Linear Static Analysis of a Plate with Hole

Transcription

1 Fergyanto E. Gunawan Department of Mechanical Engineering Toyohashi University of Technology Objectives: Modeling a symmetric structure Bottom-up and top-down approaches in modeling ANSYS-APDL Sensitivity analysis. DISCLAIMER: In this module, majority of the content is taken from Appendix E MSC.Nastran 120 Exercise Workbook. Though the reference tailors the need of Nastran and Patran; in this report, the content is modied to suit the ANSYS Interface. This document was composed in LATEX; vector graphics were generated by Adobe Illustrator 10, Matlab and ANSYS. A bitmap graphic, Fig. 9, is reproduced from a picture in p. 136 of Design of Machine Element [1].

2 Model Description: The following gure shows a uni-axial loaded plate with hole. For given data in Fig. 1, in addition to those in Table 1, calculate the maximum stress around the hole and plot the stress along the ligament. R psi 10.0 Figure 1: The plate with a circular hole; unit is in. Table 1: Model properties Plate thickness, t : in. Young modulus, E : 10.0E+06 psi Poisson ratio, : 0.3 References [1] M. F. Spotts. Design of Machine Elements. Prentice Hall, [2] Nicholas M. Baran. Finite element analysis on microcomputer. McGraw-Hill, Inc., [3] MSC/NASTRAN for Windows User's Guide, [4] R. E. Peterson. Stress Concentration Design Factors. New York: John Wiley & Sons, Inc F E G 2

3 Pre-Processing Phase: CREATE A NEW FOLDER 1. Dene some parameters: ANSYS Pulldown Menu Parameters Scalar Parameters Selection: LENGTH = 5.0 Accept Selection: WIDTH = 2.0 Accept Selection: RAD = 1.0 Accept Selection: PI = ACOS(-1.0) Accept Close 2. Select an element type: ANSYS Main Menu Preprocessor Element Type Add/Edit/Delete Add Solid 8node 82Plane Options Element behavior K3 : Plane strs w/thk Close F E G 3

4 3. Dene the plate thickness: ANSYS Main Menu Preprocessor Real Constants Add/Edit/Delete Add Type 1 PLANE82 Thickness THK Close 4. Dene material properties: ANSYS Main Menu Preprocessor Material Props Material Models Structural Linear Elastic Isotropic EX 10.0E+06 PRXY 0.3 Material Exit 5. Create ten keypoints: ANSYS Main Menu Preprocessor Modeling Create Keypoints In Active CS NPT Keypoint number: 1 X, Y, Z Location in active CS: RAD 0 0 NPT Keypoint number: 2 F E G 4

5 X, Y, Z Location in active CS: RAD*COS(PI/8) RAD*SIN(PI/8) 0 NPT Keypoint number: 3 X, Y, Z Location in active CS: RAD*COS(PI/4) RAD*SIN(PI/4) 0 NPT Keypoint number: 4 X, Y, Z Location in active CS: RAD*COS(3/8*PI) RAD*SIN(3/8*PI) 0 NPT Keypoint number: 5 X, Y, Z Location in active CS: 0 RAD 0 NPT Keypoint number: 6 X, Y, Z Location in active CS: 0 WIDTH 0 NPT Keypoint number: 7 X, Y, Z Location in active CS: WIDTH WIDTH 0 NPT Keypoint number: 8 X, Y, Z Location in active CS: WIDTH 0 0 NPT Keypoint number: 9 X, Y, Z Location in active CS: LENGTH 0 0 F E G 5

6 NPT Keypoint number: 10 X, Y, Z Location in active CS: LENGTH WIDTH 0 6. Create lines: ANSYS Main Menu Preprocessor Modeling Create Lines Arcs Through 3 KPs < Pick Keypoints: 1, 3, and then 2 > < Pick Keypoints: 3, 5, and then 4 > Preprocessor Modeling Create Lines Lines Straight line < Pick Keypoints: 1, and then 8 > < Pick Keypoints: 3, and then 7 > < Pick Keypoints: 5, and then 6 > < Pick Keypoints: 6, and then 7 > < Pick Keypoints: 7, and then 8 > < Pick Keypoints: 8, and then 9 > < Pick Keypoints: 9, and then 10 > < Pick Keypoints: 7, and then 10 > Cancel 7. Show the line number: ANSYS Pulldown Menu PlotCtrls Numbering LINE Line numbers : on F E G 6

