Numerical investigation through Finite Elements of Neuber’s and Molski-Glinka’s rules for calculation of elastoplastic stress and strain in notched elements

Proyecto Fin de Carrera Ingeniería de Telecomunicación Formato de Publicación de la Escuela Técnica Superior de Ingeniería Autor: F. Javier Payán Somet Tutor: Juan José Murillo Fuentes Dep. Teoría de la Señal y Comunicaciones Escuela Técnica Superior de Ingeniería Universidad de Sevilla Sevilla, 2013 Trabajo Fin de Grado Grado en Ingeniería de las Tecnologías Industriales Numerical investigation through Finite Elements of Neuber’s and Molski-Glinka’s rules for calculation of elastoplastic stress and strain in notched elements Autor: Fernando Pascual Goce Tutor: Alfredo de Jesús Navarro Robles Dpto. Ingeniería Mecánica y Fabricación Escuela Técnica Superior de Ingeniería Universidad de Sevilla Sevilla, 2019 Trabajo Fin de Grado Grado en Ingeniería de las Tecnologías Industriales Numerical investigation through Finite Elements of Neuber’s and Molski-Glinka’s rules for calculation of elastoplastic stress and strain in notched elements Autor: Fernando Pascual Goce Tutor: Alfredo de Jesús Navarro Robles Catedrático Dpto. Ingeniería Mecánica y Fabricación Escuela Técnica Superior de Ingeniería Universidad de Sevilla Sevilla, 2019 Trabajo Fin de Grado: Numerical investigation through Finite Elements of Neuber’s and Molski- Glinka’s rules for calculation of elastoplastic stress and strain in notched elements Autor: Fernando Pascual Goce Tutor: Alfredo de Jesús Navarro Robles El tribunal nombrado para juzgar el trabajo arriba indicado, compuesto por los siguientes profesores: Presidente: Vocal/es: Secretario: acuerdan otorgarle la calificación de: El Secretario del Tribunal Fecha: Abstract An investigation on elastoplastic stress and strain produced at notched pieces with different geometries and material properties using Finite Elements and numerical computation software. Application of Neuber’s and Molski-Glinka’s rules directed to obtaining real stress and strain at notches from data obtained with Finite Elements models. This project sets the basis for future research on the same topic, aiming to use a similar process to obtain results in a wider variety of geometries and materials. I Contents Abstract I Notation V 1 Stress concentration 1 1.1 Stress concentration factors 1 1.1.1 Example 2 1.2 Traditional calculation of stress concentration factors 2 1.3 Calculation of stress concentration factors through Finite Elements 3 2 Modeling in ANSYS 5 2.1 Single U-shaped notched plate 6 2.1.1 Parameters 6 2.1.2 Material properties 6 2.1.3 Creating a solid body with SOLID186 7 2.1.4 Creating a plane stress plate with PLANE182 7 2.1.5 Meshing, loads and constraints 7 2.1.6 Solution 9 2.1.7 Obtaining results 9 2.1.8 Results output 10 2.1.9 Codes 12 2.2 Opposite U-shape notched plate 19 2.2.1 Codes 19 2.3 Single and opposite semicircular notched plate 27 2.4 Modeling an elasto-plastic material 28 2.5 Aspects to consider 29 2.5.1 Plate’s width 29 2.5.2 Plate’s height 29 2.5.3 High stresses produced in loads applied directly to nodes 30 2.5.4 Free face boundary conditions 30 3 Stress concentration factors comparison 33 3.1 Stress concentration factors in opposite U-shaped notched plates 33 3.2 Stress concentration factors in single U-shaped notched plates 33 3.3 Stress concentration factors in opposite semicircular notched plates 35 3.4 Stress concentration factors in single semicircular notched plates 35 3.5 Issues with Pilkie’s interpolation expressions 36 3.6 Stress concentration factors in elements with different thickness 36 3.7 Charts 38 3.8 Codes 52 4 Neuber and Molski-Glinka’s rules 59 III 2 Modeling in ANSYS There is a wide variety of commercial FEM software that offer different possibilities for engineers to calculate stresses and strains for different geometries subjected to different loads. In this project, I will be using the software ansys to create models of notched pieces and provide reliable results in order to establish a way to estimate stresses at these notches whose parameters can be easily changed to obtain an infinite number of combinations. I will be modeling geometries that already appear in handbooks and articles, whose data come from laboratory experiments. The purpose of choosing geometries that already appear in handbooks is to simulate the conditions under which these experimental results were obtained and compare them to the results we get from ansys. Both results should be similar, otherwise the numerical model would not be representing the experiment fairly. If this can be achieved, one can be certain that their numerical models are reliable and so, we can change parameters to obtain reliable results without the need of costly laboratory experiments. The chosen geometries will be the ones shown in Figure 2.1 and Figure 2.2 , which appear in Peterson’s Stress Concentration Factors, Third Edition [1]. Figure 2.1 Single U-Shape notched plate. Original image taken from Peterson’s Stress Concentration Factors, Third Edition [1]. Figure 2.2 Opposite U-Shape notched plate. Original image taken from Peterson’s Stress Concentration Factors, Third Edition [1]. 5 6Chapter 2. Modeling in ANSYS 2.1 Single U-shaped notched plate For this first model, I have chosen a plate presenting a single U-shaped notch. In the experiment, a constant load was applied along a line at the center of the minimum section all across its depth as shown in Figure 2.3. t d/2 d/2 H h P Figure 2.3 Load distribution along a line at the center of the minimum section. To apply these conditions and be able to obtain results from ansys it is necessary to perform the following steps. These steps will show how I created the code in ansys to perform a Finite Elements pure elastic solid body analysis. Variations in this code and other types of analysis will be shown in following sections. 2.1.1 Parameters Parameters can be defined in ansys by means of string variables, making it easy to relate every following instruction to the program to these parameters and so on, allowing us to easily change the whole model by changing these parameters. An example of this is shown in Code 2.1. We can also create loops in order to change one parameter maintaining the rest constant. This is done with the command *DO , as it is shown in Code 2.2. In this case I am changing the notch’s radius (R) with the values obtained in parameter DIV. Then I am saving all previously saved parameters with command PARSAV and erasing all previously defined geometries with command CLEAR so we can create a new one defined with the values contained in the next position of vector DIV. Command PARRES is used to reestablish parameters saved with PARSAV . We also must define where the loop finishes, this is done with command *ENDDO . 2.1.2 Material properties Material properties are a key factor in all analysis in Finite Elements. They will provide the software with vital information about the behavior of the element being studied. Here we can set conditions of plane stress, elasto-plastic behavior and much more. In this case, I am just considering an isotropic, pure elastic material behaving as a solid body, so ansys only needs the material’s Young’s modulus, Poisson’s coefficient and the type of element we want to use for our model, in this case SOLID186 , which is a higher order 3-D 20-node solid element that exhibits quadratic displacement behavior [ 2 ]. To define material properties, we need to enter in the Preprocessor section, defined as /PREP7 , as shown in Code 2.3 If we want to set conditions for Plane Stress, we can use element PLANE182 and use the different KEYOPTIONS to define, in this case, the width of the plate, as shown in Code 2.5. It is also possible to set conditions for Plane Strain just by changing the KEYOPTIONS of the previous code and replace the with the ones shown in Code ??. 