2.2 Stress analysis of a plate with a hole
This tutorial describes how to preprocess, run and postprocess a case involving linearelastic, steadystate 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 2.15. 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 2.15.
The problem can be approximated as 2dimensional 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.
2.2.1 Mesh generation
The domain consists of four blocks, some of which have arcshaped edges. The block structure for the part of the mesh in the plane is shown in Figure 2.16. 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 crosssectional area.
The user should change into the plateHole case in the $FOAM_RUN/tutorials/stressAnalysis/solidDisplacementFoam directory and open the constant/polyMesh/blockMeshDict file in an editor, as listed below
18
19 vertices
20 (
21 (0.5 0 0)
22 (1 0 0)
23 (2 0 0)
24 (2 0.707107 0)
25 (0.707107 0.707107 0)
26 (0.353553 0.353553 0)
27 (2 2 0)
28 (0.707107 2 0)
29 (0 2 0)
30 (0 1 0)
31 (0 0.5 0)
32 (0.5 0 0.5)
33 (1 0 0.5)
34 (2 0 0.5)
35 (2 0.707107 0.5)
36 (0.707107 0.707107 0.5)
37 (0.353553 0.353553 0.5)
38 (2 2 0.5)
39 (0.707107 2 0.5)
40 (0 2 0.5)
41 (0 1 0.5)
42 (0 0.5 0.5)
43 );
44
45 blocks
46 (
47 hex (5 4 9 10 16 15 20 21) (10 10 1) simpleGrading (1 1 1)
48 hex (0 1 4 5 11 12 15 16) (10 10 1) simpleGrading (1 1 1)
49 hex (1 2 3 4 12 13 14 15) (20 10 1) simpleGrading (1 1 1)
50 hex (4 3 6 7 15 14 17 18) (20 20 1) simpleGrading (1 1 1)
51 hex (9 4 7 8 20 15 18 19) (10 20 1) simpleGrading (1 1 1)
52 );
53
54 edges
55 (
56 arc 0 5 (0.469846 0.17101 0)
57 arc 5 10 (0.17101 0.469846 0)
58 arc 1 4 (0.939693 0.34202 0)
59 arc 4 9 (0.34202 0.939693 0)
60 arc 11 16 (0.469846 0.17101 0.5)
61 arc 16 21 (0.17101 0.469846 0.5)
62 arc 12 15 (0.939693 0.34202 0.5)
63 arc 15 20 (0.34202 0.939693 0.5)
64 );
65
66 boundary
67 (
68 left
69 {
70 type symmetryPlane;
71 faces
72 (
73 (8 9 20 19)
74 (9 10 21 20)
75 );
76 }
77 right
78 {
79 type patch;
80 faces
81 (
82 (2 3 14 13)
83 (3 6 17 14)
84 );
85 }
86 down
87 {
88 type symmetryPlane;
89 faces
90 (
91 (0 1 12 11)
92 (1 2 13 12)
93 );
94 }
95 up
96 {
97 type patch;
98 faces
99 (
100 (7 8 19 18)
101 (6 7 18 17)
102 );
103 }
104 hole
105 {
106 type patch;
107 faces
108 (
109 (10 5 16 21)
110 (5 0 11 16)
111 );
112 }
113 frontAndBack
114 {
115 type empty;
116 faces
117 (
118 (10 9 4 5)
119 (5 4 1 0)
120 (1 4 3 2)
121 (4 7 6 3)
122 (4 9 8 7)
123 (21 16 15 20)
124 (16 11 12 15)
125 (12 13 14 15)
126 (15 14 17 18)
127 (15 18 19 20)
128 );
129 }
130 );
131
132 mergePatchPairs
133 (
134 );
135
136 // ************************************************************************* //
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 nonstraight 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 2.16 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 5.2.1.
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 2.17.
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:
18
19 internalField uniform (0 0 0);
20
21 boundaryField
22 {
23 left
24 {
25 type symmetryPlane;
26 }
27 right
28 {
29 type tractionDisplacement;
30 traction uniform ( 10000 0 0 );
31 pressure uniform 0;
32 value uniform (0 0 0);
33 }
34 down
35 {
36 type symmetryPlane;
37 }
38 up
39 {
40 type tractionDisplacement;
41 traction uniform ( 0 0 0 );
42 pressure uniform 0;
43 value uniform (0 0 0);
44 }
45 hole
46 {
47 type tractionDisplacement;
48 traction uniform ( 0 0 0 );
49 pressure uniform 0;
50 value uniform (0 0 0);
51 }
52 frontAndBack
53 {
54 type empty;
55 }
56 }
57
58 // ************************************************************************* //
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 .
