Industrial FEA Modeling Course 2010 [PDF]

Zitiervorschau

Industrial Finite Element Analysis

Industrial Finite Element Analysis with F Femap V10 1. V10. 1 1 and d NX Nastran N t V7 0 V7.

Re evised 2010

An introduction to Femap and NX Nastran using a blend of theory and practice that will allow the student to quickly grasp the nuances of building accurate FE models. Four Day Introductory Class with sufficient material for six days of lectures.

1

Industrial Finite Element Analysis Course Outline: I. Introduction to Finite Element Analysis a.) The concept of finite element analysis - nodes, DOF, elements b.) Basic element types - a quick overview c.) Linear, elastic FEA d.) F = K*U e.)) Workshop W kh using i Femap F and d NX N Nastran t Introduction to Femap / Panes / Toolbars / Preferences / Etc Simple Solid Model Stress Analysis

II Theory and Usage of Finite Elements II. a.) Beam Elements: i) Theory p ii)) Workshop Re evised 2010

b.) Isoparametric Elements (plate and solid): i) Theory ii) Workshops

2

Industrial Finite Element Analysis Course Outline (continued): III. Foundations of FE Analysis and Modeling a.) Units b.) Surface modeling (plate elements) i) Techniques of working with geometric surfaces and plate models ii) Workshop – basic surface modeling concepts / linear elastic analysis iii) Techniques T h i off simplifying i lif i structures t t into i t FE models d l ((use off mass elements and rigid links) iii) Workshop – mid-surfacing geometry / vibration analysis c.) Application of loads to FEA models i) Utilization of pressure loads for pressure vessels and bearing loads ii) Workshop – surface modeling of thin walled structures / pressure load iii) Workshop – working with solid models to create bearing loads (simple versus data surfaces) Re evised 2010

d.) Constraints i) Theory on the application of symmetry: geometry and loads ii) Workshop

3

Industrial Finite Element Analysis Course Outline (continued): IV. Assembly Modeling a.) Standard, linear connection technologies (rigid links) i) Technology review and commentary ii) Workshop b.) Advanced NX Nastran connection technologies i) Technology of surface-to-surface glued versus surface contact. ii) Workshops – glued connection and surface-to-surface

V. Results Validation a.) Definition of von Mises stress scalar and max/min principal stresses b.) Interpretation of stress results w.r.t. to von Mises and principal stresses c.) Fatigue in FEA Re evised 2010

d.) Using Free-Body-Diagrams (FBD) to check loading and load path

4

Industrial Finite Element Analysis Course Outline (continued): VI. Advanced Femap Modeling Topics a.) Mesh Repair i) Technology and Commentary ii) Workshop – mesh repair and introduction to Data Table b.) Hexing Solids i) Theory and Background ii) Workshop – hex meshing with introduction to master/slave pairing c.) Advanced surfacing techniques i) Theory behind surfacing within Femap ii) Workshop – using Solid Geometry menus for surfacing operations. d.) Femap Program Files i)) Theory y and limitations of Femap p macro creation Re evised 2010

ii) Workshop – create simple macro and user-defined toolbar. e.) Application Programming Interface (API) i) Introduction to Femap’s API for customization and automation of repetitive modeling tasks. tasks Discussion of “Custom Custom Tools Tools”. ii) Workshop – Create simple API and place in user-defined toolbar.

5

Industrial Finite Element Analysis Course Outline (continued): VII. Advanced Analysis Topics a.) Geometric and Material Nonlinearities b.) Dynamics: Modal and Transient i) Introduction to Eigenvalue/Normal Modes Analysis ii) Workshop – Basis Normal Modes with Optimization

VIII. Troubleshooting and Modeling Guidelines a.) Understanding online Help Documentation. b.) Femap and NX Nastran Error Messages i) Theory/Background on error messages ii) Workshop – Debug FEA model using error messages with online help c.) Modeling guidelines and best practices i)) Discussion of element q quality y indicators Re evised 2010

ii) Workshop – contouring element Jacobian over mesh d.) Open discussion / Comments

6

7

Industrial Finite Element Analysis Finite Element Analysis: A numerical analysis technique for obtaining approximate solutions to many types of engineering problems. The need for numerical methods arises from the fact that for most practical engineering problems analytical solutions do not exist. While the governing g g equations q and boundary y conditions can usually y be written for these problems, difficulties introduced by either irregular geometry or other discontinuities render the problems intractable analytically. To obtain a solution, the engineer must make simplifying assumptions, reducing the problem to one that can be solved, or a numerical procedure must be used. In an analytic solution, the unknown quantity is given by a mathematical function valid at an infinite number of locations in the region under study, while numerical methods provide approximate values of the unknown quantity only at discrete points in the region. region In the finite element method, method the region of interest is divided up into numerous connected subregions or elements within which approximate functions (usually polynomials) are used to represent the unknown quantity.

Re evised 2010

The physical concept on which the finite element method is based has its origins in the theory of structures. The idea of building up a structure by fitting together a number of structural t t l elements l t (see ( illustration) ill t ti ) was used d in i the th early l ttruss and d framework f k analysis l i approaches employed in the design of bridges and buildings in the early 1900s. By knowing the characteristics of individual structural elements and combining them, the governing equations for the entire structure could be obtained. This process produces a set of simultaneous algebraic equations. The limitation on the number of equations that could be solved posed a severe restriction on the analysis. The introduction of the digital computer has made possible the solution of the large large-order order systems of equations. The finite element method is one of the most powerful approaches for approximate solutions to a wide range of problems in mathematical physics. The method has achieved acceptance in nearly every branch of engineering and is the preferred approach in structural mechanics and heat transfer. Its application has extended to soil mechanics mechanics, heat transfer transfer, fluid flow flow, magnetic field calculations calculations, and other areas areas. From McGraw-Hill Science and Technology Encyclopedia, 5th Ed.

Structures St t modeled d l d by b fitting fitti together t th structural elements: (a) truss structure; (b) two-dimensional planar structure.

Industrial Finite Element Analysis Four things to know about FEA:

Re evised 2010

• Idealization of Geometry into a numerical Model • Engineering assessment of Loads. Loads • Visualization of structural constraints into modeling Constraints. • Discretization of continua into a finite element analysis Mesh (meshing).

8

Industrial Finite Element Analysis Finite Element Analysis Concepts: • Nodes are used to define the geometry of the finite element (that is to say “its spatial characteristics”). Nodes have degrees-of-freedom and can translate (3 DOF (TX, TY, & TZ)) and rotate ((3 DOF ((RX, RY, & RZ)) )) in space. p • Finite elements can be classed as point, line, surface and solid elements. Another way to think of these elements is as having 0-D, 1-D, 2-D and 3-D characteristics (D=dimensional). • 0-D elements are created on one node and can be meshed on geometric points. • 1-D elements are created on two nodes and can be meshed on geometric lines. • 2-D elements are created on three or four nodes (triangular or quad) and can be meshed on geometric surfaces. • 3-D elements are created on a minimum of four nodes (tetrahedral) or eight nodes (brick or hexahedral) and can be meshed on geometric solids. • Examples of various element types are: •0-D elements are mass elements used to simulate concentrated weight without stiffness. Re evised 2010

•1-D elements are beam elements used to model space-frame structures (e.g., bus frames). •2-D elements are plate elements used to model thin walled structures (e.g., pressure vessels, airplane skins, sheet metal, ships or structural steel framing). •3-D 3 D elements l t are solid lid elements l t used d tto model d l thick, thi k contoured t d objects bj t (e.g., ( castings). ti )

9

10

• Stresses can be scaled as a linear function of the loads. • The structure is elastic. • Scale displacements as a ratio of elastic moduli.

Stress

Linear, Elastic, Static Analysis (99% of the world)

Re evised 2010

Strain

Force F σ= Area

Stress is independent of your material choice.

∑F = 0

Static means no acceleration - no spinning off into space.

11

∑F = 0 FEA is i based on the displacement i method, which i boils i down to:

{F} = [K ]{u} • With a little work work, structures and materials can be described as springs. springs • We typically know something about forces and / or displacements.