2.1 Single U-shaped notched plate 7 2.1.3 Creating a solid body with SOLID186 The solid body in a numerical model is the one in charge of defining the geometry intended to study and it is also defined in the Preprocessor section. Considering the geometry’s symmetry, it is possible just to define the upper half of it and then applying symmetry boundary conditions Figure 2.4, avoiding the unnecessary use of nodes and calculation time. At first, I tried to create the whole plate geometry in a sole volume, as it was the easiest way to define solid geometries, but it turned out that it was impossible to apply the boundary conditions needed in this experiment, because there was no way to apply loads on the specific line where they should be. Instead, I opted for creating an area using lines and deliberately cutting the line that defined the upper part of the bar right at the point at the center of the minimum section, as is shown at Figure 2.5. To create the notch, in this case a U-shaped notch, I created a square area and a circular area and subtracted this from the initial rectangular bar area, obtaining in this way the final desired area, shown in Figure 2.5. P P P Plane of Symmetry Figure 2.4 Applying symmetry. After defining this area, I extruded it in both directions in order to obtain the desired depth (half of this depth in each direction) and then glued both volumes into one. The code used for this definition of geometry is shown in Code 2.6 2.1.4 Creating a plane stress plate with PLANE182 The way to define our geometry with PLANE182 is similar to the one with SOLID186 but in this case we only have to define an area as we have previously defined the desired plate’s width. This also means that all loads applied in a keypoint of our area will be displayed across the whole width of the plate, so we only need to apply our load in the keypoint defined at the center of the minimum section. The code used for this definition of geometry is shown in Code 2.7 2.1.5 Meshing, loads and constraints Later, still in the Preprocessor section, I meshed the whole volume or area, where a line of nodes was created across the geometry’s width at the place where lines were cut before, allowing us to apply loads at these nodes in our solid body model, Figure 2.6, simulating the conditions of the experiment being reproduced. The mesh was refined at certain lines and surfaces, like in the entire notch surface and moreover in its middle line (peak), Figure 2.7, and the line where the loads are applied, to make load better distributed all 8Chapter 2. Modeling in ANSYS t t+d/2 d/2 Figure 2.5 Lines that define the area of the desired geometry. Figure 2.6 Loads applied at nodes situated on the line at the center of the minimum section. along the depth. It is important to properly define the areas where we are interested in obtaining precise results. As I have decided to consider the geometry’s symmetry, symmetry boundary conditions have been applied all over the minimum section. Also, constraints to the movement in direction X have been applied at the corner of the minimum section with the unnotched face and constraints to the movement in direction Z on a line that passes along the minimum section at the center of its depth, to restrict rigid solid movement, as shown in Figure 2.15. The code that includes meshing and the application of loads and constraints in the solid body model is shown at Code 2.8. Code in the plane stress model is similar, but it is not required that the movement in the Z direction be restricted. There is another possibility in order to properly refine the mesh. It is a better but more costly way to do it. This way is to refine the entire volume or area with a fine mesh, using the smart mesh option to adapt it to the geometry that we are meshing. This way, we will avoid the appearances of warnings due to the shape of elements situated in the most refined points. To do this, we must use the code shown in Code 2.9 for the solid 2.1 Single U-shaped notched plate 9 1 X Y Z APR 23 2019 13:44:25 ELEMENTS Figure 2.7 Mesh refined at notch. Figure 2.8 Constraints at the corner of the minimum section with the unnotched face. model and Code 2.10 for the plane stress model. Another possible change in this code is if we wanted to place a distributed load instead of a load at the center of the middle of the minimum section. Codes 2.11 and 2.12 show how to do this in solid and plane stress models respectively. 2.1.6 Solution To generate results, it is needed that the software compiles Finite Elements equations for the input it has been given. For this, we need to enter in the Solution processor and run the analysis. In this case, a static structural solution is specified. This is done according to Code 2.13. 2.1.7 Obtaining results When the solution is done, it is possible to plot different results, such as stress, strain, total deformation, etc. It is also possible to create graphs with certain data for certain points we are interested in. The aim of this model is to find Kσ , so what we need to calculate is σmax . The maximum stress is going to be produced at the bottom of the notch, as it is there where the maximum stress concentration is going to be. I have represented 10 Chapter 2. Modeling in ANSYS stress distribution along the notch’s root using a path from one edge to the other, representing stress in the Y direction (Figure 2.9) and along the center of the minimum section (Figure 2.10). Figure 2.9 Stress distribution along the notch’s peak. Figure 2.10 Stress distribution along the center of the minimum section. The codes to create these paths are shown in Code 2.14 and Code 2.15. These codes are defined by the values of different keypoints, so it is important to have them well defined. 2.1.8 Results output To write results in an output file we can use command *VWRITE . If a loop is used, we need to create a macro and so we can create an array of results that we can use later in other software like excel or matlab. In this 2.1 Single U-shaped notched plate 11 case I have created the following macro, Code 2.16. There are two macros in this code, the first is for writing the first result and the second is to write the following results down in a column structure. However, before writing anything we need to define what do we want to write in this output file. To do this we use the command *GET . As we are interested in obtaining the maximum stress at the notch’s root, I decided to get the maximum stress in the Y direction of the last path I plotted and then use the macro previously defined. This is done according to Code 2.17. 