ANSYS Interface

Overview of the ANSYS interface.

The HyperMesh ANSYS interface allows you to:

Read an ANSYS ASCII database.
Create and edit an ANSYS ASCII database from within HyperMesh.
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 HyperMesh binary results file that can be read into HyperMesh for post-processing.
Assign macro commands to modify HyperMesh’s default ANSYS output.

HyperMesh treats ANSYS as a card image code.

HyperMesh 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. HyperMesh 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 HyperMesh is launched.

The ANSYS interface is only available once you have loaded the ANSYS user profile.

Import and Export Behavior

Generalp is created for elements with the Real ID and no real sets in the ANSYS deck.

An undefined section is created for valid element types if there is a sectionID referred in a element blockD.

Direct property assignment is given preference for all legacy and ANSYS-generate decks.

Export legacy comments option added to export decks with old comments.

Contact elements are not imported as components if there are no base elements associated with it.

"Convert Contact Elements" is removed in the import behavior.

Import

Import by HM comments
HM comments are honored for component, property, and material.
Import by Property
One component is created per property in the model.
Import by Material
One component is created per material in the model.
Import by one component
All the elements are organized to one component on import

Export

New HM comments for property, section and components:

Property

This has references related to name, ID, color ,sensor, and material ID.

Example:

!!HW_PROP ID=68 POOLID=1 NAME="PROP_68" COLOR=3 CARDIMAGE="BEAM4p" SENSID=3 MATID=1

Component

This has references related to component name, ID, color , and property ID.

Example:

!!HW_COMP ID=7 NAME="TYPE17-REAL46-MAT9" COLOR=55 PROPERTY_ID=0 POOLID=1

Section

This has references to section ID and color of the section entity.

Example:

!!HW_SECT ID=31 COLOR=5

Set segments

This has references to set segment ID, name, and color of the setsegment.

Example:

!!HW_CONTACT ID=<num> NAME="<name>" COLOR=<num>

Groups

This has reference to group name, color, and main and secondary sets ID.

Example:

!!HW_GROUP ID=<num> NAME="<name>" COLOR=<num> MAIN=<num>SECONDARY=<num>

General Features

Support of section and real for supported element types.

Reading old hm files from previous releases.

HM_COMP card image in the component is removed.

Component references to only property.

RBE3 Elements

In ANSYS, RBE3 card distribute the force/moment applied at the main node to a set of slave nodes, taking into account the geometry of the slave nodes as well as weighting factors.

In HyperMesh, RBE3 is an element that includes multiple 1D elements, which are defined between a single dependent (main) node and one or more independent (slave) nodes. RBE3 cards are created using the RBE3 panel (1D page).

RBE3 elements are different from Nastran RBE3 elements. In ANSYS, the RBE3 card is used to distribute the force/moments from the main node to a set of slave nodes. Whereas in Nastran, these elements define the rigid body motion. In HyperMesh, the RBE3 card is mapped as a RBE3 element. Therefore, when creating the RBE3 elements in HyperMesh for the template, the following points should be noted:

When a RBE3 element is created in HyperMesh, the DOFs are defined for the main 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 HyperMesh, the same weight factor that is applied at the main 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 HyperMesh 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.

Exportation of the SLAVE# Array:

*DIM,SLAVE#,ARRAY,      NS,       1,       1
*SET,SLAVE#(       1,       1,       1),  ID_1  
*SET,SLAVE#(       2,       1,       1),  ID_2  
*SET,SLAVE#(       3,       1,       1),  ID_3
.
.
.
*SET,SLAVE#(      NS,       1,       1),  ID_NS

Where,

#: HyperMesh element ID of the RBE3
NS: Number of slave nodes within the RBE3
ID_1, ID_2, ID_3,…,ID_NS: IDs of the slave nodes

Exportation of the WEIGHT# Array:

*DIM,WEIGHT#,ARRAY,      NS,       1,       1
*SET,WEIGHT#(       1,       1,       1),  WF_1
*SET,WEIGHT#(       2,       1,       1),  WF_2
*SET,WEIGHT#(       3,       1,       1),  WF_3
.
.
.
*SET,WEIGHT#(      NS,       1,       1),  WF_NS

Where,

#: HyperMesh element ID of the RBE3
NS: Number of slave nodes within the RBE3
WF_1, WF_2, WF_3,…,WF_NS: Weighting factors corresponding to each secondary node

Each RBE3 element is written using a RBE3 card with the following format:

RBE3, Main_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

If a combination of DOFs not listed above are checked, several RBE3 cards will be exported for the same element. For example, if ux, uy, and roty are checked, three RBE3 cards will be exported.

RBE3, Main_ID, UX, SLAVE#, WEIGHT#
RBE3, Master_ID, UY, SLAVE#, WEIGHT#
RBE3, Master_ID, ROTY, SLAVE#, WEIGHT#

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 HyperMesh- FE input translator imports CE equations as CE equations only, and not as RBE3 elements.
Importing the HyperMesh exported files: HyperMesh writes out RBE3 elements using RBE3 cards, therefore the H_ FE input translator imports the HyperMesh exported RBE3 cards as RBE3 elements.

Tips and Techniques

Tip and techniques for working with ANSYS in HyperMesh

The operations performed in HyperMesh can also be saved as a compact HyperMesh binary file using the File > Save As 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 HyperMesh 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 HyperMesh. You can restore your previous work by reading this file with the command function, which can by found by clicking File > Run > Command File. You can delete this file if it requires too much disk space.
The command.cmf file can also be used to store repetitive HyperMesh 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 HyperMesh (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 HyperMesh 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.
If both options of applying loads in local coordinate systems are used for the same node, the first method (via the Forces and Moments panels) takes precedence.

Pressure Load on Beam Elements

HyperMesh supports pressure load on bar and rod elements, which means you can import the pressure load [SFBEAM] applied on ANSYS BEAM elements.

The following items are supported under this feature:

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 HyperMesh as SFBEAM load in ANSYS solver deck. The Export feature is explained in detail below.

Pressure Load Import

SFBEAM is the keyword command in ANSYS decks to apply pressure load on BEAM elements. This command line has following arguments:

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.

Refer to the ANSYS solver documentation for information on the face of the beam and corresponding LKEY number as it changes from BEAM to BEAM.

Restrictions

The HyperMesh-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 HyperMesh.
SFLOAD, which applies a pressure load that varies across the length of the beam, is not supported in HyperMesh 9.0. Only pressure load with constant value can be imported.

Pressure Applied on BEAM Elements

You can apply a pressure load in HyperMesh 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 HyperMesh, you will see resolved loads.