ANSYS Interface
| Solver | ANSYS |
| Type of mesh | unstructured mesh |
| Dimension | 2D and 3D |
| T | U |
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:
To create the ANSYS batch input file, select the following menu entries from the ICEM CFD/CAE manager:
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
STATICThermal analysisEquation solvers(EQSLV): Direct(SPARSE), Pre-conditioned Conjugate Gradient iterative(PCG) Include or exclude large deformation effects(NLGEOM) Specifiy the number of substeps(NSUBST)
MODALMode extraction methods(MODOPT): Block Lanczos(LANB) Number of modes to expand and write(MXPAND)
STATIC3. Set number of processors (/CONFIG,NPROC)Equation solvers(EQSLV): Incomplete Cholesky Conjugate Gradient iterative(ICCG) Include or exclude large deformation effects(NLGEOM) Specifiy the number of substeps(NSUBST)
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:
|
|
Element Type(s) |
|
|||
| Low order (Linear) |
|
||||
| 2-D |
|
|
|
||
|
|
SHELL/SOLID |
|
|
|
|
|
|
HF |
|
|
|
|
| Flotran CFD | FLUID | 141(default) | 142(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 |
|
|
|
|
|
|
|
|
|
|
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:
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 supportedNote:
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:
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 supportedNotes:
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:
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 LSSTThe 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:
*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:
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, AZNodal 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:
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:
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:
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:
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