C3
    CE, HIGH, CONST, fam1.nid1, Lab4, C4, fam1.nid1, Lab5, C5, fam1.nid1, Lab6, C6
    CE, HIGH, CONST, fam2.nid1, Lab1, K1, fam2.nid1, Lab2, K2, fam2.nid1, Lab3, K3
    CE, HIGH, CONST, fam2.nid1, Lab4, K4, fam2.nid1, Lab5, K5, fam2.nid1 Lab6, K6
    ...

    pre-set variables:

    user defined variables:
    Selected first family, fam1
    Second periodic family, if specified, fam2
    Enter the value of equation constant, CONST (real)
    Selected DOF labels for CE, Lab1 through Lab6, see list below
    Enter the values of DOF multipliers for Lab1 through Lab6, for fam1, C1 through C6 (real)
    Enter the values of DOF multipliers for Lab1 through Lab6, for fam2, K1 through K6 (real)

    The CE command can be repeated as many times as required. Currently no checks are carried out to check if the DOF's appearing in the CE commands are duplicated in any D or CP commands issued.

    The DOF labels for CE available within the interface are:

        Analysis type    Label
        -------------    -----
    
        Structural       Label1=UX, Label2=UY, Label3=UZ, Label4=ROTX, Label5=ROTY, Label6=ROTZ
        Thermal          Label1=TEMP
        Emag-HF          Label1=AX
        Flotran          Not supported
    Notes:
    1. The choice lists for the selection of families appear in the solver parameters menu ONLY IF the boundary condition file is loaded earlier.
    2. When the constraint equations between nodes of a pair of families are to be defined, the IcemCFD menu, Geometry>Mesh Params>Define periodicity should be used. The interface then automatically finds the corresponding periodic nodes in these two families. In this case the constraint equations are defined only for such nodes. If no periodic nodes are found, a warning is issued.

    Defining boundary conditions for ANSYS

    The next sections describe how to define ANSYS commands using Output/Boundary conditions menu.
    Please refer to the General Remarks section for more details.

    Note:  The left pane of the menu displays families grouped according to the element dimesions. If any families appear under the type Mixed/unknown, these families should be split into more families so that each new family contains elements having same dimension. Alternatively, the choices of writing 1-D & 2-D elements can be suitably made in the write input menu.

    Element Type (ET):

    The ET command contains the following:
    ET, ITYPE, ENAME, KOP1, KOP2, KOP3, KOP4, KOP5, KOP6, INOPR

    user defined variables:
    Select the value of ELEMENT TYPE (integer)
    Select the value of KOP1 (integer)
    Select the value of KOP2 (integer)
    Select the value of KOP3 (integer)
    Select the value of KOP4 (integer)
    Select the value of KOP5 (integer)
    Select the value of KOP6 (integer)
    Select the value of INOPR (integer)
    Select the name of Real Constant Set* (string)

    The ET command needs to be specified for each family defined in the boundary condition menu. It will automatically apply to all elements of these families. The element type number correspond to the number following the element name as given in the ANSYS element library (eg. 45 would refer to SOLID45 element type). ITYPE values are internally generated by the interface.

    The element types are linked to the elements with the ANSYS command TYPE when written in unblocked format. When written in blocked format, element type is specified as part of  the EBLOCK command.

    The real constant sets are linked to the elements with the ANSYS command REAL when written in unblocked format. When written in blocked format, real set id is specified as part of the EBLOCK command.

    *Ref: "Define Real Constant sets" section for defining solver parameters.

    Material Property (MP, MPDATA/MPTEMP):

    The MP command contains the following:
    MP, LAB, MAT, C0, C1, C2, C3, C4

    user defined variables:
    Select the label (LAB), see list below.
    Property-Temperature data option "None"
    Enter the value of C0 (real)
    Enter the value of C1 (real)
    Enter the value of C2 (real)
    Enter the value of C3 (real)
    Enter the value of C4 (real)

    The temperature dependant material properties can be specified with the same menu, by using "Specify" option.

