Static structural analysis¶

This example will show you how to conduct a 3D static structural analysis for an assembly. Static structural analysis uses FrontISTR as the default solver. It also supports CalculiX or Elmer FEM as a solver.

Selecting units¶

To start, we will select the MKS unit system for the subsequential simulation. Click Preferences from the Toolbar or Menu, and set it to Metric (kg, m, s, A, N, V).

Defining materials¶

In this multi-body analysis, we assign Structural Steel and Aluminum materials to different parts. Since a Structural Steel object is already created when you initialize a FEM Project, you only need to add an aluminum material object. Click Add Material from the Toolbar or FEM Menu.

To edit the material properties, double-click the Material object, or right-click on the Material object and select Edit on the context menu. Now, in the material editor, select the Library tab > General Materials > Aluminum Alloy, then click the Import button, or double-click the Aluminum Alloy entry. The material properties are defined in the Figure below. Click OK to save and exit the material editing.

You can rename this new material object to Aluminum by pressing F2 or right-clicking.

Specifying analysis¶

Since Static Structural analysis is the default setting in WELSIM, you can keep the settings the same as below.

Preparing geometry¶

Next, import the geometry file “h_section_multibody.step” and assign materials to the corresponding parts. As shown in the Figure below, the three Part objects in the Geometry group represent the three bodies in the Graphics window, respectively. Assign Aluminum material to Part2, which is the connection body in the middle. Assign Structural Steel material to the other bodies.

Setting mesh¶

To obtain a fine mesh for the analysis, set the following Mesh Settings properties: Quadratic to True and Maximum Size to 5e-3. This is shown below.

Next, add a Mesh Method object from the Toolbar or FEM Menu. Go into its Properties View, and set the Geometry property by selecting the left body. Then, set Maximum Size value to 3e-3, as shown below.

By clicking the Mesh command from the Toolbar or FEM Menu, you can mesh the geometries. 21,117 nodes and 12,427 Tet10 elements are generated as shown in the Figure below.

Specifying contacts¶

Now, you need to define two Contact Pairs to bond the three parts into one uni-body for the analysis. Click the Add Contact command from the Toolbar or FEM Menu, and add two Contact Pair objects into the tree. You can rename these two objects to Contact1 and Contact2, respectively. Then, select the surfaces for the Master and Target Geometry properties as shown below.

Imposing conditions¶

Next, impose two boundary conditions, a Constraint (Fixed Support) and a Pressure by clicking the corresponding commands from the Toolbar and Structural Menu. In the Properties View of the Constraint object, select the left bottom surface for the Geometry property, as shown in the Figure below.

In the Properties View of the Pressure object, set the Normal Pressure value to 1e7, and select the right top surface for the Geometry property, as shown below.

Solving the model¶

To solve the model, click the Compute command from the Toolbar, FEM Menu, or right-click on the Answers object and select the Compute command from the context menu. Depending on the complexity of the model, the solving process may take anywhere from seconds to hours. The Output window displays solver messages, and it indicates the status of the solving process. As shown in the Figure below, this model is solved successfully.

Evaluating results¶

To evaluate the deformation of the structure, you can add a Deformation object to the tree by clicking the Deformation item from the Toolbar, Structural Menu. A result object may provide multiple sub-result types. For example, a Deformation result object allows you to specify one deformation type from the candidates Deformation X, Y, Z, and Total, as shown in Figure below.

After setting the property Type to Total Deformation, double-clicking on the result object displays the resulting contour in the Graphics window. You can click the Evaluate item from the Toolbar or FEM Menu to evaluate the result.

Adding a stress result object is similar. Clicking the Stress result from Toolbar or Structural Menu, you insert a stress object to the tree. Evaluating the default von-Mises Stress Type, you obtain the von-Mises stress contour on bodies in the Graphics window. The Maximum and Minimum values of stress data are displayed in the Properties View, Tabular Data, and Chart windows.