12 Chapter 2. Modeling in ANSYS 2.1.9 Codes Code 2.1 Parameters in ansys. !PARAMETERS H=1 !WIDTH B=1.5 !HEIGHT D=0.05 !DEPTH T=0.3*H !DEPTH OF TOTAL NOTCH Eyoung=202375000 !YOUNG MODULUS Poisson=0.33 !POISSON COEFFICIENT POI=40000 !LOAD Code 2.2 Loop in ansys. DIV=1.1,2.1,3.1,4.1,5.1,6.1,7.1,8.1,9.1 *DO,I,1,9 PARSAV,ALL, FINISH /CLEAR PARRES Code 2.3 Material properties for solid body model. /PREP7 ET,1,SOLID186 ! MATERIAL MP,EX,1,Eyoung MP,EY,1,Eyoung MP,EZ,1,Eyoung MP,PRXY,1,Poisson MP,PRXZ,1,Poisson MP,PRYZ,1,Poisson Code 2.4 Material properties for plane stress model. /PREP7 ET,1,PLANE182 KEYOPT,1,1,0 KEYOPT,1,3,3 KEYOPT,1,6,0 R,1,D, ! MATERIAL MP,EX,1,Eyoung 2.1 Single U-shaped notched plate 13 MP,EY,1,Eyoung MP,EZ,1,Eyoung MP,PRXY,1,Poisson MP,PRXZ,1,Poisson MP,PRYZ,1,Poisson Code 2.5 Material properties for plane stress model. /PREP7 ET,1,PLANE182 KEYOPT,1,1,0 KEYOPT,1,3,2 KEYOPT,1,6,0 Code 2.6 Geometry with SOLID186. !KEYPOINTS K,1,0,0,0 K,2,H,0,0 K,3,0,B/2,0 K,4,H,B/2,0 K,6,R+(H-R)/2,B/2,0 K,7,0,R,0 K,8,T-R,0,0 K,9,T-R,R,0 !RECTANGLE LSTR,8,2 LSTR,2,4 LSTR,4,6 LSTR,6,3 LSTR,3,7 LSTR,7,9 LSTR,9,8 FLST,2,7,4 FITEM,2,7 FITEM,2,6 FITEM,2,5 FITEM,2,4 FITEM,2,3 FITEM,2,2 FITEM,2,1 AL,P51X !NOTCH CIRCLE CIRCLE, 8, R,,,, FLST,2,4,4 FITEM,2,8 FITEM,2,9 FITEM,2,10 20 Chapter 2. Modeling in ANSYS ('S_yy_max') *VWRITE,S_yy_max ((SP)1E14.6,' ') *CFCLOS *END !PARAMETERS H=0.127 !WIDTH H=H/2 B=0.3048 !HEIGHT D=0.01 !DEPTH T=0.3*H !DEPTH OF NOTCH Eyoung=202375000 Poisson=0.33 POI=40000 !LOAD DIV=1.1,2.1,3.1,4.1,5.1,6.1,7.1,8.1,9.1 *DO,I,1,9 PARSAV,ALL, FINISH /CLEAR PARRES R=T/DIV(I) !RADIO /PREP7 ET,1,SOLID186 ! MATERIAL MP,EX,1,Eyoung MP,EY,1,Eyoung MP,EZ,1,Eyoung MP,PRXY,1,Poisson MP,PRXZ,1,Poisson MP,PRYZ,1,Poisson !KEYPOINTS K,1,0,0,0 K,2,H,0,0 K,3,0,B/2,0 K,4,H,B/2,0 K,6,R+(H-R)/2,B/2,0 K,7,0,R,0 K,8,T-R,0,0 K,9,T-R,R,0 !RECTANGLE LSTR,8,2 LSTR,2,4 LSTR,4,6 LSTR,6,3 LSTR,3,7 LSTR,7,9 LSTR,9,8 FLST,2,7,4 2.2 Opposite U-shape notched plate 21 FITEM,2,7 FITEM,2,6 FITEM,2,5 FITEM,2,4 FITEM,2,3 FITEM,2,2 FITEM,2,1 AL,P51X !CIRCULAR NOTCH CIRCLE, 8, R,,,, FLST,2,4,4 FITEM,2,8 FITEM,2,9 FITEM,2,10 FITEM,2,11 AL,P51X ASBA, 1, 2 !EXTRUSION VOFFST,3,D/2, , VOFFST,3,-D/2, , FLST,2,2,6,ORDE,2 FITEM,2,1 FITEM,2,-2 VGLUE,P51X !MESH MSHKEY,0 MSHAPE,1,3d FLST,5,2,6,ORDE,2 FITEM,5,1 FITEM,5,-2 CM,_Y,VOLU VSEL, , , ,P51X CM,_Y1,VOLU CHKMSH,'VOLU' CMSEL,S,_Y VMESH,_Y1 !REFINE FLST,5,2,5,ORDE,2 FITEM,5,9 FITEM,5,17 CM,_Y,AREA ASEL, , , ,P51X CM,_Y1,AREA CMSEL,S,_Y CMDELE,_Y AREFINE,_Y1, , ,1,0,1,1 CMDELE,_Y1 22 Chapter 2. Modeling in ANSYS FLST,5,2,4,ORDE,2 FITEM,5,17 FITEM,5,31 CM,_Y,LINE LSEL, , , ,P51X CM,_Y1,LINE CMSEL,S,_Y CMDELE,_Y LREFINE,_Y1, , ,1,1,1,1 CMDELE,_Y1 FLST,5,1,3,ORDE,1 FITEM,5,5 CM,_Y,KP KSEL, , , ,P51X CM,_Y1,KP CMSEL,S,_Y CMDELE,_Y KREFINE,_Y1, , ,1,1,1,1 CMDELE,_Y1 !LOADS FLST,5,2,4,ORDE,2 FITEM,5,17 FITEM,5,31 LSEL,S, , ,P51X NSLL,S,1 FLST,2,9,1,ORDE,7 FITEM,2,32 FITEM,2,2036 FITEM,2,4026 FITEM,2,-4028 FITEM,2,6267 FITEM,2,8257 FITEM,2,-8259 /GO F,P51X,FY,POI ALLSEL,ALL FLST,2,2,5,ORDE,2 FITEM,2,2 FITEM,2,11 DA,P51X,SYMM FLST,2,1,4,ORDE,1 FITEM,2,12 /GO DL,P51X, ,UZ,0 FLST,2,2,5,ORDE,2 FITEM,2,4 FITEM,2,12 2.2 Opposite U-shape notched plate 23 DA,P51X,SYMM FINISH /Sol ANTYPE,0 Solve FINISH /POST1 path,patron,2,,100 ppath,1,,kx(5),ky(5),kz(5) ppath,2,,kx(5)+R,ky(5),kz(5) pdef,s_yy,s,y plpath,s_yy path,alongZ,2,,1000 ppath,1,,kx(16),ky(16),kz(16) ppath,2,,kx(8),ky(8),kz(8) pdef,s_yy,s,y plpath,s_yy *GET,S_yy_max,PATH,0,MAX,s_yy *IF,I,EQ,1,THEN *USE,MACRO_ESCRIT_1 *ELSE *USE,MACRO_ESCRIT_2 *ENDIF *ENDDO FINISH Code 2.19 Complete code for plane stress opposite U-shape notched plate. /CLEAR *CREATE,'MACRO_ESCRIT_1',' ',' ' *CFOPEN,DATOS_BARATTA,dat *VWRITE,S_yy_max ((SP)1E14.6,' ') *CFCLOS *END *CREATE,'MACRO_ESCRIT_2',' ',' ' *CFOPEN,DATOS_BARATTA,dat,,APPEND *VWRITE,S_yy_max ((SP)1E14.6,' ') *CFCLOS *END !PARAMETERS H=2 !WIDTH H=H/2 B=5 !HEIGHT 24 Chapter 2. Modeling in ANSYS D=0.05 !DEPTH T=0.3*H !DEPTH OF NOTCH Eyoung=202375000 Poisson=0.33 POI=10000000 !LOAD PRE=-POI/(H*D) DIV=1.1,2.1,3.1,4.1,5.1,6.1,7.1,8.1,9.1 *DO,I,1,9 PARSAV,ALL, FINISH /CLEAR PARRES R=T/DIV(I) !RADIUS /PREP7 ET,1,PLANE182 KEYOPT,1,1,0 KEYOPT,1,3,3 KEYOPT,1,6,0 R,1,D, ! MATERIAL MP,EX,1,Eyoung MP,EY,1,Eyoung MP,EZ,1,Eyoung MP,PRXY,1,Poisson MP,PRXZ,1,Poisson MP,PRYZ,1,Poisson !KEYPOINTS K,1,0,0,0 K,2,H,0,0 K,3,0,B/2,0 K,4,H,B/2,0 K,6,R+(H-R)/2,B/2,0 K,7,0,R,0 K,8,T-R,0,0 K,9,T-R,R,0 !RECTANGLE LSTR,8,2 LSTR,2,4 LSTR,4,6 LSTR,6,3 LSTR,3,7 LSTR,7,9 LSTR,9,8 FLST,2,7,4 FITEM,2,7 FITEM,2,6 2.2 Opposite U-shape notched plate 25 FITEM,2,5 FITEM,2,4 FITEM,2,3 FITEM,2,2 FITEM,2,1 AL,P51X !CIRCULAR NOTCH CIRCLE, 8, R,,,, FLST,2,4,4 FITEM,2,8 FITEM,2,9 FITEM,2,10 FITEM,2,11 AL,P51X ASBA, 1, 2 !MESH MSHKEY,0 CM,_Y,AREA ASEL, , , , 3 CM,_Y1,AREA CHKMSH,'AREA' CMSEL,S,_Y AMESH,_Y1 !REFINE FLST,5,1,5,ORDE,1 FITEM,5,3 CM,_Y,AREA ASEL, , , ,P51X CM,_Y1,AREA CMSEL,S,_Y CMDELE,_Y AREFINE,_Y1, , ,3,0,1,1 CMDELE,_Y1 !CONSTRAINTS FLST,2,2,4,ORDE,2 FITEM,2,2 FITEM,2,12 DL,P51X, ,SYMM !LOADS !FLST,2,1,3,ORDE,1 !FITEM,2,4 !/GO !FK,P51X,FY,POI FLST,2,2,4,ORDE,2 FITEM,2,3 FITEM,2,-4 26 Chapter 2. Modeling in ANSYS /GO SFL,P51X,PRES,PRE, FINISH /SOL SOLVE FINISH /POST1 path,patron,2,,100 ppath,1,,kx(5),ky(5),kz(5) ppath,2,,kx(2),ky(5),kz(5) pdef,s_yy,s,y plpath,s_yy *GET,S_yy_max,PATH,0,MAX,s_yy *IF,I,EQ,1,THEN *USE,MACRO_ESCRIT_1 *ELSE *USE,MACRO_ESCRIT_2 *ENDIF *ENDDO FINISH 2.3 Single and opposite semicircular notched plate 27 2.3 Single and opposite semicircular notched plate This last model is obtained by setting t/r=1 . This means that the notch’s shape is one perfect semicircle. The interest for this particularity is that we can find an analytical solutions for this geometry such as those presented by Maunsell [ 7 ] and Ling [ 6 ], which will be discussed later. In relation with the modeling in ansys, the only difference with the U-shape notch codes is that there is no need to create a little rectangle before the circular part of the notch. This makes the code to create the initial unextruded area as shown in Code 2.20, leaving the rest as it was shown in the previous codes. Code 2.20 Code to create the initial unextruded area for the semicircular notch case. !KEYPOINTS K,1,0,0,0 K,2,H,0,0 K,3,0,B/2,0 K,4,H,B/2,0 K,6,R+(H-R)/2,B/2,0 K,7,0,0,0 !RECTANGLE LSTR,7,2 LSTR,2,4 LSTR,4,6 LSTR,6,3 LSTR,3,7 FLST,2,5,4 FITEM,2,5 FITEM,2,4 FITEM,2,3 FITEM,2,2 FITEM,2,1 AL,P51X !CIRCULAR NOTCH CIRCLE, 7, R,,,, FLST,2,4,4 FITEM,2,7 FITEM,2,6 FITEM,2,8 FITEM,2,9 AL,P51X ASBA, 1, 2 28 Chapter 2. Modeling in ANSYS 2.4 Modeling an elasto-plastic material The way to model an elasto-plastic material in ansys is to create a σ−ε curve that defines the material behavior, see Ramberg-Osgood relationship (Section 4.1). PLANE182 and SOLID186 allow us to create this curve by using a nonlinear, inelastic and rate independent material model, which can be defined with keyoptions. We only need to provide a maximum of 20 points and the software automatically interpolates values between adjacent points. I have defined the values of this curve in matlab and then picked an equally spaced sample of 20 points from this curve, then I introduced the values in ansys. In relation with the code, we only need to change the Material properties (Section 2.1.2) like it is shown in Code 2.21, leaving the rest as it was. The same can be applied to SOLID186 . It is very important that the starting slope of the curve we introduced agrees with the Young’s modulus we provided. Code 2.21 Code to introduce elasto-plastic material properties. ET,1,PLANE182 KEYOPT,1,1,0 KEYOPT,1,3,3 KEYOPT,1,6,0 R,1,D, MPTEMP,,,,,,,, MPTEMP,1,0 MPDATA,EX,1,,Eyoung MPDATA,PRXY,1,,Poisson TB,KINH,1,1,20,0 TBTEMP,0 TBPT,, 0.000049413319990 , 10000000 , TBPT,, 0.000307467294401 , 62105263.16 , TBPT,, 0.000574851941833 , 114210526.3 , TBPT,, 0.000884167341589 , 166315789.5 , TBPT,, 0.001306155930431 , 218421052.6 , TBPT,, 0.001962113561667 , 270526315.8 , TBPT,, 0.003035259750046 , 322631578.9 , TBPT,, 0.004781396972906 , 374736842.1 , TBPT,, 0.007539035785502 , 426842105.3 , TBPT,, 0.011739095766390 , 478947368.4 , TBPT,, 0.017914257038170 , 531052631.6 , TBPT,, 0.026708016232101 , 583157894.7 , TBPT,, 0.038883487418425 , 635263157.9 , TBPT,, 0.055331979496578 , 687368421.1 , TBPT,, 0.077081375162851 , 739473684.2 , TBPT,, 0.105304331911138 , 791578947.4 , TBPT,, 0.141326322017036 , 843684210.5 , TBPT,, 0.186633525757482 , 895789473.7 , TBPT,, 0.242880589999978 , 947894736.8 , TBPT,, 0.311898262604064 , 1000000000 , 2.5 Aspects to consider 29 2.5 Aspects to consider 2.5.1 Plate’s width In solid models, the plate’s width seems to be a problem when it is very thin. If the complete volume refine alternative is used (see Section 2.1.5), there seems to be no or very few warnings but when the results are plotted, they do not show a "perfect" parabola as one would expect, but rather a somewhat warped curve instead, as shown in Figure 2.12. In plane stress models, this problem does not appear, allowing us to apply a width as thin as we want. Figure 2.12 Stress distributions along the notch’s peak with a "thin" width. 