Re evised 2010

• The Th equations ti are solved l d for f displacements........................ di l t

12

Step 1: Satisfy static equilibrium

Re evised 2010

∑ Fx = F1 + F2 = 0 F1 = − F2

13

Step 2: Relate strain to displacements

Δ L u 2 − u1 = εx = L L

St Step 3 3: Relate R l t stress t tto strain t i

Re evised 2010

σ x = Eε x

14

Step 4: Relate force to stress

F1 σ x1 = − A

and

σ x2

F2 = A

Re evised 2010

The minus sign is required since a positive tensile stress at End 1 is in the negative x direction.

15

Step 5: Relate force to displacement Using the prior equations and performing a little substitution yields:

EA − F1 = σ x A = Eε x A = ( u 2 − u1 ) L

Re evised 2010

EA EA − F1 = u2 − u1 L L

16

Step 6: Assemble matrix

⎧F1 ⎫ EA ⎡ 1 − 1⎤ ⎧u1 ⎫ ⎨ ⎬ ⎨ ⎬= ⎢ ⎥ ⎩F2 ⎭ L ⎣ − 1 1 ⎦ ⎩u 2 ⎭

Re evised 2010

which g give us:

{F} = [K ]{u}

* If u1 and u2 are non non-zero zero then an infinite number of solutions are possible or in mathematical terms, the determinant of the stiffness matrix “K” is singular.

17

Re evised 2010

Ea A a 1 • 2 ka = = =2 La 1

Eb A b 1 • 1 kb = = =1 Lb 1

−2 0 ⎤ ⎧u1 ⎫ ⎧F1 ⎫ ⎡ 2 ⎪ ⎪ ⎢ ⎥ ⎪u ⎪ F = − 2 2 + 1 − 1 ⎨ 2⎬ ⎢ ⎥⎨ 2 ⎬ ⎪F ⎪ ⎢ 0 − 1 1 ⎥⎦ ⎪⎩u 3 ⎪⎭ ⎩ 3⎭ ⎣

*Where nodes share elements, they share stiffness terms. Off g terms are zero. diagonal

Re evised 2010

18

0 ⎤ ⎧u1 ⎫ −2 ⎧F1 ⎫ ⎡ 2 ⎪ ⎪ ⎢ ⎪ ⎪ ⎥ ⎨F2 ⎬ = ⎢− 2 2 + 1 − 1⎥ ⎨u 2 ⎬ ⎪F ⎪ ⎢ 0 ⎪u ⎪ − 1 1 ⎥ ⎦⎩ 3 ⎭ ⎩ 3⎭ ⎣

In this form, K is singular! One of the displacements must be zero to obtain a unique solution. Let’s make u1 = 0 and then try y to find a solution.

0 ⎤ ⎧0 ⎫ −2 ⎧F1 ⎫ ⎡ 2 ⎪ ⎪ ⎢ ⎪ ⎪ ⎥ ⎨F2 ⎬ = ⎢− 2 2 + 1 − 1⎥ ⎨u 2 ⎬ ⎪F ⎪ ⎢ 0 ⎪u ⎪ − 1 1 ⎥ ⎦⎩ 3 ⎭ ⎩ 3⎭ ⎣

F1 is solved as a “reaction force” at the end of the solution based on the known displacements u2 and u3. This allows us to rewrite the matrix as:

⎧F2 ⎫ ⎡ 3 − 1⎤ ⎧u 2 ⎫ ⎨ ⎬ ⎨ ⎬=⎢ ⎥ ⎩F3 ⎭ ⎣ − 1 1 ⎦ ⎩u 3 ⎭

The determinant of the stiffness matrix is no longer zero (i.e., 2) and a solution can be found using any number of matrix technologies.

19

⎧F2 ⎫ ⎡ 3 − 1⎤ ⎧u 2 ⎫ ⎨ ⎬=⎢ ⎨ ⎬ ⎥ ⎩F3 ⎭ ⎣ − 1 1 ⎦ ⎩u 3 ⎭

• Let F2 = 0 and F3 = 1, find u2 and u3:

−1

⎧u 2 ⎫ ⎧0 ⎫ ⎨ ⎬ =[K ] ⎨ ⎬ ⎩1 ⎭ ⎩u 3 ⎭

Re evised 2010

1 u2 = 2 3 u3 = 2

and

1 ⎡1 1⎤ 1 − [K ] = 2 ⎢1 3⎥ ⎣ ⎦

F1 = −2 • u 2

20

Part I: Workshop using Femap and NX Nastran Pre-Processing Workflow: • Walk through Interface. Introduce concept of Panes / Tool Bars / Menu / Selector Orientation • Talk about Preferences and setting up one directory (Scratch) to store all of the modeling files. • Femap is 100% Windows - Undo / Redo • Import Geometry / Clean up Geometry using Geometry / Solid / Remove Face. Face • Apply 1e5 load in –Z direction. • Apply Constraints – Radial and Fixed. • Analyze

Re evised 2010

Analysis Script: Geo, Mat, Prop, Mesh Sizing, Mesh, Load, Constraint & Analyze y Note: All analysis examples in this class follows this general analysis outline.

Import Geometry File: Introduction to Femap / Part I / LANDING GEAR LINK.X_T Movie File: Introduction to Femap / Part I / Introduction to Femap and NX Nastran.avi

21

Part II: Workshop using Femap and NX Nastran Pre-Processing Workflow:

Re evised 2010

• Creation of model using the Tree – all the way day Same script – except a bit slower. day. slower • Delete unneeded geometry and mesh with default mesh scaling. Talk about meshing messages. • Apply constraints via the Selector and introduce the selector logic a bit (i.e., what happens when you are in selector mode with the mouse buttons for model viewing). • Discuss Pick modes (Normal versus Front). • Create Rigid Link (create node and then element). • Apply 1000 lbf load in X-direction X direction • Create Analysis Set using Elem. Iterative Solver • Run and Post Process.

Import Geometry File: Introduction to Femap / Part II / Avionics Instrumentation Turret.X_T Movie File: Introduction to Femap / Part II / Avionics Instrumentation Turret.avi

22

Using the dialog boxes with tricks F Femap Productivity P d ti it (RTM): (RTM)

Re evised 2010

• Reading the User manual can provide insight into how Femap functions. • Explore online help under User Manual. • Short cut key and Dialog boxes • Look at “Using the Mouse”

23

Beam Elements: Nastran’s Most Challenging Element

2D Beam model:

The big difference is rotation. In 3D - each node has six degrees of freedom (DOF).

Re evised 2010

The equations for this 2D beam can be developed from straight mechanics (e.g., see Timoshenko):

⎧Fy1 ⎫ 3L 3L ⎤ ⎧v1 ⎫ −6 ⎡6 ⎪ ⎪ ⎢ 3L 2L 2 − 3L L2 ⎥ ⎪θ ⎪ M ⎪ z1 ⎪ 2EI ⎢ ⎪ 1⎪ ⎥ ⎨ ⎬= 3 ⎨ ⎬ F 6 3 L 6 3 L − − − ⎥ ⎪v 2 ⎪ ⎪ y2 ⎪ L ⎢ ⎢ 3L L2 − 3L 2L2 ⎥ ⎪θ ⎪ ⎪M ⎪ ⎦⎩ 2 ⎭ ⎣ ⎩ z1 z1 ⎭

* If we had more than one beam element how would the matrix look? * How manyy DOF does this beam element have? * What DOF would have to be fixed to solve this problem?

24

Beam Elements: Nastran’s Most Challenging Element

Re evised 2010

Beam orientation is often difficult ff to first f grasp g p but then seems obvious...

Beams can be offset from their neutral axis and/or from their shear center.

25

Re evised 2010

Beam Elements: Nastran’s Most Challenging Element

The “beam orientation vector” is the beam “Cross Section Definition” Y vector…..

26

Beam Elements: Nastran’s Most Challenging Element

Pre-Processing Workflow: • Geometry preparation is done • Create Material (Steel) • Create Beam Property: Rect. Rect tube 1.5x1.5x0.083” • Assign Mesh sizing and mesh curves (the “beam orientation vector” is the…..) • Create Loads: We are simulating 500 lb of gear on one side of the frame – distributed front and back (see graphic) • Mesh at 4” sizing / Discuss beam orientation. • Weld the parts together. • Set up Analysis Manager • Run

Post-Processing Workflow:

Re evised 2010

• View Select (F5) • View Options (F6) • Beam models have some unique things…..

