![5/22/2012
Page 1
Developing Breakout Models in FEMAP
This presentation includes:
• Definition of Breakout Models
• When to use breakouts
• [Tutorial] Adding a pass-through in a wing rib
• [Tutorial] Adding boss to orthogrid pressure plate
Presenter: Ryan Tatman](https://image.slidesharecdn.com/developingbreakoutmodelswithappendixslides-160831130000/85/Developing-Breakout-Models-in-FEMAP-Includes-Tutorial-Walk-throughs-1-320.jpg)
Developing Breakout Models in FEMAP (Includes Tutorial Walk-throughs)
- 1. 5/22/2012 Page 1 Developing Breakout Models in FEMAP This presentation includes: • Definition of Breakout Models • When to use breakouts • [Tutorial] Adding a pass-through in a wing rib • [Tutorial] Adding boss to orthogrid pressure plate Presenter: Ryan Tatman
- 2. 5/22/2012 Page 2Page 2 Presentation Summary • SDA Overview • Breakout Definition • When to use breakouts • Example - Adding a pass-through in a wing rib • Example – Adding boss to orthogrid pressure plate • Conclusions
- 3. 5/22/2012 Page 3Page 3 What is a breakout model? • A breakout model is an analysis model created to represent a portion of a large structure in order to get more specific information. Example: Assessing the stress concentration in the joint shown below
- 4. 5/22/2012 Page 4Page 4 When is a breakout model needed? • When a small design change requires analysis – When a small portion of a large design needs to be iteratively designed – When a feature is added to an existing part • When examination of localized stress risers is needed – When the size of a model does not allow for the fidelity needed in specific locations – When stress information is needed for a fillet or pad-up in a plate model
- 5. 5/22/2012 Page 5Page 5 Example - Small Design Change • Adding a pass-through to a wing rib VIEW THE DEMONSTRATION
- 6. 5/22/2012 Page 6Page 6 Map Output from Model • Model -> Load -> Map Output from Model Source Model Elements/Nodes to take results from Output sets to take results from What data to take What to do if there is no data for a node or element in target model
- 7. 5/22/2012 Page 7Page 7 Example – Local Stress Riser • Large orthogrid pressure plate with bolted exterior supports
- 8. 5/22/2012 Page 8Page 8 Popular Options • Hex-Mesh the area of the model – No element doubling – Element penetration – Element skins • Pull nodal displacements and rotations from the analysis and create SPCDs to apply on solid meshed breakout • Integrate solid meshed breakout into full model
- 9. 5/22/2012 Page 9Page 9 Control – Plate Only Model VIEW THE DEMONSTRATION
- 10. 5/22/2012 Page 10Page 10 Control – Full Solid Model VIEW THE DEMONSTRATION
- 11. 5/22/2012 Page 11Page 11 Hex Mesh – No Element Doubling Pros: • Accurate stiffness • Accurate mass Cons: • No moment supported at junction • Potentially unconservative • Potentially incorrect load path Limitations: • Solid Elements cannot resolve moments at its nodes so all plate-solid interactions are hinges
- 12. 5/22/2012 Page 12Page 12 Hex Mesh – Element Penetration Pros: • Can support moment at junction Cons: • Heightened mass • Artificially stiff • Artificially strong • Unconservative
- 13. 5/22/2012 Page 13Page 13 Hex Mesh – Element Skins Pros: • Can support moment at junction Cons: • Heightened mass • Artificially stiff • Artificially strong • Unconservative Note: a thinner skin can be used to lessen this effect, but thin skins behave like no element doubling, leading to a potentially incorrect load path.
