Documentation

## Deflection Analysis of Bracket

This example shows how to analyze a 3-D mechanical part under an applied load using finite element analysis (FEA) and determine the maximal deflection.

### Create a Structural Analysis Model

The first step in solving a linear elasticity problem is to create a structural analysis model. This is a container that holds the geometry, structural material properties, body and boundary loads, boundary constraints, and mesh.

`model = createpde('structural','static-solid');`

### Import the Geometry

Import an STL file of a simple bracket model using the `importGeometry` function. This function reconstructs the faces, edges and vertices of the model. It can merge some faces and edges, so the numbers can differ from those of the parent CAD model.

`importGeometry(model,'BracketWithHole.stl');`

Plot the geometry and turn on face labels. You will need the face labels to define the boundary conditions.

```figure pdegplot(model,'FaceLabels','on') view(30,30); title('Bracket with Face Labels')``` ```figure pdegplot(model,'FaceLabels','on') view(-134,-32) title('Bracket with Face Labels, Rear View')``` ### Specify Structural Properties of the Material

Specify Young's modulus and Poisson's ratio for this material.

```structuralProperties(model,'Cell',1,'YoungsModulus',200e9, ... 'PoissonsRatio',0.3);```

### Define the Boundary Conditions

The problem has two boundary conditions: the back face (face 4) is immobile and the front face has an applied load. All other boundary conditions, by default, are free boundaries.

`structuralBC(model,'Face',4,'Constraint','fixed');`

Apply a distributed load in the negative $z$-direction to the front face (face 8).

```distributedLoad = 1e4; % Applied load in Pascals structuralBoundaryLoad (model,'Face',8,'SurfaceTraction',[0;0;-distributedLoad]);```

### Create a Mesh

Create a mesh that uses 10-node tetrahedral elements with quadratic interpolation functions. This element type is significantly more accurate than the linear interpolation (four-node) elements, particularly in elasticity analyses that involve bending.

```bracketThickness = 1e-2; % Thickness of horizontal plate with hole, meters generateMesh(model,'Hmax',bracketThickness); figure pdeplot3D(model) title('Mesh with Quadratic Tetrahedral Elements');``` ### Calculate the Solution

Use `solve` to calculate the solution.

`result = solve(model);`

### Examine the Solution

Find the maximal deflection of the bracket in the $z$ direction.

```minUz = min(result.Displacement.uz); fprintf('Maximal deflection in the z-direction is %g meters.', minUz)```
```Maximal deflection in the z-direction is -4.48952e-05 meters. ```

### Plot Components of the Displacement

To see the solution, plot the components of the solution vector. The maximal deflections are in the $z$-direction. Because the part and the loading are symmetric, the $x$-displacement and $z$-displacement are symmetric, and the $y$-displacement is antisymmetric with respect to the center line.

Here, the plotting routine uses the `'jet'` colormap, which has blue as the color representing the lowest value and red representing the highest value. The bracket loading causes face 8 to dip down, so the maximum $z$-displacement appears blue.

```figure pdeplot3D(model,'ColorMapData',result.Displacement.ux) title('x-displacement') colormap('jet')``` ```figure pdeplot3D(model,'ColorMapData',result.Displacement.uy) title('y-displacement') colormap('jet')``` ```figure pdeplot3D(model,'ColorMapData',result.Displacement.uz) title('z-displacement') colormap('jet')``` ### Plot von Mises Stress

Plot values of the von Mises stress at nodal locations. Use the same `jet` colormap.

```figure pdeplot3D(model,'ColorMapData',result.VonMisesStress) title('von Mises stress') colormap('jet')``` ##### Support Get trial now