2.2 Stress analysis of a plate with a hole

This tutorial describes how to pre-process, run and post-process a case involving linear-elastic, steady-state stress analysis on a square plate with a circular hole at its centre. The plate dimensions are: side length 4 eqn and radius eqn 0.5 eqn. It is loaded with a uniform traction of eqn 10  eqneqn over its left and right faces as shown in Figure 2.16 . Two symmetry planes can be identified for this geometry and therefore the solution domain need only cover a quarter of the geometry, shown by the shaded area in Figure 2.16 .


 y σ=10kPa σ = 10 kPa symmetry plane x R = 0.5 m symmetry plane 4.0 m \relax \special {t4ht=


Figure 2.16: Geometry of the plate with a hole.


The problem can be approximated as 2-dimensional since the load is applied in the plane of the plate. In a Cartesian coordinate system there are two possible assumptions to take in regard to the behaviour of the structure in the third dimension: (1) the plane stress condition, in which the stress components acting out of the 2D plane are assumed to be negligible; (2) the plane strain condition, in which the strain components out of the 2D plane are assumed negligible. The plane stress condition is appropriate for solids whose third dimension is thin as in this case; the plane strain condition is applicable for solids where the third dimension is thick.

An analytical solution exists for loading of an infinitely large, thin plate with a circular hole. The solution for the stress normal to the vertical plane of symmetry is

 ( ( ) { R2-- 3R4- (σxx ) = σ 1 + 2y2 + 2y4 for |y| ≥ R x=0 ( 0 for |y| < R \relax \special {t4ht=
(2.14)
Results from the simulation will be compared with this solution. At the end of the tutorial, the user can: investigate the sensitivity of the solution to mesh resolution and mesh grading; and, increase the size of the plate in comparison to the hole to try to estimate the error in comparing the analytical solution for an infinite plate to the solution of this problem of a finite plate.

2.2.1 Mesh generation

The domain consists of four blocks, some of which have arc-shaped edges. The block structure for the part of the mesh in the eqn plane is shown in Figure 2.17. As already mentioned in section 2.1.1.1 , all geometries are generated in 3 dimensions in OpenFOAM even if the case is to be as a 2 dimensional problem. Therefore a dimension of the block in the eqn direction has to be chosen; here, 0.5 eqn is selected. It does not affect the solution since the traction boundary condition is specified as a stress rather than a force, thereby making the solution independent of the cross-sectional area.


 up 7 up 8 6 left 4 3 right x 2 9 x1 x2 left 0 4 3 x1 10 x2 x1 2 right 5 1 hole y x2 x2 x 0 x1 1 x1 down 2 down \relax \special {t4ht=


Figure 2.17: Block structure of the mesh for the plate with a hole.


The user should change to the run directory and copy the plateHole case into it from the $FOAM_TUTORIALS/stressAnalysis/solidDisplacementFoam directory. The user should then go into the plateHole directory and open the blockMeshDict file in an editor, as listed below

16convertToMeters 1;
17
18vertices
19(
20    (0.5 0 0)
21    (1 0 0)
22    (2 0 0)
23    (2 0.707107 0)
24    (0.707107 0.707107 0)
25    (0.353553 0.353553 0)
26    (2 2 0)
27    (0.707107 2 0)
28    (0 2 0)
29    (0 1 0)
30    (0 0.5 0)
31    (0.5 0 0.5)
32    (1 0 0.5)
33    (2 0 0.5)
34    (2 0.707107 0.5)
35    (0.707107 0.707107 0.5)
36    (0.353553 0.353553 0.5)
37    (2 2 0.5)
38    (0.707107 2 0.5)
39    (0 2 0.5)
40    (0 1 0.5)
41    (0 0.5 0.5)
42);
43
44blocks
45(
46    hex (5 4 9 10 16 15 20 21) (10 10 1) simpleGrading (1 1 1)
47    hex (0 1 4 5 11 12 15 16) (10 10 1) simpleGrading (1 1 1)
48    hex (1 2 3 4 12 13 14 15) (20 10 1) simpleGrading (1 1 1)
49    hex (4 3 6 7 15 14 17 18) (20 20 1) simpleGrading (1 1 1)
50    hex (9 4 7 8 20 15 18 19) (10 20 1) simpleGrading (1 1 1)
51);
52
53edges
54(
55    arc 0 5 (0.469846 0.17101 0)
56    arc 5 10 (0.17101 0.469846 0)
57    arc 1 4 (0.939693 0.34202 0)
58    arc 4 9 (0.34202 0.939693 0)
59    arc 11 16 (0.469846 0.17101 0.5)
60    arc 16 21 (0.17101 0.469846 0.5)
61    arc 12 15 (0.939693 0.34202 0.5)
62    arc 15 20 (0.34202 0.939693 0.5)
63);
64
65boundary
66(
67    left
68    {
69        type symmetryPlane;
70        faces
71        (
72            (8 9 20 19)
73            (9 10 21 20)
74        );
75    }
76    right
77    {
78        type patch;
79        faces
80        (
81            (2 3 14 13)
82            (3 6 17 14)
83        );
84    }
85    down
86    {
87        type symmetryPlane;
88        faces
89        (
90            (0 1 12 11)
91            (1 2 13 12)
92        );
93    }
94    up
95    {
96        type patch;
97        faces
98        (
99            (7 8 19 18)
100            (6 7 18 17)
101        );
102    }
103    hole
104    {
105        type patch;
106        faces
107        (
108            (10 5 16 21)
109            (5 0 11 16)
110        );
111    }
112    frontAndBack
113    {
114        type empty;
115        faces
116        (
117            (10 9 4 5)
118            (5 4 1 0)
119            (1 4 3 2)
120            (4 7 6 3)
121            (4 9 8 7)
122            (21 16 15 20)
123            (16 11 12 15)
124            (12 13 14 15)
125            (15 14 17 18)
126            (15 18 19 20)
127        );
128    }
129);
130
131
132// ************************************************************************* //

