ANSYS Interface
Overview of the ANSYS interface.
- Read an ANSYS ASCII database.
- Create and edit an ANSYS ASCII database from within HyperWorks.
- Preview and edit ANSYS cards after they are created.
- Summarize ANSYS elements, loads, and properties.
- Output an ANSYS ASCII database.
- Convert an ANSYS binary results file into a HyperWorks binary results file that can be read into HyperWorks for post-processing.
- Assign macro commands to modify HyperWorks’s default ANSYS output.
HyperWorks treats ANSYS as a card image code.
HyperWorks supports ANSYS element types for STATIC STRUCTURAL, THERMAL, and MODAL analyses using ANSYS versions 2019 R2 and earlier. Result (.rst, .rmg, and .rth) files from ANSYS 2019 R2 and earlier are read in HyperView. HyperWorks can read .rst, .rmg and .rth files from ANSYS 8.1 or earlier versions. To read result files later than 8.1, use HyperView. Warnings and error messages are written to a file called ansys.msg. Unrecognized lines are written to a *.hmx file. These files are created in the directory from which HyperWorks is launched.
The ANSYS interface is only available once you have loaded the ANSYS user profile.
RBE3 Elements
In ANSYS, RBE3 card distribute the force/moment applied at the master node to a set of slave nodes, taking into account the geometry of the slave nodes as well as weighting factors.
In HyperWorks, RBE3 is an element that includes multiple 1D elements, which are defined between a single dependent (master) node and one or more independent (slave) nodes. RBE3 cards are created using the RBE3 panel (1D page).
- When a RBE3 element is created in HyperWorks, the DOFs are defined for the master as well as for the slave nodes. However, since the slave node DOFs are not applicable in , they are not exported.
- By default, when a RBE3 element is created in HyperWorks, the same weight factor that is applied at the master node is also applied on all the slave nodes. The Update subpanel in the RBE3 panel allows you to modify the weight factors for the individual slave nodes. Since the master node weight factor is not applicable in ANSYS, it is not exported.
- The RBE3 elements created in HyperWorks using other solver templates, such as Nastran, are exported according to template terminology.
Parameter Arrays Exported for RBE3 Elements
Two parameter arrays are exported for each RBE3 element. The first array contains slave node IDs and the second array contains slave node weights. These arrays appears in the beginning of the exported file.
RBE3, Master_ID, DOF, SLAVE#, WEIGHT#
Where,Master_ID
- ID of the master node
DOF
- Degrees of freedom checked in the RBE3 panel for RBE3 elements with ID #. DOF is
exported as follows:
- U
- If ux is checked
- UY
- If uy is checked
- UZ
- If uz is checked
- ROTX
- If rotx is checked
- ROTY
- If roty is checked
- ROTZ
- If rotz is checked
- UXYZ
- If ux, uy, and uz are checked
- RXYZ
- If rotx, roty, and rotz are checked
- ALL
- If all are checked
SLAVE#
- Name of the slave node ID array
WEIGHT#
- Name of the weighting factor array
Where, # is the RBE3 element ID.
The exportation location is the CP or CERIG elements.
FE Input Translator Support for RBE3
- Importing the exported files
- In ANSYS, RBE3 is not an element; it is created by a command called RBE3. ANSYS does not export these RBE3s as an RBE3 card, but rather as a set of constraint equations (CE). The HyperWorks- FE input translator imports CE equations as CE equations only, and not as RBE3 elements.
- Importing the HyperWorks exported files
- HyperWorks writes out RBE3 elements using RBE3 cards, therefore the H_ FE input translator imports the HyperWorks exported RBE3 cards as RBE3 elements.
Tips and Techniques
Tip and techniques for working with ANSYS in HyperWorks
- The operations performed in HyperWorks can also be saved as a compact HyperWorks binary file using the option.
- Bolt simulation configuration files are available in the ANSYS profile. In the Bolt panel, you can create general bolt, bolt with one or two washers, bolt with spider option and clips.
- Use the Mass Calc panel (Tool page) to determine the mass of your finite element model. Select the ansys.tpl template file through the Import tab. The mass calculation is supported for the following element type numbers: 1, 2, 3, 4, 5, 8, 10, 13, 16, 18, 20, 21, 23, 24, 25, 28, 31, 32, 33, 41, 42, 43, 44, 45, 46, 51, 53, 54, 55, 57, 58, 60, 61, 62, 63, 64, 67, 69, 70, 71, 75, 77, 78, 80, 82, 83, 87, 90, 91, 92, 93, 95, 96, 97, 98, 99, 107, 116, 117, 118, 119, 120, 121, 143, 145, 147, 148, 150, 152, 153, 154, 157, 162, 163, 164, 173, 174, 180, 181, 182, 183, 185, 186, 187, 191
- Each operation in HyperWorks results in an ASCII command that is added to a command.cmf
file. This file is useful if your computer shuts down while working in HyperWorks. You can restore your previous work by reading this file with the
command function, which can by found by clicking . You can delete this file if it requires too much disk space.