    The MPDATA/MPTEMP commands contain the following:
    MPDATA, LAB, MAT, STLOC, C1, C2, C3, C4, C5, C6
    MPTEMP, STLOC, T1, T2, T3, T4, T5, T6

    pre-set variables:

    *** For Flotran analyses:
    Material id(MAT) = IcemCFD family id + 1, for non-fluid families.
                                 = 1, for fluid families.

    user defined variables:
    Select the label (LAB), see list below.
    Property-Temperature data option "Specify"
    Select the name of Property-Temperature Data Set* (string)

    The valid material property labels are:

        Description                                 Label 
        -----------                                 -----
    
        Elastic moduli                              EX, EY, EZ
        Coefficients of thermal expansion           ALPX, ALPY, ALPZ
        Reference temperature                       REFT
        Major Poisson's ratios                      NUXY, NUYZ, NUXZ
        Minor Poisson's ratios                      PRXY, PRYZ, PRXZ
        Shear moduli                                GXY, GYZ, GXZ
        K matrix multiplier for damping             DAMP
        Coefficient of friction                     MU
        Mass density                                DENS
        Specific heat                               C
        Enthalpy                                    ENTH
        Thermal conductivities                      KXX, KYY, KZZ
        Convection or film coefficient              HF
        Emissivity                                  EMIS
        Heat generation rate                        QRATE
        Viscosity                                   VISC
        Sonic velocity                              SONC
        Electrical resistivities                    RSVX, RSVY, RSVZ
        Electrical conductivities**                 CNDX, CNDY, CNDZ
        Electrical permitivities                    PERX, PERY, PERZ
        Magnetic relative permeabilities            MURX, MURY, MURZ
        Magnetic coercive forces                    MGXX, MGYY, MGZZ
        Loss tangent                                LSST
    The material properties are linked to the elements with the ANSYS command MAT when written in unblocked format. When written in blocked format, material id is specified as part of the EBLOCK command.

    *Ref: "Define temperature dependant property data" section for defining solver parameters.
    ** CNDn = 1/RSVn, RSVn values appear in the Ansys batch file.

    Local coordinate system (CSKP):

    The CSKP command is written alongwith a fixed set of other commands as follows:
    CSYS, 0
    K,1,x1,y1,z1
    K,2,x2,y2,z2
    K,3,x3,y3,z3
    CSKP,KCN,KCS,1,2,3
    KDELE,1,3,1

    pre-set variables:
    Local Coordinate Systems are created using View/Coord systems/Define menu of MED. The pre-set variable values are set as follows:

    user defined variables:
    Select the name of Local Coordinate System* (string)

    *As defined in MED.

    When a family is associated with a Local Coordinate system, all the nodes of elements in the family are aligned with this system with CSYS,KCN and NROTAT commands before applying nodal DoF constraints(D), nodal body loads(BF) and nodal forces(F).

    If any two families which have common nodes are associated with different local coordinate systems, a warning is issued.

    Nodal DoF Constraints (D):

    Before a D command is issued, the DOF accumulation flag is set for addition with
    DCUM, ADD, 1.0, 1.0, 0.0

    The D command contains the following:
    NSEL, ALL
    D, NODE, LAB, VALUE, VALUE2, NEND, NINC, Lab2, Lab3, Lab4, Lab5, Lab6

    pre-set variables:

    user defined variables:
    Select the degree of freedom label (LAB), see list below
    Enter the degree of freedom value (real)
    Enter the imaginary part of the DoF value2, if applicable (real)

    If the ANSYS interface option "output components" is "yes", the D command is issued in the following steps:
    CMSEL, S, family_name
    D, ALL, LAB, VALUE, VALUE2, NEND, NINC, Lab2, Lab3, Lab4, Lab5, Lab6

    The valid degree of freedom labels are:

        Description                                 Label
        -----------                                 -----
        Use all appropriate labels                  ALL
        Structural labels:
            displacements                           UX, UY, UZ
            rotations                               ROTX, ROTY, ROTZ
        Thermal labels:
            temperature                             TEMP
        Fluid labels:
            pressure                                PRES
            velocities                              VX, VY, VZ
            turbulent kinetic energy                ENKE
            turb.kin. E dissipation rate            ENDS
        Electric labels:
            voltage                                 VOLT
        Magnetic labels:
            scalar magnetic potential               MAG
            vector magnetic potentials              AX, AY, AZ
    Nodal Surface Loads (SF):

    The SF command contains the following:
    ESEL, ALL
    NSEL, S, NODE, ,nid1,nid1
    NSEL, A, NODE, nid2, nid2
    ...
    SF, ALL, LAB, VALUE, VALUE2

    pre-set variables:

    user defined variables:
    Select the surface load label (LAB), see list below
    Enter the surface load value (real)
    Enter the surface load value2, if applicable (real)

    If the ANSYS interface option "output components" is "yes", the SF command is issued in the following steps:
    ESEL, ALL
    CMSEL, S, family_name
    SF, ALL, LAB, VALUE, VALUE2

    The valid surface load labels are:
        Description                                 Label
        -----------                                 -----
        Structural labels:
            pressure                                PRES
        Thermal labels:
            convection                              CONV
            heat flux                               HFLUX
            radiation                               RAD
        Fluid labels:
            constant total pressure                 PTOT
        Electric labels:
            surface charge density                  CHRGS
        Magnetic labels:
            magnetic circuit interface              MCI
        HF Emag labels:
            exterior surface flag                   INF
            exterior waveguide port                 PORT
            surface shielding properties            SHLD
            impedance                               IMPD
    The SF command applies to 2-D or 3-D families only. The "ESEL, ALL" command is issued first, since SF command requires the elements to be exposed before the application.

