12
$\begingroup$

enter image description here

I'm trying to get the displacements u(x,y) and v(x,y) of a beam simply suported, the stress distribution in the middle section should be a linear function: enter image description here

but i'm getting this:

enter image description here

My code is:

Needs["NDSolve`FEM`"];
PS = {
  Inactive[
     Div][{{0, -((Y \[Nu])/(1 - \[Nu]^2))}, {-((Y (1 - \[Nu]))/(
        2 (1 - \[Nu]^2))), 0}}.Inactive[Grad][v[x, y], {x, y}], {x, 
     y}] + Inactive[
     Div][{{-(Y/(1 - \[Nu]^2)), 
       0}, {0, -((Y (1 - \[Nu]))/(2 (1 - \[Nu]^2)))}}.Inactive[Grad][
      u[x, y], {x, y}], {x, y}],
  Inactive[
     Div][{{0, -((Y (1 - \[Nu]))/(2 (1 - \[Nu]^2)))}, {-((Y \[Nu])/(
        1 - \[Nu]^2)), 0}}.Inactive[Grad][u[x, y], {x, y}], {x, y}] + 
   Inactive[
     Div][{{-((Y (1 - \[Nu]))/(2 (1 - \[Nu]^2))), 
       0}, {0, -(Y/(1 - \[Nu]^2))}}.Inactive[Grad][
      v[x, y], {x, y}], {x, y}]
  }

L = 2;
q = 6000;
Propiedades = {Y -> 205940000000, \[Nu] -> 30/100};

h1 = 1/2;
h2 = 2;
h3 = 3;

Reg1 = Rectangle[{0, 0}, {L, h1}];
Reg2 = Rectangle[{0, 0}, {L, h2}];
Reg3 = Rectangle[{0, 0}, {L, h3}];

Mesh1 = ToElementMesh[Reg1, MeshQualityGoal -> 0];
Mesh2 = ToElementMesh[Reg2];
Mesh3 = ToElementMesh[Reg3];
{u1, v1, \[Sigma]x1, \[Sigma]y1, \[Tau]xy1} = NDSolveValue[{
     PS == {0, NeumannValue[-q, {0 <= x <= L, y == h1}]},
     \[Sigma]x[x, y] == 
      Y/(1 - \[Nu]^2) (D[u[x, y], x] + \[Nu] D[v[x, y], y]),
     \[Sigma]y[x, y] == 
      Y/(1 - \[Nu]^2) (D[v[x, y], y] + \[Nu] D[u[x, y], x]),
     \[Sigma]xy[x, y] == (Y*\[Nu])/(
       1 - \[Nu]^2) (D[u[x, y], x] + D[v[x, y], y]),
     DirichletCondition[v[x, y] == 0, {x == 0, y == 0}],
     DirichletCondition[v[x, y] == 0, {x == L, y == 0}],
     DirichletCondition[u[x, y] == 0, {x == 0, y == 0}]
     } /. Propiedades, {u, 
    v, \[Sigma]x, \[Sigma]y, \[Sigma]xy}, {x, y} \[Element] Mesh1];

DMesh1 = ElementMeshDeformation[Mesh1, {u1, v1}, 
   "ScalingFactor" -> 2000000];

Row[{
  Show[{Mesh1[
     "Wireframe"[
      "ElementMeshDirective" -> 
       Directive[EdgeForm[Gray], FaceForm[]]]], 
    Graphics[{EdgeForm[Thickness[0.001]], RGBColor[0, 0, 0, 0.1], 
      Reg1}]}, ImageSize -> 300, Epilog -> {
     Scale[Translate[Apoyo2, {-0.5, -0.5}], 0.2],
     Scale[Translate[Apoyo1, {-0.5 + L, -0.5}], 0.2]
     }, PlotRange -> {{-0.1, L + 0.1}, {-0.15, h1 + 0.15}}],
  Show[{
    Mesh1[
     "Wireframe"[
      "ElementMeshDirective" -> 
       Directive[EdgeForm[Gray], FaceForm[]]]],
    DMesh1[
     "Wireframe"[
      "ElementMeshDirective" -> 
       Directive[EdgeForm[RGBColor[0, 0.3, 0.8]], FaceForm[]]]]
    }, ImageSize -> 300]
  }]

Plot[\[Sigma]x1[L/2, y]/1000, {y, 0, h1}, Filling -> Axis, 
 AxesLabel -> {"h[m]", 
   "\!\(\*SubscriptBox[\(\[Sigma]\), \(x\)]\)[kPa]"}, 
 ImageSize -> 400]

I don't why is this happening, but when i set the y coordinate in the Dirichlet Condition to y=h1/2 i get the correct stress distribution

