Browsers supply a great deal of view-related functionality in HyperMesh by listing the parts of a model in a tabular and/or tree-based format, and providing controls inside the table
that allow you to alter the display of model parts.
Connectors are geometric entities (not FE) used to create connections between components. Connectors are used to realize
FE idealizations of the physical connection. Just as you create an FE mesh on a surface, you create FE connections
by realizing a connector.
There are many advantages to the way connectors store information. Not only does this local storage allow you to edit
the connector definition, it also allows you to review connector details and the quality of the realization.
Most of the information stored in the connector entity can be exported to a master connectors file, which contains
connector entity information such as location, link entity, link entity state, link entity rules. The exported file
may also contain metadata information stored in the connector.
Create weld points at a predefined pitch distance so that the model build process can continue without the need to
wait for the published weld data from CAD. Autopitch is useful when working with elements, not geometry.
Perform automatic checks on CAD models, and identify potential issues with geometry that may slow down the meshing
process using the Verification and Comparison tools.
The FE configuration file (feconfig.cfg) is used to define custom
welds such as ACM (Area Contact Method) and other special types.
Weld definitions are solver dependant (Nastran, LS-DYNA, and so on). The weld definition in the file includes the type of
weld to create and the surrounding connector to shells. The specific solver template for the
type of weld must be loaded before the welds can be created using a connector entity. When
HyperWorks Desktop or HyperMesh launches, it
searches for feconfig.cfg in the following locations, listed in search
order:
The product installation path
HW_CONFIG_PATH (a specified environment variable)
Your home directory (in UNIX, for example)
The current working directory.
By default, the feconfig.cfg file from the
<install_directory>/hm/bin directory is loaded in each of the
panels related to each connector type, such as Spot, Seam and Area. It is not recommended to
have more than one config file of the same name, even in different directories, as the
results can be unpredictable as to which one will be used by default.
Weld Definition Template
Where,
CFG
Keyword to start a custom weld definition.
SOLVER
The solver template for which FE needs to be created.
A unique (with respect to a solver) user defined configuration type ID.
Customer-defined CFGs should use numbers greater than 10,000 to ensure no
collisions with future native HM CFGs.
USER_FE_NAME
The user-specified name for the FE configuration. The specified name is saved
and displayed in the Connector Browser.
Note: This should be the first line in
the custom weld definition.
*filter
Allows 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 of respective realize
panels.
*filter lines also set which panel the CFG is visible in.
CE_TYPE
The connector type, spot, bolt, seam, area, and so on.
*style
Indicates that the configurations have specific behaviors associated during
realization, and that they are native types.
Note: The style definition line for these
configurations must not be edited.
For example, *style bolt 1 indicates that this is a bolt connection of type 1 that
creates a specific bolted connection between the parts.
STYLE_TYPE
The connector style name, such as "adhesive", "bolt", "acm", "quad",
"continuous", and so on.
STYLE_NUM
The connector style number:
Adhesive:
"1" mesh independent adhesive nodes tie to shells with
RBE3/RBE2.
"2" force shell gap length on. Adhesive (HEXA element) shares nodes
with shell at co-incident locations.
Bolt:
"0" normal bolt: "wagon wheels" in the holes.
"1" symmetrical spider bolt.
"2" unsymmetrical spider bolt: the middle node is biased towards one
hole.
"3" cylinder bolt: ties together all nodes within virtual
cylinder.
ACM:
"1" share the nodes of HEXA element for consecutive layers (> 2T) and
the length of HEXA is average of part thickness.
"2" HEXA elements in consecutive layers have unique nodes and the
length of HEXA is average of part thickness.
"3" share the nodes of HEXA elements for consecutive layers and the
length of HEXA is the gap distance between parts.
"5" HEXA nodes are not equivalenced with the shell nodes/washer
nodes, if a washer is present.
Quad
"1" create two sets of QUAD4 elements, first along projection
direction and second at an orientation determined by average part
thickness.
"2" create one set of QUAD4 elements at an orientation determined by
average part thickness.
*head
The string head is required to specify that a rigid 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.
HM_FE_CONFIG
The config for the rigid currently supported.
