Area Panel (Connectors)

Use the connector Area panel to create connectors that represent connections of larger regions, such as adhesives. These connectors can later be realized as standard or custom weld representations.

Location: Connectors module

The test points of an area connector are characterized by nodes of an internal mesh dedicated to the connector. During connector creation the internal mesh can be created by adopting the mesh used for location, or the defined region is automeshed with a certain mesh type.

When the Area panel is active, only area-type connectors display in the modeling window; graphics for other connector types are suppressed until you exit the panel.

Subpanel Organization

The Area panel is arranged into several subpanels. You can move freely between subpanels. Your work on one subpanel will not be lost if you switch to a different subpanel.

Area Subpanel: Create and realize area connectors.
Create Subpanel: Create, but do not realize area connectors.
Realize Subpanel: Realize existing area connectors (no creation or editing possible).
Edit Subpanel: Edit existing area connectors.

The Area, Create and Realize subpanels use the same set of options.

The first column contains everything related to connector creation and link detection.
The second column contains everything related to realization type, post script and property assignment.
The third column contains everything related to the final connection to the link entities.

Connector Creation and Link Detection Options

Option	Action
location	Specify the location of the connector to be created. elems Define the region for the area connector by the selected shell elements. Create the internal connector mesh by adopting the mesh used for location. It is automatically detected if all the selected elements are attached to each other. If this is not the case, create one area connector per each element patch. surfs Create one area connector for each selected surface, even if the surfaces are attached to each other and share the same green edge. The internal connector mesh is created dependent on the defined mesh type and mesh size. lines/linelist Select lines or a linelist and specify the mesh type, the width and/or the offset. If you select several lines, HyperLife Weld Certification determines whether lines share the same start points and end points or not. This means HyperLife Weld Certification is able to determine whether several lines form a continuous line. From these lines only one single area connector is created. Note: There is a limitation for lines with sharp vertices; in such a case the area connector might not provide satisfactory results. The quality depends on the vertex angle on the line, the width and if an offset needs to be done. Figure 1. The area connector will automatically be oriented parallel to the closest link. It is recommended to use free lines or free surface edges. If a free line is selected, then the area connector is created with the defined width centered about it. The offset option is considered only in cases where the selected free line is on a free mesh edge, in which case the behavior is exactly the same as for the free surface edge. If the offset option is considered with the default of 0.0, the area connector is positioned with its one outline on the free mesh edge, such that the complete connector lays exactly along the free edge but inside the link. nodes/nodelist/nodepath Select a nodelist and specify the mesh type, the width, and/or the offset. From this nodelist HyperLife Weld Certification internally creates a line, so the behavior of a nodelist is very comparable to a linelist. With this method only one area connector is created. Note: There is a limitation for node lists with sharp vertices; in such a case the area connector might not provide satisfactory results. The quality depends on the vertex angle on the nodelist, the width, and if an offset needs to be done. The area connector will automatically be oriented parallel to the closest link. It is recommended to use mesh nodes, although temp nodes can be used. When nodes are selected with the by path option, a check is run to determine if the selected nodes are located along a free mesh edge. If fewer than 3 nodes are on a free mesh edge the area connector is created centered about the selected nodes. If the nodes are on a free edge then one of the edges of the area connector will coincide with the node path (offset = 0.0).
width	Width of the connector area centered along the line. Note: Only available when the location is set to lines or nodelist.
offset	Connector is offset from the free mesh edge along the link by this distance. Note: Only available when the location is set to lines or nodelist. Figure 2.
connectors	Select the connector(s) to be realized.
line combine	Create one seam connector for each sequence of lines and each single line. With this option enabled, a sequence of lines will be internally treated as on line. This option is preferred for continuous seams together with realization types where the body element is positioned between the weld points of all quad and hexa seam realizations. With this option, neither the vertices nor the start point and end point of the initial lines are considered, and there likely will not be any weld points at the exact positions. Note: Default setting when location is set to linelist.
mesh type	Select the mesh type to mesh the connector with. Note: There is no interactive mesh manipulation available. A few more options can be used during editing an area connector.
mesh size	Specify the mesh size the connector should be meshed with.
connect what	Select the entities to become link candidates. Link candidates are certain entities of a chosen link type, which are supposed to be connected during the realization. Entities outside the tolerance are not taken into account. comps Select components to be added as link entities. Choose to connect to either the geometry or elements of the selected components. assems Select assemblies to be added as link entities. Choose to connect to either the geometry or elements of the selected assemblies. surfs Select surfaces to be added as link entities. Choose to connect to either the geometric surfaces or elements associated to the selected surfaces. Note: Connectors can be created with different types of entities; for example, a connector can be defined by selecting a component on one side and an assembly on the other side. This can be done by creating a connector to specify one of the entity types and selecting that entity. Add the second entity by updating the connector via the add links functionality in the Connector browser or the Add Links panel.
num layers	Define how many thicknesses (layers) have to be connected at the connector position. This number is predefined as 2. There is not a field in the this panel where you can set the number of layers; however, you can find the number of layers in the Connector browser. When link detection is performed the valid connector links are established with respect to the given tolerance and the selected link candidates. By default the links are reduced to the minimum needed. The number of links is typically higher than the number of layers, because a valid pair of projections need to be found per test point.
tolerance	Define a distance from the connector location (per each test point). Only entities within this tolerance can be taken into account for the link detection and the final realization. Thus, the tolerance is used twice: first for the link determination and again for the realization. In the second step the tolerance is used to verify whether adequate link candidates are available to be connected. During pure connector creation on the Create subpanel, the tolerance is used for the link determination, but not necessarily stored on the connector unless the checkbox in front of the tolerance field is marked. In this way different tolerances can be used. The tolerance used during the realization process is always written to the connector.
connect when	Select when to perform link detection. now Add link entity information now, directly together with the connector creation. at fe-realize Create a connector without any specific information regarding its links. Links are determined when performing the final realization with respect to the connector position. Using this option defines the re-connect rule at-fe-realize for all created links.
reconnect rule	While realizing the connector, HyperLife Weld Certification looks for link entities based on the re-connect rule. Tip: This option is useful in situations where the parts to be connected have been changed/replaced. none No re-connect rule is defined. If the link entity is not currently in the model, the connector with this re-connect rule will fail to realize. If no re-connect rule is defined for a link, this link disappears from the connector when the linked entity is deleted. use id Use the selected link entity’s IDs to re-connect. If the link entity is not currently in the model, the connector with this re-connect rule will search for entities with the same ID. use name Use the selected link entity’s names to re-connect. If the link entity is not currently in the model, connectors using this re-connect rule search for entities with the same name.