- 14. 5/22/2012 Page 14Page 14 Solid Breakout – Interface Nodes Pros: • Quick to model • Accurate mass Cons: • Potentially incorrect stress • Artificially high stress if stiffness increased • Artificially low stress if stiffness decreased • Fairly accurate stress if stiffness is not significantly changed
- 15. 5/22/2012 Page 15Page 15 Solid Breakout – Zipped In Pros: • Accurate stress • Accurate mass Cons: • Slower to model • Requires more solution time
- 16. 5/22/2012 Page 16Page 16 Conclusions • “Map output from model” is a quick way to set up loads on a breakout – Try to keep nodes in original location (use mesh refine, not remesh) – Try to keep breakout stiffness similar to original model if using enforced displacements • Plate to solid transitions can work in some instances, but have limitations • “Dummy elements” can be used for ballpark estimates if needed, but will often give inaccurate results • “Zipped in” breakout models will give the most consistently accurate results – Grow breakout model by at least three elements lengths from the point of interest
- 17. 5/22/2012 Page 17Page 17 Additional Resource What New book published Fall 2014 Why Learning with the help documentation can be like drinking from a fire hose. Learning Femap succinctly covers the bases on using Femap without being a “bible”. Covers Introduction Femap Application Interface Modeling/ Pre-Processing Analysis Post-Processing Programming Femap How Explanation of features Numerous illustrations Annotated examples Guided tutorials Learning Femap ISBN 978-1-4951-2963-6 By Eric Gustafson (eric@structures.aero), Senior Aerospace Stress Analyst, SDA Available online at www.learningfea.com $49.99
- 18. 5/22/2012 Page 18Page 18 Contact Us: Contact: Marty Sivic Email: msivic@structures.aero Website: http://structures.aero/ Phone: (724) 382-5290 Try FEMAP For Free! Download a free 45-day trial of FEMAP with NX Nastran • Full FEMAP capabilities • All Nastran solution sequences included • (http://structures.aero/femap-trial/) Presenter: Ryan Tatman Email: rtatman@structures.aero Website: http://structures.aero/ Phone: (703) 935-2818
- 19. 5/22/2012 Page 19 About SDA (aka “Structures.Aero”) • SDA was founded in 1997 and provides expert aerospace structural analysis • We serve a variety of industries • We specialize in composites, and developing strong, lightweight structures that are readily manufacturable • Low level support up through developing test plans and advanced stress analysis • Typical support programs include small to large UAVs, manned and unmanned spacecraft, naval structures • Our team consists of over a dozen B.S., M.S., and PhD level engineers • SDA is located in Sterling, VA, just north of Dulles Airport near Washington DC Learn more about Structural Design and Analysis
- 20. 5/22/2012 Page 20Page 20 Typical Projects We Support • Some of our previous projects include: – Aircraft • Aurora Excalibur • MHADD ARES • Vanilla VA1 • Lockheed Constellation restoration for Lufthansa – Spacecraft • NASA NESC Composite Crew Module (CCM) • NASA NESC Max Launch Abort System (MLAS) • NASA James Webb Space Telescope/IEC • NASA Orion Heatshield mass reduction for NESC • NASA Orion Crew Module (with Lockheed) • NASA WFIRST Telescope for Goddard Aerosonde Heatshield Shadow M2 CCM Orion Crew Module
- 21. 5/22/2012 Page 21Page 21 Partnerships Siemens Value Added Reseller Collier Research Corporation Reseller FEMAP NX Nastran Fibersim Solid Edge HyperSizer Pro HyperSizer Express
- 22. 5/22/2012 Page 22 APPENDIX: TUTORIAL WALKTHROUGHS
- 23. 5/22/2012 Page 23Page 23 Small Design Change Example Walkthrough • First we used the “Draw Erase Selective Mesh – Property” command (new in 11.3). • This allows the user to selectively hide elements and surfaces using a variety of options • Next we used the “Create New Group” command followed by the “Group Element ID - by Property” command to select the rib
- 24. 5/22/2012 Page 24Page 24 Small Design Change Example Walkthrough • “Add Related Elements” adds all entities needed to fully define the group • We then created a new modfem • File -> Merge lets you merge portions of models into other models • We chose our model then clicked “All Off” because we don’t want the entire model • We then went to the “Entity selection” section and chose “From Group” and picked our group • Clicking “Add Related Entities” then “Update All” completes the action
- 25. 5/22/2012 Page 25Page 25 Small Design Change Example Walkthrough • We then used the “Element Refine” tool to refine our mesh (new in 11.3) • We chose the 4:1 pattern with the Add/Refine Action and used Area Drag to select all of our elements.