The command.cmf file can also be used to store repetitive HyperWorks operations. If you deal with the same set of geometrical and material properties, you can record the creation of these collectors, such as steel plate, foam solids and aluminum rods, into series of command files and read them as needed.
- The ANSYS template is associated with the Composites panel. Using this panel for
laminated elements, such as SHELL99, enables the following:Element orientation by two methods:
- By system assigns a system to the element (set ESYS for the element).
- By vector projects a vector on the element plane. A coordinate system, in which the x-axis is parallel to the defined vector, is created and assigned to the element as ESYS.
- The by system axis and by angle options are not available for this template.
- Visualization of the element orientation
- Visualization of the ply direction on a layer-by-layer basis. Visualizes the angles defined in the R card with respect to the element orientation.
- If you change KEYOPT3 for MASS21 and KEYOPT6 for BEAM23 elements, make sure you do so on the component as well as on property collector.
- When you click the card image button while creating a property collector, the GENERAL card is shown at the end of the list. This card is used to card edit the properties that are not used by any element.
- The ANSYS connectivity for a second order (3-node) line element (such as BEAM189 or SURF153), is as follows: End-node-I, End-node-J and Mid-node-K. However, for creation of a bar3 element in HyperWorks (using the bar panel/bar3 subpanel), pick node A, node B, and node C in the following order: End-node-I, Mid-node-K and End-node-J, respectively. The ANSYS template will export the bar3 element using the ANSYS connectivity.
- Apply loads in local coordinate systems (ANSYS NROTAT
card) using HyperWorks with the following methods:
- The Forces panel and the Moments panel allow you to apply loads in a local coordinate system by using the local system option.
- The set analysis option in the Systems panel, Assign subpanel can be used to assign a node to a coordinate system. A load applied to that node would be displayed correctly after exportation and importation of the ANSYS deck.
Pressure Load on Beam Elements
HyperWorks supports pressure load on bar and rod elements, which means you can import the pressure load [SFBEAM] applied on ANSYS BEAM elements.
- Import pressure load applied on BEAM3, BEAM4, BEAM23, BEAM44 elements. Import restrictions are explained below.
- Use the Pressure panel to apply SFBEAM load on beam elements.
- Export pressure load applied on BEAM elements in HyperWorks as SFBEAM load in ANSYS solver deck. The Export feature is explained in detail below.
Pressure Load Import
SFBEAM,ELEM,LKEY,Lab,R5.0,DIOFFST,DJOFFST
ELEM
- Element ID and Lab is always pres(pressure).
LKEY
- Load key number which determines the face of the beam where the pressure load is applied.
Restrictions
- The HyperWorks-ANSYS interface presently
supports the following LKEY values for each BEAM element. You can import SFBEAM load
with these LKEYs.
Table 1. ELEMENT TYPE SUPPORTED LKEYs BEAM3 1, 3, 4 BEAM4 1, 2, 4, 5 BEAM23 1, 3, 4 BEAM24 1, 2, 4, 5 BEAM44 1, 2, 4, 5 BEAM54 1, 3, 4 BEAM188 1, 2, 4, 5 BEAM189 1, 2, 4, 5 - DIOFFST, DJOFFST, which define offset values for pressure value at node I and J, are not supported in HyperWorks.
- SFLOAD, which applies a pressure load that varies across the length of the beam, is not supported in HyperWorks. Only pressure load with constant value can be imported.
Pressure Applied on BEAM Elements
- You can apply a pressure load in HyperWorks on any bar2, bar3 and rod, elements. Only the pressure loads which are applied on supported BEAM element types can be exported.
- If no option for direction is selected, pressure is applied on ‘element – y’ direction by default. You can use the options available in the Pressure Load panel to specify the direction of the load.
- The ANSYS solver allows pressure on beam elements in only specified faces of the elements, as mentioned by LKEYS. In other words, pressure on beam elements is applied in element co-ordinate system. Keep this in mind before determining the direction of the pressure.
- You cannot apply a pressure load that varies across the length of the BEAM even though it is allowed in the ANSYS Solver.
- Load offsets at node I and J are not supported.
Export Pressure Load on BEAM Elements
- Pressure on beams is exported as SFBEAM cards.
- Pressure only applied on BEAM3, BEAM4, BEAM23, BEAM44, BEAM54, BEAM188, BEAM189 elements will be exported.
- Pressure applied in any arbitrary direction is resolved in to corresponding element systems, and relevant LKEYs will be assigned while exporting. When you import the deck back to HyperWorks, you will see resolved loads.