Until now, we have only specified straight edges in the geometries of previous tutorials but here we need to specify curved edges. These are specified under the edges keyword entry which is a list of non-straight edges. The syntax of each list entry begins with the type of curve, including arc, simpleSpline, polyLine etc., described further in section 5.3.1 . In this example, all the edges are circular and so can be specified by the arc keyword entry. The following entries are the labels of the start and end vertices of the arc and a point vector through which the circular arc passes.

The blocks in this blockMeshDict do not all have the same orientation. As can be seen in Figure 2.17 the eqn direction of block 0 is equivalent to the eqn direction for block 4. This means care must be taken when defining the number and distribution of cells in each block so that the cells match up at the block faces.

6 patches are defined: one for each side of the plate, one for the hole and one for the front and back planes. The left and down patches are both a symmetry plane. Since this is a geometric constraint, it is included in the definition of the mesh, rather than being purely a specification on the boundary condition of the fields. Therefore they are defined as such using a special symmetryPlane type as shown in the blockMeshDict.

The frontAndBack patch represents the plane which is ignored in a 2D case. Again this is a geometric constraint so is defined within the mesh, using the empty type as shown in the blockMeshDict. For further details of boundary types and geometric constraints, the user should refer to section 5.2 .

The remaining patches are of the regular patch type. The mesh should be generated using blockMesh and can be viewed in paraFoam as described in section 2.1.2 . It should appear as in Figure 2.18 .


 \relax \special {t4ht=


Figure 2.18: Mesh of the hole in a plate problem.


2.2.1.1 Boundary and initial conditions

Once the mesh generation is complete, the initial field with boundary conditions must be set. For a stress analysis case without thermal stresses, only displacement D needs to be set. The 0/D is as follows:

16dimensions      [0 1 0 0 0 0 0];
17
18internalField   uniform (0 0 0);
19
20boundaryField
21{
22    left
23    {
24        type            symmetryPlane;
25    }
26    right
27    {
28        type            tractionDisplacement;
29        traction        uniform (10000 0 0);
30        pressure        uniform 0;
31        value           uniform (0 0 0);
32    }
33    down
34    {
35        type            symmetryPlane;
36    }
37    up
38    {
39        type            tractionDisplacement;
40        traction        uniform (0 0 0);
41        pressure        uniform 0;
42        value           uniform (0 0 0);
43    }
44    hole
45    {
46        type            tractionDisplacement;
47        traction        uniform (0 0 0);
48        pressure        uniform 0;
49        value           uniform (0 0 0);
50    }
51    frontAndBack
52    {
53        type            empty;
54    }
55}
56
57// ************************************************************************* //

Firstly, it can be seen that the displacement initial conditions are set to eqn eqn. The left and down patches must be both of symmetryPlane type since they are specified as such in the mesh description in the constant/polyMesh/boundary file. Similarly the frontAndBack patch is declared empty.

The other patches are traction boundary conditions, set by a specialist traction boundary type. The traction boundary conditions are specified by a linear combination of: (1) a boundary traction vector under keyword traction; (2) a pressure that produces a traction normal to the boundary surface that is defined as negative when pointing out of the surface, under keyword pressure. The up and hole patches are zero traction so the boundary traction and pressure are set to zero. For the right patch the traction should be eqn eqn and the pressure should be 0 eqn.