- 26. 5/22/2012 Page 26Page 26 Small Design Change Example Walkthrough • The “Map Output From Model” command is going to bring loads from our full model into our breakout model. • We chose to use nodal displacements in this breakout
- 27. 5/22/2012 Page 27Page 27 Small Design Change Example Walkthrough • We applied these loads to the perimeter nodes as well as creating a new pinned constraint. • The breakout is now set up and ready to be run
- 28. 5/22/2012 Page 28Page 28 Local Stress Riser Example Walkthrough • First, we defined our breakout location by creating a square with the “Rectangle” Command • The “Solid – Slice” Command lets us slice our solid into the size of our breakout.
- 29. 5/22/2012 Page 29Page 29 Local Stress Riser Example Walkthrough • After deleting the geometry and mesh we no longer needed, we used the “Mesh – Geometry – Solid” command to mesh our solid • The “Connect – Rigid” command was used to connect our plates to our solids
- 30. 5/22/2012 Page 30Page 30 Local Stress Riser Example Walkthrough • The source nodes are on the plate elements and the target nodes are on the solid elements • We used RBE2s in the webinar, but RBE3s can be used as well. Which RBE to use can depend on its application in your breakout • The bolt interface RBE was updated to connect to the new solid mesh using the “Modify – Edit – Element” Command. • The model is finished and ready to run
Editor's Notes
- #3: ~30 seconds
- #6: Live demo creating a passthrough breakout model on one of the ribs ~5-7 minutes
- #9: FEMAP: -Go through each of the 6 models showing how it was modeled and point out the shortfalls of each and when they may be used. Make sure to compare each to the control models -Mention that the “zipped in” breakout is the best way to get consistently accurate results, but mention that it requires running the entire model (or at least a large section of it) in order to be accurate. - Mention that in order for the breakout to be accurate, the stiffness of your breakout model must be very similar to the stiffness of that section in the original model. If it isn’t, you will need to run the entire model. Live Demo: ~8-10 minutes -Take the plate model (control 1) and import geometry. -Take them through the steps of creating a “Zipped In” breakout model -Make bounding geometry -Slice solid -Mesh solid (do tet mesh, but mention that hex is an option as well) -Mesh-connect-rigid -Mention the CBUSH in the center and that all interfaces with other structure must be accounted for
- #10: Switch over to FEMAP. Discuss the stress concentration at the middle junction and show geometry “This is a good place to use a breakout model”
- #11: The best option is to solid mesh the entire part, but most of the time this is not possible. Using this as a control, we know that we are looking for a stress concentration around 96ksi at the junction of the pad-up and the ribs
- #12: A very common solution is to hex mesh the pad-up and merge the nodes of the ribs to the nodes on the pad-up. *Show what parts of the model are solid and what parts are plates The problem with this method is that solid elements don’t support moments, so you will have a hinge at all of the plate-solid junctions. It works for this application because the moments can be resolved with translations in all dimensions. This solution works well for this application with a stress concentration of 92ksi in the correct location. It is unconservative, but gives a good idea of what the stresses will be like in the area with relatively little effort
- #13: Another common solution in response to the inability of solid elements to support moments is to extend the plate elements into the solid section. This supports all 6 DOF at each node. *Show what parts of the model are solid and what parts are plates This method solves the moment problem, but adds artificial mass, stiffness and strength. This solution is not the best for this application because the moment at the interface nodes is not needed. The stress concentration has a margin of error of 15% and is pushed away from the real location by
- #14: Another common solution that solves the inability of solid elements to support moments is to skin the solid elements in plate. This supports all 6 DOF at each node. *Show what parts of the model are solid and what parts are plates This method solves the moment problem, but adds artificial mass, stiffness and strength. This solution is not the best for this application because the moment at the interface nodes is not needed.