Open Model File: Beam Modeling / Part I / Pickup Cargo Rack – Start.mod Movie File: Beam Modeling/ Part I/ Cargo Rack Simulation Pre.avi

27

Beam Elements: Nastran’s Most Challenging Element

P P Pre-Processing i Workflow: W kfl • Geometry preparation is done • Create Material and Multiple Properties (Beams) Beams are tube 1.5x1.5x0.083”, rect. Tube 2x1x0.125” and plate 3x0.73 2x1x0.125 3x0.73” • Assign Mesh sizing and Attributes on Curves • Mesh Geometry (curves) • Create Loads (500 lbf thrust per motor at top and bottom of frame) and Constraints (welded onto frame). • Set up Analysis Manager • Run

Post-Processing Workflow:

Re evised 2010

• View Select (F5) • View Options (F6) • Validating the Beam Model

Open Model File: Beam Modeling / Part II / Beam-Thruster Structure - Start.MOD Movie File: Beam Modeling / Part II / Beam-Thruster Structure-Pre.avi

28

Beam Elements: Nastran’s Most Challenging Element

Post-Processing: Beam Stresses • Beam stresses are calculated at the

stress recovery (SR) points (think beam th theory: stress t = mc/I). /I) • Beams have End A and End B’s – this is a beam world convention. Not a big deal since the program will contour selected items at both ends of the beam.

Re evised 2010

• Stresses are reported as Max combined or Min combined or at SR points – you chose chose. The Max is the maximum value of the SR points. Combined is just the combined axial and bending stresses. Torsion is not included. • Be careful about your torsion assumptions.

29

Beam Elements: Common pitfall when creating beam models

Pre-Processing Workflow: • Meshing curves separately – you are then laying d down th the beam b elements l t as separate t “independent” entities. In this case, the program does not know what to connect since they are created independently. That is, each time you mesh a curve it creates its own set of nodes and elements When you run the model and you elements. have elements that are not connected – then you may see the Error Message below. • If you are meshing curves one at a time (so to speak) then you will need to merge up the coincident nodes or weld the structure. This is done under Tools / Check / Coincident Nodes. Note: go slow on this one since you need to check the Merge Coincident Node box.

Just the tubes….sequential meshing g of the structure..

Re evised 2010

Error Message: g

^^^ USER FATAL MESSAGE 9137 (SEKRRS) ^^^ RUN TERMINATED DUE TO EXCESSIVE PIVOT RATIOS IN MATRIX KLL. ^^^ USER ACTION: CONSTRAIN MECHANISMS WITH SPCI OR SUPORTI ENTRIES OR SPECIFY PARAM,BAILOUT,-1 TO CONTINUE THE RUN WITH MECHANISMS. *** USER INFORMATION MESSAGE 4110 (OUTPX2)

Note: When merging coincident nodes make k sure you actually t ll Merge’em M ’ – this thi box needs to be checked.

Beam-Thruster / Beam-Thruster Structure - Finish.MOD Beam-Thruster Structure-Extra Credit.avi

30

General All Purpose Elements: Isoparametric Elements

Re evised 2010

Isoparametric elements can model anything - since they approximate the behavior of the structure through the use of many, simple polynomial f ti functions. However, H since i they are approximate, the user must apply good engineering judgment throughout the modeling process.

31

General All Purpose Elements: Isoparametric Elements

In order to develop stiffness equations, we must be able to map displacements within the solid element from its nodal locations. 4

u xp = ∑ N i ( ξ , η ) u xi i =1 4

x xp = ∑ N i ( ξ , η ) x xi i =1

Re evised 2010

Ni is known as the shape function, which does double duty as the interpolation function for both displacements and coordinates. coordinates

η = eta ξ = xi

An example of a linear shape function:

1 N1 = (1 − ξ )(1 − η ) 4

32

General All Purpose Elements: Isoparametric Elements

The development of an element stiffness matrix is somewhat analogous to that for a simple rod.

Step 1: Satisfy static equilibrium

∑F = 0

Re evised 2010

Step 2: Relate strain to displacements - simple 2D example

⎡∂ ⎧ε x ⎫ ⎢ ∂x ⎪ ⎪ ⎢ ⎨ε y ⎬ = ⎢ 0 ⎪ ⎪ ⎢ ⎩γ xy ⎭ ⎢ ∂ ∂y ⎣

⎤ 0 ⎥ ∂ ⎥ ⎧⎨u ⎫⎬ ∂y ⎥ ⎩ v ⎭ ∂ ⎥ ∂x ⎦⎥

or

ε = ∂u

33

General All Purpose Elements: Isoparametric Elements

Step 2: Relate strain to displacements - simple 2D example Displacements within the quadrilateral are interpolated from nodal displacements ui and vi using the shape functions Ni

Re evised 2010

⎧u ⎫ ⎡N1 0 N 2 ⎨ ⎬=⎢ ⎩v ⎭ ⎣ 0 N1 0

0 N2

⎧ u1 ⎫ ⎪v ⎪ ...⎤ ⎪⎪ 1 ⎪⎪ ⎨u 2 ⎬ ⎥ ...⎦ ⎪ ⎪ v2 ⎪ ⎪ ⎪⎩ . ⎪⎭

or

u = Nd

34

General All Purpose Elements: Isoparametric Elements

Step 2: Relate strain to displacements - simple 2D example

ε = ∂Nd

or

ε = Bd

Step 3: Relate stress to strain

σ = Eε

or

where

B = ∂N

Matrix “B” is called the strain-displacement strain displacement matrix.

σ = EBd

Re evised 2010

Step 4 and 5: Relate force to stress and then force to displacement

F = EεA

or

F = EBdA

35

General All Purpose Elements: Isoparametric Elements

F = EBAd Although this may look pretty simple, we need a more robust expression that will provide an element stiffness at each nodal location. Without going into the math in great detail, the element stiffness matrix looks like this:

{k} = ∫ ∫ [B ] [E][B ]dxdy T

Re evised 2010

{k} = ∫−11 ∫−11[B ]T [E][B ][ J ]dξdη

{F} = {k}{d}

To determine “k”, one must numerically integrate over the whole h l area or volume l off the h element. Moreover, since we are using the general coordinate system, we need to make one last change g (Jacobian ( transformation matrix).

36

General All Purpose Elements: Isoparametric Elements

Gaussian integration points - if we didn’t use them - we would be hurting in a big way. This technique is also known as Gauss Quadrature. 1 1 k = { } ∫−1 ∫−1[B ] [E][B ][ J ]dξdη T

Numerical integration will use thousands of CPU cycles solving for “k”

Gaussian Integration: n m

I = ∑ ∑ Wi Wjφ ( ξ i , η j )

Re evised 2010

i =1j=1

*We have skipped pp a bunch off math,, but the theme is that a lot of the action happens at the Gauss points.

37

General All Purpose Elements: Isoparametric Elements

Stresses are computed at the Gaussian integration points. Nodal stress values used in stress contouring are then extrapolated (using the shape functions) out to the nodal points.

Re evised 2010

If the element is badly distorted, these Gaussian integration points will do a poor job in capturing the correct area or volume and an even poorer job in delivering accurate stress values.

38

General All Purpose Elements: Isoparametric Elements

FEA Isoparametric Stresses • In Isoparametric elements, stress are first calculated at the Gauss points and then extrapolated out to the nodal points and interpolated to the centroid of the element. island and the • Each element is an “island” computation of stress within that element is unique to that element. • For a basic quad element with four nodes, each stress component will be reported at the nodes and the centroid.

Re evised 2010

• FEA post-processors present plots of averaged nodal stresses between elements. • An element stress convergence check can be made by comparing the element’s l t’ centroid t id to t nodal d l stress t values. l

39

General All Purpose Elements: Isoparametric Elements

Re evised 2010

Many types of structures are modeled best using plates • Thin walled structures, e.g., sheet metal, tanks, tubes, and composites • Detailed analysis of structural steel shapes • Slabs where a shear loading is not dominant, e.g., a Length/Thickness > 10 • or the thickness of the structure does not change due to loading

Classically, plates carry only transverse loads and are flat. Whereas, shells can be curved and carry membrane loads. In practice, we just use FEA “plates” that combine both behaviors.