2.2.1.2 Physical properties

The physical properties for the case are set in the physicalProperties dictionary in the constant directory, shown below:

16
17rho
18{
19    type        uniform;
20    value       7854;
21}
22
23nu
24{
25    type        uniform;
26    value       0.3;
27}
28
29E
30{
31    type        uniform;
32    value       2e+11;
33}
34
35Cp
36{
37    type        uniform;
38    value       434;
39}
40
41kappa
42{
43    type        uniform;
44    value       60.5;
45}
46
47alphav
48{
49    type        uniform;
50    value       1.1e-05;
51}
52
53planeStress     yes;
54thermalStress   no;
55
56
57// ************************************************************************* //

The file includes mechanical properties of steel:

  • Density rho = 7854 eqn
  • Young’s modulus E = eqn eqn
  • Poisson’s ratio nu = 0.3

The planeStress switch is set to yes to adopt the plane stress assumption in this 2D case. The solidDisplacementFoam solver may optionally solve a thermal equation that is coupled with the momentum equation through the thermal stresses that are generated. The user specifies at run time whether OpenFOAM should solve the thermal equation by the thermalStress switch (currently set to no). The thermal properties are also specified for steel for this case, i.e.:

  • Specific heat capacity Cp = 434 eqneqneqn
  • Thermal conductivity kappa = 60.5 eqneqneqn
  • Thermal expansion coefficient alphav = eqn eqn

For thermal calculations, the temperature field variable T is present in the 0 directory.

2.2.1.3 Control

As before, the information relating to the control of the solution procedure are read in from the controlDict dictionary. For this case, the startTime is 0 eqn. The time step is not important since this is a steady state case; in this situation it is best to set the time step deltaT to 1 so it simply acts as an iteration counter for the steady-state case. The endTime, set to 100, then acts as a limit on the number of iterations. The writeInterval can be set to eqn.

The controlDict entries are as follows:

16
17application     solidDisplacementFoam;
18
19startFrom       startTime;
20
21startTime       0;
22
23stopAt          endTime;
24
25endTime         100;
26
27deltaT          1;
28
29writeControl    timeStep;
30
31writeInterval   20;
32
33purgeWrite      0;
34
35writeFormat     ascii;
36
37writePrecision  6;
38
39writeCompression off;
40
41timeFormat      general;
42
43timePrecision   6;
44
45graphFormat     raw;
46
47runTimeModifiable true;
48
49
50// ************************************************************************* //

2.2.1.4 Discretisation schemes and linear-solver control

Let us turn our attention to the fvSchemes dictionary. Firstly, the problem we are analysing is steady-state so the user should select SteadyState for the time derivatives in timeScheme. This essentially switches off the time derivative terms. Not all solvers, especially in fluid dynamics, work for both steady-state and transient problems but solidDisplacementFoam does work, since the base algorithm is the same for both types of simulation.

The momentum equation in linear-elastic stress analysis includes several explicit terms containing the gradient of displacement. The calculations benefit from accurate and smooth evaluation of the gradient. Normally, in the finite volume method the discretisation is based on Gauss’s theorem. The Gauss method is sufficiently accurate for most purposes but, in this case, the least squares method will be used. The user should therefore open the fvSchemes dictionary in the system directory and ensure the leastSquares method is selected for the grad(U) gradient discretisation scheme in the gradSchemes sub-dictionary:

16
17d2dt2Schemes
18{
19    default         steadyState;
20}
21
22ddtSchemes
23{
24    default         Euler;
25}
26
27gradSchemes
28{
29    default         leastSquares;
30    grad(D)         leastSquares;
31    grad(T)         leastSquares;
32}
33
34divSchemes
35{
36    default         none;
37    div(sigmaD)     Gauss linear;
38}
39
40laplacianSchemes
41{
42    default         none;
43    laplacian(DD,D) Gauss linear corrected;
44    laplacian(kappa,T) Gauss linear corrected;
45}
46
47interpolationSchemes
48{
49    default         linear;
50}
51
52snGradSchemes
53{
54    default         none;
55}
56
57// ************************************************************************* //

The fvSolution dictionary in the system directory controls the linear equation solvers and algorithms used in the solution. The user should first look at the solvers sub-dictionary and notice that the choice of solver for D is GAMG. The solver tolerance should be set to eqn for this problem. The solver relative tolerance, denoted by relTol, sets the required reduction in the residuals within each iteration. It is uneconomical to set a tight (low) relative tolerance within each iteration since a lot of terms in each equation are explicit and are updated as part of the segregated iterative procedure. Therefore a reasonable value for the relative tolerance is eqn, or possibly even higher, say eqn, or in some cases even eqn (as in this case).

16
17solvers
18{
19    "(D|T)"
20    {
21        solver          GAMG;
22        tolerance       1e-06;
23        relTol          0.9;
24        smoother        GaussSeidel;
25        nCellsInCoarsestLevel 20;
26    }
27}
28
29stressAnalysis
30{
31    compactNormalStress yes;
32    nCorrectors     1;
33    D               1e-06;
34}
35
36
37// ************************************************************************* //

The fvSolution dictionary contains a sub-dictionary, stressAnalysis that contains some control parameters specific to the application solver. Firstly there is nCorrectors which specifies the number of outer loops around the complete system of equations, including traction boundary conditions within each time step. Since this problem is steady-state, we are performing a set of iterations towards a converged solution with the ‘time step’ acting as an iteration counter. We can therefore set nCorrectors to 1.

