1. Working with Femap Free bodies and Global / Local Modeling

2. Siemens PLM UK Symposium Femap Track Agenda
11:00: Femap – introduction and what’s new 11:50: Working with Femap – free bodies and global / local modeling 13:30: Femap industry customer case studies: Aerospace & marine Customer presentation Longitude Consulting Engineers (London Offshore Consulting) Your presenters today: Nick Rakkar UK Channel Sales Manager, Siemens PLM Software Al Robertson Product Marketing Manager, Siemens PLM Software Joe Brackin Senior Software Engineer, Siemens PLM Software Peter Kingsland Naval Architect, Longitude Consulting Engineers

3. Siemens PLM UK Symposium Femap Track Agenda
15:40: Event wrap up
We will be available for questions and discussion after the event
Femap futures and roadmap
Femap technical queries
How can Femap help in your business
Who can you talk to regarding software solution testing
Nick Rakkar – UK Channel Sales Manager

4. FEMAP Freebody Deep Dive
Topics
What is a Freebody?
Recovering Grid Point Forces in NASTRAN
Understanding Grid Point Force Output
Freebodies in FEMAP
Using the FEMAP Freebody Toolbox
FEMAP Freebody Options
Global / Local Modelling with Freebodies
Additional Topics

5. What is a Freebody?
Freebody Displays provide an insight into the internal forces and moments of the FEM
In FEMAP, Freebody display can
be used to display a balanced set of loads on a portion of the structure
or calculate the load across an interface
Freebody displays are commonly
used when modeling practices dictate that the resulting FE mesh is a “coarse-grid” mesh but is suitable as an “internal loads” model
Commonly modeled structures are often too complicated to model in sufficient detail to obtain directly useable stresses
Allows for forces / moments to be extracted for detail stress analysis
Freebody displays are heavily used (but not limited to) in the aerospace industry

6. Freebody Display Requires 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
Enabling GPFORCE Output in NASTRAN Case Control
Analysis Manager
Master Requests and Conditions
Output Requests
Force Balance
GPFORCE requests can return a large amount of data, so this option is not enabled by default

7. Freebody Display Requires Recovering Grid Point Forces in NASTRAN
FEMAP can work with a reduced set of data including applied load (OLOAD), constraint force (SPCFORCE), and constraint equation (MPCFORCE)
This is generally not recommended unless only a generic freebody display of the entire structure is all that’s required.
Care should be taken when not requesting GPFORCE data for the entire model.

8. Understanding Grid Point Force Output
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
Search for “G R I D P O I N T F O R C E B A L A N C E”
G R I D P O I N T F O R C E B A L A N C E
POINT-ID ELEMENT-ID SOURCE T T T R R R F-OF-SPC E E E QUAD E E E E E E QUAD E E E E E E *TOTALS* E E E E E QUAD E E E E E E QUAD E E E E E E QUAD E E E E E E QUAD E E E E E E *TOTALS* E E E E E E QUAD E E E E E E QUAD E E E E E E QUAD E E E E E E QUAD E E E E E E *TOTALS* E E E E E E-17

9. Understanding Grid Point Force Output
NASTRAN F06 Output
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 Load(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

10. Understanding Grid Point Force Output
How GPFO Relates to Structure
Freebody display is dependent on the nodes and elements included in the summation
Deciding which nodes and elements are to be used is based on how the model was idealized as well as what specific quantity is desired

11. Freebody Display in FEMAP
Freebodies in FEMAP exist as creatable objects, like nodes, elements, etc.
They persist in the database
This is a huge benefit for recreating freebody displays in the future
Can help reduce analysis errors and rework
Any number of freebodies can be displayed simultaneously
Many tools exist to automate freebody-related tasks, such as creating loads and substructure modeling

12. Freebody Display in FEMAP
FEMAP Freebody Types – There are 3 types of freebody displays in FEMAP
Freebody – user selects the elements, FEMAP automatically selects related nodes. Intended to display a balanced set of loads on a discrete piece of structure

13. Freebody Display in FEMAP
FEMAP Freebody Types – There are 3 types of freebody displays in FEMAP
Interface Load – user selects both nodes and elements and FEMAP calculates a summation of loads and forces across the interface and displays as a single vector

14. Freebody Display in FEMAP
FEMAP Freebody Types – There are 3 types of freebody displays in FEMAP
Section Cut – similar to interface load, a summed load across an interface is calculated and displayed, however node and element selection is automated by FEMAP. The user selects a “cutting plane”. The cutting plane can then be dynamically located within the model using different methods.