40

General All Purpose Elements: Isoparametric Elements

Plate theory: 6 DOF at every node Plate loading is dominantly defined by transverse loads. This type of loading causes the plate to have lateral displacement w=w(x,y) in the z direction. The strain-displacement t i di l t ffunctions ti are then th formulated f l t d as:

∂2w ε x = −z 2 ∂x

∂2w ε y = −z 2 ∂y

γ xy

∂2w = −2 z ∂ x∂ y

Re evised 2010

From this point forward, approximately the same approach is used for isoparametric elements is followed, i.e., shape functions are used to interpolate the coordinates and displacements. Consequently, your mileage may vary depending upon the shape of your elements. elements

41

Plate Elements: Nastran’s Most Commonly Used Element

T i Covered: Topics C d • Introduction of curves/surfaces/plates. • Using the Selector logic for modeling versus other methods within the interface. • Femap is a database that allows you to “tag” tag things – like plate properties to surfaces. • Plates have top and bottom and so do surfaces. Start to think about idealization. • Post processing is more than just contouring…..

Re evised 2010

Workflow: • Build your own geometry starting with curves and then extruding the curves. The I beam is a 6x8” by 64” long with 5” diameter web holes at 8” centers. t • Flange is 3/8” with a ¼” web. Create two plate properties and assign using the Selector. • Mesh size (1”) and Mesh using the Selector. • Assign Load (pressure load of 50 psi) and simply constrain on ends with pinned constraint. constraint • Run and post process looking at element stresses top and bottom. • Cover von Mises, Major and Minor Prin stress components.

Start: Plate Modeling / No Geometry – you get to build your own Movie File: Plate Modeling and a Bit More Part I.avi / …..Part II.avi

42

General All Purpose Elements: Isoparametric Elements

Re evised 2010

Why do we care about this stuff? • Shape functions are simple polynomials. • The area or volume of the element is approximated. pp • Stresses are computed at Gauss points not at nodal points. • Highly distorted elements - lead to poor Gaussian integration. “Rocks in your Jello” • The whole process uses quite a few “approximations”. • Displacement p results will always y be more accurate than stresses. • That is, stresses, reaction forces, etc. are derived.

A knowledgeable user makes better assumptions.

43

Isoparametric Elements: Convergence

12 48

Re evised 2010

FL3 v2 = 3EI

bh 3 I= = 1 • 12 2 = 144 12 1 • 483 FL3 = v2 = = 2 .56 3EI 3 • 100 • 144

44

Isoparametric Elements: Convergence

3

Tip Displacementt

Exact 4 elements 2 elements 1 element

Quad

2.5

2

1.5

1

Re evised 2010

0.5

0

0

5

10

15

20

25

30

Beam Length, x

35

40

45

50

45

Isoparametric Elements: Convergence

Quadrilaterals don’t like to be skewed. 2

4

1.

6

8

General rules: Aspect < 10 to 1 Skew < 30o Taper < 30o

10

123

1

1

3

5

2

3

4

7

“Avoid Diamonds”

9

123

3

Y

Z

X

Re evised 2010

Skewed elements are “stiff” and give dangerous results. That is, you can under predict the stresses by large margins. This is the downside to Isoparametric elements.

Tip Displacement

2.5

2

1.5

1

0.5

0

0

5

10

15

20

25

30

Beam Length Length, x

35

40

45

50

46

Isoparametric Elements: Convergence

Topics Covered:

Re evised 2010

• Femap provides mesh quality diagnostics within the Tools menu under Tools / Check / Distortion. One can also use the Custom Tools menu to create a contour map of these items (see Custom Tools / Model Query / Distortion to Output Vector). The plot on the upper left was created with this custom tool. • Even though we may have quad elements with a high Jacobian, they still outperform three-node triangular elements. • See Bonus.mod for the six-node triangular mesh example.

Jacobian / Open model files and investigate. No AVI file

47

Isoparametric Elements: Convergence

The P-element or polynomial escalation

Re evised 2010

*The whole trick is that the shape p ffunction is now parabolic - it can handle a parabolic distribution of displacement ffrom one node to the next.

1 1 1 N 2 = (1 + ξ )(1 − η ) − (1 − ξ 2 )(1 − η ) − (1 + ξ )(1 − η2 ) 4 4 4 1 N 6 = (1 + ξ )(1 − η2 ) 2

48

Isoparametric Elements: Convergence

The P-element or polynomial escalation

12 48 3

Tip Displacement

2.5

Q d8 Quad8

2

1.5

1

Re evised 2010

0.5

0

0

5

10

15

20

25

30

Beam Length, x

35

40

45

50

49

Isoparametric Elements: Convergence

Why we don’t like triangular elements....

12 48 3

Tri

Tip Displacement

2.5

2

parabolic

1.5

1

Re evised 2010

0.5

0

linear 0

5

10

15

20

25

30

Beam Length, x

35

40

45

50

50

Isoparametric Elements: Convergence Pre Processing Workflow: Pre-Processing • Geometry preparation is done • Create Material and Property • Set Mesh sizing g and then Mesh Geometry y • Apply Loads and Constraints • Define Analysis Manager • Run

P tP Post-Processing i Workflow: W kfl

Re evised 2010

•View Select (F5) - Contour • View Options (F6) • Interrogation of model with Selector Tool. • Refine Mesh / Rerun

Plate-Hole / Plate-Hole-Start.mod

51

Mesh Convergence - Only one part of obtaining an accurate FE solution

Re evised 2010

h-refinement versus p-refinement. • Simple tests can verify mesh convergence (comparing th stress the t att the th centroid t id versus the th nodal d l locations). l ti ) • Mesh convergence is just minimizing the JUMPS from element-to-element; nothing more - nothing less.

“Mistakes in loads, support conditions, and so on will propagate through adaptive cycles and produce an improved solution to the wrong problem. Also, poor choices of element types or an initial mesh that is too coarse may not disclose enough detail to permit the revised mesh to be an improvement Automatic improvement. adaptivity seems to guarantee that final results will be adequate, but of course there can be no such guarantee. guarantee.” From R.D. Cook - FEM for Stress Analysts, p.143 (1995).

Knowing when to say when?

52

Pre-Processing Workflow: • Geometry preparation: slice off extra geometry and refining g the “load patch”. p • Create Material and Property • Define Load (40 lbf) and Constraint (Fixed) • Set up Analysis Manager (Iterative Solver)

Post-Processing Workflow:

Re evised 2010

• View Select (F5) • View Options (F6) • Using View Options and saving View Options within the Window environment • Post-Processing tricks • Using the selector to interrogate the model between nodal and elemental stresses (extra) • Remesh of Model for tighter convergence

Import Geometry File: Solid-Anvil / Solid-Anvil.x_t There are a few avi files….start with –Pre file

53

Hardest are Beams

Beams are line elements that represent geometry (mechanical structure) t t ) that th t has h a uniform if cross-section ti and d iis llong ((e.g., it its length is 10 times longer than its height or width). Beams are exact - no approximations are used. Lateral contraction or expansion (Poisson’s effect) is not accounted for - but for linear, linear elastic, elastic static analysis work it is an extremely minor effect in beam structures. Beams offer you the maximum design optimization opportunity!

Re evised 2010

Somewhat easier are Plates

If an engineering structure looks like a collection of surfaces from a distance - say a car body or a vessel (tank) or submarine or airplane skin - then it is a good candidate to be modeled with plate elements. Plate thickness is an easily changed variable. Sizing optimization can be performed extremely quickly. Good results for plate like structures but assumptions are still used. used Poisson’s effect is accounted for.

54

Re evised 2010

Easiest are Solids

Solids make the fewest geometric approximations but make the most numerical approximations. It takes a lot of solid elements to give good results. This means that “solids” analysis work can be time consuming and slow. This leaves you with fewer chances to pursue design optimization strategies.

55

Units in FEA

Re evised 2010

Lbf = (in3)*(lbf*s2/in4)*(in/s2) For a dynamic analysis, how would we check the structure? (Hint: if in English units the mass of the structure x 386 should be the weight (Tools / Mass Properties)).

