This guide provides an in-depth overview of freebodies in FEMAP.
If you would like to see the breakdown of each particular step and get a better understanding of freebodies, view the accompanying webinar hosted by Russ Hilley.
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.
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 is 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.
In the Freebody Properties, click the Entity dropdown menu and choose “Entity Select”.
WarningIf you are going to use a group, you have to make sure that all of the elements and element’s related nodes are in that group for the freebody to display correctly.
Select the Freebody elements and draw a box around the entire model and press “OK”.
You can turn the nodal display on or off. In fact, any of the settings applied in the New Freebody dialog can be changed at any time within the toolbox.
Accessing Different Freebodies
Multiple Freebodies can be displayed at anytime. However, only a single freebody can be active at anytime within the toolbox.
Use the drop-down menu to change the active freebody and modify settings.
Display of individual freebodies can be controlled with the “Is Visible” checkbox as well as with the Visibility Quick View Dialog.
Freebody Vector Types
Depending on the freebody type, there are vector quantities for nodal vectors and a single total summation vector.
- Displays the summation at each node, based on the selected freebody contributions
- Available for all freebody types
Total Summation Vector:
- Available only for Interface Load and Section Cut freebodies.
- Displays the total summation across all nodes at a pre-defined position.
- The selected position does not affect summed force calculations, but will affect summed moment calculations due to the difference in moment arms.
Both force and moment vectors are available and can be individually toggled.
Vectors can be displayed as either components or resultant vectors.
Individual components can be toggled on and off.
Freebody Vector Visualization
Visibility Quick Toggle Buttons
- All On / All Off
- Forces On/Off
- Moments On/Off
- Toggle between resultant/component
- Select summation location (interface load and section cut only)
- Additional detailed options for visualization can be found by expanding the Total Summation Vector and Nodal Vector(s) nodes
- Select components displayed (Fx, Fy, Fz), (Mx, My, Mz)
- 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.
- Nodal vectors may optionally be displayed in the nodal output coordinate system.
- If no nodal output system was specified on the node, the default coordinate system used is the global rectangular system.
When using “Freebody Mode”, the user selects elements and FEMAP automatically selects related nodes.
This mode is designed to display a balanced set of loads on a selected set of elements.
Entities may be selected manually (default) or inferred for a selected group.
The default contribution selections will display forces/moments acting on the selected elements.
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:
- Plane/path intersection
- Nodal centroid
- Static location
Nodal and total summation vectors can optionally be aligned tangent to the path without having to create additional coordinate systems.
Entity Selection Modes
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.
Cutting plane is normal to the defined vector. Path is the defined vector; cutting plane will always be normal to the path.
Cutting plane is normal to the tangent vector at a point along the plane. Cutting plane will always be normal to the tangent vector.
Additional Section Cut Options
- The Slider tool can be used to move the cutting plane along the length of the path interactively within the available entities
- 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
- The cutting plane can optionally be given a thickness tolerance that will allow for accurate selection of entities that are slightly out-of-plane
- Clipped entities can either be included or excluded from the summation calculations
- List freebody to message window
- List freebody to data table
- List freebody summation to message window (interface load / section cut)
- List freebody summation to data table (interface load / section cut)
- 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
FEMAP can work with a reduced set of data including applied load (OLOAD), constraint force (SPCFORCE), and constraint equation (MPCFORCE). However this is generally not recommended unless only a generic freebody display of the entire structure is all that’s required.
Additionally, care should be taken when not requesting GPFORCE data for the entire model
NASTRAN F06 Output
When the results destination is set to “Print Only” or “Print and PostProcess” GPFORCE data can be viewed in the F06 file
To find the output, search for “G R I D P O I N T F O R C E B A L A N C E” with the spaces.
GPFORCE results are listed per grid and include Fxyz (T1, T2, T3) and Mxyz (R1, R2, R3)
Results are separated into 4 different categories, plus a summation:
- Elemental (discrete; per connecting flexible element)
- Applied (total forces / moments applied on node; single quantity per node)
- F-of-SPC (SPC forces on node; single quantity per node)
- F-of-MPC (MPC forces on node, including both constraint equations and RBE contributions; single quantity per node)
- *TOTALS* (total summation of all contributions; single quantity per node)
- 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.