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.
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.
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.
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 in FEMAP are split into six categories:
- Applied – represents applied loads
- Reaction – results of SPC forces
- MultiPoint Reaction – results of MPC forces
- Peripheral Elements – effects of elements surrounding selected elements.
- Freebody Elements – effects of elements selected by the user or by FEMAP
- 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.
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.