Tutorial 9 1/6

ANSYS - Structural Analysis/FEA

Nonlinear Analysis

Problem: Consider a rectangular plate 6 m × 4 m × 20 mm subject to pressure on an area (1

m × 2.5 m) in the middle of the plate.The plates and stiffeners are made of steel (E = 2 × 105

MPa, ν = 0.3). Assume elastic plastic material and yield stress σy = 207 MPa.

(a) Find limit pressure for the plate if it is simply supported all around the outer edges (no

stiffeners).

(b) Reanalyze for the limit load the plate if there are stiffeners (30 cm width x 8 mm thick)

around the outer edges of the plate and the plate is supported at the corner as shown in the

figure below.

*note: Apply pressure 100000 and see when the structure collapse (or the analysis stops) Notice buckling of the stiffeners in case (b)

2 m

3 m

0.3 m

y

x

z

Sym.along y = 3

Sym.along x = 0

Tutorial 9 2/6

STEP 1: Start up

Preference> Structural

/UNITS, SI

STEP 2: Preprocessor

Select the element type to be Shell 8-node 93 (SHELL93)

Create 2 real constant sets for the above thicknesses (0.02 and 0.008)

Create the material model

- Main Menu> Preprocessor > Mat Props > Material Models> Linear > Elastic> Isotropic

Enter EX = 2e11 Pa and PRXY = 0.3

- Main Menu> Preprocessor > Mat Props > Material Models> Inelastic> Rate Independent>

Isotropic Hardening Plasticity > Mises Plasticity > Bilinear

Enter yield stress = 207 e6 Pa and Tangent modulus = 0

Click “Graph” to check your material model.

Tutorial 9 3/6

Create plate model (as explained in Tutorial 7)

Set the element size of the all the areas to be 0.1 and mesh all the areas. Don’t forget to

assign meshing attribute corresponding to the thickness of the plates for case (b).

Apply boundary conditions.

Set Symmetry B.C. for all the lines on plane X = 0, and for those on plane Y = 3.

For (a), set UZ = 0 for outer edge of the plate (plane X = 2 and plane Y = 0).

For (b), set UZ = 0 for the corner node

Apply pressure 100000 Pa on area 1

STEP 5: Solution

Main Menu > Solution > Analysis Type > Solution Controls

For (a), in “Basic” tab,

Analysis Options –Small Displacement Analysis

Time Control – Time at the end of load step = 1

– Automatic time stepping = Program Chosen

Tutorial 9 4/6

– Number of substeps = 20, Min no. of substeps = 10

Write Items to Results File – All solution items

Frequency – Write every Nth substep, N= 1

Click OK

For (b), in “Basic” tab,

Analysis Options –Large Displacement Analysis

Time Control – Time at the end of load step = 1

– Automatic time stepping = Program Chosen

– Number of substeps = 20, Max no. of substeps = 30, Min no. of substeps = 10

Write Items to Results File – All solution items

Frequency – Write every Nth substep, N= 1

Click OK

Main Menu > Solution > Solve > Current LS

Tutorial 9 5/6

STEP 6: Postprocessor

Main Menu > General Postproc > Read Results > By Pick >

Pick the substep of interest and check Von Mises stress/ strain distribution.

You can also use Results Viewer to view results and animation of the substeps.

Batch File for (b) /FILNAME, NonlinearPlate /TITLE, Nonlinear Analysis for Plate with Stiffeners /UNITS, SI *SET, B, 2 ! Assigns values to user-named parameter *SET, W, 3 ! SET, par, value *SET, T, 0.3 *SET, WL, 1.25 *SET, BL, 0.5 *SET, P, -100000 /PREP7 ! Enter Preprocessing Module ET,1,SHELL93 ! Specify element type (ET, itype, ename) R, 1,0.02 ! Specify real constant (R, nset, r1, r2) R, 2, 0.008 ! Specify material properties MP,EX,1,2 E11 ! MP, lab, mat, c0 (label EX = Young’s modulus) MP,PRXY,1,0.3 ! PRXY = Poisson’s ratio ! Activate a data table for nonlinear material properties (Bikinematic hardening) TB,BISO,1 TBDATA,,207E6,0 ! Data table, Yield stress= 30000 psi, Second slope = 0 K, 1, 0, 0, T !Create keypoints (top of the shell) K, 2, B, 0, T K, 3, B, W, T K, 4, 0, W, T KGEN, 2, 1, 3,1,,,-T ! Generates keypoints from a pattern of keypoints K, 8, 0, W-WL,T ! Keypoints for area under loading K, 9, BL, W-WL, T K,10, BL, W, T ! Create a line between two keypoints L, 1, 2 L, 2, 3 L, 3, 10 L, 10, 4 L, 4, 8 L, 8, 1 L, 8, 9 L, 9, 10 L, 5, 6 L, 6, 7 L, 1, 5 L, 2, 6 L, 3, 7 ! Generates an area bounded by lines ( AL, l1, l2, l3, l4, l5, l6, l7, l8, l9, l10) AL, 4, 5, 7, 8 AL, 3, 8, 7, 6, 1, 2

Tutorial 9 6/6

AL, 1, 12, 9, 11 AL, 2, 13, 10, 12 AESIZE, ALL, 0.1 ! Specifies the element size to be meshed onto areas REAL, 1 TYPE, 1 ! Select element type MAT, 1 ! Select material type ASEL, S, AREA,,1,2 ! Select a subset of area (type S = select a new set) AMESH, ALL ! Mesh areas (AMESH, na1, na2, ninc) REAL, 2 ASEL, INVE ! type INVE = invert the current set AMESH, ALL ASEL, ALL SFA,1,,PRES,P ! SFA, area, lkey, lab, value, value2 ! Boundary Conditions NSEL,S,LOC,X,0 ! Select nodes with location X= 0 DSYM,SYMM,X ! Symmetry along plane with normal in X direction NSEL,S,LOC,Y,W ! Select nodes with location Y = 3 DSYM,SYMM,Y ! Symmetry along plane with normal in X direction NSEL,S,LOC,X, B ! Select nodes with location X = B NSEL,R,LOC,Y, 0 ! Reselect nodes with location Y = 0 and Z = 0 NSEL,R, LOC, Z, 0 D, ALL, UZ, 0 ! Defines DOF constraints at nodes (D, node, lab, value) NSEL, ALL SFTRAN ! Transfer the solid model surface loads to the FE model /SOLU ! Enter the solution processor SOLCONTROL,ON ! Use optimized nonlinear solution defaults AUTOTS,ON ! Automatic time stepping NLGEOM, ON ! Large Deformation Analysis NSUBST, 20,30 ,10 ! Number of substeps to be used for this load step OUTRES, ALL, ALL SOLVE ! Solve the current load step SAVE /POST1 ! Enters the database results postprocessor SET, LAST ! Read the last data set PLESOL, S, EQV, 2 ! Displays the solution results (PLESOL, item, comp, kund)