Configuration File

Element Structure

Weld definitions are solver dependant (OptiStruct, Radioss, and so on). The specific solver template for the type of weld must be loaded before the welds can be created using a connector entity.

The configuration file can be manually loaded via the Control Manager.

Weld Definition Template

All the configurations follow the same template.

Each * flag is explained in detail below.

CFG <SOLVER> <USER_FE_TYPE> <USER_FE_NAME>
*filter <CE_TYPE>
*style <STYLE_TYPE> <STYLE_NUM>
*head
<HM_FE_CONFIG> <HM_FE_TYPE> <RIGID_FLAG> [<DOFS>]
*bodyext <BODY_FLAG> 
<HM_FE_CONFIG> <HM_FE_TYPE> <RIGID_FLAG> [<DOFS>]
*body <BODY_FLAG>
<HM_FE_CONFIG> <HM_FE_TYPE> <LENGTH_LOCATION_FLAG> [<DOFS>]
[<HM_FE_CONFIG> <HM_FE_TYPE> <LENGTH_LOCATION_FLAG> [<DOFS>]]
*post <POST_SCRIPT_NAME>
*calcmethod <CALCULATION_METHOD>

CFG <SOLVER> <USER_FE_TYPE> <USER_FE_NAME>

SOLVER

The solver template for which FE needs to be created. Supported solvers are: Abaqus, ANSYS, LS-DYNA, Nastran, OptiStruct, or PAM-CRASH.

USER_FE_TYPE

A unique (with respect to a solver) user-defined configuration type ID. User-defined CFGs should use numbers greater than 10,000 to ensure no collisions with future native HyperMesh CFGs.

USER_FE_NAME

The user-specified name for the FE configuration. The specified name is saved and displayed in the Connector Browser.

*filter <CE_TYPE>

*filter <CE_TYPE> can be used to allow only the specified connector types to realize the configuration.

For example: *filter spot seam indicates that this configuration can be realized only by the spot and seam connector types. In addition, this option is used as a filter when displaying FE configurations in the type = field representative controls.

CE_TYPE

• spot = Point tool
• bolt = Fastener tool
• seam = Line tool
• area = Area tool

*style <STYLE_TYPE> <STYLE_NUM>

The *style option indicates that the configurations have specific behaviours associated during realization, and that they are native types.

There is quite a large comprehensive list of styles and style numbers. This list is fully explained in the feconfig.cfg file.

The style and style number affect the attributes shown in the control. In the example in Figure 3, the only difference is the style, but the control attributes are very different.

*head

The head string is required to specify that a rigid, 1D, or contact is to be created to connect the weld node to the surrounding shell element.

*head lines must be followed with at most one HM_FE_CONFIG line.

*bodyext

The bodyext string is required to specify that the body of a weld has an extension associated with it. Currently, this extension can be created by a group of weld elements protruding at a distance of 0.5*times the thickness of the connected shell elements. *bodyext lines may be followed by one or more HM_FE_CONFIG lines.

Currently, it is used for the Hilock realization, but it can also be used with other realizations if you want the body element to have extra protrusion.

*body

The *body string is required.

*body lines may be followed by one or more HM_FE_CONFIG lines.

How the defined body elements are used is controlled by the *style.

*post

The lines are optional, but if specified it must be followed by the name (excluding path) of a valid TCL script with a .tcl extension. This TCL script must be located in, and will be searched in, the following order:

• Current working directory
• Your home directory
• Paths in HW_CONFIG_PATH environment variable
• Installation directory
• hm/bin directory
• hm/scripts directory
• hm/scripts/connectors/ directory

This post script will be automatically executed post FE realization. The post script is explained in more detail in Post Script.

*calcmethod

The *calcmethod tag can be used to define any valid custom realization (points/fasteners) to have a calculation method.

Currently this is only supported for Huth and Rutman.

FE Specification Rules