2.5.2 Plate’s height In both solid and plane stress models, the plate’s height seems to be crucial in order to obtain reliable results. If we apply a "short" height, stress distributions along the minimum section are distorted due to the effect of the area of application of the loads, Figure 2.13. This effect is more noticeable when when the distribution along the middle line of the minimum section is applied. Figure 2.13 Stress distributions along the minimum section with a "short" height. 36 Chapter 3. Stress concentration factors comparison 3.5 Issues with Pilkie’s interpolation expressions 1 When comparing the data obtained from the FE models with Peterson’s results [ 1 ], I have found that there is a big discrepancy between the information that Peterson gives in his original handbooks [ 8 ], plotted in charts, and the interpolation expressions that Pilkie [ 1 ] offers for these plots that appear in Figure 3.1. These discrepancies appear, at least, for Kσ at single and opposite U-shaped notches, and can be seen in Figure 3.12 and Figure 3.13 respectively. The error, in %, produced in reference to Peterson’s data can be seen in the tables 3.1 and 3.2: Table 3.1 Error table for Pilkie’s interpolation of opposite U-shaped notches. H/d=1.05 H/d=1.10 H/d=1.15 H/d=1.20 H/d=1.30 H/d=1.50 H/d=2.00 r/d=0.10 0.5305 1.1664 4.3877 6.7344 7.5541 8.6806 10.1544 r/d=0.15 1.0883 0.5512 2.7686 4.2633 7.6440 7.7483 8.6763 r/d=0.20 1.5757 1.7244 2.5698 3.5332 6.1570 7.3548 9.2938 r/d=0.25 1.8402 2.1503 2.7186 3.7571 5.3193 7.0790 9.1205 r/d=0.30 2.8176 2.8786 2.8965 4.3797 5.9895 6.9514 7.6625 Average 1.5704 1.6942 3.0682 4.5336 6.5328 7.5628 8.9815 Table 3.2 Error table for Pilkie’s interpolation of single U-shaped notches. H/d=2.00 H/d=1.50 H/d=1.20 H/d=1.10 r/d=0.10 8.2826 8.9642 3.2888 6.3841 r/d=0.15 8.6869 9.5690 3.0743 4.5167 r/d=0.20 8.3483 9.5271 1.8798 2.4996 r/d=0.25 8.7008 10.0792 0.7766 0.9261 r/d=0.30 8.7940 9.3465 1.0150 0.8803 Average 8.5625 9.4972 2.0069 3.0414 If we compare the expressions for the case of semicircular notch ( r/d=1 ), Pilkie’s interpolation [ 1 ] seems to be accurate for the case of single semicircular notch, Figure 3.14, and somewhat better for the case of opposite semicircular notch, Figure 3.15. Due to these mistaken interpolating expressions, I decided to create my own using matlab. By picking points from Peterson’s charts [ 8 ] and interpolating them, I created an expression for each one of these curves. So, for each relation of H/dI offer an expression depending on the r/dratio. Expression for Single Semicircular: Kσ=3.0743 −7.2303 r d+4.8645(r d)2+14.8185(r d)3 Expression for Opposite Semicircular: Kσ=3.0571 −5.8969 r d+8.4157(r d)2−3.8922(r d)3 3.6 Stress concentration factors in elements with different thickness An interesting topic that can be studied with these models is how do Neuber’s and Moslki-Glinka’s rules adapt to elements with different thickness. I have created solid, elasto-plastic models with the exact same 1The codes used to create the comparisons and expressions that appear in this section appear in Section 3.8. 3.6 Stress concentration factors in elements with different thickness 37 Table 3.3 Interpolation expressions for Opposite U-shaped notches. H/dInterpolation expression 1.05 Kσ=2.4780 −8.1476 r d+24.2857(r d)2−26.6667(r d)3 1.10 Kσ=3.1600 −14.6190 r d+51.7143(r d)2−66.6667(r d)3 1.15 Kσ=3.6620 −18.3714 r d+63.4286(r d)2−80.0000(r d)3 1.20 Kσ=4.0820 −21.9381 r d+75.4286(r d)2−93.3333(r d)3 1.30 Kσ=3.9120 −15.4452 r d+38.5714(r d)2−33.3333(r d)3 1.50 Kσ=4.6120 −23.8381 r d+77.4286(r d)2−93.3333(r d)3 2.00 Kσ=5.1960 −30.0810 r d+104.2857(r d)2−133.3333(r d)3 Table 3.4 Interpolation expressions for single U-shaped notches. H/dInterpolation expression 1.10 Kσ=3.6800 −17.4333 r d+56.0000(r d)2−66.6667(r d)3 1.20 Kσ=3.7420 −17.0786 r d+52.5714(r d)2−60.0000(r d)3 1.50 Kσ=3.6900 −15.7262 r d+44.8571(r d)2−46.6667(r d)3 2.00 Kσ=3.6900 −15.7262 r d+44.8571(r d)2−46.6667(r d)3 parameters but different thickness, varying for every model the parameter t/r from 1 to 9, and compared the values obtained from them with the results taken from plane stress and plane strain analysis. Theoretically, the thinner the plate is, the closer these values must get to plane stress results. On the contrary, the thicker it is, the closer they must be to plane strain results. The values obtained appear in Figure 3.16 and they show little variation when plates are very thick, for example, the curves from the models with ratios H/h equal to 1 and 2 are very close to the values obtained for the Plane Strain model, this means that plates with a ratio H/h close to or lower to 2 can be consider as to be in Plane Strain. The application of Neuber’s and Moslki-Glinka’s rules are shown in Section 4.5. 38 Chapter 3. Stress concentration factors comparison 3.7 Charts All charts commented above are included in this section. 0.10.15 0.20.25 0.3 1.5 2 2.5 3 3.5 r/d Kσ ANSYS Peterson Figure 3.4 Comparison between Kσ at an U-shape notch in one side of a flat tension plate taken from different methods. 3.7 Charts 39 0.10.15 0.20.25 0.3 1.5 2 2.5 3 3.5 r/d Kσ ANSYS Barrata & Neal Heywood Peterson Figure 3.5 Comparison between Kσ at an U-shape notch in one side of a flat tension plate taken from different methods. 40 Chapter 3. Stress concentration factors comparison 123456789 1 2 3 4 5 6 7 8 9 t/r Kσ Plane Stress 30 % Plane Stress 10 % Plane Stress 5 % Baratta & Neal Figure 3.6 Comparison between Kσin an opposite U-shaped notched plate. 3.7 Charts 41 1234567 8 9 1 2 3 4 5 6 7 8 9 t/r Kσ Plane Stress 30 % Plane Stress 10 % Plane Stress 5 % Baratta & Neal Inglis Figure 3.7 Comparison between Kσin a single U-shaped notched plate. 42 Chapter 3. Stress concentration factors comparison 05·10−20.10.15 0.20.25 0.30.35 1 1.5 2 2.5 3 3.5 r/d Kσ ansys Plane Stress Pilkie Ling Peterson Figure 3.8 Comparison between Kσin an opposite semicircular notched plate. 3.7 Charts 43 05·10−20.10.15 0.20.25 0.30.35 0.4 1 1.5 2 2.5 3 3.5 r/d Kσ Load applied at the center of the minimum section Distributed load Figure 3.9 Comparison between Kσ in an opposite semicircular notched plate with a uniform load and a load applied at the center of the minimum section. 44 Chapter 3. Stress concentration factors comparison 05·10−20.10.15 0.20.25 0.30.35 1 1.5 2 2.5 3 3.5 r/d Kσ ansys Plane Stress Pilkie Peterson Figure 3.10 Comparison between Kσin a single semicircular notched plate. 3.7 Charts 45 05·10−20.10.15 0.20.25 0.30.35 1 1.5 2 2.5 3 3.5 4 4.5 5 r/d Kσ Load applied at the center of the minimum section Distributed load Figure 3.11 Comparison between Kσ in a single semicircular notched plate with a uniform load and a load applied at the center of the minimum section. 