$\endgroup$
  • $\begingroup$ This may be relevant $\endgroup$ – Hugh Nov 28 '16 at 9:18
  • $\begingroup$ Welcome to Mathematica.SE! 1) As you receive help, try to give it too, by answering questions in your area of expertise. 2) Take the tour and check the faqs! 3) When you see good questions and answers, vote them up by clicking the gray triangles, because the credibility of the system is based on the reputation gained by users sharing their knowledge. Also, please remember to accept the answer, if any, that solves your problem, by clicking the checkmark sign! $\endgroup$ – user9660 Nov 28 '16 at 9:23
  • 1
    $\begingroup$ Can you also draw a picture of your mechanical problem, I don't know what you mean with "simply supported" and I would like to know how your forces are acting on the body. $\endgroup$ – Mauricio Fernández Nov 28 '16 at 9:44
  • $\begingroup$ Sorry, but i'm not allowed to add more images: i.imgur.com/VOcF0y7.png $\endgroup$ – Gonza_ Nov 28 '16 at 9:54
  • $\begingroup$ Simply supported means that there are no restraining moments at the pivot resting locations. $\endgroup$ – Jose Enrique Calderon Nov 28 '16 at 12:54
16
+100
$\begingroup$

Your boundary conditions seem to be not quite correct according to the mechanical problem. Sorry, I don't have the time to go through your code today, but I got a version running, although this will take some time and might be an overkill, since it is based on the full 3D theory. I have to go home now, I will try to take a look at your code again tomorrow, if nobody else finds the error.


EDIT: correction of your boundary conditions

Hey Gonza_! In your code, you wanted to treat the mechanical problem as follows.

enter image description here

You only had a slight syntax error in your boundary conditions

(*Wrong*)
bcwrong = {
   DirichletCondition[v[x, y] == 0, {x == 0, y == 0}]
   , DirichletCondition[u[x, y] == 0, {x == 0, y == 0}]
   , DirichletCondition[v[x, y] == 0, {x == L, y == 0}]
   };
(*Correct*)
bccorrect = {
   DirichletCondition[{u[x, y] == 0, v[x, y] == 0}, x == 0 && y == 0]
   , DirichletCondition[v[x, y] == 0, x == L && y == 0]
   };

The difference is that the bcwrong impose a vanishing displacement field at every point with x==0 and at every point with y==0. The correct syntax is given in bccorrect. Working code:

Needs["NDSolve`FEM`"];
(*Geometry*)
L = 2;
h1 = 1/2;
Reg1 = Rectangle[{0, 0}, {L, h1}];
Mesh1 = ToElementMesh[Reg1, MeshQualityGoal -> 0];
(*Forces*)
q = 6000;
(*Material properties*)
Propiedades = {Y -> 205940000000, \[Nu] -> 30/100};
(*2D Hooke's law*)
hl = {
   \[Sigma]x[x, y] == 
    Y/(1 - \[Nu]^2) (D[u[x, y], x] + \[Nu] D[v[x, y], y])
   , \[Sigma]y[x, y] == 
    Y/(1 - \[Nu]^2) (D[v[x, y], y] + \[Nu] D[u[x, y], x])
   , \[Sigma]xy[x, 
     y] == (Y*\[Nu])/(1 - \[Nu]^2) (D[u[x, y], x] + D[v[x, y], y])
   };
(*Equations*)
PS = {Inactive[
      Div][{{0, -((Y \[Nu])/(1 - \[Nu]^2))}, {-((Y (1 - \[Nu]))/(2 (1 \
- \[Nu]^2))), 0}}.Inactive[Grad][v[x, y], {x, y}], {x, y}] + 
    Inactive[
      Div][{{-(Y/(1 - \[Nu]^2)), 
        0}, {0, -((Y (1 - \[Nu]))/(2 (1 - \[Nu]^2)))}}.Inactive[Grad][
       u[x, y], {x, y}], {x, y}], 
   Inactive[
      Div][{{0, -((Y (1 - \[Nu]))/(2 (1 - \[Nu]^2)))}, {-((Y \
\[Nu])/(1 - \[Nu]^2)), 0}}.Inactive[Grad][u[x, y], {x, y}], {x, y}] + 
    Inactive[
      Div][{{-((Y (1 - \[Nu]))/(2 (1 - \[Nu]^2))), 
        0}, {0, -(Y/(1 - \[Nu]^2))}}.Inactive[Grad][
       v[x, y], {x, y}], {x, y}]};
(*BCs*)
(*Neumann*)
bcN = {0, NeumannValue[-q, y == h1]};
(*Wrong*)
bcwrong = {
   DirichletCondition[v[x, y] == 0, {x == 0, y == 0}]
   , DirichletCondition[u[x, y] == 0, {x == 0, y == 0}]
   , DirichletCondition[v[x, y] == 0, {x == L, y == 0}]
   };
(*Correct*)
bccorrect = {
   DirichletCondition[{u[x, y] == 0, v[x, y] == 0}, x == 0 && y == 0]
   , DirichletCondition[v[x, y] == 0, x == L && y == 0]
   };
(*FEM-solution*)
{u1, v1, \[Sigma]x1, \[Sigma]y1, \[Tau]xy1} = 
  NDSolveValue[{PS == bcN, hl, bccorrect} /. Propiedades, {u, 
    v, \[Sigma]x, \[Sigma]y, \[Sigma]xy}
   , Element[{x, y}, Mesh1]];
(*Deformation*)
DMesh1 = ElementMeshDeformation[Mesh1, {u1, v1}, 
   "ScalingFactor" -> 6*10^4];
Show[{Mesh1[
   "Wireframe"[
    "ElementMeshDirective" -> Directive[EdgeForm[Gray], FaceForm[]]]],
   DMesh1[
   "Wireframe"[
    "ElementMeshDirective" -> 
     Directive[EdgeForm[RGBColor[0, 0.3, 0.8]], FaceForm[]]]]}, 
 ImageSize -> 300]
(*Normal stress at x=L/2 depending on y*)
Plot[\[Sigma]x1[L/2, y]/1000, {y, 0, h1}, Filling -> Axis, 
 AxesLabel -> {"h[m]", 
   "\!\(\*SubscriptBox[\(\[Sigma]\), \(x\)]\)[kPa]"}, 
 ImageSize -> 400]

