Spot Panel

Location: Connectors module

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

Subpanel Organization

The Spot panel is organized into subpanels. The information on each panel is independent, therefore anything specified on one subpanel will not carry over to another. Such information is also non-volatile while you remain inside the Spot panel, so you will not lose work by changing from one subpanel to another. You will, however, lose settings by leaving the Spot panel and then returning.

Spot Subpanel: Create and realize spot connectors.
Create Subpanel: Create, but do not realize spot connectors.
Realize Subpanel: Realize an existing spot connector (no creation or editing is possible).
Edit Subpanel: Edit an existing spot connector.

The Spot, Create and Realize subpanels use the same set of entry controls.

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

Select the location of the connector to be created.

nodes: Select an existing node (also temp nodes).
points: Select an existing point (fixed point or free point).
nodelist: Select a node list and specify spacing or density and end offset.; The selected nodes are used to internally create a smoothed line, which is used exactly as a real line. The connector will not remember the position of the selected nodes, unless you select the preserve nodes check box.
lines: Select a line and specify spacing or density and end offset.

add location node as link

Store the selected location node as an additional link of the link type node.

This checkbox appears when the location is defined by nodes. Many realization types do not work together with nodes as links. When these realization types are chosen the option is not provided.

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.

spacing / density


spacing: Distance between each weld location on the line.
density: Number of weld location on the line.

The number of weld points is approximated to the closest integer, based on the length of the line and spacing given while considering the end offset (or half spacing) value given on the Connector Options panel. The spacing is also calculated based on the length of the line and density for the half-spacing option.

preserve nodes

Preserve the position of the nodes when you create and realize a connector.

Note: Only available if location is set to nodelist/nodepath.

split to points

Split the line into individual points and create spot connectors for each resultant point.

Note: Only available if location is set to nodelist/nodepath or by a line.

connectors

Select the connector(s) to be realized.

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.; You can choose to connect to either the geometry or elements of the selected components.
assems: Select assemblies to be added as link entities.; You can choose to connect to either the geometry or elements of the selected assemblies.
surfs: Select surfaces to be added as link entities.; You can choose to connect to either the geometric surfaces or elements associated to the selected surfaces.
elems: Select elements to be added as link entities.
nodes: Select nodes to be added as link entities.
tags: Select tags to be added as link entities.

link state

Connect to either the geometry or the elements of selected link entities.

Note: Only available when connect what is set to comps, assems, or surfs.

num layers

Define how many thicknesses (layers) have to be connected at the connector position.

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 layers for spots is typically identical to the number of links, though the number of links can be lower in case of flaps.

For spot connectors it is possible to set the number of layers to auto in order to identify and write the exact number of layers during link detection to each individual connector.

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.

re-connect rule

While realizing the connector, HyperMesh 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.

use rbe3 radius

RBE3 elements are typically created with three or four legs dependent on the element type (quadface, triaface) the projection of the appropriate hexa node is landing on. To be more accurate, especially regarding different mesh sizes, an rbe3 radius can be defined, so that more nodes nodes can be joined by each RBE3 element. In any case, at least one element face will be joined by each RBE3 element.

All of the nodes of the appropriate link (outer nodes, if it is a solid link), which are positioned inside a sphere around the projection point, are considered to be joined to the RBE3 element. A feature angle is also considered. The nodes that are on a different side of the feature edge than the projection point will not be joined to the RBE3 element.

When enabled you must define:

rbe3 radius

Define the search radius.

feature center

Define which projection point(s) are used as the radius center.

Figure 3. Individual rbe3	Figure 4. Cluster Center

weight factor

Define which formula should be used for the calculation.

Inverse Distribution

w_{i} = \frac{1}{r_{i}}

Normal Distribution

w_{e i} = e^{- \frac{r_{i}^{2}}{{(0.5 \cdot r)}^{2}}}

normalize rbe3 weights

Enables the normalization of all the weights per a single rbe3.