    Uniformly distributed forces over surfaces (SURF154/SFE):

    The interface uses overlaid SURF154 elements in combination with SFE command to apply uniformly distributed forces over surfaces. This command is only valid in the structural analyses. The real constant set number and element coordinate system are set to zero before the subsequent ESURF command that generates the overlaid elements.

    The SFE command contains the following:
    ESEL, ALL
    NSEL, S, NODE, ,nid1,nid1
    NSEL, A, NODE, nid2, nid2
    ...
    MAT, mid
    ET, eid, 154
    ! Keyopt for normal pressure
    KEYOPT, eid, 6, kop6
    ! Keyopts for directional pressure
    KEYOPT, eid, 11, kop11
    KEYOPT, eid, 12, kop12
    TYPE, eid
    ESURF
    ESEL,S,MAT,,mid,,,
    ! For normal pressure
    SFE, ALL, 1, PRES, , (Total Force)/family_area
    ! For directional pressure
    SFE, ALL, 5, PRES, , (Total Force)/family_area, Px, Py, Pz

    pre-set variables:

    user defined variables:
    Enter the surface Total Force value (real)
    Select key option for SURF154 elements for normal pressure, kop6 (int)
    Select key options for SURF154 elements for directional pressure, kop11/12 (int)
    Enter the vector for directional pressure, "Px Py Pz" (real real real)

    If the ANSYS interface option "output components" is "yes", the set of NSEL commands are replaced by:
    CMSEL, S, family_name

    The valid surface load labels are:
        Description                                 Label
        -----------                                 -----
        Structural labels:
            pressure                                PRES

    Nodal Body Loads (BF):

    The BF command contains the following:
    NSEL, ALL
    BF, NODE, LAB, VAL1, VAL2, VAL3, PHASE

    pre-set variables:

    user defined variables:
    Select the body load label (LAB), see list below
    Enter the body load value1 (real)
    Enter the body load value2, if applicable (real)
    Enter the body load value3, if applicable (real)
    Enter value for phase, if applicable (real)

    If the ANSYS interface option "output components" is "yes", the BF command is issued in the following two steps:
    CMSEL, S, family_name
    BF, ALL, LAB, VAL1, VAL2, VAL3, PHASE

    The valid body load labels are:
        Description                                 Label
        -----------                                 -----
        Structural labels:
            temperature                             TEMP
            fluence                                 FLUE
        Thermal labels:
            heat generation rate                    HGEN
        Electric labels:
            charge density                          CHRGD
            temperature                             TEMP
        Magnetic labels:
            magnetic virtual displacement flag      MVDI
            temperature                             TEMP
        HF Emag labels:
            current density                         JS
            interior port                           PORT
            magnetic field                          H
            electric field                          EF
        Flotran labels:
            force density in momentum equation      FORC
            heat generation rate                    HGEN

    Nodal Forces (F):

    The F command contains the following:
    NSEL, ALL
    F, NODE, LAB, VALUE, VALUE2, NEND, NINC

    pre-set variables:

    user defined variables:
    Select the force label (LAB), see list below
    Enter the force value (real)
    Enter the imaginary part of the force value2, if applicable (real)

    If the ANSYS interface option "output components" is "yes", the F command is issued in the following steps:
    CMSEL, S, family_name
    F, ALL, LAB, VALUE, VALUE2

    The valid force labels are:
        Description                                 Label
        -----------                                 -----
        Structural labels:
            forces                                  FX, FY, FZ
            moments                                 MX, MY, MZ
        Thermal labels:
            heat flow                               HEAT
        Fluid labels:
            fluid flow                              FLOW
        Electric labels:
            electric charge                         CHRG
            current flow                            AMPS
        Magnetic labels:
            magnetic current segments               CSGX, CSGY, CSGZ
            magnetic flux                           FLUX
        Flotran labels:
            forces                                  FX, FY, FZ

    (Return)