2.2Stress 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  and radius  0.5 . It is loaded with a uniform traction of  10   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 .

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

 (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.

2.2.1Mesh 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 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 direction has to be chosen; here, 0.5  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.

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
131mergePatchPairs
132(
133);
134
135// ************************************************************************* //

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 direction of block 0 is equivalent to the 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 .

2.2.1.1Boundary 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  . 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   and the pressure should be 0 .

2.2.1.2Mechanical properties

The physical properties for the case are set in the mechanicalProperties dictionary in the constant directory. For this problem, we need to specify the mechanical properties of steel given in Table 2.1 . In the mechanical properties dictionary, the user must also set planeStress to yes.

 Property Units Keyword Value Density rho 7854 Young’s modulus E Poisson’s ratio — nu 0.3

Table 2.1: Mechanical properties for steel

2.2.1.3Thermal properties

The temperature ﬁeld variable T is present in the solidDisplacementFoam solver since the user may opt to 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 in the thermophysicalProperties dictionary. This dictionary also sets the thermal properties for the case, e.g. for steel as listed in Table 2.2 .

 Property Units Keyword Value Speciﬁc heat capacity C 434 Thermal conductivity k 60.5 Thermal expansion coeﬀ. alpha

Table 2.2: Thermal properties for steel

In this case we do not want to solve for the thermal equation. Therefore we must set the thermalStress keyword entry to no in the thermophysicalProperties dictionary.

2.2.1.4Control

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 . 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 .

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// ************************************************************************* //

2.2.1.5Discretisation 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{
20}
21
22ddtSchemes
23{
24    default         Euler;
25}
26
28{
29    default         leastSquares;
32}
33
34divSchemes
35{
36    default         none;
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
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 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 , or possibly even higher, say , or in some cases even (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, for this problem.

2.2.2Running 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 the run has converged and can be stopped by killing the batch job.

2.2.3Post-processing

Post processing can be performed as in section 2.1.4 . The solidDisplacementFoam solver outputs the stress ﬁeld 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, , 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 stresses can be viewed in paraFoam as shown in Figure 2.19 .

We would like to compare the analytical solution of Equation 2.14 to our solution. We therefore must output a set of data of 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 and , 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  s is found within the ﬁle graphUniform/100/line_sigmaxx.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_sigmaxx.xy",
1e4*(1+(0.125/(x**2))+(0.09375/(x**4)))
An example plot is shown in Figure 2.20 .

2.2.4Exercises

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

2.2.4.1Increasing mesh resolution

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