52 Chapter 3. Stress concentration factors comparison 3.8 Codes Code 3.1 matlab code to calculate stress concentration factor in different models. E=202375e6; n=0.211; K=1283e6; H=0.127; % WIDTH h=0.00254; % DEPTH P=4e4; % LOAD B=0.3048; T=0.1*H; hr=[1.1 2.1 3.1 4.1]; R=T./hr; d=zeros([1 length(R)]); ratio=zeros([1 length(R)]); Pn=zeros([1 length(R)]); for i=1:length(R) d(i)=H-T; ratio(i)=R(i)/d(i); Pn(i)=P/(h*d(i)); end %% PETERSONS RESULTS Ktn=zeros([1 length(R)]); for i=1:length(R) if 0.5<=T/R(i)<2 C1=0.907+2.125*sqrt(T/R(i))+0.023*T/R(i); C2=0.710-11.289*sqrt(T/R(i))+1.708*T/R(i); C3=-0.672+18.754*sqrt(T/R(i))-4.046*T/R(i); C4=0.175-9.759*sqrt(T/R(i))+2.365*T/R(i); end if 2<=T/R(i)<20 C1=0.953+2.136*sqrt(T/R(i))-0.005*T/R(i); C2=-3.255-6.281*sqrt(T/R(i))+0.068*T/R(i); C3=8.203+6.893*sqrt(T/R(i))+0.064*T/R(i); C4=-4.851-2.793*sqrt(T/R(i))-0.128*T/R(i); end Ktn(i)=C1+C2*(R(i)/H)+C3*(R(i)/H)^2+C4*(R(i)/H)^3; end %% RESULTS FROM ANSYS Kte=zeros([1 length(R)]); S=[3244.185e5 4762.184e5 5844.532e5 6725.240e5]; for i=1:length(R) Kte(i)=S(i)/Pn(i); end 3.8 Codes 53 %% PLOT figure(1) plot(ratio,Ktn,ratio,Kte) legend('Kt Petersons','Kt ANSYS') title('Stress concentration factor at U-shape notch') xlabel('r/d') ylabel('Kt') figure(2) KCB=[2.4 2.9 3.4 3.7]; plot(hr,S./(P/((H-T)*h)), hr, KCB) legend('ANSYS', 'C&B aprox.') title('Cole & Brown') xlabel('h/r') ylabel('fm/P/(D-h)t') Code 3.2 matlab code to compare Pilkie’s expression for opposite U-shape notch with Peterson’s chart. rd=[0.1 0.15 0.2 0.25 0.3]; Hd=[1.05 1.10 1.15 1.2 1.3 1.5 2]; H=1; h=0.0254; B=0.3048; ratioSP=rd(1):0.01:rd(length(rd)); Ktn=zeros([length(rd) length(Hd)]); t=zeros([1 length(Hd)]); d=zeros([1 length(Hd)]); r=zeros([length(rd) length(Hd)]); for j=1:length(Hd) d(j)=H/Hd(j); t(j)=H-d(j); for i=1:length(rd) r(i,j)=d(j)*rd(i); if 0.1<=(t(j)/r(i,j))<2 C1=0.955+2.169*sqrt(t(j)/r(i,j))-0.081*t(j)/r(i,j); C2=-1.557-4.046*sqrt(t(j)/r(i,j))+1.032*t(j)/r(i,j); C3=4.013+0.424*sqrt(t(j)/r(i,j))-0.748*t(j)/r(i,j); C4=-2.461+1.538*sqrt(t(j)/r(i,j))-0.236*t(j)/r(i,j); end if 2<=(t(j)/r(i,j))<50 C1=1.037+1.991*sqrt(t(j)/r(i,j))+0.002*t(j)/r(i,j); C2=-1.886-2.181*sqrt(t(j)/r(i,j))-0.048*t(j)/r(i,j); C3=0.649+1.086*sqrt(t(j)/r(i,j))+0.142*t(j)/r(i,j); C4=1.218-0.922*sqrt(t(j)/r(i,j))-0.086*t(j)/r(i,j); end Ktn(i,j)=C1+C2*(2*t(j)/H)+C3*(2*t(j)/H)^2+C4*(2*t(j)/H)^3; end 54 Chapter 3. Stress concentration factors comparison end KTN=zeros([length(ratioSP) length(Hd)]); for j=1:length(Hd) KTN(:,j)=spline(rd,Ktn(:,j),ratioSP); end Peter(7,:)=[3.1 2.58 2.3 2.1 1.98]; Peter(6,:)=[2.9 2.46 2.2 2.02 1.91]; Peter(5,:)=[2.71 2.35 2.1 1.94 1.85]; Peter(4,:)=[2.55 2.17 1.96 1.85 1.77]; Peter(3,:)=[2.37 2.05 1.89 1.78 1.7]; Peter(2,:)=[2.15 1.9 1.76 1.69 1.64]; Peter(1,:)=[1.87 1.71 1.61 1.54 1.5]; KTP=zeros([length(ratioSP) length(Hd)]); for j=1:length(Hd) KTP(:,j)=spline(rd,Peter(j,:),ratioSP); end Muestra_Opposite=[KTN KTP]; Table_1 = table(ratioSP',Muestra_Opposite(:,1),Muestra_Opposite(:,2), Muestra_Opposite(:,3),Muestra_Opposite(:,4),Muestra_Opposite(:,5), Muestra_Opposite(:,6),Muestra_Opposite(:,7),Muestra_Opposite(:,8), Muestra_Opposite(:,9),Muestra_Opposite(:,10),Muestra_Opposite(:,12), Muestra_Opposite(:,12),Muestra_Opposite(:,13),Muestra_Opposite(:,14)); for j=1:7 plot(ratioSP,KTN(:,j),'b--'); hold on plot(ratioSP,KTP(:,j),'r'); hold on end xlabel('r/d') ylabel('Ktn') hold off Code 3.3 matlab code to compare Pilkie’s expression for single U-shape notch with Peterson’s chart. H=1; h=0.0254; B=0.3048; rd=[0.1 0.15 0.2 0.25 0.3]; Hds=[2 1.5 1.2 1.1]; ts=zeros([1 length(Hd)]); ds=zeros([1 length(Hd)]); rs=zeros([length(rd) length(Hd)]); Ktns=zeros([1 length(rd)]); for j=1:length(Hds) ds(j)=H/Hds(j); ts(j)=H-ds(j); for i=1:length(rd) 3.8 Codes 55 rs(i,j)=ds(j)*rd(i); if 0.5<=(ts(j)/rs(i,j))<2 C1=0.907+2.125*sqrt(ts(j)/rs(i,j))+0.023*ts(j)/rs(i,j); C2=0.710-11.289*sqrt(ts(j)/rs(i,j))+1.708*ts(j)/rs(i,j); C3=-0.672+18.754*sqrt(ts(j)/rs(i,j))-4.046*ts(j)/rs(i,j); C4=0.175-9.759*sqrt(ts(j)/rs(i,j))+2.365*ts(j)/rs(i,j); end if 2<=(t(j)/r(i,j))<20 C1=0.953+2.136*sqrt(ts(j)/rs(i,j))-0.005*ts(j)/rs(i,j); C2=-3.255-6.281*sqrt(ts(j)/rs(i,j))+0.068*ts(j)/rs(i,j); C3=8.203+6.893*sqrt(ts(j)/rs(i,j))+0.064*ts(j)/rs(i,j); C4=-4.851-2.793*sqrt(ts(j)/rs(i,j))-0.128*ts(j)/rs(i,j); end Ktns(i,j)=C1+C2*(ts(j)/H)+C3*(ts(j)/H)^2+C4*(ts(j)/H)^3; end end KTNS=zeros([length(ratioSP) length(Hds)]); for j=1:length(Hds) KTNS(:,j)=spline(rd,Ktns(:,j),ratioSP); end PeterS(4,:)=[2.53 2.18 1.97 1.84 1.75]; PeterS(3,:)=[2.53 2.18 1.97 1.84 1.75]; PeterS(2,:)=[2.50 2.16 1.95 1.81 1.72]; PeterS(1,:)=[2.42 2.10 1.90 1.77 1.69]; KTPS=zeros([length(ratioSP) length(Hds)]); for j=1:length(Hds) KTPS(:,j)=spline(rd,PeterS(j,:),ratioSP); end Muestra_Single=[KTNS KTPS]; Table_2 = table(ratioSP',Muestra_Single(:,1),Muestra_Single(:,2),Muestra_Single (:,3),Muestra_Single(:,4),Muestra_Single(:,5),Muestra_Single(:,6), Muestra_Single(:,7),Muestra_Single(:,8)); figure(2) for j=1:4 plot(ratioSP,KTNS(:,j),'b--'); hold on plot(ratioSP,KTPS(:,j),'r'); hold on end xlabel('r/d') ylabel('Ktn') Code 3.4 matlab code to compare Pilkie’s expression for single semicircular notch with Peterson’s chart. H=1; h=0.0254; 56 Chapter 3. Stress concentration factors comparison B=0.3048; rdcs=[0.01 0.05 0.1 0.15 0.2 0.25 0.3]; ratioSPS=rdcs(1):0.01:rdcs(length(rdcs)); Ktpcs=[3 2.72 2.43 2.14 1.94 1.82 1.74]; KTPCS=spline(rdcs,Ktpcs,ratioSPS); dcs=zeros([1 length(rdcs)]); tcs=zeros([1 length(rdcs)]); Ktcs=zeros([1 length(rdcs)]); for i=1:length(rdcs) dcs(i)=H/(1+rdcs(i)); tcs(i)=rdcs(i)*dcs(i); Ktcs(i)=3.065-8.87*(tcs(i)/H)+14.036*(tcs(i)/H)^2-7.219*(tcs(i)/H)^3; end KTCS=spline(rdcs,Ktcs,ratioSPS); Table_3=table(ratioSPS', KTPCS', KTCS'); figure(3) plot(ratioSPS', KTPCS',ratioSPS', KTCS') xlabel('r/d') ylabel('Ktn') legend('Peterson','Pilkie') Code 3.5 matlab code to compare Pilkie’s expression for opposite semicircular notch with Peterson’s chart. H=1; h=0.0254; B=0.3048; rdco=[0.01 0.05 0.1 0.15 0.2 0.25 0.3]; ratioSPO=rdco(1):0.01:rdco(length(rdco)); Ktpco=[3 2.79 2.55 2.35 2.17 2.05 1.97]; KTPCO=spline(rdco,Ktpco,ratioSPO); dco=zeros([1 length(rdco)]); tco=zeros([1 length(rdco)]); Ktco=zeros([1 length(rdco)]); for i=1:length(rdco) dco(i)=H/(1+rdco(i)); tco(i)=rdco(i)*dco(i); Ktco(i)=3.065-3.472*(2*tco(i)/H)+1.009*(2*tco(i)/H)^2+0.405*(tco(i)/H)^3; end KTCO=spline(rdco,Ktco,ratioSPO); Table_4=table(ratioSPO', KTPCO', KTCO'); figure(4) 3.8 Codes 57 plot(ratioSPO', KTPCO',ratioSPO', KTCO') xlabel('r/d') ylabel('Ktn') legend('Peterson','Pilkie') 4 Neuber and Molski-Glinka’s rules 4.1 Ramberg-Osgood relationship 1 In 1943, Ramberg and Osgood proposed a relationship between strain and strain for both, elastic and plastic zones, that could be summed in the same expression. Strain in the elastic zone is directly related with the Young’s modulus of the material, whilst, in the plastic zone, it presents an exponential expression that depends on two parameters, Hand n, that are estimated for every material. εe=σ E εp= ( σ H)1 n So, if we sum both of these strains, we get the Ramberg-Osgood expression ε=εe+εp ε=σ E+( σ H)1 n If we give values to the three parameters, E , H and n , and plot the expression, we obtain a single and smooth curve, Figure 4.1, which is not discontinuous at the yield point. 5·10−20.10.15 0.20.25 0.3 100 200 300 400 500 600 700 800 900 1,000 ε σ(MPa) Figure 4.1 Ramberg-Osgood expression curve. 1 The expressions showed in this section were taken from Mechanical Behavior of Materials. Engineering Methods for Deformation, Fracture and Fatigue. Fourth Ed. [9] 59 60 Chapter 4. Neuber and Molski-Glinka’s rules 4.2 Neuber’s rule 2 Neuber’s rule [ 11 ] is a mathematical relationship that relates nominal stress and strain with local stress and strain. The rule says that the product of nominal stresses and strains is proportional to the product of the local elastic plastic stresses and strains. Kσ·σn·Kσ·εn=σ·ε Some modifications can be made to this expression which allow to write it only in terms of nominal stress. We can assume the behavior of strain as pure elastic even though the real strain is above the yield point. Doing this, we obtain the following hyperbola expression σ ε =(Kσσn)2 E This relationship allow us to obtain the real local stress and strain from the nominal stress applied to the element and the Kσ produced by the notch. However, we need another expression to obtain both stress and strain, for this we use the Ramberg-Osgood expression that relates these two variables. If we obtain the point where these two curves intersect, Figure 4.2, we will obtain the real local stress and strain. Therefore, the equation system we have to solve is the following: σ ε =(Kσσn)2 E ε=σ E+( σ H)1 n Where E,Hand nare material properties. It can be proved that this intersection is unconditionally convergent, and so, we can apply a simple algorithm to solve this system. I’ll be using the algorithm published by Navarro [ 12 ], implemented in a matlab code (Code 4.1). 