The D keyword specifies a convergence tolerance for the outer iteration loop, i.e. sets a level of initial residual below which solving will cease. It should be set to the desired solver tolerance specified earlier, eqn for this problem.

2.2.2 Running the code

The user should run the code here in the background from the command line as specified below, so he/she can look at convergence information in the log file afterwards.


    solidDisplacementFoam > log &
The user should check the convergence information by viewing the generated log file which shows the number of iterations and the initial and final residuals of the displacement in each direction being solved. The final residual should always be less than 0.9 times the initial residual as this iteration tolerance set. Once both initial residuals have dropped below the convergence tolerance of eqn the run has converged and can be stopped by killing the batch job.

2.2.3 Post-processing

Post processing can be performed as in section 2.1.4 . The solidDisplacementFoam solver outputs the stress field eqn as a symmetric tensor field sigma. This is consistent with the way variables are usually represented in OpenFOAM solvers by the mathematical symbol by which they are represented; in the case of Greek symbols, the variable is named phonetically.

For post-processing individual scalar field components, eqn, eqn etc., can be generated by running the postProcess utility as before in section 2.1.5.7 , this time on sigma:


    postProcess -func "components(sigma)"
Components named sigmaxx, sigmaxy etc. are written to time directories of the case. The eqn stresses can be viewed in paraFoam as shown in Figure 2.19 .

 30 25 20 15 σxx (kPa ) 10 5 0 \relax \special {t4ht=


Figure 2.19: eqn stress field in the plate with hole.


We would like to compare the analytical solution of Equation 2.14 to our solution. We therefore must output a set of data of eqn along the left edge symmetry plane of our domain. The user may generate the required graph data using the postProcess utility with the graphUniform function. Unlike earlier examples of postProcess where no configuration is required, this example includes a graphUniform file pre-configured in the system directory. The sample line is set between eqn and eqn, and the fields are specified in the fields list:

9    Writes graph data for specified fields along a line, specified by start and
10    end points. A specified number of graph points are used, distributed
11    uniformly along the line.
12
13\*---------------------------------------------------------------------------*/
14
15start           (0 0.5 0.25);
16end             (0 2 0.25);
17nPoints         100;
18
19fields          (sigmaxx);
20
21axis            y;
22
23#includeEtc "caseDicts/postProcessing/graphs/graphUniform.cfg"
24
25// ************************************************************************* //

The user should execute postProcessing with the graphUniform function:


    postProcess -func graphUniform
Data is written in raw 2 column format into files within time subdirectories of a postProcessing/graphUniform directory, e.g. the data at eqn s is found within the file graphUniform/100/line.xy. If the user has GnuPlot installed they launch it (by typing gnuplot) and then plot both the numerical data and analytical solution as follows:


    plot [0.5:2] [0:] "postProcessing/graphUniform/100/line.xy",
        1e4*(1+(0.125/(x**2))+(0.09375/(x**4)))
An example plot is shown in Figure 2.20 .


 35 30 25 20 Stress(σxx)x=015(kPa) 10 5 0 0.6 0.8 1.0 1.2 1.4 1.6 1.8 2.0 Distance, y (m) Numerical prediction Analytical solution \relax \special {t4ht=


Figure 2.20: Normal stress along the vertical symmetry eqn


2.2.4 Exercises

The user may wish to experiment with solidDisplacementFoam by trying the following exercises:

2.2.4.1 Increasing mesh resolution

Increase the mesh resolution in each of the eqn and eqn directions. Use mapFields to map the final coarse mesh results from section 2.2.3 to the initial conditions for the fine mesh.

2.2.4.2 Introducing mesh grading

Grade the mesh so that the cells near the hole are finer than those away from the hole. Design the mesh so that the ratio of sizes between adjacent cells is no more than 1.1 and so that the ratio of cell sizes between blocks is similar to the ratios within blocks. Mesh grading is described in section 2.1.6 . Again use mapFields to map the final coarse mesh results from section 2.2.3 to the initial conditions for the graded mesh. Compare the results with those from the analytical solution and previous calculations. Can this solution be improved upon using the same number of cells with a different solution?

2.2.4.3 Changing the plate size

The analytical solution is for an infinitely large plate with a finite sized hole in it. Therefore this solution is not completely accurate for a finite sized plate. To estimate the error, increase the plate size while maintaining the hole size at the same value.

OpenFOAM v10 User Guide - 2.2 Stress analysis of a plate with a hole
CFD Direct