FBD Create and Edit

Use the Free-Body Create tool to create and edit free-body section entities.

A free-body section entity can be defined by selecting a group of elements which will give a contribution of forces and moments at selected interface nodes. A free-body section can also be defined by a cutting plane in space, finite or infinite, with optional limitation of contributing parts.

In each section, you can define the summation point location and the system used by the section to resolve forces and moments components. The definition of multiple free body sections can be saved in a template file (*.csv file) and can be imported in another session later.

Create a Mesh Based Section

Steps 4 - 7 are optional, but recommended.

From the Post ribbon, select the Create Free-Body tool.

Figure 1.
From the guide bar, verify Mesh is selected.
From the guide bar, select Elements and select elements to account for in the modeling window.
The location is defined.
A new entity is created and edit mode is activated for the entity.

The icon on the guide bar is populated.
Tip:
- If the tool is called from idle mode with the element selector populated, the selection is propagated as location.
- In edit mode, click from the guide bar to fit to entity location.
- Resetting elements turns the entity into an invalid state since location is a mandatory selection. The entity will remain invalid until new elements are selected. Leaving the tool will not commit the change to the database and the last element selection is restored as location.
Optional: From the guide bar, select Nodes and select interface nodes in the modeling window.
The force and moment will be extracted from these interface nodes when using the Plot tool. Only the elements selected in location can contribute to interface nodes.
If no nodes are selected, then all nodes of the selected location will be considered.

Nodes not belonging to location elements are filtered out.
Optional: From the guide bar, select the Boundary Nodes check box.
Free nodes and nodes shared with other elements not part of location are selected.
The interface node selector is disabled.

As location updates interface nodes, elements selection is changed.
Optional: From the microdialog, select the system in which force and moment components are extracted.
- Click to use node output system.
- Unselect to set resolved-in to the basic system.
- Click to select a local system to resolve in.
Optional: From the microdialog, select the summation location.
- Click to use the section geometric center.
- Click to pick a node to reference the node ID as summation point or change the selector type to Location and pick a location in space to save X, Y, Z coordinates.
- Click to pick another location to update or change the selector type to Node and select a node ID to save as summation point.
  Restriction: This option is only available when Edit mode of a free-body section using a summation (X, Y, Z) location.
From the guide bar, click to apply the updates and remain in the tool or click to apply the updates and exit the tool.

Create a Infinite or Finite Cut Section

Using a cutting plane defines a dynamic cross-section. In this case, all of the elements intersected by this plane will be considered as defining such cross-section, while the nodes belonging to these elements at one or another side of the plane will be considered for the calculation.

Steps 6 - 9 are optional, but recommended.

From the Post ribbon, select the Free-Body Create tool.

Figure 2.
From the guide bar, select Finite Cut or Infinite Cut.
Select a plane.
1. In the modeling window, select a plane.
2. Drag the plane to the desired base point.
3. Define the plane normal by using the frame rotate manipulators on each edge to change the orientation and size.
  Tip: Plane manipulator tips:
  - You can change the plane base point coordinates by clicking in the microdialog.
  - You can click to display the vector tool manipulator on top of the plane frame.
  - You can pick a vector handle:
    
    Select to control the point global coordinates in space.
    
    Select to provide plane normal components.
  - You can pick corners to change plane manipulator size independently or keeping the ratio.
  For Infinite Cut, the plane size is only used for display purposes. For Finite Cut, the plane size is used to evaluate intersection and Corner location as part of the plane definition.
  With Infinite Cut, the plane preview always shows the intersection with the entire model even if some parts are not displayed.
Define plane orientation.
The plane local system defined with dataname Orientation is equivalent to the Resolved-in field available in mesh based sections. The plane normal acts as local z-axis.
1. Click to open the vector tool.
2. Click to open the move tool.
3. Rotate the x-axis of the manipulator to fully define the local system onto which results will be resolved.
For Finite plane, define the plane size.
1. Select a plane frame to activate its handles.
2. Select a corner to change its position.
3. In the microdialog, define the plane length and width.
Optional: Select intersected entities.
By default, the section will try to intersect all entities in the model (even if not displayed) with the plane defined (Finite or Infinite). It is possible to limit the intersection to only a few components or parts.
1. From the guide bar, select Component or Part as the entity type.
2. Pick entities to consider in section cut.
Optional: In the microdialog, define the plane thickness.
Plane thickness acts as centered tolerance to capture on-plane nodes.
The plane thickness defaults to twice as great as node tolerance.

The last value used is retained as the default for the next session.

The plane thickness increases the number of nodes considered in-plane. Increasing thickness to a very large value can’t exceed the region defined by the nodes of intersected elements.
Optional: From the Entity Editor, select Include for Rigids.
By default, rigids elements connected to nodes found as interface nodes are excluded. It is possible to force HyperMesh to include rigid elements in contributing elements connected to nodes. When converting a section to a mesh based section (see Create a Mesh Based Section), rigids will be included or excluded based on this selector.
Optional: Select summation location.
- Click to use the section geometric center on plane.
- Click to pick a node to reference the node ID as summation point or change the selector type to Location and pick a location in space to save X, Y, Z coordinates.
- Click to pick another location to update or change the selector type to Node and select a node ID to save as summation point.
  Restriction: This option is only available when Edit mode of a free-body section using a summation (X, Y, Z) location.
From the guide bar, select the Show Realization check box to visualize intersected elements and interface nodes used for result extraction.

