An Advanced Overview of Freebodies in Femap

An Advanced Overview of Freebodies in Femap


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.

      Wing Freebodies in Femap

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.

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.

      Femap freebody interface load

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.

      Femap freebody section cut

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.

      femap new freebody dialog window

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.

      Femap freebody vector results

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).

            Femap postprocessing toolbox

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.

      10 creating a new freebody

In the Freebody Properties, click the Entity dropdown menu and choose “Entity Select”.
Warning: If 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.

      femap freebody dropdown

Display of individual freebodies can be controlled with the “Is Visible” checkbox as well as with the Visibility Quick View Dialog.

      Femap 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.

Nodal Vectors

  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.

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

      Femap freebody nodal vector

            femap freebody total summation vector

Visibility Quick Toggle Buttons

  1. All On / All Off
  2. Forces On/Off
  3. Moments On/Off
  4. Toggle between resultant/component
  5. Select summation location (interface load and section cut only)

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.

Freebody Mode

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.
      femap freebody mode

      femap freebody mode 2

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

      femap interface load mode - interface selecting nodes

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.

      Femap Summed Components Interface

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.

      femap postprocessing section cut

Entity Selection Mode

      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.


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.

      section cut using plane
      section cut using curve

Additional Section Cut Options

  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
      The Slider Tool

Freebody Tools

      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

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

      NASTAN grid point force balance    

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:
  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.

      femap freebody gpfo
    • Related Articles

    • Understanding Freebodies in Femap

      What is in this webinar? In this Webinar, Russ Hilley will discuss the use of free body diagrams. Referencing his previous presentation at the Femap Symposium Series (FEMAP Freebody Deep-Dive) Russ will demonstrate how to create free body diagrams ...
    • Femap Advanced API Programming Development

      What is in this webinar? This Webinar will dive more deeply into to abilities and usefulness of API’s in FEMAP. Experience programming in Microsoft Excel, MATLAB, or other engineering programming languages is easily extensible to programming with ...
    • Meshing Toolbox in FEMAP

      Quickly and interactively edit geometry and create quality mesh using the Femap Meshing Toolbox The Meshing Toolbox is a centralized collection of FEMAP's geometry clean-up and meshing functionalities in a single pane. Below you will find an overview ...
    • Post Buckling Behavior Analysis in Femap using NX Nastran Advanced Nonlinear

      What is Advanced Nonlinear Advanced Nonlinear is an add-on solver to the basic FEMAP suite of tools. It does not come standard but is an added package that you can buy. It runs the ADINA Solver through NASTRAN. You can find it in the FEMAP Analysis ...
    • Integrating the Femap API with Python

      What is in this webinar? This demonstration will show how Python can be utilized to interface with Femap’s API, allowing access to Python’s large range of packages to extend the power of Femap. In this webinar, Blake Jeans covers programming in the ...