enter image description here


General 3D theory

I treated the problem as follows (length in x direction L1, in virtual y direction L2 and in z direction L3)

enter image description here

First, let's get a reference solution of the 1D theory:

(*Geometry - in m*)
L1 = 2;
L2 = 0.1;
L3 = 0.2;
Iy = L2*L3^3/12;
(*Force and densities - in N*)
F = 10;
qA = F/(L1*L2); (*area density - for 3D FEM*)
ql = qA*L2; (*line density - for 1D theory*)
(*Material parameters*)
Em = 2.1*10^9; (*Young's modulus*)
nu = 0.3;(*Poisson's ration*)
(*1D theory*)
wsol1D = DSolveValue[{
    Em*Iy*D[w[x], {x, 4}] == ql
    , (w[0]) == 0, (w[L1]) == 0
    , (w''[0]) == 0, (w''[L1]) == 0
    }, w, x];
My = -Em*Iy*wsol1D''[x];(*Moment*)
sig = My/Iy*z;(*normal stress*)
GraphicsRow[{
  Plot[wsol1D[x], {x, 0, L1}, AxesLabel -> {"x", "w(x)"}]
  , Plot[sig /. x -> L1/2, {z, -L3/2, L3/2}, 
   AxesLabel -> {"z", "\[Sigma](x=L1/2,z)"}]
  }
 , ImageSize -> Large
 ]

enter image description here

Now, let's get the full 3D FEM solution (takes 1.4 seconds for me) with a area force density

(*FEM solution*)
Needs["NDSolve`FEM`"]
(******************************)
(*Region definition*)
reg = Cuboid[{0, -L2/2, -L3/2}, {L1, L2/2, L3/2}];
(******************************)
(*Isotropic material stiffness - fourth-order tensor*)
(*Identities*)
I2 = IdentityMatrix@3;
IdI = TensorProduct[I2, I2];
I4 = TensorTranspose[IdI, {1, 3, 2, 4}];
IS = (I4 + TensorTranspose[I4, {1, 2, 4, 3}])/2;
(*Isotropic projectors*)
P1 = 1/3*IdI;
P2 = IS - P1;
(*Isotropic stiffness*)
Ciso = l1*P1 + l2*P2;
l1 = 3*Km;
l2 = 2*Gm;
Km = 1/3*Em/(1 - 2*nu);
Gm = 1/2*Em/(1 + nu);
(******************************)
(*Equations*)
eq = Table[
   Inactive[Div][
     Ciso[[i, ;; , 1, ;;]].Inactive[Grad][u[x, y, z], {x, y, z}], {x, 
      y, z}]
    + Inactive[Div][
     Ciso[[i, ;; , 2, ;;]].Inactive[Grad][v[x, y, z], {x, y, z}], {x, 
      y, z}]
    + Inactive[Div][
     Ciso[[i, ;; , 3, ;;]].Inactive[Grad][w[x, y, z], {x, y, z}], {x, 
      y, z}]
   , {i, 3}
   ];
(******************************)
(*BCs*)
(*Dirichlet*)
bcD = {
   DirichletCondition[{u[x, y, z] == 0, v[x, y, z] == 0, 
     w[x, y, z] == 0}, x == 0 && z == 0]
   , DirichletCondition[{v[x, y, z] == 0, w[x, y, z] == 0}, 
    x == L1 && z == 0]
   };
(*Neumann*)
bcN = {0, 0, NeumannValue[-qA, z == -L3/2]};
(******************************)
(*Solution*)
{usol, vsol, wsol} = 
   NDSolveValue[{eq == bcN, bcD}, {u, v, w}, Element[{x, y, z}, reg], 
    Method -> {"PDEDiscretization" -> {"FiniteElement", 
        "MeshOptions" -> {"MaxCellMeasure" -> 0.0001, 
          "MeshOrder" -> 2}}}
    ]; // AbsoluteTiming