56

Units in FEA

Re evised 2010

Conversions for exotic units based on generic steel lb f/in lb f/mm N/mm Geometry in mm mm Elastic Modulus 30 •10 6 lb f/in 2 4.65 • 10 4 lb f/mm 2 206.8 • 10 3 N/mm 2 gravity 386 in/sec 2 9810 mm/sec 2 9810 mm/sec 2 Mass Density 7.324 • 10 -4 1.76 • 10 -9 7.827 • 10 -9 lb • sec 2 /in 4 lb f• sec 2 /mm 4 N • sec 2 /mm 4 Output Displacements in mm mm Stresses lb f/in 2 lb f/mm 2 N/mm 2 (MPa)

N/in in 1.334 • 10 8 N/in 2 386 in/sec 2 3.258 • 10 -3 N • sec 2 /in 4 in N/in 2

57

Loads and Constraints Loads: • Loads within an analysis deck get boiled down to the node and element level – there is no geometry in an analysis deck. • In the pre pre-processor processor (a.k.a., Femap), you can apply loads to geometry or directly to nodes and elements. However, at the end of the day – everything goes to the nodes and elements in the analysis deck.

Constraints:

Re evised 2010

• Application of constraints follows the same pattern – you can apply them to geometry or directly to the underlying nodes. (Note: constraints always go to nodes – see prior discussion on FEA Theory). • Whether you go the Geometric route or via Direct nodes – it is y your decision and whatever you feel most comfortable with.

The most important concept is that you p y what y you are understand completely doing……

58

Surface Modeling Pre-Processing Workflow: • Geometry preparation: mid-surface solid

(thickness is 0.118”). • Create Material (steel) and Property (plate element) • Mesh sizing and meshing of surfaces. • Create Motor Mass (10 lbf) and attach to motor mount with rigid links • Create constraints around base. • Set up Eigenvalue analysis (natural frequency).

Re evised 2010

Post-Processing Workflow: • View Select (F5) • View Options (F6) • Delete Results and Resize plate model to 0.1875” (not covered in AVI – but I think you guys know what to do). do) • Rerun analysis and compare results. • Perform Static Stress Analysis using Body Acceleration Load of 10 g. • Interrogate plate element stress results (top and bottom).

I Import tG Geo: S Surface f M Modeling d li / Part P t I / Motor M t Mount M t w Motor.STP M t STP Movie File: Surface Modeling / Part I / Surface Modeling-Pre Classic.avi Movie File: Surface Modeling / Part I / Surface Modeling-Pre Selector.avi Movie File: Surface Modeling / Part I / Surface Modeling-Post.avi

59

Surface Modeling Pre-Processing Pre Processing Workflow: • Geometry preparation from 3-D solid into

Surface Model for Plate Meshing: using “hidden” Femap tools to measure distances (CTRL-D) while within another dialog box, box Midsurface tools (Extend), Geometry / Solid / Stitch, Intersect, Curve from Surface (slice). Another command discussed is changing the pick mode from Normal to Front while “picking”: • Create Material and Property ((two plate sizes)) • Apply Mesh sizing and Mesh Geometry • Apply Loads and Constraints • Set up Analysis Manager and Run

Re evised 2010

P t P Post-Processing i Workflow: W kfl • View Select (F5) • View Options (F6) • Using View Options and saving View Options within the Window environment • Post-Processing tricks • Optimization of plate models by changing the gusset thickness

Import Geo: Surface Modeling / Part II / Surface-Midplane Modeling.X_T Movie File: Surface Modeling / Part II / Surface-Midplane Modeling-Pre.avi

60

Surface Modeling Workshop flow:

Re evised 2010

• Import model, find symmetry and slice down

center. • The model has three components with thicknesses of 0.125, 0.185 and 0.250”. • Create mid-surface geometry using the target thickness of the thickest component. Stitch geometry together into three infitisimally thin solids. • Prepare geometry for clean meshing. Offset curves around dimples by 0.25, imprint several curves and then create washes around the holes with a distance of 0.10”. • Work through trial meshes. Final mesh size will be 0.25”. Use Meshing Toolbox to tweak mesh into something nice. Use Mesh Add and Mesh Set. • Glued connections via Automatic • Create load: 1,000, 1,000 and 1,000. • Apply constraint and run. run • Postprocessing with plate stresses on top and bottom.

Import Geometry: Surface Modeling / Part III / SUPPORT STRUCTURE FRAME.X_T Movie File: Surface Modeling / Part III / Support Structure Frame Workshop.avi

61

Surface Modeling Pre-Processing Workflow: • Import model and create group of the yellow

Re evised 2010

geometry part. Work with groups and Automatic Add Add. • Explore Custom Tools / GeometryProcessing / Find Tangent Surfaces. Use CTRL-D to measure offset (-0.09/2). • Understand Geometry / Solid / Stitch (Femap surfaces are infinitesimally thin solids. • Mesh Surfaces using the selector. Play with surface meshing options to obtain improved mesh.

Import Model: Surface Modeling / Part IV / Bus Seat Start.mod Movie File: Surface Modeling / Part IV / Industrial Mid-Planning.avi

62

Engineering Assessment of Loads

First Law: A body will remain at rest or will continue its straight line motion if left alone. Second Law: F=ma Third Law: Action and Re-action (or conservation of forces) - this is the critical law for piece-parting assemblies.

Re evised 2010

Simple stuff is quite useful: You

can check your actual FEA applied loads via the f06 file within the analysis manager after the analysis has been completed. The OLOAD is the applied load and the SPCFORCE is the reaction load after the analysis. These should tie….Third Law.

63

Engineering Assessment of Loads The giant slab of steel.

• Gravity? • Straight forces? • Pressures? • Interaction loads which might be a combination of forces and moments? • Dynamic / Impact?

0.998 0.893 0.788 0.683 0.578 0.473

• Nonlinear -- e.g., Follower Forces / Stress Stiffening

0.368 0.263 0.158 0.0525 -0.0525 -0.158 -0.263 -0.368 -0.473

• Frictional forces?

-0.578 -0.683 -0.788 -0.893 -0.998 6.25

12.5

18.75

25.

31.25

37.5

Re evised 2010

0.

Think worst case..

43.75

50.

56.25

62.5

68.75

75. Sin

64

Engineering Assessment of Loads

• Pressurized structures are pretty common. The trick to their loading is not the structure must be balanced. It can’t move off into space space.

Re evised 2010

• Sum of Forces is important to check your loading loading.

Counter forces were applied at the flanges to balance the system.

65

Engineering Assessment of Loads

V1 L1 C1 380.24 286.38

28.419 34.458 356.12

589.09 512.8

• Free body diagrams are still useful after all these years. years • Yes - we could do it all as an assembly. However, this part went through five revisions. revisions

Re evised 2010

• The FBD was invaluable.

198. 288.

140.74 Z

34.458 Y X

66

Constraints Symmetry - you gotta love it to be a good modeler. • Geometric Symmetry - mirror planes in model. • Loading Symmetry - loading is identical across or between mirror planes.

ux= 0 Y X

Re evised 2010

uy= 0

67

Constraints Beams’ and Plates’ nodes have six degrees-of-freedom. Consequently, six constraint DOF can be applied (e.g., TX, TY, TZ, RX, RY, and RZ).

Solid elements’ nodes have three degrees-of-freedom. Consequently, three constraint DOF can be applied (e.g., TX, TY, and TZ).

V1 L1 C1 1.7321 123

Re evised 2010

123

Z 123 Y Output X Set: MSC/NASTRAN Case 1 Contour: Solid Von Mises Stress

• What do you think happens when you pp y a RX or RY or RZ constraint to a solid apply element node? • What do all FEA models have in common in regard to “rigid body motion”?

68

Constraints Simple rules of symmetry • Visualize motion • Sketch it out on paper

45

Re evised 2010

Cyclic symmetry will occur in many rotating structures. This type of symmetry is also known as sectorial symmetry or rotational periodicity.

69

Constraints

• Don’t be reluctant to exploit symmetry Fast models allows you symmetry. to check, check, and check your results. • The key questions: - Is the structure symmetric? - Are the loads symmetric?

Re evised 2010

• Avoid over constraining your models. This can actually hide your hot spots. spots If in doubt - bound your solutions with different boundary conditions. This is no big deal if you model runs fast.

70

Constraints Pre-Processing Workflow: • Geometry preparation: Symmetry and Surface

Preparation: Hidden Ctrl-Z command to bring up the Locate dialog box to assist in locating the Geometry / Solid / Slice plane • Auto meshing with control of mesh sizing from Solid to Surface to Curve • Application of pressure load as a pin force. Use of pressure load and then to the use of Modify / Update Other / Scale Load to get the final 5,000 lbf load. • Constraints to enforce symmetry with respect to the 6 DOF for every structure. Use of Geometry Based versed Nodal Based – same but different. • Analysis Manager / Run.

