ANSTOASAS

ANSTOASAS, Fname, KEY
Creates an ASAS input file from the current Mechanical APDL model.

Valid Products: Pro | Premium | Enterprise | PrepPost | Solver | AS add-on

Fname

ASAS file name. Defaults to Jobname.

KEY

Key indicating type of file to produce:

0  

 — 

ASAS file for use by Ansys Aqwa (no loads written). Creates the file Fname.asas.

1  

 — 

ASAS file (all data written, including loads). Creates the file Fname.asas.

2  

 — 

ASAS(NL) file. Creates the file Fname.asnl.

Notes

This command creates an input file for the Ansys Asas Finite Element Analysis System from the model and loads currently in the database, based on the currently selected set of elements. Most common structural element types are written, as well as sections (or real constants), materials, boundary conditions and loads, and solution and load step options.

Data Written

The following data is written:

Details are provided in the following sections.

Not all data is written. You must verify the completeness and accuracy of the data. Only loading at the current step is transferred; hence, no load step history is captured.

Solution Control Options

The ASAS project name is defined as "Ansys".

The solution control options are converted as follows:

Mechanical APDL Analysis TypeASAS(L) / AQWA-WAVE OptionASAS(NL) Option
Static (0)JOB NEW LINEJOB STAT
Buckling (1) Not applicable

JOB STAT
SPIT KGEOM

Modal (2) JOB NEW FREQ

JOB STAT
SPIT KGEOM

Transient (4)Not applicableJOB TRAN
Remaining analysis typesJOB NEW LINEJOB STAT

For conversion to ASAS(NL), the large displacement option is set based on NLGEOM, final load solution time is set based on TIME, and sub-step times are set based on DELTIM or NSUBST (assuming constant step size).

Element Data

If you intend to use the data only with AQWA-WAVE, only the elements that form the wetted surface are required. Selecting these elements before invoking the ANSTOASAS command will improve performance. In order for AQWA-WAVE to identify the direction of the wave loading, all elements must be defined by nodes in a clockwise direction. For further information, refer to the AQWA-WAVE manual.

The element types are converted as follows:

Element TypeSupported Facilities Notes
COMBIN14 - Spring-Damper

SPR1 
SPR2 if rotational spring 
FLA2 (ASAS(L) only) 
if nodes are not coincident 
and longitudinal spring 

ASAS(L) does not support spring elements with non-coincident nodes. In this case, COMBIN14 is converted to FLA2.
MASS21 - Structural Mass N/AIn ASAS, additional mass is not added as an element. Hence, if this element is included, equivalent ASAS lumped added mass information is written.
PLANE42 - 2D Structural Solid [1]

QUM4 
TRM3 - if Triangular

-
SOLID45 - 3D Structural Solid [1]

BRK8 
TET4 - if Tetrahedral 
BRK6 - if Prism

TET4 elements are only available in ASAS(L). Element is not converted if Pyramidal.
SHELL61 - Axisymmetric-Harmonic Structural Shell ASH2ASH2 elements are only available in ASAS(L).
SHELL63 - Elastic Shell [1]

QUS4 
TBC3 - if Triangular

TBC3 elements are only available in ASAS(L).
PLANE82 - 2D 8-Node Structural Solid [1]

QUM8 
TRM6 - if Triangular

-
SOLID92 - 3D 10-Node Tetrahedral Structural Solid [1]TE10-
SOLID95 - 3D 20-Node Structural Solid [1]

BR20 
TE10 - if Tetrahedral  
BR15 - if Prism

TE10 elements are only available in ASAS(L). Element is not converted if Pyramidal.
LINK180 - 3D Finite Strain Spar (or Truss) FLA2-
SHELL181 - 4-Node Finite Strain Shell

QUS4 
TBC3 - if Triangular

TBC3 elements are only available in ASAS(L).
PLANE182 - 2D 4-Node Structural Solid

QUM4 
TRM3 - if Triangular

-
PLANE183 - 2D 8-Node or 6-Node Structural Solid

QUM8 
TRM6 - if Triangular

-
SOLID185 - 3D 8-Node Structural Solid or Layered Solid

BRK8 
TET4 - if Tetrahedral 
BRK6 - if Prism

TET4 elements are only available in ASAS(L). Element is not converted if Pyramidal.
SOLID186 - 3D 20-Node Structural Solid or Layered Solid