Note: Clearing the Show Realization check box restores the preview only (red line) and avoid intersection evaluation (lighter on large model).
From the guide bar, click to apply the updates and remain in the tool or click to apply the updates and exit the tool.

Edit Existing Free-Body Sections

From the Free Body Sections browser, select and right-click a free-body section and select Edit from the context menu.
Make and apply edits to the free-body section.

Convert Sections to Mesh Based

Realize an Infinite Cut or Finite Cut section to convert it to an explicitily defined section by elements and nodes by changing the support to Mesh.

In Edit mode of the Create Free-Body tool, change type to Mesh on the guide bar to convert the section.

Note: If no further editing is done on elements, changing the type back to Infinite Cut restores the plane definition.

Tip: From the Free Body Sections browser, you can bulk edit multiple sections at a time and change the support to Mesh.

Export Free-Body Sections

Export free-body sections to an ASCII file.

Export free-body sections by completing one of the following:

Option	Actions
Export from Free Body Sections Browser	From the Post ribbon, select the List Free-Body Sections tool. Figure 3. From the Free Body Sections Browser, select and right-click one or multiple free-body sections and select FBD Import/Export > Export to File from the context menu. Enter a file name, select a save location, and click Save.
Export from FBD Manager	From the Post ribbon, select the FBD Manager tool from the Plot group. Figure 4. The FBD Manager dialog opens. From the FreeBodySections area, select and right-click one or multiple free-body sections and select Export to File from the context menu. Enter a file name, select a save location, and click Save.

The free-body section(s) are written in a *.csv file with the following comma separated schema.

SectionName

The free-body section name.

SectionColor

The free-body section color (Integer 0-64).

SectionType

Defines the type of free-body section.

Mesh, FiniteCut, or InfiniteCut

Element List/BasePoint

Defines a list of elements ID for the Mesh type or the coordinates of a base point for other types.

NodeList/Normal

Defines a list of nodes for the Mesh type or the components of a plane normal vector for plane based sections.

SumPointType

Defines whether the resultant point for moment summation is defined by position, node, or centroid.

SumPointValue

Defines the actual location where moments will be summed up:

If the summation type is at the centroid it must be left empty.
If the summation point is at a node it must store a node ID.
If the summation point is a position it must store coordinates.

ResolvedInSystem/Orientation

Defines in which coordinate system the forces and moments should be calculated.

If SectionType is Mesh, valid values are:

Analysis System (node output system)
Global System (laboratory system ID=0)
User System: SystemId column must refer to a system ID

If SectionType is either InfiniteCut or FiniteCut, then this column must contain a triple.

Coordinates of a vector that defines the local x-axis.
Orientation vector does not need to be orthogonal to Normal. It defines the XZ plane along with the Normal information.

SystemID

Stores a Coordinate System ID.

Only used if the ResolvedInSystem System is set to User System. Otherwise, this field can be left blank.

PlaneBreadth

Height of the finite section (along y-axis) centered on the base point.

For infinite plane, it will be used for displayed size of the manipulator, but have no impact on intersection.

This field can be left blank for Mesh SectionType.

PlaneLength

Width of the finite section (along x-axis) centered on the based point.

For infinite plane, it will be used for displayed size of the manipulator, but have no impact on intersection.

This field can be left blank for Mesh SectionType.

IntersectType

Entity type of the list defined in IntersectionList.

Valid values are COMP and PART.

This field can be left blank.

IntersectionList

List of entity IDs of type defined in IntersectType.

This is used by plane based section to limit the entities considered in plane intersection.

When it is empty, all elements in the model are considered for intersection.

The field can be left blank if not used.

Thickness

Float that represents the plane thickness.

Half of the thickness is considered on both sides of plane as tolerance to capture the node on plane. If a node normal distance to the plane is smaller than thickness/2.0, then it is considered on the plane.

This field can be left blank for Mesh SectionType.

Create Free-Body Sections From File

Import a *.csv file to import free-body sections.

Following the export of free-body sections, you can import a *.csv file and create several free body sections.

Import a *.csv by completing one of the following:

Option	Actions
Import from Free Body Section browser	From the Post ribbon, select the List Free-Body Sections tool. Figure 5. From the Free Body Section browser, right-click in the Free Body Section browser, and select FBD Import/Export > Import from File from the context menu. Browse, select, and open the desired *.csv file.
Import from FBD Manager	From the Post ribbon, select the FBD Manager tool from the Plot group. Figure 6. From the FBD Manager dialog, right-click in the FreeBody Sections area and select Import from File from the context menu. Browse, select, and open the desired *.csv file.