ANSTOASAS, Fname, KEY
Creates an ASAS input file from the current ANSYS model.
FnameASAS file name. Defaults to Jobname.
KEYKey indicating type of file to produce:
0 | — | ASAS file for use by ANSYS Aqwa (no
loads written). Creates the file |
1 | — | ASAS file (all data written,
including loads). Creates the file |
2 | — | ASAS(NL) file. Creates the
file |
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:
Nodes
ANSYS element components (ASAS sets)
Added mass (via MASS21 element)
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.
The ASAS project name is defined as "ANSYS".
The solution control options are converted as follows:
| ANSYS Analysis Type | ASAS(L) / AQWA-WAVE Option | ASAS(NL) Option |
|---|---|---|
| Static (0) | JOB NEW LINE | JOB STAT |
| Buckling (1) | Not applicable | JOB STAT |
| Modal (2) | JOB NEW FREQ | JOB STAT |
| Transient (4) | Not applicable | JOB TRAN |
| Remaining analysis types | JOB NEW LINE | JOB 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).
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 Type | Supported Facilities | Notes |
|---|---|---|
| COMBIN14 - Spring-Damper | SPR1 | ASAS(L) does not support spring elements with non-coincident nodes. In this case, COMBIN14 is converted to FLA2. |
| MASS21 - Structural Mass | N/A | In ASAS, additional mass is not added as an element. Hence, if this element is included, equivalent ASAS lumped added mass information is written. |
| PLANE42 - 2-D Structural Solid [1] | QUM4 | - |
| SOLID45 - 3-D Structural Solid [1] | BRK8 | TET4 elements are only available in ASAS(L). Element is not converted if Pyramidal. |
| SHELL61 - Axisymmetric-Harmonic Structural Shell | ASH2 | ASH2 elements are only available in ASAS(L). |
| SHELL63 - Elastic Shell [1] | QUS4 | TBC3 elements are only available in ASAS(L). |
| PLANE82 - 2-D 8-Node Structural Solid [1] | QUM8 | - |
| SOLID92 - 3-D 10-Node Tetrahedral Structural Solid [1] | TE10 | - |
| SOLID95 - 3-D 20-Node Structural Solid [1] | BR20 | TE10 elements are only available in ASAS(L). Element is not converted if Pyramidal. |
| LINK180 - 3-D Finite Strain Spar (or Truss) | FLA2 | - |
| SHELL181 - 4-Node Finite Strain Shell | QUS4 | TBC3 elements are only available in ASAS(L). |
| PLANE182 - 2-D 4-Node Structural Solid | QUM4 | - |
| PLANE183 - 2-D 8-Node or 6-Node Structural Solid | QUM8 | - |
| SOLID185 - 3-D 8-Node Structural Solid or Layered Solid | BRK8 | TET4 elements are only available in ASAS(L). Element is not converted if Pyramidal. |
| SOLID186 - 3-D 20-Node Structural Solid or Layered Solid | BR20 | TE10 elements are only available in ASAS(L). Element is not converted if Pyramidal. |
| SOLID187 - 3-D 10-Node Tetrahedral Structural Solid | TE10 | TE10 elements are only available in ASAS(L). |
| BEAM188 - 3-D Linear Finite Strain Beam | BM3D | - |
| BEAM189 - 3-D Quadratic Finite Strain Beam | TCBM - if ASAS(L) | 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 | ASH2 | ASH2 elements are only available in ASAS(L). |
| SHELL281 - 8-Node Finite Strain Shell | TCS8 | - |
| PIPE288 - 3-D Linear Finite Strain Pipe | TUBE | - |
Documentation for this legacy element type appears in the Feature Archive.
Linear isotropic material conversion is supported for ASAS and ASAS(NL).
The following ASAS element geometry data is supported:
| ASAS Element Type | Support Facilities | Notes |
|---|---|---|
| BM3D | Sections, orientation by 3rd node position. | Sections are always defined separately. |
| TUBE | Thickness 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 ANSYS). |
| BM2D | A, IZ & AY properties defined. | |
| TCBM | Uniform 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. |
| STF4 | CTUB, RECT, and HREC ANSYS subtypes supported. | STF4 elements are only supported in ASAS(NL). Local y and z are 90° to the ANSYS definition. |
| FLA2 | Uniform cross sectional area. | |
| SPR1 / SPR2 | Stiffness (and also linear damping if ASAS(NL)) included. | |
| All non-beam elements | Constant 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.
No user sections are generated if AQWA-WAVE data is selected.
The following sections are converted for ASAS and ASAS(NL):
| ANSYS Section Type | ASAS Section Type | Notes |
|---|---|---|
| CTUB | TUB | Tubular section |
| I | FBI | Fabricated I beam |
| HREC | BOX | Fabricated box |
| All others | PRI | Prismatic section, only flexural properties defined. |
The following boundary conditions are converted for ASAS and ASAS(NL):
| ANSYS Boundary Condition | ASAS Boundary Condition | Notes |
|---|---|---|
| Nodal U* and ROT* constraints | SUPPressed freedoms: X, Y, Z, RX, RY, RZ | Skewed systems are not supported. |
| Nodal U* and ROT* imposed non-zero values | DISPlaced freedoms: X, Y, Z, RX, RY, RZ | Skewed systems are not supported. |
| CP and CE constraint equations | CONStraint equation data | Skewed systems are not supported. |
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:
| ANSYS Load Type | ASAS Load Type | Notes |
|---|---|---|
| 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 | 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, RZ | Skewed systems are not supported. |
| D (U* and ROT*) | PRESCRIBed displacements | |
| ACEL | BODY FORce |