15. Freebody Display in FEMAP
Freebody Load Contributions
Freebody load contributions in FEMAP are split into six categories
Applied – All applied loads
Reaction – SPC forces(Constraint forces)
MultiPoint Reaction –
MPC(MultiPoint Constraint forces)
Peripheral Elements – include elements surrounding the selected elements
Freebody Elements – include elements selected by the user or by FEMAP
Nodal Summation – nodal summation values from the solver, not FEMAP calculated values
Default contributions are Applied, Reaction, MultiPoint Reaction and Peripheral elements
This provides forces and moments acting on the selected structure

16. Freebody Display in FEMAP
Freebody Result Vectors – As previously mentioned, 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 italicized rows above represent default output requests in FEMAP and are sufficient for displaying a balanced freebody on the entire structure, but not for display of internal load distribution.
Primary
Secondary
Applied
GPFORCE
OLOAD
SPC
SPCFORCE
MPC
MPCFORCE
Elemental
None
Nodal Summation

17. Using the FEMAP Freebody Toolbox
Accessing the Freebody Toolbox
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 Properties – These controls are related to individual freebodies, such as selecting nodes and elements
View Properties – These are global settings that affect freebody visualization (symbol sizes, vector scaling, etc). Same as found in View Options (F6)

18. Using the FEMAP Freebody Toolbox
Creating a New Freebody
In the Freebody Toolbox, new Freebody Displays are created within the Freebody Manager
The New Freebody dialog allows for setup of basic settings, such as freebody type, vector display, and contribution selection
Any of the settings applied in the New Freebody dialog can be changed at any time within the toolbox

19. Using the FEMAP Freebody Toolbox
Accessing Different Freebody Displays
Multiple Freebody Displays can be viewed at any time however, only a single freebody can be active at any time within the toolbox
Use the drop-down menu to change the active freebody and then modify settings
Visibility of individual freebody displays can be controlled with the “Is Visible” checkbox as well as with the Visibility Quick View Dialog

20. Using the FEMAP Freebody Toolbox
Freebody Vector Types
Depending on the freebody type, there can be nodal vectors and a single total summation vector
Nodal Vectors
Displays the summation at each node, based on the selected freebody contributions
Available for all freebody types
Total Summation Vector
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 (moment arms are different).
Available for Interface Load and Section Cut freebodies only.
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

21. Using the FEMAP Freebody Toolbox
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)

22. Using the FEMAP Freebody Toolbox
Freebody Vector Visualization
Detail Options
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)

23. Using the FEMAP Freebody Toolbox
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

24. Using the FEMAP Freebody Toolbox
Freebody Mode
When using “Freebody Mode”, the user selects elements and FEMAP will automatically select all 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 by a group select
The default contribution selections will display forces/moments acting on the selected elements
Select Elements
Reset Element Selection
Highlight Selected Elements

25. Using the FEMAP Freebody Toolbox
Display of balanced set of loads on wingpost model. All elements in the model were selected for this display

26. Using the FEMAP Freebody Toolbox
Interface Load Mode
Interface load freebodies display nodal vectors for the selected nodes as well as a total summation vector at a selected location
Unlike freebody mode, interface load mode is not likely to be in equilibrium
In addition to element selection, nodes must be user selected– FEMAP does not infer them based on the selected elements
When selecting entities by group, both the nodes and elements of interest must exist in the group

27. Using the FEMAP Freebody Toolbox
Interface Load Mode – Selecting Nodes
Locate Summation Vector at Node Centroid
Select Free Edge Nodes
Select Nodes
Reset Node Selection
Highlight Selected Nodes
Only those elements connected to the selected nodes will be used in calculations

28. Using the FEMAP Freebody Toolbox
Interface Load Mode – Selecting Components in Summation
Individual force and moment contributions that are included in the total summation vector calculation 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

29. Using the FEMAP Freebody Toolbox
Interface Load Display, Showing Summed Shear Load at a Rib
Selected Nodes Highlighted
Selected Elements Highlighted

30. Using the FEMAP Freebody Toolbox
Section Cut Mode
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

31. Using the FEMAP Freebody Toolbox
Curve: Cutting plane is normal to the tangent vector at a point along the plane. Cutting plane will always be normal to the tangent vector
Freebody Section Cut
Entity Select Modes
Plane: 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, 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
Vector: Cutting plane is normal to the defined vector. Path is the defined vector; cutting plane will always be normal to the path

32. Using the FEMAP Freebody Toolbox
Section cut defined using plane

33. Using the FEMAP Freebody Toolbox
Section cut defined using curve

34. Using the FEMAP Freebody Toolbox
Additional Section Cut options
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