Post Script and Property Assignment Options

Option	Action
type	Select the realization type which should be used. The realization type is a description of the FE representation. Note: The available realization types are dependant on the configuration file loaded under fe file on the general connector Options panel.
fe file	A default feconfig.cfg file that is available in the installation is automatically loaded. If you choose to add a unique realization type, copy this file into the user home directory and add custom types. Click ... to load a user-modified feconfig.cfg file, if necessary.
post script treatment	Choose whether or not a post script has to be used for the specific realization type. These scripts are used to automatically create materials, properties, and/or contacts necessary for realizing the connectors. default post script Default for any realization type having a post script defined in its FE configuration. user post script Select your own .tcl file which should be used. Such a file can perform a special treatment on the FE representation. no/skip post script Default for all realization types without any post script defined. No post script is used.
elems to current comp / connector comp	Select which component the FE representations are stored in once they have been realized. current comp Store newly-realized connectors in the current component. connector comp Store newly created FE representations in the same component that the connector was originally created in. Note: Only available in the realize subpanel when post script treatment is set to no/skip post script.
property treatment	Select a property treatment. property Click property= and select a property to assign to all newly created elements. no property No property gets assigned. Note: Only available when post script treatment is set to no/skip post script.
direct property assignment	Directly assign the property, otherwise assign the property to the destination components. Note: Only available when property treatment is set to property =, and the solver interface is Nastran, OptiStruct, Radioss or Abaqus.

Hexa Realization Options

Option	Action
coats	Defines the number of hexa elements required along the thickness. Note: Multiple solid coats are supported when adhesive-hemming is selected.
thickness	Select a method for defining the thickness of a hexa weld. shell gap Project the hexa to touch the shell elements. The position is independent from any thickness. (T1+T2)/2 Hexa size (thickness) depends on the shell thickness of the connected parts. mid thickness Calculate the hexa size (thickness) as the air gap between the two connected parts. If there is no gap, or even a penetration, the hexa size is always modeled with 1.0. const. thickness Specify the hexa size (thickness). maintain gaps Calculate the hexa size (thickness) as the gap distance reduced by two times the specified value for maintain gaps. The position is independent from any thickness. Note: The exact hexa position is also influenced by the option consider shell thickness and offset for hexa positioning. Figure 3.
direction node	Define the direction node.

Penta Realization Options

The Penta (Mig) realization type is the primary form of penta realization for areas.

Edit Subpanel Options

Table 1. Trim Options
Option	Action
multiple nodes: connector	Select the area connector that you would like to trim. Once you alter the selected connectors' options, click edit to update the selected connectors with respect to the new settings. The connectors will become unrealized.
multiple nodes: node list	Select a nodelist on the area connector or a nodelist on existing nodes. nodelist on an area connector Trims the first and the last node to the connector area edge within the given snapping distance. nodelist on existing nodes The line defined by the nodelist is projected normal to the area connector surface, and the connector will be trimmed along that projected line. The line must be long enough to guarantee a full trim.
snap to connector point	Trim the connector at the closest connector point per each selected node within the specified tolerance. By default this option is selected, and the tolerance is set to 1.0. If you selected a nodelist on existing nodes, this option will have no influence on the trimming behavior.
delete smaller connector piece	Delete the smallest connector piece when the connector is trimmed.
trim	Trim the connector into a new, unrealized connector. The new connector contain all of the information that was retained from the original connector.

Table 2. Remesh Options
Option	Action
location	Select connectors to edit. Once you alter the selected connectors' options, click edit to update the selected connectors with respect to the new settings. The connectors will become unrealized.
mapped type	Select the shape of elements to use on surfaces that can be mapped to simple geometric shapes like a triangle, rectangle, or rhombus.
free type	Select the shape of elements to use on more complex surfaces that cannot easily map to simple shapes.
size control	Keep elements roughly the same size.
skew control	Prevent the mesh from producing highly-skewed elements.
link opposite edges	Force opposite edges of the area connector to use consistent edge densities, provided that the starting densities are close enough. This creates tapered lines of elements, instead of using trias to transition between inconsistent densities. Figure 4. Link Opposite Edges Example. Meshing with (left) and without (right) linked edges.
size and bias/edge deviation	Select meshing criteria. element size Specify the size of each element. min elem size Specify a minimum element size. Elements of varying size will never exceed this value. max elem size Specify a maximum element size. Elements of varying size will never exceed this value. max deviation Define the maximum allowable distance between an edge of the surface being meshed and an element edge. max angle Define the maximum allowable angle between two element edges.

Command Buttons

Button	Action
mesh	Apply the mesh using the new settings when remeshing connectors.
options	Open the Connector Options panel, where various settings can be defined.
create	Create the connector(s) with provided input (if sufficient).
reject	Undo the last action.
return	Exit the panel.