7 Plot Lines You should see a model similar to that in Fig. 2. In the next steps, we will create three areas; those areas are surrounded by lines, for Area 1: L2, L4, L6, L5; for Area 2: L1, L3, L7, L4; and for Area 3: L7, L8, L9, L10. Figure 2: Model of plate with hole having line numbers turned on. 8. Create three areas: ANSYS Main Menu Preprocessor Modeling Create Areas Arbitrary By Lines < Pick lines: L2, L4, L6, and then L5 > < Pick lines: L1, L3, L7, and then L4 > < Pick lines: L7, L8, L9, and then L10 > F E G 7

8 9. Control the mesh density: ANSYS Main Menu Preprocessor Meshing MeshTool Lines : Set < Pick lines: 1, 2, 3, 4, 5, 6, 7, and then 9 > NDIV No. of element divisions 4 < Pick lines: 7 and 9 > NDIV No. of element divisions 6 Ok 10. Show the area number: ANSYS Pulldown Menu PlotCtrls Numbering AREA Area numbers : on Plot Areas 11. Mesh the model: ANSYS Main Menu Preprocessor Meshing MeshTool Shape : Shape : Quad Mapped Mesh < Pick areas: A1, A2, and then A3 > F E G 8

9 NDIV = 4 PLANE42 PLANE82 PLANE42 PLANE82 Figure 3: MeshTool of ANSYS and some of its functionality. F E G 9

10 l 1 l 2 l 3 Linear Static Analysis of a Plate with Hole Figure 4: The plate with hole model having area numbers turned on. Important note The results, especially the stress, of a nite element analysis strongly depends on the mesh. Concerning the mesh, Nicholas M. Baran [2] suggests followings: Mesh Transition: You can use a tringle or control the mesh spacing ratio. However, in using the mesh spacing ratio, keep l 2 2l 1 and l 4 2l 3. l 4 Element Aspect Ratio: Aspect ratio (l=w) should be kept less than 3, if possible. l w l w Excessive aspect ratio Element Skewness: Try to keep the skew angle,, less than 30 degrees. Nastran issues a warning if the angle is greater than 30 degrees [3]. θ F E G 10

11 Figure 5: The nite element mesh of the plate with hole model. Important note The general guidelines are: Fine mesh in the area of interest Fine mesh in the region that has high stress gradient. Use quadratic element instead of linear element if possible. Solution Phase: 1. Dene the analysis type: ANSYS Main Menu Solution Analysis Type New Analysis [ANTYPE] Type of analysis: Static 2. the boundary condition: ANSYS Main Menu Solution Dene Loads Structural Displacement Symmetry B.C < Pick Lines: L5, L3, L8 > F E G 11

12 Important Notes Following gures show several types of symmetry structures: (a) Axial Symmetry (b) Planar Symmetry (c) Cyclic Symmetry (d) Repetitive Symmetry However, the symmetricalness does not only about the geometry, but also the constraints and the loading conditions. For an example, see following: Symmetry point 3. uniform stress: ANSYS Main Menu Anti-symmetry point Solution Dene Loads Structural Pressure On Lines < Pick Line: L9 >. VALUE Load PRES: Solve the problem: ANSYS Main Menu Solution Solve Current LS Close F E G 12

13 Post Processing Phase: 1. Plot deformation: ANSYS Main Menu General Postproc Plot Results Deformed Shape KUND Items to be plotted: Def + undef edge The result is shown Fig. 6. Figure 6: The deformation and undeformed plate with hole. 2. Plot the von Misses stress: ANSYS Main Menu General PostProc Plot Results Contour Plot Nodal Solu Nodal Solution Stress von Misses stress Undisplaced shape key: Deformed shape with undeformed edge F E G 13

14 The results are shown in Fig. 7. Figure 7: The von Misses stress in the loaded plate with hole. 3. Select the nodes along ligament: ANSYS Pulldown Menu Plot Nodes Select Entities Nodes Select Nodes: Box < Click and drag your mouse to form a box; for example, see Fig. 8. > 4. List the results of stresses: ANSYS Main Menu F E G 14

15 Figure 8: Nodes selection using a box. General PostProc List Results Nodal Solution Nodal Solution Stress X-Component of stress You should obtain: NODE SX SY SZ SXY SYZ SXZ E E E E E E E E The exact solution can be seen in Refs. [1, 4] that the stress concentration factor, K is dened as K = Highest value of actual stress on hole; max Nominal stress for minimum cross section : (1) For d=w = 0:50, where d is the hole diameter, and W is the plate width, the K is (see Fig. 9). Meanwhile, the nominal stress for the minimum cross section is 4=2 1 psi = 2.0 psi; therefore, the highest theoretical stress is max = 2:169 2:0 = 4:338 psi: (2) ANSYS provides you, at Node 2, x = psi, or 2.37 % lower than the exact solution. 5. In addition, you also needs those nodes locations: ANSYS Pulldown Menu List Nodes Sort rst by: NODE Number F E G 15