Re evised 2010

Post-Processing Workflow: • View Vi Select S l t (F5) • View Options (F6) • Using View Options and saving View Options within the Window environment • Modeling Bearing/Pin Forces - Does it look right. • Discussion of modeling results. results Import Geo: Constraints / MESSIER-DOWTY-LINK-CONSTRAINTS.X_T Movie File: Constraints / M-D-Link-Constraints - Pre.avi and then –Post.avi

71

Constraints Pre-Processing Workflow: • Import geometry file and inspect. Model is symmetric. • Prepare geometry (Geo / Curve from Surface with U d t Surface Update S f On) O ) for f the th line li contact t t constraint. t i t • Elegant constraint modeling is done by defining “user coordinate systems” – see Model / Coord Sys / Define Coordinate System. • Apply pin bearing constraint via user defined cylindrical coord system at the center of the hook’s pin bearing. • Apply “line contact” constraint where the hook contacts the bushing. • Apply 13,000 hook load. • Set up Analysis Manager – enable Iterative Solver.

Re evised 2010

Post-Processing Workflow: • Contour the Max. Prin Stress to verify behavior of the hook model.

Import Geo: Constraints / Raw Constraints / HOOK MODEL - SYMMETRIC.X_T Movie File: Constraints / Raw Constraints / Raw Constraints Tutorial.avi

72

Assembly Modeling

Re evised 2010

Sway bar modeled with 10-node tetrahedrals.

This model required the attachment of a solid tetrahedral model (the sway bar) with bolts to a suspension frame made out of plate elements.

73

Assembly Modeling

Re evised 2010

A spider’s web of RBE3’s

SDOF elements

The bolts (beam elements) were attached to the frame (plate elements) with MPC elements (RBE3’s). The same strategy was used to attach the solid elements onto the bolts. Single degree-of-freedom springs (CBUSH elements) were used to simulate a flexible rubber bushing between the suspension components.

74

Assembly Modeling

Comments: Tying structures together can be quite •Tying easy with a little idealization. •This exercise covers the use of RBE2 (super-stiff links that transmit rigidity and spatial relationships) and RBE3 (links that transmit force (no rigidity) and spatial relationships).

Re evised 2010

Tasks: •Use template model to apply the various connection technologies and evaluate the results.

Open Model File: Assembly Modeling / Connections / Connection-Start.mod

Assembly Modeling

Surface-to-Surface Contact NX Nastran Linear Contact for Sol 101:

Re evised 2010

• It is almost necessary to read the manual…. (NX Nastran User’ss Guide / Chapter 19) User 19). • The NX Nastran linear contact has a legacy directly from SDRC-Ideas. It is a well-proven technology and they are still improving it. • Be careful of the defaults for Min and Max Contact Search Dist. Actual contact elements are created within the solver based on the regions that you create in Femap and then the distances specified in these entries. One can create virtual contact elements where one least suspects it…. • Num Allow Contact Changes default of 0.0 is often too rigorous One suggestion from an experienced user is that it rigorous. should be 1% of the number of contact elements formed within the solver (see your F06 file – it’ll be listed in the first contact iteration dialog) • Setting up contact regions can be done automatically but it may be more effective in the long run to carefully select your contact regions via the Connection Region dialog boxes. • The last dialog box to make contact. Think of the total process as 1.) Connection Property; 2.) Region and 3.) Connector.

75

Assembly Modeling

76

Surface-to-Surface Contact Pre-Processing Workflow: • We are ready to create our contact behavior between the four parts. Create contact and glued property cards within the tree. Be careful. Default Contact Search is 0.1 and for Glued Contact it is 0.0001. • Follow avi and create connection regions using surfaces and then create the connectors. • Run Analysis and view F06 file while running.

Re evised 2010

Analysis Workflow: • View Select (F5) and Review Results • Interrogate the results and see if the contact behavior is reasonable. Contour contact pressure. • Use the defaults for the Contact Property Card. Review the results. • Reset Max Contact Search Dist to 0.1 and set Glued Contact to defaults. Rerun and review the results. Open Model File: Assembly Modeling / Intro to Contact / Cutting the Mustard Start.MOD Movie File: Assembly Modeling / Intro to Contact / Intro to Contact.avi

Assembly Modeling

77

Surface-to-Surface Contact Pre-Processing Workflow: • Model has been created with bolts created (beam elements and rigid links) • Create rigid link spider at the end of the cylinder using the Femap API (see Custom Tools). Apply FX=-2500 and MY=2500 to the center node of the rigid link spider. • Create constraint on base of model at the inside of the four holes (use Selector / Surface / multiple). • Run Analysis

Re evised 2010

Analysis and Optimization Workflow: • View Select (F5) and Review Results • Create contact surface between cylinder and base (Geometry / Automatic / Contact) • Rerun Analysis • Create Bolt Preload (10,000 - elements) • Rerun Analysis Note: The model Advanced Assembly Modeling y runs completed. p Final.mod has all the analysis Assembly Modeling / Adv Assembly / Advanced Assembly Modeling Start.MOD Assembly Modeling / Adv Assembly / Advanced Assembly Modeling Pre.avi Assembly Modeling / Adv Assembly / Advanced Assembly Modeling Surface Contact.avi Assembly Modeling / Adv Assembly / Advanced Assembly Modeling Bolt Preload.avi

Assembly Modeling Glued Contact Between Solid Elements Pre-Processing Workflow: • Geometry has been prepared for meshing. • Tet mesh the top with a mesh sizing = 0.2 for the Hex mesh on the bottom pick min. number of elements = 4. • Create glued contact (Geometry / Automatic) • Apply loads via Selector (FY = 1000 lbf per surface) • Create constrains around base • Run Analysis

Analysis and Optimization Workflow:

Re evised 2010

• View Select (F5) and Review Results • Interrogate the results and see if the stress transfer across the glue connection appears reasonable

Open Model File: Assembly Modeling / Hex to Tet Glued Contact / Hex to Tet Glued Contact Fitting Start.MOD Movie File: Assembly Modeling / Hex to Tet Glued Contact / Glued Contact Example.avi

78

Assembly Modeling Glued Contact between Plate Elements Pre-Processing Workflow: • A detailed description is given on how Glued Contact

Re evised 2010

works. • Individual regions are created for each plate element property. • An Eigenvalue analysis is done to show how the Glued Contact Works.

Open Model File: Assembly Modeling / Plate Element Glued Contact / Plate Element GC Start.MOD Movie File: Assembly Modeling / Plate Element Glued Contact / Plate to Plate Glued Contact.avi

79

Assembly Modeling

80

Surface-to-Surface Contact Plate Elements Comments: •This model is already to go - with only the contact definition remaining to be defined. •The theme of this exercise is that plate elements have normals -- that they have directions (outward or inward). These normals can be viewed within the Model Info tree via the Highlight Button. •We also explore debugging the model. Workflow: •Define Contact behavior between the tubes using the tree structure. •Run the analysis after defining the C Connection. ti •Analysis fails - check plate element normals and correct via Modify / Update Elements / Reverse.

Re evised 2010

•Rerun Rerun analysis and post process results. results

Open Model File: Assembly Modeling / Square Tube Contact / Square Tube Contact.MOD Assembly Modeling / Square Tube Contact / Linear Contact - Rectangular Tube.avi

Mastering Femap

81

Grand Slam of WorkShops: Comments: • This is the grand daddy of models. We will use most everything taught in this course and a few new things. • Using Beam Elements for Bolts • Rigid Links • Bolt Preload • Sinusoidal Bearing Load • Scaling loads. Workflow: ) • Create curves for bolts ((beam elements). • Create beam elements (1.5” diameter) and mesh curves. • Mesh Solids sizing on solids is at 1.25.

Re evised 2010

• Create group with just geometry and beam elements to apply rigid links. • Create Bolt Preload 100,000 lbf. • Create Surface-to-Surface contact and then run the analysis. • So much more……………. Master Exercise / WINCH DRUM SUPPORT.X_T Mastering Femap Part I.avi / …Part II .ave/ ….Part III.avi / ……Part IV.avi

82

Two types of stress results are commonly used to provide insight into the behavior of the structure: • von Mises stress • maximum principal stress von Mises criterion - states that yielding of an isotropic p material will begin g when the von Mises stress reaches a limiting value regardless of whether it is compressive or tensile (e.g., yield stress or ultimate stress of the material).

