COMSOL 6.4 - Bracket — Shell Analysis

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 the same as in the solid model which forms the basis, but is now applied along the edges at the bracket holes.

Results and Discussion

The Shell interface generates a 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 plot, also available under , 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.

There are several types of automatic connections available in the Shell interface. When using such features, it is recommended that you inspect that the connections have been applied as intended. In Figure 5, such a plot is shown. It indicates the boundaries of the solid that are connected to shell elements.

Figure 5: Generated connections between shell and solid elements.

Figure 6 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 6: First principal strain distribution in the solid and at the top and bottom of the shell.

A special result type in the shell elements are the section forces. The section forces contain the stresses integrated through the thickness of the shell and represent three fundamental types of action:

•

Membrane (shell.Nl11, shell.Nl22, and shell.Nl12)

•

Bending (shell.Ml11, shell.Ml22, and shell.Ml12)

•

Out-of-plane shear (shell.Ql1 and shell.Ql2)

The section forces are always aligned with the shell local system.

As an example of section forces, they evaluated along a cut line through the left arm of the bracket, shown in Figure 7. In this cross section, it is reasonable to expect that the stress state is similar to that of a rectangular beam, subjected to a transverse force at the hole location.

In order to know which components of the section force to study, the local directions can be examined in Figure 4. The first direction is the one along the arm, so shell.Nl11 corresponds to the bending stresses in a beam and shell.Nl12 corresponds to the shear stresses.

Figure 7: The cut line used for examining the section forces.

The relevant membrane forces along the cut are shown in Figure 8.

Figure 8: Membrane forces along the cut line.

The values can be compared with analytical results according to beam theory. As the cut is located at a distance from the hole center of a = 100 mm, the bending moment is

(1)

The peak bending stress in a rectangular beam is

(2)

where t is the thickness and h is the height. The distribution along the cut should be linear.

The section force is the stress multiplied by the thickness, giving the peak value

(3)

According to beam theory, the shear stress has a parabolic distribution with the peak value

(4)

Thus, the peak value of the shear membrane force is

(5)

As can be seen, the stress state in this part of the structure is very close to that of a beam. Checks like this can be valuable for model verification.

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 multiphysics coupling is used for connecting shell edges to solid boundaries.

Structural_Mechanics_Module/Tutorials/bracket_shell

Application Libraries

From the menu, choose .

In the window, select > > in the tree.

Click

Component 1 (comp1)

Start by removing the results from the loaded model.

In the window, expand the node.

Results

Study 1/Solution 1 (sol1)

In the window, expand the > node.

Right-click > > and choose .

Right-click > and choose .

Component 1 (comp1)

Add a Shell interface to the model.

Add Physics

In the toolbar, click

to open the window.

Go to the window.

In the tree, select > .

Click the button in the window toolbar.

In the toolbar, click

to close the window.

Definitions

Add a number of selections.

Solid

In the toolbar, click

In the window for , type Solid in the text field.

Select Domains 2, 3, 7, and 8 only.

Click the

button in the toolbar.

Click the

button in the toolbar.

Shell

In the toolbar, click

In the window for , type Shell in the text field.

Locate the section. From the list, choose .

Select Boundaries 1, 32, 37, 50, and 86 only.

Click the

button in the toolbar.

Solid Mechanics (solid)

In the window, under click .

In the window for , locate the section.

From the list, choose .

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.

In the window, expand the node.

Boundary Load 1, Fixed Constraint 1

In the window, under > , Ctrl-click to select and .

Right-click and choose .

Not Used; Applied in Shell Interface

In the window for , type Not Used; Applied in Shell Interface in the text field.

Right-click and choose .

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)

Click the

button in the toolbar.

In the window, under click .

In the window for , locate the section.

From the list, choose .

Thickness and Offset 1

In the window, under > click .

In the window for , locate the section.

In the d0 text field, type 8[mm].

From the list, choose .

Fixed Constraint 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Edge Load 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Select Edges 4 and 188 only.

Locate the section. From the list, choose .

Specify the fA vector as


p0*cos(sys2.phi)	r

Multiphysics

Add the connection between the shells and the solids.

Solid–Thin Structure Connection 1 (sshc1)

In the toolbar, click

and choose > .

In the window for , locate the section.

Select the checkbox.

Select Boundaries 9, 11, 13, 14, 30, 34, 58, 62, 80, 81, 83, and 84 only.

From the list, choose .

Click the

button in the toolbar.

Materials

The current material is attached only to the domains. A separate material definition is needed for the boundaries where the Shell interface is active.

Structural steel 1 (mat2)

In the window, expand the > node.

Right-click > > and choose .

In the window for , locate the section.

From the list, choose .

Study 1

Run the analysis.

In the toolbar, click

Results

Stress (solid)

The default plot for the Shell interface shows the von Mises stress using a dataset. Create a combined stress plot with the results from both interfaces by copying the default stress plot for the solid.

Volume 1

In the window, expand the node.

Right-click and choose .

Stress, Solid + Shell

In the window, under click .

In the window for , type Stress, Solid + Shell in the text field.

Volume 1

Right-click and choose .

In the window for , click to expand the section.

From the list, choose .

Locate the section. From the list, choose .

Surface 1

In the window, click .

In the window for , click to expand the section.

Select the checkbox.

In the text field, type 70.

In the toolbar, click

Add plots from , showing the shell geometry, the thickness and local shell system orientation, and the solid-shell connections. The first plot shows the top surface in red and the bottom surface in blue.

Result Templates

In the toolbar, click