16 2.169 Figure 9: Stress concentration factor for a at bar with a transverse hole in axial tension [1]. You should obtain, after removing the midside nodes NODE X Y Z THXY THYZ THZX Therefore, we can now plot the stress along the ligament: Y Axis (in) FEM Peterson SX (psi) Figure 10: The normal stress along the plate ligament. Figure 10 concludes the rst part of this module. In the second part, we will discusss the top-down approach in creating a nite element model. In addition, we also discuss about ANSYS-APDL code for the present problem. F E G 16

17 Top-down Modeling Approach Two approachs in modeling: Bottom-up approach: keypoints lines area volume meshing Top-down approach: primitives boolean operations meshing We study the top-down approach in this section. In the next section, the APDL code also will be based on the present log le. CREATE A NEW FOLDER Pre-Processing Phase: 1. Select element type, dene the thickness, and also dene material properties. Repeat the previous pre-processing phase, the rst four steps. 2. Create two rectangles: ANSYS Main Menu Preprocessor Modeling Create Areas Rectangle By 2 Corners WP X 0.0 WP Y 0.0 Width Height WIDTH WIDTH WP X WIDTH WP Y 0.0 Width Height LENGTH-WIDTH WIDTH 3. Turn on the keypoint number, the area numbers and the line numbers: ANSYS Pulldown Menu F E G 17

18 PlotCtrls Numbering KEYPOINT Keypoint numbers: On AREA Area Numbers LINE Line numbers On On 4. Create a circle: ANSYS Main Menu Preprocessor Modeling Create Area Circl Solid Circle WP X 0.0 WP Y 0.0 Radius RAD 5. Substract Area A1 to Area A3: ANSYS Main Menu Preprocessing Modeling Operate Booleans Substract Areas < Pick Area A1 > < Pick Area A3 > You should see the new area which has a number of A4 6. Merges coincident Keypoints: ANSYS Main Menu Preprocessor Numbering Ctrls Merge Items F E G 18

19 Label Type of item to be merge Keypoints 7. Create a keypoint: ANSYS Main Menu Preprocessing Modeling Create Keypoints In Active CS NPT Keypoint number 100 X, Y, Z Location in active CS Create a line: ANSYS Main Menu Preprocessing Modeling Create Lines Lines Strainght Line < Pick Node 100 and 8 > 9. Cut the area into two areas: ANSYS Main Menu Preprocessing Modeling Operate Booleans Divide Area by Line < Pick Area A4 > < Pick Line L1 > You should obtain A1, A2, and A3 10. Merges coincident Keypoints: ANSYS Main Menu F E G 19

20 Preprocessor Numbering Ctrls Merge Items Label Type of item to be merge Keypoints Figure 11: Model with the line numbers turned on. 11. Create a new parameter: ANSYS Pulldown Menu Parameter Scalar Parameters Selection: NOE = Control the mesh density: ANSYS Pulldown Menu Preprocessor Meshing MeshTool Lines Set < Pick Lines L10, L11, L13, L14, L3, L4, L2, L6 > NDIV No. of element divisions NOE F E G 20

21 < Pick Lines 5, and 7 > NDIV No. of element divisions NOE*3/2 Shape Shape Quad Mapped Mesh < Pick Area A1, A2, A3 > Close See the previous solution phase. Mesh Sensitivity Study The stress depends on the mesh in a nite element analysis; although, physically it should not. To study how the stress depend on the mesh, we perform a mesh sensitivity study. In this study, we analyse the structure for a number of the mesh-size. In short, we change NOE, and see how it aect the maximum x. The important lines from your log le are reproduced following. 1 *SET,LENGTH,5 2 *SET,WIDTH,2 3 *SET,RAD,1 4 *SET,PI,ACOS(-1.0) 5 /PREP7 6 ET,1,PLANE82 7 KEYOPT,1,3,3 8 KEYOPT,1,5,0 9 KEYOPT,1,6,0 10 R,1,0.125, MPTEMP,,,,,,,, 13 MPTEMP,1,0 14 MPDATA,EX,1,,10E6 15 MPDATA,PRXY,1,,0.3 F E G 21