The maximum principal stress criterion states that fracture will occur when the maximum principal stress reaches a limiting value in tension.

⎡(σ − σ ) + (σ − σ ) + (σ − σ )2 ⎤ y y z z x 1 ⎢ x ⎥ = ⎥ 2 ⎢+ 6 τ 2 + τ 2 + τ 2 xy yz zx ⎦ ⎣ 2

Re evised 2010

σ vonMises

(

2

)

1

2

83

Under pure uniaxial tension;

σ vonMises

[

1 2 2 = (σ x ) + ( − σ x ) 2

]

1

2

σ vonMises = σ x

Re evised 2010

*The biggest *Th bi st thing thin to t note n t about b ut the th vonn Mises stress is that it is neither positive or negative!

=

84

Principal stresses: why is the maximum principal stress mostly positive?

σ max,min =

σx

Re evised 2010

τ xy

σy

⎡σ x − σ ⎢ DET ⎢ τ xy ⎣⎢ τ zx

σ max

τ xy σy − σ τ yz

σ min

τ zx ⎤ ⎥ τ yz ⎥ = 0 σ z − σ ⎦⎥

σx − σy 2

⎛ σx − σy ⎞ 2 ± ⎜ ⎟ + τ xy 2 ⎠ ⎝

2τxy 1 −1 θprincipal= Tan 2 σx − σy In 3D the math gets a little bit hairier and requires the use of determinants. determinants The roots of the final equation are the three principal stresses.

85

Predicting failure is highly individualistic

SEndurance σa

Re evised 2010

S Endurance

+

σa S Endurance

σm S Ultimate

+

=

1 Factor − of − Safety

1 σm = S Yield Factor − of − Safety

Your load cycle was a half-sine wave?

86

Comments: • Stress results exist for the model which contains solid, plate and beam elements. • The goal of this exercise is to contour stress results over the solid solid, plate and beam elements elements. • Explore definitions of von Mises, max prin stress, majorprn, etc.

Things to do: • Play with the View Select (F5 or tool bar pick) and understand the concept of centroidal versus nodal stresses. • Contour C t TType iis about b t simple i l versus intelligent stress contouring.

Re evised 2010

• Data Conversion is how the nodal or centroidal stresses are averaged. Corner data = Nodal Data • Element Contour Discontinuities is used for plate elements and corrects for idealization problems with plate elements.

Load Model File: Post Processing / Comparison of Element Types Under Simple Bending.MOD Movie File: Post Processing / Post-Processing Stress Scalers.avi

87

y options p g • Default analysis gives y you

applied loads and reaction loads (forces/moments at constraints) within the model.

Re evised 2010

• Internal forces require q Analysis y / Advanced options (see next slide). • Free-body diagrams help you check your work at a glance.

Free-Body-Diagram / Free-Body-Diagram Beam Elements.mod

Re evised 2010

88

With this lash-up - you see all the internal forces acting g at each node this is most useful when you are trying to debug interfaces or strange connections.

Free-Body-Diagram /Free-Body-Diagram Beam Elements.mod

89

Re evised 2010

•Another useful thing about the FBD option is the ability to check your RBE2, RBE3 connections (Multi Point Reaction (Multi-Point Loads).

Free-Body-Diagram / Free-Body-Diagram with RBE3.mod

90

Advanced Femap Modeling Topics: Mesh Repair Comments: • Our goal is be able to get any type of solid to mesh! It is possible! This interface has the tools to allow you to mesh anything. The trick is to recognize the steps and to figure out where the meshing process is failing. • In this exercise - we hand fix a mesh and then mesh the resulting surface mesh.

Solid meshing is all surfaces, surfaces, surfaces. Tasks:

Solid Mesher Steps:

•With the above solid, solid mesh it using the default sizing, uncheck Suppress Short Edges.

1 Meshes surfaces 1.

•Read Meshing Messages and then find the hole in the surface via View Select / Free Edge.

3. Grows surface mesh into a solid tet mesh.

Re evised 2010

problem,, fix-it,, and then create a solid mesh •Find p from the sealed skin.

2. Seals surfaces into continuous shell.

Fixing: 1. Bad surfaces - won’t mesh. 2. Create sealed surface. 3. Play and learn. No easy way.

Adv Femap Topics / Meshing / DETROIT STOKER LINK MESH EXAMPLE.X_T / Mesh Repair.avi

Advanced Femap Modeling Topics: Hex Meshing Comments: • Hex meshing is ideal for easy solids since one brick is equivalent to five tetrahedrals (8 nodes versus six 10-node tetrahedrals (27 nodes)

Re evised 2010

• The concept is to break the solid down into eight-sided meshable solids. Think of slicing and embedding faces.

Import Geometry File: Adv Femap Topics / Hex Meshing / Hex Mesh Geometry.x_t Movie File: Adv Femap Topics/ Hex Meshing/ Hex Meshing Geometry.avi

91

92

Advanced Femap Modeling Topics: Surfaces as Infitisimally thin solids Introduction: Before the age of modern CAD, we had simple surfacing techniques (a.k.a., dumb surfaces). These simple surfaces could not be manipulated downstream once they were created. Nowadays, the only legacy simple surface th t one can create that t is i the th “boundary “b d surface f from f curves”. ”

Re evised 2010

Femap now uses the parasolid geometric kernal to creates geometric surfaces and solids. Manipulation of geometric solids within Femap is native to most CAD users and needs little explanation. explanation The converse is true when one induces the concept of surface modeling within Femap and thinking about surfaces as “infitisimally thin solids”. In Femap, surfaces are treated as very thin solids -- like infitisimally thin solids. solids What you can do with geometric (parasolid) solids you can also do with surfaces. My favorite trick is to create manifold skins from disparate but contiguous individual surfaces. This trick is under Geometry / Solid / Stitch. Once you have this stiched up skin, you can then treat it as a collection of surfaces within one infitisimally thin solid. A little tutorial is provided showing these featues. Work Flow: Run tutorial and then try to create the work flow pattern at your own pace. Adv Femap Topics / Surface_Concepts / New Model - Nothing to load / Surface_Concepts.avi

93

Advanced Femap Modeling Topics: Surfaces as Infitisimally thin solids Comments: • This sections expands upon working with smart surfaces (parasolid based infitisimally thin solids) within Femap. • Many commands from the Geometry / Solid menu can be used within Femap. For example, one can fillet surfaces and remove faces much as you do for solids (likewise you can also remove holes in surfaces). • We also explore mapping a perfect quad mesh onto a not-so-perfect warped geometry via Boundary Surface / Surface on Solids to create one “surface” and then using Mesh / Mesh Control / Approach on Surface.

Surface_Manipulation.avi

Work Flow Tips:

Re evised 2010

• Open model file and set the mesh sizing via Mesh / Mesh Control / Size on Surface. Mesh the surfaces and note the quality of the elements. • Create boundary surface using the underlying surfaces. Repeat the steps above. • Create mapped surface via Mesh / Mesh C t l / Approach Control A h on Surface. S f Repeat. R t Adv Femap Topics / Surface_as_Solid / Cargo Net_Start.mod / Surface_as_Solid.avi

Advanced Analysis Topics

94

F Force = Mass M ∗ Radius R di ∗ ω2 • Rotation motion, although might be consider dynamic is actually a static body load.

Re evised 2010

• The same might be said about gravity. gravity Gravity is actually enforced as an acceleration. A force is generated based on F = m*a.

Advanced Analysis Topics

m

∂ 2u ∂t 2

+c

∂u + ku = r ( t ) ∂t

• Linear dynamic systems are

wonderfully well behaved and can be simulated extremely accurately. • As in all modeling, start simple with a linear, elastic solution, then progress to a modal solution, and then kick in the full transient.

Re evised 2010

• Geometric and material nonlinearities can be included but they should be added after you have a good dynamic run. Generate a history of results and you’ll convince yourself and others that what you are seeing is real and not a modeling “gasim”.