Normalized Inverse Distribution

w_{i} = \frac{\frac{1}{r_{i}}}{\sum_{i = 1}^{n} \frac{1}{r_{i}}}

Normalized Normal Distribution

w_{e i} = \frac{e^{- \frac{r_{i}^{2}}{{(0.5 \cdot r)}^{2}}}}{\sum_{i = 1}^{n} e^{- \frac{r_{i}^{2}}{{(0.5 \cdot r)}^{2}}}}

feature angle

Define the feature angle to be considered.

Note: Only available for the realization type acm (general).

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.
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 / elems to 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.

Specific Realizations Options

Table 1. Common Options

Option

Action

diameter / use diameter mapping

This field is used for realizations based on hexa elements such as ACM, where the size of the realized element (hexa, and so on) is created based on the diameter value, or for certain realization types where the diameter is used by a post script.

The size of the hexa face is calculated from the diameter value $α = \sqrt{d^{2} \cdot \frac{π}{4}}$ .

When you have weld nuggets from hexa patterns (more than one hexa), the diameter will be measured from two opposite nodes.

Figure 5. Hexa	Figure 6. Weld Nugget

diameter: Specify a single diameter value.
use diameter mapping: Obtain diameter values that you assigned to a range of flange thicknesses in the Diameter Table.; Along with flange thickness ranges, you can also specify the main flange thicknesses to consider when assigning diameter values.

Table 2. ACM Options
Option	Action
thickness	Select a thickness option used for dimensioning and positioning hexas. shell gap Project the hexa spot to touch the shell elements. The position is independent from any thickness. equival. (T1+T2)/2 Create hexa elements with RBE3 elements projecting and connecting to the surrounding shell elements. This realization uses the shell thickness to calculate the hexa offset from the shell elements. In the case where the model is a 3T connection, the acm (equivalenced-(T1+T2)/2) realization will join the hexa elements. Figure 7. detached (T1+T2)/2 Create hexa elements with RBE3 elements projecting and connecting to the surrounding shellstr elements. This realization uses the shell thickness to calculate the hexa offset from the shell elements. In the case where the model is a 3T connection, the acm (detached-(T1+T2)/2) realization will not join the hexa elements. Figure 8. mid thickness Calculate the hexa spot size (thickness) as the air gap between the two connected parts. If there is no gap, or even a penetration, the hexa spot size will always be modeled with 1.0. const thickness Specify the hexa spot size (thickness). maintain gaps Calculate the hexa spot size (thickness) as the gap distance reduced by two times the specified value for maintain gaps. The position is independent from any thickness.
num hexas	Create a hexa cluster with 1, 4, 8, 12, 16 or 32 hexas, which are arranged in a predefined pattern. Figure 9. Note: Available for all ACM realization types.
coats	Define the number of hexa elements required along the thickness. Multiple solid coats are supported.
orthogonal faces	Force the creation of perfectly orthogonally-shaped hexas. Figure 10. . The two leftmost realizations were performed with the orthogonal faces option enabled. Note: Available for any kind of ACM weld, if num hexas is set to 1.

Table 3. Sealing Options
Option	Action
create vector	Create orthogonal vectors for each CBUSH element created during the sealing realization. These vectors are used to define the orientations of the CBUSH elements, which is important to the stiffness defined in the related PBUSH cards.

Table 4. Penta Options

Option

Action

width

Specifies the length of a penta.

Note: Available for: penta (mig + L), penta (mig + T), and penta (B).

depth

Specifies the depth of a penta.

Note: Available for: penta (mig + L), penta (mig + T), and penta (B).

fitted/equilateral/ equilateral-fitted

Select the size and shape of a penta.

fitted: The length of one penta edge is the exact projection distance, and the length of the other penta edge is defined by the width value; the penta has an right-angle.

Figure 11. Example: Fitted
equilateral: Create an equilateral penta; leg lengths are defined by the width value.

Figure 12. Example: Equilateral
equilateral/fitted: Combination of fitted and equilateral; you do not need to define a width when you select this option.

Figure 13. Example: Equilateral/Fitted

Note: Available for: penta (mig + L).

right-angled

Create a right-angled penta that is oriented around the bisector. Clear this checkbox to create an angle adapted penta.

Note: Available for: penta (mig + T).

both sides/positive sides/negative sides

Select which side of the normal to create the penta on.

