PDF
Bracket — Shell Analysis
Introduction
The various examples based on a bracket geometry form a suite of tutorials which summarizes the fundamentals when modeling structural mechanics problems in COMSOL Multiphysics and the Structural Mechanics Module.
In this example you study the stress in a bracket subjected to external loads. The thin parts with constant thickness are modeled using the Shell interface, and the transition regions where 3D effects are important are modeled using the Solid Mechanics interface. This example also shows how to connect shell elements with solid elements.
For thin geometries, it can be more efficient to use shell elements than solid elements, thus saving computational time and memory. The Shell interface in the Structural Mechanics Module can be used to model structures approximated by thin or thick shells. There is also a similar Plate interface for 2D problems. The thickness of the shell or plate is taken into account in the equations instead of being explicitly modeled in the geometry.
It is recommended that you review the Introduction to the Structural Mechanics Module, which includes background information and discusses the bracket_basic.mph model relevant to this example.
Model Definition
The model is described in the section “The Fundamentals: A Static Linear Analysis” in the Introduction to the Structural Mechanics Module.
The parts of the geometry modeled with shells are highlighted in Figure 1 and the parts modeled with solids are highlighted in Figure 2.
Figure 1: Shell domains in the bracket geometry.
Figure 2: Solid domains in the bracket geometry.
The load is applied along the edge at the bracket holes.
Results and Discussion
The Shell interface generates a predefined plot which indicates the physical location of top and bottom surfaces. Especially when working with offsets, as in the current example, this is an excellent tool for checking that the input data is correct. This plot is shown in Figure 3.
Figure 3: The shell geometry plot. Red indicates top surface and blue indicates bottom surface.
In another predefined plot, the thickness is indicated by color contours, and the directions of the shell local coordinate systems are shown. This plot is shown in Figure 4.
Figure 4: Plot of thickness and local directions. The Red-Green-Blue convention is used for ordering of the coordinate axes.
Figure 5 shows the first principal strain in both the solid domains and in the shells. When using the Shell dataset, the shell is represented by a solid with thickness and offset taken from the shell interface. The through-thickness representation of, for example, stresses is also full 3D. You can increase the resolution of the evaluation in the thickness direction, but using a high resolution may give slower plotting.
As can be seen, the continuity over the transition between the shell and the solid is very good.
Figure 5: First principal strain distribution in the solid and at the top and bottom of the shell.
Notes About the COMSOL Implementation
You can specify an offset in the shell definition that the meshed surface is not the same as the midsurface of the real geometry. This is used here, since the external geometrical boundaries are immediately available.
The Solid-Thin Structure multiphysics coupling is used for connecting shell edges to solid boundaries.
Application Library path: Structural_Mechanics_Module/Tutorials/bracket_shell
Application Libraries
1
From the File menu, choose Application Libraries.
2
In the Application Libraries window, select Structural Mechanics Module>Tutorials>bracket_static in the tree.
3
Click  Open.
Component 1 (comp1)
Start by removing the results from the loaded model.
1
In the Model Builder window, expand the Component 1 (comp1) node.
Results
Study 1/Solution 1 (sol1)
1
In the Model Builder window, expand the Results>Datasets node.
2
Right-click Results>Datasets>Study 1/Solution 1 (sol1) and choose Delete.
3
Right-click Results>Tables and choose Delete All.
Add a Shell interface to the model.
Add Physics
1
In the Home toolbar, click  Add Physics to open the Add Physics window.
2
Go to the Add Physics window.
3
In the tree, select Structural Mechanics>Shell (shell).
4
Click Add to Component 1 in the window toolbar.
5
In the Home toolbar, click  Add Physics to close the Add Physics window.
Add a number of selections.
Definitions
Solid
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Solid in the Label text field.
3
Select Domains 2, 3, 7, and 8 only.
4
Click the  Zoom Extents button in the Graphics toolbar.
5
Click the  Wireframe Rendering button in the Graphics toolbar.
Shell
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Shell in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Boundary.
4
Select Boundaries 1, 32, 37, 50, and 86 only.
5
Click the  Wireframe Rendering button in the Graphics toolbar.
Solid Mechanics (solid)
1
In the Model Builder window, under Component 1 (comp1) click Solid Mechanics (solid).
2
In the Settings window for Solid Mechanics, locate the Domain Selection section.
3
From the Selection list, choose Solid.
Disable not used boundary conditions from the Solid Mechanics interface. Both the loads and constraints will be applied to the shell part. This is just to clean up the Model Builder tree. Since these nodes now have an empty selection, they would not influence the analysis if kept.
4
In the Model Builder window, expand the Solid Mechanics (solid) node.
Boundary Load 1, Fixed Constraint 1
1
In the Model Builder window, under Component 1 (comp1)>Solid Mechanics (solid), Ctrl-click to select Fixed Constraint 1 and Boundary Load 1.
2
Right-click and choose Group.
Not Used; Applied in Shell Interface
1
In the Settings window for Group, type Not Used; Applied in Shell Interface in the Label text field.
2
Right-click Not Used; Applied in Shell Interface and choose Disable.
Add settings to the Shell interface. Since the mesh is placed on the outer boundary, the location of the midsurface is described by an offset.
Shell (shell)
1
Click the  Wireframe Rendering button in the Graphics toolbar.
2
In the Model Builder window, under Component 1 (comp1) click Shell (shell).
3
In the Settings window for Shell, locate the Boundary Selection section.
4
From the Selection list, choose Shell.
Thickness and Offset 1
1
In the Model Builder window, under Component 1 (comp1)>Shell (shell) click Thickness and Offset 1.
2
In the Settings window for Thickness and Offset, locate the Thickness and Offset section.
3
In the d0 text field, type 8[mm].