2.2.1.2 Mechanical 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.
2.2.1.3 Thermal 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 thermalProperties 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  




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 thermalProperties dictionary.
2.2.1.4 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 . 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 steadystate 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:
18 application solidDisplacementFoam;
19
20 startFrom startTime;
21
22 startTime 0;
23
24 stopAt endTime;
25
26 endTime 100;
27
28 deltaT 1;
29
30 writeControl timeStep;
31
32 writeInterval 20;
33
34 purgeWrite 0;
35
36 writeFormat ascii;
37
38 writePrecision 6;
39
40 writeCompression off;
41
42 timeFormat general;
43
44 timePrecision 6;
45
46 graphFormat raw;
47
48 runTimeModifiable true;
49
50
51 // ************************************************************************* //
2.2.1.5 Discretisation schemes and linearsolver control
Let us turn our attention to the fvSchemes dictionary. Firstly, the problem we are analysing is steadystate 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 steadystate and transient problems but solidDisplacementFoam does work, since the base algorithm is the same for both types of simulation.
The momentum equation in linearelastic 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 subdictionary:
18 d2dt2Schemes
19 {
20 default steadyState;
21 }
22
23 ddtSchemes
24 {
25 default Euler;
26 }
27
28 gradSchemes
29 {
30 default leastSquares;
31 grad(D) leastSquares;
32 grad(T) leastSquares;
33 }
34
35 divSchemes
36 {
37 default none;
38 div(sigmaD) Gauss linear;
39 }
40
41 laplacianSchemes
42 {
43 default none;
44 laplacian(DD,D) Gauss linear corrected;
45 laplacian(DT,T) Gauss linear corrected;
46 }
47
48 interpolationSchemes
49 {
50 default linear;
51 }
52
53 snGradSchemes
54 {
55 default none;
56 }
57
58 fluxRequired
59 {
60 default no;
61 D yes;
62 T no;
63 }
64
65
66 // ************************************************************************* //
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 subdictionary 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).
18 solvers
19 {
20 ”(DT)”
21 {
22 solver GAMG;
23 tolerance 1e06;
24 relTol 0.9;
25 smoother GaussSeidel;
26 cacheAgglomeration true;
27 nCellsInCoarsestLevel 20;
28 agglomerator faceAreaPair;
29 mergeLevels 1;
30 }
31 }
32
33 stressAnalysis
34 {
35 compactNormalStress yes;
36 nCorrectors 1;
37 D 1e06;
38 }
39
40
41 // ************************************************************************* //
The fvSolution dictionary contains a subdictionary, 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 steadystate, 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.
2.2.2 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 the run has converged and can be stopped by killing the batch job.
2.2.3 Postprocessing
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 postprocessing individual scalar field components, , etc. , can be generated by running the foamCalc utility as before in section 2.1.5.7, this time on 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 2.18.
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 sample utility. The utility uses a sampleDict dictionary located in the system directory, whose entries are summarised in Table 6.3. The sample line specified in sets is set between and , and the fields are specified in the fields list:
18 interpolationScheme cellPoint;
19
20 setFormat raw;
21
22 sets
23 (
24 leftPatch
25 {
26 type uniform;
27 axis y;
28 start ( 0 0.5 0.25 );
29 end ( 0 2 0.25 );
30 nPoints 100;
31 }
32 );
33
34 fields ( sigmaxx );
35
36
37 // ************************************************************************* //
The user should execute sample as normal. The writeFormat is raw 2 column format. The data is written into files within time subdirectories of a postProcessing/sets directory, e.g. the data at s is found within the file sets/100/leftPatch_sigmaxx.xy. In an application such as GnuPlot, one could type the following at the command prompt would be sufficient to plot both the numerical data and analytical solution:
1e4*(1+(0.125/(x**2))+(0.09375/(x**4)))
An example plot is shown in Figure 2.19.
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 and 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.