1234567 ·10−3 100 200 300 400 500 600 700 Intersection point ε σ(MPa) Neuber’s hyperbola Ramberg-Osgood curve Figure 4.2 Ramberg-Osgood curve intersection with Neuber’s hyperbola. 2Some of the information given in this section was taken from https://www.efatigue.com/ [10] 4.3 Molski-Glinka’s Rule 61 4.3 Molski-Glinka’s Rule In 1980, Molski and Glinka [ 13 ] published a similar relationship between stress and strain, but this time it was an energy-based method which also holds when localized plastic yielding occurred at the notch root. They claimed that their method predicts local strain more accurately than Neuber’s method. Molski-Glinka’s method always show lower values of real stress than the ones obtained by Neuber’s method. Molski-Glinka’s expression can be arranged as the following [13]. (Kσσn)2 2E=σ2 2E+σ n+1(σ H)1 n Just as with Neuber’s method, the equations in this case can also be solved with a simple algorithm very similar to that used for Neuber’s method [12] (Code 4.2). 4.4 Application of Neuber’s and Molski-Glinka’s rules to Finite Elements models The aim of this project is to obtain real stress and strain by applying these methods to FE models. Having already created and proved that the FE models work properly, the application of these methods is quite simple. For this I will be using again the software matlab. In Codes 4.1 and 4.2 appear two functions, NeuberSe and MolskiGlinkaSe, whose inputs are the material parameters E , H and n and a pseudo-stress, which is defined as σ∗ e=Kσσn and whose outputs are the real local stress and strain after having applied the previously mentioned unconditionally convergent algorithms. To use these functions, we only need to know the material parameters, the value of the applied load and the Kσ produced at the notch. The material parameters used in these project are shown in 4.1, but they can be easily changed in both ansys and matlab codes. Stress concentration factors have been calculated in previous sections and the applied load has always been 10 000 000 N. Due to some problems of convergence in elasto-plastic models, that appeared when using loads applied to the center line at the middle of the minimum section, I decided to only use distributed loads in this section. Table 4.1 Material parameters. Young’s modulus (E) 202 375 MPa Poisson’s coefficient (α) 0.3 Hardening coefficient (H) 1 283 MPa Hardening exponent (n) 0.211 I have made charts comparing Kσ produced at the notch in different situations, a pure elastic model, an elasto-plastic model and the results obtained from Neuber’s and Molski-Glinka’s algorithms taking as input the stress produced in the pure elastic model. As it was expected, pure elastic results are much greater than the elasto-plastic ones when the stress produced is beyond the yield point. If stress is so low that is under the yield point, both results are equal. As for Neuber’s and Molski-Glinka’s results, they are also always lower than the elasto-plastic Kσ and similar in value, Molski-Glinka being slightly lower than Neuber. Charts are presented in the following section and codes to apply algorithms and create these charts appear at section "Codes". An Index of these charts and codes is shown in Table 4.2 4.5 Application of Neuber’s and Moslki-Glinka’s rules to elements with different thickness Just as they have been applied in the previous sections, Neuber’s and Moslki-Glinka’s rules have been applied to the models mentioned in Section 3.6. The results are shown in Figure 4.11 and Figure 4.12. In this chart we can see the difference between Neuber’s and Molski-Glinka’s results and the values obtained from elasto-plastic models. They show an almost straight line at a 45 degree angle, which means that values obtained from the mentioned methods compared to the ones obtained from elasto-plastic models are very 68 Chapter 4. Neuber and Molski-Glinka’s rules 123456789 1 2 3 4 t/r Kσ Elasto-plastic Neuber’s Rule Molski-Ginka’s Rule Figure 4.7 Comparison between Kσ from elastic and elasto-plastic models and values from Neuber’s and Molski-Glinka’s methods in single U-shaped notched plates with t/H=0.1. 4.6 Charts 69 1234567 8 9 1 2 3 4 t/r Kσ Elasto-plastic Neuber’s Rule Molski-Ginka’s Rule Figure 4.8 Comparison between Kσ from elastic and elasto-plastic models and values from Neuber’s and Molski-Glinka’s methods in single U-shaped notched plates with t/H=0.05. 70 Chapter 4. Neuber and Molski-Glinka’s rules 0.1 0.2 0.3 0.40.5 1 2 3 r/d Kσ Elasto-plastic Neuber’s Rule Molski-Ginka’s Rule Figure 4.9 Comparison between Kσ from elastic and elasto-plastic models and values from Neuber’s and Molski-Glinka’s methods in opposite semicircular notched plates. 4.6 Charts 71 5·10−20.10.15 0.20.25 0.30.35 1 1.5 2 2.5 3 r/d Kσ Elasto-plastic Neuber’s Rule Molski-Ginka’s Rule Figure 4.10 Comparison between Kσ from elastic and elasto-plastic models and values from Neuber’s and Molski-Glinka’s methods in single semicircular notched plates. 72 Chapter 4. Neuber and Molski-Glinka’s rules 234567 8 9 10 11 12 13 14 15 16 17 18 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 KσElasto −plastic KσNeuber H/h=10 H/h=4 H/h=2 H/h=1 Figure 4.11 Comparison between Kσ obtained from elasto-plastic models and Neuber’s method from plates with different thickness. 234567 8 9 10 11 12 13 14 15 16 17 18 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 KσElasto −plastic KσMolski −Glinka H/h=10 H/h=4 H/h=2 H/h=1 Figure 4.12 Comparison between Kσ obtained from elasto-plastic models and Molski-Glinka’s method from plates with different thickness. 4.6 Charts 73 67 8 9 10 11 12 13 14 15 16 17 18 19 20 21 22 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20 21 22 KεElasto −plastic KεNeuber H/h=10 H/h=4 H/h=2 H/h=1 Figure 4.13 Comparison between Kε obtained from elasto-plastic models and Neuber’s method from plates with different thickness. 67 8 9 10 11 12 13 14 15 16 17 18 19 20 21 22 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20 21 22 KεElasto −plastic KεMolski −Glinka H/h=10 H/h=4 H/h=2 H/h=1 Figure 4.14 Comparison between Kε obtained from elasto-plastic models and Molski-Glinka’s method from plates with different thickness. 