95

Advanced Analysis Topics

96

Eigenvalue problem: undamped free vibration

∂ 2u m 2 + ku = 0 ∂t Assuming a solution of the form:

u = u o sin ω t

Then:

[k − ω m ]{u 2

o

}=0

Re evised 2010

For non-trivial solutions (i.e., solutions that are more than just zeros):

[

]

k − ω 2m = 0

giving us the well know frequency relationship:

k ω= m

Advanced Analysis Topics

97

Normal Modes / Eigenvalue problem: undamped free vibration

k

Re evised 2010

ω=

k 23,000 = = 15.16rad sec m 100

NX Nastran reports frequencies in cycles per second. Hence, 15.16 radians/sec is equal to 2.41 cycles/sec.

llet: t Kvertical=1000/0.0435 m=100

Advanced Analysis Topics

98

Comments: • Analysis Manager • Vibration - Normal Modes • Optimization Tasks: • Model has already been constructed create new analysis set (Model / Analysis / New). Set model up for Normal Modes run and only analyze the first three modes. For output you’ll only need displacements. • Analyze and animate the mode shape. Play with the animation settings (View Options / Category - Post-Processing).

Re evised 2010

•Optimize Optimize structure by increasing the Cross Rod diameter from 2.54 to 25.4 mm. • Analyze again...

Open Model File: Vibration / Coors Tek Forming Board.mod

Advanced Analysis Topics

∂ 2u ∂u m 2 +c + ku = r ( t ) • sin( ω • t ) ∂t ∂t • Details, D t il d details, t il

details, details will kill you. • Data management is a big issue when doing dynamics. Small models will make or break you.

Re evised 2010

• Simple but effective dynamic models are created by dedicated, brutal modelers that are willing to make and take big assumptions th t are valid. that lid

99

Advanced Analysis Topics

Re evised 2010

• Stress S

100

NX Nastran Error Messages

Unsuccessful Analysis (from the Femap V9.3 help section) There may be times when your analysis is unsuccessful. NX Nastran for FEMAP will indicate an error in the solver in the Message Review Dialog Box. By pressing "Show Details" you can review the individual messages from the NASTRAN printed output file file. While reviewing each detailed message, you can press the Help button and jump into this help file directly to the appropriate message and review any additional information that may be available. Common causes of analysis errors include: Not merging coincident nodes. Coincident nodes are multiple nodes that share the same coordinates. While coincident nodes may be desired due to the type of model being made, they improperly occur when nodes and elements are generated around an enclosed surface. It is a good idea to do a coincident node and element check prior to performing the analysis.

Re evised 2010

Not having mass in the model. Normal modes analysis requires that the structure contain mass. Similarly, when performing static analysis with a gravity load the structures mass is required, or else the applied loads will be zero. It is a good idea to always make sure that mass density has been entered for the properties. Nott constraining N t i i the th model d l properly. l Static St ti analysis l i requires i that th t th the model d l be b constrained t i d against rigid-body motion (translation and rotation). Note that many textbook type problems show an incomplete set of constraints because they are working in 2D as opposed to 3D. NX Nastran for FEMAP assumes 3D, and you must properly constrain your model.

101

NX Nastran Error Messages

Solver Error/Warning Messages: There may be times when the analysis fails, and gives you messages in the Message Review window. Most often analysis failure happens when NX Nastran finds an error. Errors can vary from problems in the input data definition to problems with your operating system and there are many possible error messages. Some of the more common error messages that you might encounter are listed below: MESSAGE 3060,, SUBROUTINE MODEL Ð OPTION NAST NOT IN APPROVED LIST. This error message indicates a problem with NX Nastran security on your system. You have either a bad security device or an invalid authorization key. Check the device and/or request another EDS PLM Solutions authorization key. Be sure to enter the correct EDS PLM Solutions ID and Model Number in the EDS PLM Solutions Authorization Key Request form.

MESSAGE 9050 (SEKRRS) - RUN TERMINATED DUE TO EXCESSIVE PIVOT RATIOS This error happens when the model has not been restrained properly. In linear static analysis, you must restrain the body sufficiently to prevent rigid b d motion. body ti Ch k the Check th applied li d constraints t i t and d correctt them. th USER FATAL MESSAGE 4276 Error Code xxx. This error also indicates insufficient resources during the simulation process. Try to increase the virtual memory setting on your computer. Refer to the Installation and Operations Guide for the recommended swap space settings.

USER FATAL MESSAGE 5271. The ratio of the longest edge to the shortest altitude exceeds 100. This error shows Thi h th thatt the th quality lit off one or more elements l t iin th the simulation i l ti model d l iis unacceptable t bl tto th the NX N Nastran.Nastran t N t solver. l T re-meshing Try hi th the model with a different average element size.

USER FATAL MESSAGE 316 - Illegal data on Bulk Data Card XXXX This will occur whenever you have "bad" data in your model definition. One common example is the incorrect definition of material or property data, such as defining a Young's Modulus of 0.0.

Re evised 2010

USER WARNING MESSAGE 2148 - SPCD on a Point not in the S-set This will occur when you are using Displacement loads that are not accompanied by a nodal constraint. The nodes which have displacement loads must have a constraint on the same Degrees of Freedom as the displacement load, otherwise the displacement loads are skipped. Warning Message 4420 - The following degrees of freedom are potentially singular If you get this message, you will not get any results, even though it may not be accompanied by any FATAL messages. This message could occur because your model is underconstrain, or you may have rigid body motion in your model.

102

Advanced Analysis Topics MESSAGE 9050 (SEKRRS) - RUN TERMINATED DUE TO EXCESSIVE PIVOT RATIOS

• This is one trick - Solve model for first six modes (an eigenvalue solution). solution)

∂ u m 2 + ku = 0 ∂t 2

Eigenvalue solutions don’t require loads or constraints.

• This is one of the most powerful

Re evised 2010

model debugging tools that I know to figure out where parts of your y g off into space. p model are flying • You can also force your model to solution by setting the PARAM,BAILOUT,-1 in the Nastran bulk data deck (see Analysis Manager Bulk Data Options / Start Text

103

104

Re evised 2010

• How accurate are the loads? Model to the accuracy of the loads.

• Verify the FEA applied load against the calculated load. • Is the pull of gravity important? y dimensions of y your structure. Do they y make sense? • Check a few key • Plate models have top and bottom surfaces. When you apply pressure loads on plate elements verify that the load direction is in the “right” direction. • Play y with y your constraints. An overconstrained model will under report the true stress state. • Convergence checking is as simple as comparing the centroidal stress against the adjacent nodal stress. If they are within 30% you can be assured of g good convergence. g An even simpler p check is to look at the element shapes and the contour gradations, if they look good then the stress results will most likely be good. These convergence checks are superior to a software based solution. • Can’t g get the model to run without negative g pivot p ratio’s? Run the model as a Normal modes / Eigenvalue job and animate the near zero frequencies. The near zero frequencies are rigid body motions! Another technique is to insert the PARAM,BAILOUT,-1 into the Nastran Bulk Data Options p as a Manual Control / Start Text / then p place the above param control card.

105

• Remember - loads, forces, gravity, etc, are not used in an Eigenvalue

Re evised 2010

analysis. • The first three modes or Eigenvalues represent the dominant vibrational response of your structure. Their corresponding mode shapes indicate how the structure will vibrate but give you no idea of the magnitude of the vibration. • The mass of the FEA model should be close (say within 5%) of the structure that you are modeling. If you are working in U.S. units remember to multiple the mass of the FEA model by 386 to obtain its corresponding weight. • Eigenvalue analysis can be quite handy in debugging linear linear, elastic elastic, static models that are not fully constrained.

106

• Follow all the steps for an Eigenvalue analysis FIRST. I know this sounds

Re evised 2010

a little redundant but it will save tons of time in the long run. • You will need two functions for a Modal Frequency Analysis (MFA): 1) A function for the driving force (scaler versus Hz) and a function that defines the solutions that you are interested in obtaining information about. • See examples in tutorial book and run then before proceeding with your first MFA. • In a MFA, you are obtaining X0 where X = X0*sin(ωt-φ). To see the full field solution you need to expand your solution using the absolute magnitude (X0) at a particular frequency (ω) and phase angle (φ). (φ) This holds true for all displacement, stresses, etc. • Extremely accurate form of dynamic analysis since it is basically a form of a linear, elastic, static solution. • Damping dominantly affects only the magnitude of the response and not its frequency.