(mig + L)

The negative side is the side where the links are fairly parallel to each other. The angle that is close to 90° (88° to 90°) the element normal of the first found shell element at the free edge decides which side is the positive and the negative side.

(mig + T)

The positive side is normally the side with the obtuse angle. The angle that is close to 90° (88° to 92°) the element normal of the first found shell element at the free edge decides which side is the positive and negative side.

(mig + B)

The positive side is the side where the element normal of the first link points to.

Note: Available for: penta (mig + L), penta (mig + T), and penta (B).

Table 5. RBE3 (Load Transfer) Options
Option	Action
use shortest projection for center / use connector position for center / use coarse mesh for center	use shortest projection for center The closest node becomes the center of the RBE3 element. During the realization based on the connector position and the tolerance the closest links are determined up to the number of required layers (num layer). All other link candidates are not taken into account for the next step. The closest node is also determined, and it becomes the center of the RBE3 element. Based on this center position all nodes within the given tolerance (distance from center to node) and belonging to the remaining links are attached to the RBE3 element. If the connector has been created with the option add location node as link, the option use shortest projection for center is ignored and the linked node becomes the center of the RBE3 element. use connector position for center The exact position of the connector becomes the center of the RBE3 element. use coarse mesh for center During the realization based on the connector position and the tolerance, the closest links are determined up to the number of required layers (num layer). All other link candidates are not taken into account for the next step. From the remaining links the one with the coarsest mesh is identified and a node on this mesh (close to the perpendicular connector projection) becomes the center of the RBE3 element. Based on this center position all nodes within the given tolerance (distance from center to node) and belonging to the remained links are attached to the RBE3 element. If the connector has been created with the option add location node as link, the option use shortest projection for center is ignored and the linked node becomes the center of the RBE3 element.
max nodes per layer	Specify the maximum number of nodes per layer to attach to the RBE3 element. The minimum number of nodes you can specify is 3.

Table 6. CWELD Options

Option

Action

use shortest projection for center / use connector position for center

use shortest projection for center: From the connector position the closest node (shell or solid) is identified. This node becomes the GS node.; If a node is defined as link, this option will be ignored and use connector position for center is selected instead.
use connector position for center: The connector position is used for the later GS node.; If the connector has a node link defined, this node becomes the GS node. This can be used to create a CWELD attached to a SPC node.; If the connector is very close to an existing node of a link (shell, solid, 1D element), this node will be taken as a GS node.; If the connector is somewhere in space, a tempnode is created at that position and then taken as a GS node.

Note: (Only available for type CWELD (general), when the nodetype GS (point to face) is selected)

CWELD Type

Select a CWELD type definition.

ELEMID
GRIDID
PARTPAT
ELPAT
ALIGN

Note: Only available for type CWELD (general).

Nodetype

Select a nodetype. Available nodetypes depend upon the CWELD type selected.

ELEMID

GA-GB

GS (face to face)

GS (point to face)

GRIDID

GA-GB

GS (face to face)

GS (point to face)

PARTPAT

GA-GB

GS (face to face)

ELPAT

GA-GB

GS (face to face)

ALIGN

GA-GB

GS (face to face)	GS (point to face)

Note: Only available for type CWELD (general).

recenter GS

Reposition the initial GS position between node GA and GB. After re-positioning, projections are done a second time to identify the correct node/element IDs.

Note: Only available for type CWELD (general), when the nodetype GS (point to face) is selected.

centered quad

Perform a mesh modification during the realization to guarantee that the CWELD nodes will be close to the CQUAD centroids.