74 Chapter 4. Neuber and Molski-Glinka’s rules 4.7 Codes Code 4.1 matlab implementation for Neuber’s method algorithm. function [ S, e ] = NeuberSe( E, n, K, Se ) %[ S, e ] = NeuberSe( E, n, K, Se ) % Given E, n, K and a Pseudostress (Se = Kt*Sn), NeuberSe calculates real Stress % and Strain in a notched piece intersecting Neuber's Hyperbola and Ramberg- Osgood function. tol=1.0; Lc=((2*n)/(n+1))*((3*n+1)/(n+1))^((1-n)/(2*n)); Bc=sqrt((n+1)/(3*n+1)); L=(E/Se)*(Se/K)^(1/n); if Lc==L B=Bc; elseif L<Lc Bo=Bc; Bi=sqrt(1-L*Bo^(1/n+1)); while abs((Bo-Bi)/Bo)*100>tol Bo=Bi; Bi=sqrt(1-L*Bo^(1/n+1)); end B=Bi; else Bo=Bc; Bi=((1-Bo^2)/L)^(n/(n+1)); while abs((Bo-Bi)/Bo)*100>tol Bo=Bi; Bi=((1-Bo^2)/L)^(n/(n+1)); end B=Bi; end S=B*Se; e=S/E+(S/K)^(1/n); end Code 4.2 matlab implementation for Molski-Glinka’s method algorithm. function [ S, e ] = MolskiGlinkaSe( E, n, K, Se ) %[ S, e ] = MolskiGlinkaSe( E, n, K, Se ) % Given E, n, K and a Pseudostress (Se = Kt*Sn), MolskiGlinkaSe calculates real Stress % and Strain in a notched piece according to Molski-Glinka's rule. tol=1.0; 4.7 Codes 75 Lc=((2*n)/(n+1))*((3*n+1)/(n+1))^((1-n)/(2*n)); Bc=sqrt((n+1)/(3*n+1)); L=2/(n+1)*E/Se*(Se/K)^(1/n); if Lc==L B=Bc; elseif L<Lc Bo=Bc; Bi=sqrt(1-L*Bo^(1/n+1)); while abs((Bo-Bi)/Bo)*100>tol Bo=Bi; Bi=sqrt(1-L*Bo^(1/n+1)); end B=Bi; else Bo=Bc; Bi=((1-Bo^2)/L)^(n/(n+1)); while abs((Bo-Bi)/Bo)*100>tol Bo=Bi; Bi=((1-Bo^2)/L)^(n/(n+1)); end B=Bi; end S=B*Se; e=S/E+(S/K)^(1/n); end Code 4.3 matlab implementation for Neuber’s and Molski-Glinka’s methods algorithms for opposite U-shape notched plates. clear close all clc E=202375e6; n=0.211; K=1283e6; H=1; % ANCHO h=0.05; % PROFUNDIDAD P=4e6; % Carga B=0.3048; T30=0.3*H; T10=0.1*H; T05=0.05*H; hr=[1.1 2.1 3.1 4.1 5.1 6.1 7.1 8.1 9.1]; R30=T30./hr; R10=T10./hr; R05=T05./hr; 76 Chapter 4. Neuber and Molski-Glinka’s rules d=zeros([1 length(hr)]); ratio30=zeros([1 length(hr)]); ratio10=zeros([1 length(hr)]); ratio05=zeros([1 length(hr)]); Pn=zeros([1 length(hr)]); for i=1:length(hr) ratio30(i)=T30/R30(i); ratio10(i)=T10/R10(i); ratio05(i)=T05/R05(i); Pn(i)=P/(h*H); end %% PS30 DATOS_PLANE_STRESS_30 = load('OPPOSITE_PLANE_STRESS/PS_30/DATOS.dat'); Sps30=DATOS_PLANE_STRESS_30'; Ktps30=zeros([1 length(hr)]); for i=1:length(hr) Ktps30(i)=Sps30(i)/Pn(i); end ratiofinoPS30=ratio30(1):0.01:ratio30(length(ratio30)); KTPS30=spline(ratio30,Ktps30,ratiofinoPS30); KTPS30_FIT=fit(ratio30',Ktps30','smoothingspline'); %% PS10 DATOS_PLANE_STRESS_10 = load('OPPOSITE_PLANE_STRESS/PS_10/DATOS.dat'); Sps10=DATOS_PLANE_STRESS_10'; Ktps10=zeros([1 length(hr)]); for i=1:length(hr) Ktps10(i)=Sps10(i)/Pn(i); end ratiofinoPS10=ratio10(1):0.01:ratio10(length(ratio10)); KTPS10=spline(ratio10,Ktps10,ratiofinoPS10); KTPS10_FIT=fit(ratio10',Ktps10','smoothingspline'); %% PLASTICITY 30 DATOS_PLAS_30 = load('OPPOSITE_PLASTICITY/PLAS_30/DATOS.dat'); S_PLAS_30=DATOS_PLAS_30'; Kt_PLAS_30=zeros([1 length(hr)]); for i=1:length(hr) Kt_PLAS_30(i)=S_PLAS_30(i)/Pn(i); end KT_PLAS_30=spline(ratio30,Kt_PLAS_30,ratiofinoPS30); KT_PLAS_30_FIT=fit(ratio30',Kt_PLAS_30','smoothingspline'); 4.7 Codes 77 %% PLASTICITY 10 DATOS_PLAS_10 = load('OPPOSITE_PLASTICITY/PLAS_10/DATOS.dat'); S_PLAS_10=DATOS_PLAS_10'; Kt_PLAS_10=zeros([1 length(hr)]); for i=1:length(hr) Kt_PLAS_10(i)=S_PLAS_10(i)/Pn(i); end KT_PLAS_10=spline(ratio10,Kt_PLAS_10,ratiofinoPS10); KT_PLAS_10_FIT=fit(ratio10',Ktps10','smoothingspline'); %% RESULTADOS NEUBER 30 Kt_neu_30=zeros([1 length(hr)]); for i=1:length(hr) [ Sn, en ] = NeuberSe( E, n, K, S_PLAS_30(i) ); Kt_neu_30(i)=Sn/Pn(i); end KT_NEU_30=spline(ratio30,Kt_neu_30,ratiofinoPS30); KT_NEU_30_FIT=fit(ratio30',Kt_neu_30','smoothingspline'); %% RESULTADOS NEUBER 10 Kt_neu_10=zeros([1 length(hr)]); for i=1:length(hr) [ Sn, en ] = NeuberSe( E, n, K, S_PLAS_10(i) ); Kt_neu_10(i)=Sn/Pn(i); end KT_NEU_10=spline(ratio10,Kt_neu_10,ratiofinoPS10); KT_NEU_10_FIT=fit(ratio10',Kt_neu_10','smoothingspline'); %% MOLSKI-GLINKA 30 Kt_mg_30=zeros([1 length(hr)]); for i=1:length(hr) [ Smg, emg ] = MolskiGlinkaSe( E, n, K, S_PLAS_30(i) ); Kt_mg_30(i)=Smg/Pn(i); end KT_MG_30=spline(ratio30,Kt_mg_30,ratiofinoPS30); KT_MG_30_FIT=fit(ratio30',Kt_mg_30','smoothingspline'); %% PLOT figure(1) plot(KTPS30_FIT,'b') hold on plot(KT_PLAS_30_FIT,'g--') hold on plot(KT_NEU_30_FIT,'r-.') 84 Chapter 4. Neuber and Molski-Glinka’s rules DATOS_PLANE_STRESS_PLAS = load('SEMICIRCULAR_OPPOSITE_PLASTICITY/DATOS.dat'); S_PLAS=DATOS_PLANE_STRESS_PLAS'; Ktps_plas=zeros([1 length(R)]); for i=1:length(R) Ktps_plas(i)=S_PLAS(i)/Pn; end KT_PLAS=polyval(polyfit(rd,Ktps_plas,3),ratiofino); %% NEUBER Kt_neu=zeros([1 length(rd)]); for i=1:length(rd) [ Sn, en ] = NeuberSe( E, n, K, S_PLAS(i) ); Kt_neu(i)=Sn/Pn; end KT_NEU=polyval(polyfit(ratio,Kt_neu,3),ratiofino); %% MOLSKI-GLINKA Kt_mg=zeros([1 length(rd)]); for i=1:length(rd) [ Smg, emg ] = MolskiGlinkaSe( E, n, K, S_PLAS(i) ); Kt_mg(i)=Smg/Pn; end KT_MG=polyval(polyfit(rd,Kt_mg,3),ratiofino); %% PLOT figure(1) plot(ratiofino,KTPS_FIT_DIST,'b') hold on plot(ratiofino,KT_PLAS,'g-.') hold on plot(ratiofino,KT_NEU,'r--') hold on plot(ratiofino,KT_MG,'m--') xlabel('r/d') ylabel('Kt') axis([0 0.5 1 4]) legend('Plane Stress (Pure Elastic)','Elasto-plastic','Neuber','Molski-Glinka') grid on grid minor Code 4.6 matlab implementation for Neuber’s and Molski-Glinka’s methods algorithms for single semicircular notched plates. clear close all clc E=202375000000; 4.7 Codes 85 n=0.211; K=1283e6; H=2; % ANCHO h=0.05; % PROFUNDIDAD P=10000000; % Carga Pn=P/(H*h); B=5; DIV=[2,2.5,3,3.5,4,4.5,5,5.5,6,6.5,7,7.5,8,8.5,9,9.5,10]; R=(H/2)./DIV; d=H-R; Pnd=P./(d*h); rd=R./d; ratio=rd; ratiofino=rd(length(rd)):0.01:rd(1); %% ANSYS SINGLE DIST DATOS_PLANE_STRESS_DIST = load('SEMICIRCULAR_SINGLE_DIST/DATOS.dat'); Sps_dist=DATOS_PLANE_STRESS_DIST'; Ktps_dist=zeros([1 length(R)]); for i=1:length(R) Ktps_dist(i)=Sps_dist(i)/Pn; end KTPS_FIT_DIST=polyval(polyfit(rd,Ktps_dist,3),ratiofino); %% ANSYS SINGLE PLASTICITY DATOS_PLANE_STRESS_PLAS = load('SEMICIRCULAR_SINGLE_PLASTICITY/DATOS.dat'); S_PLAS=DATOS_PLANE_STRESS_PLAS'; Ktps_plas=zeros([1 length(R)]); for i=1:length(R) Ktps_plas(i)=S_PLAS(i)/Pn; end KT_PLAS=polyval(polyfit(rd,Ktps_plas,3),ratiofino); %% NEUBER Kt_neu=zeros([1 length(rd)]); for i=1:length(rd) [ Sn, en ] = NeuberSe( E, n, K, S_PLAS(i) ); Kt_neu(i)=Sn/Pn; end KT_NEU=polyval(polyfit(ratio,Kt_neu,3),ratiofino); %% MOLSKI-GLINKA Kt_mg=zeros([1 length(rd)]); for i=1:length(rd) [ Smg, emg ] = MolskiGlinkaSe( E, n, K, S_PLAS(i) ); 86 Chapter 4. Neuber and Molski-Glinka’s rules Kt_mg(i)=Smg/Pn; end KT_MG=polyval(polyfit(rd,Kt_mg,3),ratiofino); %% PLOT figure(1) plot(ratiofino,KTPS_FIT_DIST,'b') hold on plot(ratiofino,KT_PLAS,'g-.') hold on plot(ratiofino,KT_NEU,'r--') hold on plot(ratiofino,KT_MG,'m--') xlabel('r/d') ylabel('Kt') axis([0.05 0.35 2 5]) legend('Plane Stress (Pure Elastic)','Elasto-plastic','Neuber','Molski-Glinka') grid on grid minor 5 Conclusions The Finite Elements models created in this project have been compared with experimental and theoretical data from various authors in order to provide reliable results. This reliability allow us to easily modify the parameters that define these models and to obtain useful data from an infinity of different geometries and materials, avoiding the need of expensive laboratory studies. This gives this project a lot of potential, being a more ambitious goal of creating a big database including several different geometries of diverse materials. This could be the starting point for future end-of-degree or research projects that can use these texts and codes as a guide to expand the database. The goal of applying Neuber’s and Molski-Glinka’s rules to the data obtained from the Finite Elements models has been fulfilled having set a particular file structure to create an output file with the data obtained from ansys, where several loop codes have been implemented to ease the job, to input in matlab where Kσ have been calculated and convergence algorithms have been implemented to apply the mentioned rules. The goals that have not been achieved are to create a reliable solid model for very thin plates and to create a convergent elasto-plastic model with a load applied in a line at the center of the minimum section. Regarding the data obtained from the analysis that have been carried out in this project, we can get the following conclusions: 1. The effect of the notch’s depth is increased when it is bigger than recommended, a distance at least 3 times it’s depth to the end of the plate. 2. Plates with a ratio H/hlower or close to 2 can be considered as to be in Plane Strain. 3. Neuber’s and Molski-Glinka’s methods adapt well for stresses and strains in all range of thicknesses, giving very similar values to the ones obtained from elasto-plastic models. 