22 16 17 BLC4,0,0,WIDTH,WIDTH 18 BLC4,WIDTH,0.0,LENGTH-WIDTH,WIDTH 19 CYL4,0.0,0.0,RAD 20 ASBA, 1, 3 21 K,100,0.0,0.0,0.0, 22 LSTR, 100, 3 23 ASBL, 4, 1 24 NUMMRG, KP 25 *SET,NOE,4 26 LESIZE,_Y1,,,NOE,,,,,1 27 LESIZE,_Y1,,,NOE*3/2,,,,,1 28 MSHAPE,0,2D 29 MSHKEY,1 30 AMESH,_Y1 31 FINISH 32 /SOL 33 ANTYPE,0 34 DL,P51X,,SYMM 35 SFL,P51X,PRES,-1.0, 36 SOLVE The commands that need to be retouched are shown in lines 26, 27, 34, and 35. Those funny stus, Y1 and P51X, are the problem. For the command LESIZE in lines 26 and 27, the complete command is (see manual) LESIZE, NL1, SIZE, ANGSIZ, NDIV, SPACE, KFORC, LAYER1, LAYER2, KYNDIV where NL1 is the line number, and NDIV is the number of elements. We modied those two commands with following commands: LESIZE, 10,,,NOE,,,,,1 LESIZE, 11,,,NOE,,,,,1 LESIZE, 13,,,NOE,,,,,1 LESIZE, 14,,,NOE,,,,,1 LESIZE, 3,,,NOE,,,,,1 LESIZE, 4,,,NOE,,,,,1 LESIZE, 2,,,NOE,,,,,1 LESIZE, 5,,,NOE*3/2,,,,,1 LESIZE, 6,,,NOE*3/2,,,,,1 For the symmetry constraints, the complete command is DL, LINE, AREA, Lab, Value1, Value2 where LINE is the line number; therefore, we rewrite line 34 with F E G 22

23 DL, 14,,SYMM DL, 13,,SYMM DL, 5,,SYMM The last is SFL command; as you may guess, it should be replaced with SFL, 6, PRES,-1.0, When we put everything together, we have a working APDL code: /clear *set, length, 5 *set, width, 2 *set, rad, 1 *set, pi, acos(-1.0) *set, NOE, 128 /prep7 et, 1, plane82! Eight-node plane element keyopt, 1, 3, 3! Plane stress with thickness keyopt, 1, 5, 0 keyopt, 1, 6, 0 r, 1, 0.125,! Thickness mptemp,,,,,,,, mptemp, 1, 0 mpdata, ex, 1,, 10e6! Young s modulus mpdata, prxy, 1,, 0.3! Poisson s ratio blc4, 0, 0, width, width! Create a rectangle blc4, width, 0.0, length-width, width! Create a rectangle cyl4, 0.0, 0.0, rad! Create a circle asba, 1, 3! Cut the rectangle k, 100, 0.0, 0.0, 0.0,! Create a point lstr, 100, 3! Create a line asbl, 4, 1! Divided an area nummrg, kp! Merge nodes lesize, 10,,, NOE,,,,,1 lesize, 11,,, NOE,,,,,1 lesize, 13,,, NOE,,,,,1 lesize, 14,,, NOE,,,,,1 lesize, 3,,, NOE,,,,,1 lesize, 4,,, NOE,,,,,1 lesize, 2,,, NOE,,,,,1! NOE along L10 lesize, 5,,, NOE*3/2,,,,,1 lesize, 6,,, NOE*3/2,,,,,1 mshape, 0, 2d F E G 23

24 mshkey, 1 amesh, 1! Mesh Area 1 amesh, 2! Mesh Area 2 amesh, 3! Mesh Area 3 finish /sol antype, 0! Static analysis dl, 14,,symm! Symmetric constraints dl, 13,,symm! dl, 5,,symm! sfl, 6, pres,-1.0,! uniform tensile stress solve! Solve finish Within the miracle of APDL and a set of untold bedtime stories, following lines may save your time and may keep your laziness above everything: /post1 xstressexact = 2.169*2.0 mynode = node(0.0, RAD, 0.0) *get, xstress, node, mynode, S, X error = ABS(xStressExact - xstress)/xstressexact*100 *cfopen, sensitivitystudyresult, dat,, append *vwrite, NOE, xstress, xstressexact, error (F15.0, 2X, E15.4, 2X, E15.5, 2X, E15.4) *cfclos finish which produce a nice formatted data in the le: sensitivitystudyresult.dat; such as: E E E E E E E E E E E E E E E E E E+00 or graphically Finally, you know what you see, grasp the reality that ANSYS may dissappoint you. F E G 24

25 SX (psi) FE Solution Exact Solution Number of elements (NOE) Figure 12: Eect of mesh density to the maximum stress. F E G 25