35. Using the FEMAP Freebody Toolbox
Cut plane initial position
Cut plane moved along the path
Freebody nodes
Freebody elements

36. Freebody Display Output Options
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

37. Global-Local Modeling with Freebodies
The Create Load from Freebody/Multi-Model tool automates the creation of global-local models
Used to map freebody loads from a coarse grid model to a fine grid model and automatically create connections with RBE3 elements
Start with a balanced freebody in a coarse model
FEMAP can automatically locate suitable
target nodes in the fine grid FEM and will
connect with RBE3 elements
Once properly constrained, the detail FEM is ready to run with a mapped set of loads
The detail FEM must exist in the same
space as the part in the coarse grid FEM

38. Global-Local Modeling with Freebodies
Select Source Model
Select Freebody
Select Output Sets
Multiple Sets allowed
Select Forces and/or Moments
to be included

39. Global-Local Modeling with Freebodies
Define Target Model Parameters
Freebody loads can be applied to target nodes based on:
Existing nodes (IDs must match)
Closest node in space to source node
Existing nodes to be connected with RBE3 elements
User can define target nodes or FEMAP can automatically find
Search distance can be limited
Maximum nodes to map can be limited

40. Global-Local Modeling with Freebodies
Source Model Freebody(Global Model)
Target Model with RBE3 Load Distribution

41. Additional Topics – Freebodies with NX Nastran Glue / Contact
As of NX Nastran v10.1, the GPFORCE output request does not include contributions from glue or contact in the F06 or OP2 datablock
The result is a nodal imbalance that is the summation of all other contributions
Nodes that are affected by glue or contact will not be in equilibrium
The “TOTALS” quantity is equal and opposite to the existing summation
G R I D P O I N T F O R C E B A L A N C E POINT-ID ELEMENT-ID SOURCE T T T R R R HEXA E E E HEXA E E E HEXA E E E HEXA E E E HEXA E E E HEXA E E E HEXA E E E HEXA E E E *TOTALS* E E E HEXA E E E *TOTALS* E E E
Glue/Contact Force balances the element force, but is not included in table

42. Additional Topics – Freebodies with NX Nastran Glue / Contact
In FEMAP 11.2, the ability to reverse the nodal summation value was added, allowing the nodal imbalance to be treated as a separate contribution in the equal-and-opposite direction
This option should only be used if the cause of the imbalance is known to be
the result of data missing from the GPFO
table(glue/contact force) and not caused
by a modeling error.

43. Additional Topics – Freebodies with NX Nastran Glue / Contact
Default contributions
Freebody elements / nodal summation
Freebody elements + nodal summation
Reversed nodal summation

44. Additional Topics – Load from Freebody Tool
Freebody results can be used to create loads within an existing model using the Model->Load->From Freebody tool
Works with all freebody modes
For interface load and section cut freebodies, total summation load can be created at a new node in the model
Loads can be created in an existing load set as well as in a new load set

45. Additional Topics – Load from Freebody Tool
Freebody Loads

46. Additional Topics – Load from Freebody Tool
Created Loads

47. Additional Topics – Sum Data on Nodes Option
By default, freebody vectors at each node are displayed as a summation of the selected components
A global setting allows for nodal quantities to be displayed as individual contributions. It affects all displayed freebodies
This allows for comparison of individual
contributions to F06 data, as well as
troubleshooting of models
This option is best used with the element shrink view option

48. Additional Topics – Sum Data on Nodes Option
Sum Data on node checked
Sum Data on node unchecked, element shrink display
ID: 342
Source Fx Fy Fz Mx My Mz
ELEM 8
ELEM 182
ELEM 80

49. Q and A

50. Siemens PLM UK Symposium Femap Track Agenda
11:00: Femap – introduction and what’s new 11:50: Working with Femap – free bodies and global / local modeling 13:30: Femap industry customer case studies: Aerospace & marine Customer presentation Longitude Consulting Engineers (London Offshore Consulting) Your presenters today: Nick Rakkar UK Channel Sales Manager, Siemens PLM Software Al Robertson Product Marketing Manager, Siemens PLM Software Joe Brackin Senior Software Engineer, Siemens PLM Software Peter Kingsland Naval Architect, Longitude Consulting Engineers

51. Siemens PLM UK Symposium Femap Track Agenda
15:40: Event wrap up
We will be available for questions and discussion after the event
Femap futures and roadmap
Femap technical queries
How can Femap help in your business
Who can you talk to regarding software solution testing
Nick Rakkar – UK Channel Sales Manager