4. Considering Kσ based on the gross section, Neuber’s and Molski-Glinka’s methods are generally less conservative than the results obtained from elasto-plastic models. 87 List of Figures 1.1 Stress flow lines perturbed by alteration in geometry 1 1.2 Stress distribution in a thin metal sheet with a hole in the center. Image from Peterson’s Stress Concentration Factors, Third Edition. [1] 2 1.3 Chart representing Kσproduced in an elliptical notch. Image from Peterson’s Stress Concentration Factors, Third Edition. [1] 3 2.1 Single U-Shape notched plate. Original image taken from Peterson’s Stress Concentration Factors, Third Edition [1] 5 2.2 Opposite U-Shape notched plate. Original image taken from Peterson’s Stress Concentration Factors, Third Edition [1] 5 2.3 Load distribution along a line at the center of the minimum section 6 2.4 Applying symmetry 7 2.5 Lines that define the area of the desired geometry 8 2.6 Loads applied at nodes situated on the line at the center of the minimum section 8 2.7 Mesh refined at notch 9 2.8 Constraints at the corner of the minimum section with the unnotched face 9 2.9 Stress distribution along the notch’s peak 10 2.10 Stress distribution along the center of the minimum section 10 2.11 Applying symmetry to double symmetrical geometry 19 2.12 Stress distributions along the notch’s peak with a "thin" width 29 2.13 Stress distributions along the minimum section with a "short" height 29 2.14 High stress produced in the line of application of loads 30 2.15 Constraints at the corner of the minimum section with the unnotched face. Whole line 31 2.16 Constraints at the corner of the minimum section with the unnotched face. Just one node 31 3.1 Stress concentration factors for a flat tension plate with opposite U-shape notches. Image from Peterson’s Stress Concentration Factors, Third Edition. [1] 34 3.2 Chart from Baratta & Neal article [3] 35 3.3 Chart from Ling’s article [6] 35 3.4 Comparison between Kσat an U-shape notch in one side of a flat tension plate taken from different methods 38 3.5 Comparison between Kσat an U-shape notch in one side of a flat tension plate taken from different methods 39 3.6 Comparison between Kσin an opposite U-shaped notched plate 40 3.7 Comparison between Kσin a single U-shaped notched plate 41 3.8 Comparison between Kσin an opposite semicircular notched plate 42 3.9 Comparison between Kσin an opposite semicircular notched plate with a uniform load and a load applied at the center of the minimum section 43 3.10 Comparison between Kσin a single semicircular notched plate 44 3.11 Comparison between Kσin a single semicircular notched plate with a uniform load and a load applied at the center of the minimum section 45 89 90 List of Figures 3.12 Comparison between Kσat a single U-shape notch obtained by Peterson (in red) and values from Pilkie’s interpolation expression (in blue) 47 3.13 Comparison between Kσat a opposite U-shape notch obtained by Peterson (in red) and values from Pilkie’s interpolation expression (in blue) 48 3.14 Comparison between Kσat a single semicircular notch obtained by Peterson (in red) and values from Pilkie’s interpolation expression (in blue) 49 3.15 Comparison between Kσat a opposite semicircular notch obtained by Peterson (in red) and values from Pilkie’s interpolation expression (in blue) 50 3.16 Comparison between Kσat a U-shaped notch in one side of a flat tension plate with different thickness 51 4.1 Ramberg-Osgood expression curve 59 4.2 Ramberg-Osgood curve intersection with Neuber’s hyperbola 60 4.3 Comparison between Kσfrom elastic and elasto-plastic models and values from Neuber’s and Molski-Glinka’s methods in opposite U-shaped notched plates with t/H=0.15 63 4.4 Comparison between Kσfrom elastic and elasto-plastic models and values from Neuber’s and Molski-Glinka’s methods in opposite U-shaped notched plates with t/H=0.05 65 4.5 Comparison between Kσfrom elastic and elasto-plastic models and values from Neuber’s and Molski-Glinka’s methods in opposite U-shaped notched plates with t/H=0.025 66 4.6 Comparison between Kσfrom elastic and elasto-plastic models and values from Neuber’s and Molski-Glinka’s methods in single U-shaped notched plates with t/H=0.367 4.7 Comparison between Kσfrom elastic and elasto-plastic models and values from Neuber’s and Molski-Glinka’s methods in single U-shaped notched plates with t/H=0.168 4.8 Comparison between Kσfrom elastic and elasto-plastic models and values from Neuber’s and Molski-Glinka’s methods in single U-shaped notched plates with t/H=0.05 69 4.9 Comparison between Kσfrom elastic and elasto-plastic models and values from Neuber’s and Molski-Glinka’s methods in opposite semicircular notched plates 70 4.10 Comparison between Kσfrom elastic and elasto-plastic models and values from Neuber’s and Molski-Glinka’s methods in single semicircular notched plates 71 4.11 Comparison between Kσobtained from elasto-plastic models and Neuber’s method from plates with different thickness 72 4.12 Comparison between Kσobtained from elasto-plastic models and Molski-Glinka’s method from plates with different thickness 72 4.13 Comparison between Kεobtained from elasto-plastic models and Neuber’s method from plates with different thickness 73 4.14 Comparison between Kεobtained from elasto-plastic models and Molski-Glinka’s method from plates with different thickness 73 List of Tables 3.1 Error table for Pilkie’s interpolation of opposite U-shaped notches 36 3.2 Error table for Pilkie’s interpolation of single U-shaped notches 36 3.3 Interpolation expressions for Opposite U-shaped notches 37 3.4 Interpolation expressions for single U-shaped notches 37 4.1 Material parameters 61 4.2 Chart index 62 91 Listings 2.1 Parameters in ANSYS 12 2.2 Loop in ANSYS 12 2.3 Material properties for solid body model 12 2.4 Material properties for plane stress model 12 2.5 Material properties for plane stress model 13 2.6 Geometry with SOLID186 13 2.7 Geometry with PLANE182 14 2.8 Meshing, loads and constraints in solid model 15 2.9 Refining for complete volume 16 2.10 Refining for complete area 16 2.11 Distributed load in solid model 17 2.12 Distributed load in plane stress model 17 2.13 Solve 17 2.14 Code to create a path along the notch’s peak 17 2.15 Code to create a path along the center of the minimum section 17 2.16 Code to create a macro to write array of results 17 2.17 Code to get the maximum stress in the Y direction of the last path plotted and use macro 18 2.18 Complete code for solid body opposite U-shape notched plate 19 2.19 Complete code for plane stress opposite U-shape notched plate 23 2.20 Code to create the initial unextruded area for the semicircular notch case 27 2.21 Code to introduce elasto-plastic material properties 28 3.1 MATLAB code to calculate stress concentration factor in different models 52 3.2 MATLAB code to compare Pilkie’s expression for opposite U-shape notch with Peterson’s chart 53 3.3 MATLAB code to compare Pilkie’s expression for single U-shape notch with Peterson’s chart 54 3.4 MATLAB code to compare Pilkie’s expression for single semicircular notch with Peterson’s chart 55 3.5 MATLAB code to compare Pilkie’s expression for opposite semicircular notch with Peterson’s chart 56 4.1 MATLAB implementation for Neuber’s method algorithm 74 4.2 MATLAB implementation for Molski-Glinka’s method algorithm 74 4.3 MATLAB implementation for Neuber’s and Molski-Glinka’s methods algorithms for opposite U-shape notched plates 75 4.4 MATLAB implementation for Neuber’s and Molski-Glinka’s methods algorithms for single U-shape notched plates 78 4.5 MATLAB implementation for Neuber’s and Molski-Glinka’s methods algorithms for opposite semicircular notched plates 83 4.6 MATLAB implementation for Neuber’s and Molski-Glinka’s methods algorithms for single semicircular notched plates 84 93