Developing Breakout Models in FEMAP Presenter: Ryan Tatman This - - PowerPoint PPT Presentation

▶
developing breakout models in femap
SMART_READER_LITE
LIVE PREVIEW

Developing Breakout Models in FEMAP Presenter: Ryan Tatman This - - PowerPoint PPT Presentation

Jul 13, 2023 6 likes •309 views

Developing Breakout Models in FEMAP Presenter: Ryan Tatman 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

slide-1
SLIDE 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

slide-2
SLIDE 2

5/22/2012 Page 2 Page 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
slide-3
SLIDE 3

5/22/2012 Page 3 Page 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

slide-4
SLIDE 4

5/22/2012 Page 4 Page 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

slide-5
SLIDE 5

5/22/2012 Page 5 Page 5

Example - Small Design Change

  • Adding a pass-through to a wing rib

VIEW THE DEMONSTRATION

slide-6
SLIDE 6

5/22/2012 Page 6 Page 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

slide-7
SLIDE 7

5/22/2012 Page 7 Page 7

Example – Local Stress Riser

  • Large orthogrid pressure plate with bolted exterior supports
slide-8
SLIDE 8

5/22/2012 Page 8 Page 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
  • n solid meshed breakout
  • Integrate solid meshed breakout into full model
slide-9
SLIDE 9

5/22/2012 Page 9 Page 9

Control – Plate Only Model

VIEW THE DEMONSTRATION

slide-10
SLIDE 10

5/22/2012 Page 10 Page 10

Control – Full Solid Model

VIEW THE DEMONSTRATION

slide-11
SLIDE 11

5/22/2012 Page 11 Page 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

slide-12
SLIDE 12

5/22/2012 Page 12 Page 12

Hex Mesh – Element Penetration

Pros:

  • Can support moment at

junction Cons:

  • Heightened mass
  • Artificially stiff
  • Artificially strong
  • Unconservative
slide-13
SLIDE 13

5/22/2012 Page 13 Page 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.

slide-14
SLIDE 14

5/22/2012 Page 14 Page 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

slide-15
SLIDE 15

5/22/2012 Page 15 Page 15

Solid Breakout – Zipped In

Pros:

  • Accurate stress
  • Accurate mass

Cons:

  • Slower to model
  • Requires more solution time
slide-16
SLIDE 16

5/22/2012 Page 16 Page 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

slide-17
SLIDE 17

5/22/2012 Page 17 Page 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

slide-18
SLIDE 18

5/22/2012 Page 18 Page 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

slide-19
SLIDE 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

slide-20
SLIDE 20

5/22/2012 Page 20 Page 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

slide-21
SLIDE 21

5/22/2012 Page 21 Page 21

Partnerships

Siemens Value Added Reseller Collier Research Corporation Reseller

FEMAP NX Nastran Fibersim Solid Edge HyperSizer Pro HyperSizer Express

slide-22
SLIDE 22

5/22/2012 Page 22

APPENDIX: TUTORIAL WALKTHROUGHS

slide-23
SLIDE 23

5/22/2012 Page 23 Page 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

  • ptions
  • Next we used the “Create New Group”

command followed by the “Group Element ID - by Property” command to select the rib

slide-24
SLIDE 24

5/22/2012 Page 24 Page 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

slide-25
SLIDE 25

5/22/2012 Page 25 Page 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.

slide-26
SLIDE 26

5/22/2012 Page 26 Page 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

slide-27
SLIDE 27

5/22/2012 Page 27 Page 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

slide-28
SLIDE 28

5/22/2012 Page 28 Page 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
  • ur solid into the size of our breakout.
slide-29
SLIDE 29

5/22/2012 Page 29 Page 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

slide-30
SLIDE 30

5/22/2012 Page 30 Page 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