What is a Freebody?

Freebodies provide an insight into nodal forces and moments that are a result of surrounding finite element entities. They can be used to display a balanced set of loads or calculate loads across any interface in the structure that you choose. Freebodies are commonly used when finite element meshes are too coarse to get usable stresses. This dictates the use of a “coarse-grid” model for internal loads. You can then take those forces and moments and extract them for detailed stress analysis.

Freebodies in FEMAP

Freebodies in FEMAP exist as creatable objects, like nodes, elements, etc. They persist in the database. This allows us to recreate freebody displays in the future and can help reduce analysis errors and rework. Any number of freebodies can be displayed simultaneously. There are a number of tools that exist to automate free-body-related tasks, such as creating loads and substructure modeling.

FEMAP Freebody Types

There are three types of freebodies in Femap.

Freebody

User selects the elements, Femap automatically selects the related notes. This is intended to display a balanced set of loads on a discrete piece of structure. You should see equilibrium in the structure between the applied loads and the reaction loads.

Interface Load

User selects both nodes and elements and Femap calculates a summation of loads and forces across the interface and displays it as a single vector.

      

      

Section Cut

Similar to the interface loads. A summed load across an interface is displayed and calculated. However, node and element selection are automated by FEMAP. The user selects a “cutting plane”, defined by a plane, vector, or a curve. The cutting plane can be dynamically located within the model.

      

      

Freebody Contributions

Freebody contributions in FEMAP are split into six categories:

1. Applied – represents applied loads
   
2. Reaction – results of SPC forces
   
3. MultiPoint Reaction – results of MPC forces
   
4. Peripheral Elements – effects of elements surrounding selected elements.
   
5. Freebody Elements – effects of elements selected by the user or by FEMAP
   
6. Nodal summation – nodal summation values from the solver, not FEMAP calculated values.
   

The default and most commonly used contributions are Applied, Reaction, MultiPoint Reaction, and Peripheral elements. This provides forces and moments acting on the selected structure.

      

Freebody Result Vectors – As mentioned earlier, the NASTRAN GPFORCE request is recommended to fully take advantage of the freebody tool, however the result quantities may be obtained from several different quantities.

      

Freebody Toolkit

The Freebody Toolbox is located in the PostProcessing toolbox and can only be accessed when results are present in the model.

Global Settings: These controls affect all freebodies in the model. Control global display of freebodies, select output set (tied to contour and deform), and enable data summation on nodes.

Freebody Settings: These controls are related to individual freebodies, such as selecting nodes and elements.

View Settings: These are global settings that affect freebody visualization (symbol sizes, vector scaling, etc) – same as found in View Options (F6).

            

Creating a New Freebody

Selecting “Add Freebody” will take you into the Freebody Manager. From there click “New Freebody”. The New Freebody dialog allows for setup of basic settings, such as freebody type, vector display, and contribution selection.

      

      

      

Freebody Vector Types

1. Displays the summation at each node, based on the selected freebody contributions
   
2. Available for all freebody types
   

Total Summation Vector

1. Available only for Interface Load and Section Cut freebodies.
2. Displays the total summation across all nodes at a pre-defined position.
   
1. The selected position does not affect summed force calculations, but will affect summed moment calculations due to the difference in moment arms.
   

Freebody Vector Visualization

            

Visibility Quick Toggle Buttons

Detail Options

1. Additional detailed options for visualization can be found by expanding the Total Summation Vector and Nodal Vector(s) nodes
   
2. Select components displayed (Fx, Fy, Fz), (Mx, My, Mz)
   
3. Select components included in calculation (interface load and section cut only)
   

Freebody Coordinate Systems

The selected freebody coordinate system controls the coordinate system for both nodal vectors and the total summation vector (if applicable) for the selected freebody.

1. Nodal vectors may optionally be displayed in the nodal output coordinate system.
   
2. If no nodal output system was specified on the node, the default coordinate system used is the global rectangular system.
   

                  

Interface Load Mode

Interface load freebodies display nodal vectors for selected nodes as well as a total summation vector at a selected location. Unlike freebody mode freebodies, interface load freebodies are not likely to be in equilibrium. In addition to element selection, nodes must be selected manually – FEMAP does not infer them based on the selected elements. When selected entities from a group, both the nodes and elements of interest must exist in the group.

Selecting Nodes - Interface Load Mode

      

      

Selecting Components in Summation – Interface Load Mode

Individual force and moment contributions that are included in the total summation vector calculation can be toggled on and off. By default, all force and all moment vectors are included in the calculation. Changes made here will affect the total summation calculation. Turning on and off certain contributions is dependent on how the model was idealized; it is up to the analyst to understand how the FE model correlates to real-world structure.

      

      

Section Cut Mode

Section cut is an extension to Interface Load mode. The user defines a cutting plane in the model and the contributing freebody nodes and elements are determined automatically. Total summation location can be placed at:

1. Plane/path intersection
   
2. Nodal centroid
   
3. Static location
   

Nodal and total summation vectors can optionally be aligned tangent to the path without having to create additional coordinate systems.

      

      

Entity Selection Mode

      

      

Plane / Normal

Cutting plane is defined via base point and normal vector. Path is defined as the normal vector; cutting plane will always be normal to the path.

Plane / Vector

Similar to Plane / Normal, however an additional vector is defined for the path. The cutting plane will always remain co-planar to the original plane and does not have to be normal to the path.

1. The Slider tool can be used to move the cutting plane along the length of the path interactively within the available entities
   
2. Section cut entities may be limited to a specific group or selected from the entire model, and can be limited to a search distance from the base location of the cutting plane
   
3. The cutting plane can optionally be given a thickness tolerance that will allow for accurate selection of entities that are slightly out-of-plane
   
1. Clipped entities can either be included or excluded from the summation calculations
   
   

Freebody Tools

        

1. List freebody to message window
   
2. List freebody to data table
   
3. List freebody summation to message window (interface load / section cut)
   
4. List freebody summation to data table (interface load / section cut)
   
5. Freebody validation tool; warns user when freebody results are potentially missing from the model
   

Recovering Grid Point Forces in NASTRAN

Turning on the NASTRAN GPFORCE case control request is required to take full advantage of the Femap Freebody Tool. GPFORCE requests can return a large amount of data, so this option is not enabled by default. You can turn it on by going to:

Analysis Manager > Master Requests and Conditions > Nastran Output Requests > Force Balance

      

Note, that it is still recommended to read GPFORCE data into FEMAP from the OP2 file, not the F06 file.

          

1. Elemental (discrete; per connecting flexible element)
   
2. Applied (total forces / moments applied on node; single quantity per node)
   
3. F-of-SPC (SPC forces on node; single quantity per node)
   
4. F-of-MPC (MPC forces on node, including both constraint equations and RBE contributions; single quantity per node)
   
5. *TOTALS* (total summation of all contributions; single quantity per node)
   
1. For the majority of cases, this value should be near zero, indicating equilibrium at the node
   

How GPFO Relates to Structure

Freebody output can be very dependent on the nodes and elements included in the summation. How the model was idealized and what specific quantity is desired determines which nodes and elements are to be used.