BR20 
TE10 - if Tetrahedral 
BR15 - if Prism

TE10 elements are only available in ASAS(L). Element is not converted if Pyramidal.
SOLID187 - 3D 10-Node Tetrahedral Structural Solid TE10TE10 elements are only available in ASAS(L).
BEAM188 - 3D Linear Finite Strain Beam BM3D-
BEAM189 - 3D Quadratic Finite Strain Beam

TCBM - if ASAS(L) 
STF4 - if ASAS(NL)

Refer to geometry details for limitations for TCBM elements. An orientation node is needed for STF4 and must be specified.
SHELL208 - 2-Node Finite Strain Axisymmetric Shell ASH2ASH2 elements are only available in ASAS(L).
SHELL281 - 8-Node Finite Strain ShellTCS8-
PIPE288 - 3D Linear Finite Strain Pipe TUBE-
  1. Documentation for this archived element type appears in the Feature Archive.

Material Data

Linear isotropic material conversion is supported for ASAS and ASAS(NL).

Geometry Data

The following ASAS element geometry data is supported:

ASAS Element TypeSupport FacilitiesNotes
BM3DSections, orientation by 3rd node position.Sections are always defined separately.
TUBEThickness and diameter defined, orientation by 3rd node or default local axes.Using the default local axes will result in BETA being set to 90° (to ensure that the ASAS local axes are the same as those in Mechanical APDL).
BM2DA, IZ & AY properties defined. 
TCBMUniform section properties supported.TCBM does not support general local axis orientations. Hence, elements will only be correct if they lie in the global XY plane.
STF4CTUB, RECT, and HREC Mechanical APDL subtypes supported.STF4 elements are only supported in ASAS(NL). Local y and z are 90° to the Mechanical APDL definition.
FLA2Uniform cross sectional area. 
SPR1 / SPR2Stiffness (and also linear damping if ASAS(NL)) included. 
All non-beam elementsConstant element thickness. 

For all beam elements, the third node position must be explicitly defined. If the position is not defined, the program generates an error code (-1) in the output file.

Section Data

No user sections are generated if AQWA-WAVE data is selected.

The following sections are converted for ASAS and ASAS(NL):

Mechanical APDL Section TypeASAS Section TypeNotes
CTUBTUBTubular section
IFBIFabricated I beam
HRECBOXFabricated box
All othersPRIPrismatic section, only flexural properties defined.

Boundary Conditions

The following boundary conditions are converted for ASAS and ASAS(NL):

Mechanical APDL Boundary ConditionASAS Boundary ConditionNotes
Nodal U* and ROT* constraintsSUPPressed freedoms: X, Y, Z, RX, RY, RZSkewed systems are not supported.
Nodal U* and ROT* imposed non-zero valuesDISPlaced freedoms: X, Y, Z, RX, RY, RZSkewed systems are not supported.
CP and CE constraint equationsCONStraint equation dataSkewed systems are not supported.

Loads

No user loading is generated if AQWA-WAVE data is selected. However, a load case (number 1000) is automatically defined to identify the wetted surface of the elements for use by AQWA-WAVE based on the normal surface loads applied to the solid or shell elements.

Pressure loads from SURF154 elements are converted to equivalent nodal loads for ASAS. For AQWA-WAVE, the SURF154 pressures are used to identify the wetted surface of the underlying elements. The following loads are converted for ASAS:

Mechanical APDL Load TypeASAS Load TypeNotes
SFE (PRES)PRESSURE (no sub-types)Element families supported: Solids, shells (excluding edge pressures), planes (edge pressures only), and axisymmetric shells.
SFE (PRES)

DISTRIBUted loading 
Shells - ML2 
Beams - BL1 / BL2 
Tubes - GL1 
Curved beams - CB1

Element families supported: Shells (edge pressures only), Beams (includes tubes and curved beams).
F (F* and M*)NODAL Load, in X, Y, Z, RX, RY, RZSkewed systems are not supported.
D (U* and ROT*)PRESCRIBed displacements 
ACELBODY FORce 

Menu Paths

This command cannot be accessed from a menu.