The various types supported are "bar2", "bar3", "equations", "gap",
"hex8"(3D), "plot", "mass"(0D), "rigid", "rigidlink", "rbe3", "rod", "spring",
"weld", "quad4"(2D seam only), or "penta6"(3D adhesive only).
HM_FE_TYPE
Unique (with respect to a solver) user defined configuration type id defined
in the solver template.
RIGID_FLAG
Defines the number and arrangement of rigids.
"0" is a single rigid
"1" is multiple rigids
"2" is multiple rigids to outer shell nodes (for 2D bolt washers
only)
"3" is multiple rigids to outer alternate shell nodes (for 2D bolt
washers only)
"10" is multiple rigids with a 0 length leg connecting with body (for
bolt only)
"12" is multiple rigids to inner and outer shell nodes (for 2D bolt
washers only)
"13" is multiple rigids to inner and outer alternate shell nodes (for 2D
bolt washers only)
DOFS (Optional)
Degrees of freedom of the rigid (1-6).
*body
Specifies that a weld is to be created to connect the link entities added to the
connector.
*body lines may be followed by one or more HM_FE_CONFIG lines
BODY_FLAG
The body flag is used to calculate the length of the weld. If the body flag =
0, the length is calculated based on the distance between the connecting layers
(link entities). If the body flag = 1, the length is calculated based on the
average thickness of the connecting layers (link entities).
HM_FE_CONFIG
The config for the rigid currently supported. The various types supported are
"bar2", "bar3", "equations", "gap", "hex8"(3D), "plot", "mass"(0D), "rigid",
"rigidlink", "rbe3", "rod", "spring", "weld", "quad4"(2D seam only), or
"penta6"(3D adhesive only).
HM_FE_TYPE
The solver defined type for the HyperMesh config.
For example, CBUSH is of config spring and type 6. The type number is defined in
respective solver templates and differs, based on the solver.
LENGTH_LOCATION_FLAG
0D element details.
"0" place the 0D element along the proposed 1D element path. If this 0D
element is the only config given in the *body, then it is placed at the
center of the proposed 1D element path.
"1" has the same behavior as "0" except only a single 0D element is
created even if multiple bodies are created (as happens in >2T welds)
"2" place the 0D element at the connector location.
1D element details.
"0" force zero length welds.
>"0" but <"1" denote a percentage of the distance between shells the
length of a given weld should be. To create series welds, all the
PERCENT_LENGTH_FLAG variables for a given *body must add up less than or
equal to 1.0. Example: 0.33 or 0.50
"1" force each body weld to have a length equal to the distance between
the shells, which can be used for parallel welds.
"2" place the 1D element at the connector location, with both nodes
coincident.
"3" place multiple (thickness-1) 1D elements at the connector location
connected end-to-end, with all nodes coincident.
3D element details.
"0" force a floating hexa element to have a length equal to half the
distance specified by the BODY_FLAG.
"1" force the hexa element's length to be equal to the full distance
specified by the BODY_FLAG.
DOFS (Optional)
The degrees of freedom (1-6) of the rigid.
*post
*post lines are optional, but if specified, they must be followed by the name,
excluding path, of a valid TCL script with a .tcl extension. HyperMesh searches for the TLC
script in the locations and order specified below:
Current working directory
Users 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, and can be
used to edit weld properties, attributes, and other solver specific details.
FE Specification Rules
Each solver will have a specific definition so the same user-defined types can be repeated
for each solver.
The head and the body definition must begin with a "*" to define rigid and weld
definitions.
Multiple solid element combinations are not currently supported. Therefore, an ACM can have
only one hexa weld element specified in the definition.
1D and 3D element combinations are not supported.
The total length of series welds cannot exceed 1.0 (100 percent). Hence there cannot be
three welds specified in series having a length factor of 0.5 (50 percent) each.
Series and parallel weld element combinations are not supported.
Series welds are not supported where the link entities are coincident. Series welds are not
created when the distance between the connecting link entities is zero.
User comments should start with a hash character "#".
FE Configuration Examples
FE configuration examples for washers, ACM welds, series welds, parallel welds, and 0D welds.