Specify a desired quad size in the quad size field, or click centered quad to access additional centered quad settings.

centered quad tolerance

size tol: Dictates the maximum allowed deviation from the requested centered quad size.; Size tol. is calculated using the following formula:
$\frac{absolute value (current quadsize - requested quadsize)}{requested quadsize}$; The default value is set to 0.25, which allows, for example, for a requested centered quad size of 4 to result in a centered quad size of 5.; If a specific centered quadsize is not requested, the tolerance will be used. The average mesh size in that area will then be used as the requested quadsize.
position tol: The maximum allowed distance between the cweld node and the element centroid of the centered quad.; Position tol. is calculated using the following formula:
$\frac{absolute distance (center of current quad - cweld node)}{position tolerance * requested quadsize} < 1$; The default value is set to 0.25, which allows, for example, for a centered quad size of 4 a distance between the cweld node and the element centroid of < 1.; If a specific centered quadsize is not requested, the tolerance will be used. The average mesh size in that area will then be used as the requested quadsize.

centered quad mesh imprint

Washer preservation settings enable washer elements close to spot connectors to be modified, depending on the chosen settings.

No washer preservation: Treats washer elements in the same manner as normal elements. Washers are not protected, and could be remeshed along with its surrounding elements.

Figure 21. Mesh with Centered Quad Mesh Imprint Set to No Washer Preservation
Preserve washer, allow remesh: Only remesh the washer elements so that a washer can still be detected.

Figure 22. Mesh with Centered Quad Mesh Imprint Set to Preserve Washer, Allow Remesh
Preserve washer, no remesh: Do not modify the washer during imprint realizations. Note that with this option, nearby spot connectors might fail because of this restriction.

Figure 23. Mesh With Centered Quad Mesh Imprint Set to Preserve Washer, No Remesh
feature angle: If the nodes of the mesh are not associated with surfaces, the feature angle is needed to identify the features, which might need to be protected. By default, this value is set to 30.0°. The minimum value is 10.0°. Features will not be protected when they are close to imprint regions.

Note: Only available for type CWELD (general), CWELD (GA-GB ELEMID) and CWELD (GA-GB GRIDID).

Final Connection to Link Entities Options

Option	Action
mesh dependent / mesh Independent	Determine whether the realizations require a node connection. mesh independent For a realization which does not need any node connection and the connection is primarily defined via a solver-specific card or the nodes which need to be connected are defined by just a cylinder. mesh dependent All other cases.
adjust realization / adjust mesh	adjust realization Adjust the realization itself, such as allowing non-normal realizations for the sake of locating nodes to create the realization. adjust mesh Adjust the mesh should locally (such as creating transition elements or remeshing) to ensure proper realization. Note: Only available when mesh independent is selected.
quad transition / remesh / smooth	Select a mesh adjustment options. quad transition Creates quads to serve as a transition. remesh Remeshes the linked entities to achieve better links. smooth Adjusts the mesh in such a way that the closest node to each layer is moved into the position of the projection point. The advantage of this option is that neither the element IDs nor the node IDs will be changed, and the element topology will remain the same. Note: Only available when mesh dependent and adjust mesh are selected.
imprint / skip imprint	imprint Merge two meshes from two different link entities to create a transition mesh that matches up well with both. skip imprint Close-set connectors' transition quads may overlap and interfere with each other, causing one or more realizations to fail. Note: Only available when mesh independent, adjust mesh, and quad transition are selected.
resolve conflicting imprints	Resolve small conflicts between overlapping transition meshes automatically. Larger conflicts may require a manual imprint. Note: Only available when mesh independent, adjust mesh, quad transition, and imprint are selected.
allow snapping	Note: Only available when mesh independent, adjust mesh, and quad transition are selected.
quad size	Specify a preferred size for the transition quads. Clear this checkbox to use the default element size from the Connector Options panel. Note: Only available when mesh independent, adjust mesh, and quad transition are selected.
find nearest nodes / project and find nodes / ensure projection	Select how the realization will adjust to locate nodes in the linked entities in order to establish links. Note: Only available when adjust realization is selected.

Edit Subpanel

Option	Action
connectors	Select the connectors to edit. Click edit to update the selected connectors with respect to the new chosen settings. The connectors will become unrealized.
spacing = / density =	spacing Distance between each weld location on the line. density Number of weld location on the line.
end offset = / half spacing	end offset = Offset first and last weld locations from the ends of the line by the end offset value. half spacing Offset by a value equal to half thee distance between weld locations.
split to points	Split the line into individual points and create spot connectors for each resultant point. Note: Only available if location is set to nodelist/nodepath or by a line.