{1.4435, Null}

You can take a look at the deformed mesh if you want

mesh = usol["ElementMesh"];
Show[{
  mesh["Wireframe"]
  , ElementMeshDeformation[mesh, {usol, vsol, wsol}, 
    "ScalingFactor" -> 10^4][
   "Wireframe"[
    "ElementMeshDirective" -> Directive[EdgeForm[Red], FaceForm[]]]]
  }, Axes -> True, AxesLabel -> {x, y, z}]

enter image description here

The FEM solution (FEM solution as red points) is in good accordance with the analytical 1D theory

Plot[wsol1D[x], {x, 0, L1}, 
 Epilog -> {PointSize -> Medium, Red, 
   Point[Table[{x, wsol[x, 0, 0]}, {x, 0, L1, L1/10}]]}]

enter image description here

You can get the stress distribution at any point with the full 3D Hooke's law $\sigma_{ij} = C_{ijkl} u_{k,l}$ (FEM solution as red points) (remark: you dont need to symmetrize the displacement grandient in my code in order to obtain the infinitesimal strain, since the stiffness $C_{ijkl}$ I used symmetrizes automatically the mapped tensor). Let's get $\sigma_{xx} = \sigma_{11}$

uv[x_, y_, z_] := {usol[x, y, z], vsol[x, y, z], wsol[x, y, z]}
eps[xs_, ys_, zs_] := 
 D[uv[x, y, z], {{x, y, z}, 1}] /. {x -> xs, y -> ys, z -> zs}
(*linear map of second order tensor B over fourth-order tensor A*)
lm[A_, B_] := TensorContract[TensorProduct[A, B], {{3, 5}, {4, 6}}]
(*Get Cauchy stress sigma_xx = sigma[[1,1]], at x=L1/2 depending on z with 3D Hooke's law*)
sigloc = lm[Ciso, eps[L1/2, 0, z]][[1, 1]];
siglocdata = Table[{zi, sigloc /. z -> zi}, {zi, -L3/2, L3/2, L3/10}];
Plot[sig /. x -> L1/2, {z, -L3/2, L3/2}, 
 AxesLabel -> {"z", "\[Sigma](x=L1/2,z)"}, 
 Epilog -> {PointSize -> Medium, Red, Point@siglocdata}]

enter image description here

$\endgroup$
  • $\begingroup$ Thank you very much for your help! yeah, i knowed that the problem was in the boundary conditions. It's my first time using FEM and i really didn't know how to define the conditions. $\endgroup$ – Gonza_ Nov 29 '16 at 8:46
  • $\begingroup$ Very nice answer! Two small remarks. The deformation is in the positive z axis, but the force is in the negative z axis, probably a sign issue. Concerning the (small) discrepancy between beam theory and the FEM, I think some of that is due to numerical error and some it due to the difference in the theory behind the two approaches. It would be nice to show a pre-stressed beam, which looks like it would not be too hard in your formulation - though that had not been asked for ;-) It's great to seem some struct. mech. knowledge here. $\endgroup$ – user21 Nov 29 '16 at 8:53
  • $\begingroup$ @Gonza_ what do you all think should we have a FEM for structural mechanics tutorial? $\endgroup$ – user21 Nov 29 '16 at 8:54
  • $\begingroup$ @Gonza_ no worries, I just added the response to your code, you only had a small syntax error. $\endgroup$ – Mauricio Fernández Nov 29 '16 at 9:20
  • $\begingroup$ @user21 thank you! It was kind of fun to work on a good example between the 1D theory and the FEM solution combined with the full 3D theory. I used the $z$ axis in that direction since it is the "common" way to do it where I studied. I think this one would actually be a very good introduction example for structural mechanics. $\endgroup$ – Mauricio Fernández Nov 29 '16 at 9:23

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.