4
From the Position list, choose Top surface on boundary.
Fixed Constraint 1
1
In the Physics toolbar, click  Edges and choose Fixed Constraint.
2
In the Settings window for Fixed Constraint, locate the Edge Selection section.
3
From the Selection list, choose Bolt Hole Edges.
Edge Load 1
1
In the Physics toolbar, click  Edges and choose Edge Load.
2
In the Settings window for Edge Load, locate the Coordinate System Selection section.
3
From the Coordinate system list, choose Local edge system.
4
Select Edges 4 and 188 only.
5
Locate the Force section. From the Load type list, choose Force per unit area.
In order to use the local edge system, you need to know the orientation of the edges and the positive shell normal orientation. The orientation of the shell normal can be displayed by enabling physics symbols, and then moving to the Linear Elastic Material node. The line orientation arrows are controlled from the View node.
6
In the Model Builder window, click Shell (shell).
7
In the Settings window for Shell, locate the Physics Symbols section.
8
Select the Enable physics symbols check box.
Definitions
View 1
1
In the Model Builder window, expand the Component 1 (comp1)>Definitions>View 1 node, then click View 1.
2
In the Settings window for View, locate the View section.
3
Select the Show edge direction arrows check box.
Shell (shell)
Edge Load 1
1
In the Model Builder window, under Component 1 (comp1)>Shell (shell) click Edge Load 1.
2
In the Settings window for Edge Load, locate the Force section.
3
Specify the FA vector as
0
xl
load(P0*sign(X),Y-YC,Z)
yl
0
zl
Add the connection between the shells and the solids.
Multiphysics
Solid-Thin Structure Connection 1 (sshc1)
1
In the Physics toolbar, click  Multiphysics Couplings and choose Global>Solid-Thin Structure Connection.
2
In the Settings window for Solid-Thin Structure Connection, locate the Connection Settings section.
3
Select the Manual control of selections check box.
4
Select Boundaries 9, 11, 13, 14, 30, 34, 58, 62, 80, 81, 83, and 84 only.
5
From the Method list, choose Flexible.
6
Click the  Wireframe Rendering button in the Graphics toolbar.
The current material is attached only to the domains. A separate material definition is needed for the boundaries where the Shell interface is active.
Materials
Structural steel 1 (mat2)
1
In the Model Builder window, expand the Component 1 (comp1)>Materials node.
2
Right-click Component 1 (comp1)>Materials>Structural steel (mat1) and choose Duplicate.
3
In the Settings window for Material, locate the Geometric Entity Selection section.
4
From the Geometric entity level list, choose Boundary.
5
From the Selection list, choose Shell.
Run the analysis.
Study 1
In the Home toolbar, click  Compute.
Results
Stress (solid)
The default plot for the Shell interface shows the von Mises stress on top and bottom surfaces. Create a combined stress plot with the results from both interfaces by copying the default stress plot for the solid.
Volume 1
1
In the Model Builder window, expand the Stress (solid) node.
2
Right-click Volume 1 and choose Copy.
Stress, Solid + Shell
1
In the Model Builder window, under Results click Stress (shell).
2
In the Settings window for 3D Plot Group, type Stress, Solid + Shell in the Label text field.
Volume 1
1
Right-click Stress, Solid + Shell and choose Paste Volume.
2
In the Settings window for Volume, click to expand the Inherit Style section.
3
From the Plot list, choose Surface 1.
4
Locate the Data section. From the Dataset list, choose Study 1/Solution 1 (sol1).
5
Locate the Expression section. From the Unit list, choose MPa.
Surface 1
1
In the Model Builder window, click Surface 1.
2
In the Settings window for Surface, locate the Expression section.
3
From the Unit list, choose MPa.
4
Click to expand the Range section. Select the Manual color range check box.
5
In the Maximum text field, type 70.
6
In the Stress, Solid + Shell toolbar, click  Plot.
Add predefined plots showing the shell geometry as well as the thickness and local shell system orientation. The first plot shows the top surface in red and the bottom surface in blue.
7
In the Home toolbar, click  Add Predefined Plot.
Add Predefined Plot
1
Go to the Add Predefined Plot window.
2
In the tree, select Study 1/Solution 1 (sol1)>Shell>Shell Geometry (shell).
3
Click Add Plot in the window toolbar.
4
In the tree, select Study 1/Solution 1 (sol1)>Shell>Thickness and Orientation (shell).
5
Click Add Plot in the window toolbar.
6
In the Home toolbar, click  Add Predefined Plot.
7
Click  Add Predefined Plot.
Results
Shell Geometry (shell)
1
In the Model Builder window, under Results click Shell Geometry (shell).
2
In the Shell Geometry (shell) toolbar, click  Plot.
3
Click the  Zoom Extents button in the Graphics toolbar.
Thickness and Orientation (shell)
1
In the Model Builder window, click Thickness and Orientation (shell).
2
In the Thickness and Orientation (shell) toolbar, click  Plot.
Create a plot of the maximum principal stresses.
Principal Strain
1
In the Model Builder window, right-click Stress, Solid + Shell and choose Duplicate.
2
In the Settings window for 3D Plot Group, type Principal Strain in the Label text field.
Surface 1
1
In the Model Builder window, expand the Principal Strain node, then click Surface 1.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type shell.ep1.
4
Locate the Range section. In the Minimum text field, type 0.
5
In the Maximum text field, type 2.0E-4.
6
Locate the Coloring and Style section. From the Color table type list, choose Discrete.
Volume 1
1
In the Model Builder window, click Volume 1.
2
In the Settings window for Volume, locate the Expression section.
3
In the Expression text field, type solid.ep1.
4
Click the  Zoom Extents button in the Graphics toolbar.
5
In the Principal Strain toolbar, click  Plot.