COMSOL 6.4 - Bracket — Static 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.

This is the first model in the suite, showing a linear static analysis. It includes the definition of material properties and boundary conditions. After the solution is computed, you learn how to analyze the results.

Model Definition

The model used in this guide is a bracket made of steel. This type of bracket can be used to install an actuator that is mounted on a pin placed between the two holes in the bracket arms. The geometry is shown in Figure 1.

Figure 1: Bracket geometry.

In this analysis, the mounting bolts are assumed to be fixed and securely bonded to the bracket. One of the arms is loaded upward and the other downward. The loads are applied as a pressure on the inner surfaces of the holes, and their intensity is p = p0 cos(α), where α is the angle from the direction of the load resultants. This is a common assumption for pins with a small clearance. Figure 2 below shows the loads applied to the bracket.

Figure 2: Load distribution in the bracket arms.

The resultant load in each hole is Fh = 800 N. The pressure intensity p0 can be determined from an integration of the projected pressure

(1)

where t is the thickness of the arm, and d is the diameter of the hole.

Results

Figure 3 shows the von Mises stress distribution together with an exaggerated (automatically scaled) picture of the deformation. The high stress values are located in the vicinity of the mounting bolts and at the transition between the plates. The stress at the bolt holes is, to some extent, an effect of the assumed boundary condition which causes a singularity. This is a common situation in structural mechanics models.

The von Mises equivalent stress is a good measure of the safety against plastic deformations for a material like steel which essentially is independent to the sign and orientation of the stresses.

Figure 3: Von Mises stress distribution in the bracket under a twisting load.

In Figure 4, you can see that the bracket base remains fixed while only the arms are deformed. The maximum total displacement is about 0.25 mm, which is in agreement with the assumption of small deformations.

Figure 4: Total displacement.

Figure 5 shows the principal stresses in the bracket. The largest principal stress is shown with red arrows, the intermediate principal stress with green arrows, and the smallest principal stress with blue arrows. Since a state of plane stress prevails in large parts of the structure (the thin plates) one of the principal stresses is mostly zero. Note that the principal stress arrows in this figure are shown using a logarithmic scale. This will give a good overview of the orientation of the stress components. With a linear scale, only a few arrows at the stress concentrations would be visible.

Figure 5: Principal stress in the bracket left arm (logarithmic scale).

In Figure 6 and Figure 7, you can see the stress variation along an edge of the fillet connecting one of the arms of the bracket to the mounting plate. The difference between these two plots is that in the second one, there is no averaging between adjacent elements. By disabling averaging in graphs or color plots, you can get an indication of the discretization error in the solution. The default stress plot (Figure 3) actually has a setting making the averaging optional. If the stress jump between two adjacent elements is larger than a certain threshold value, no averaging is performed.

Figure 6: First principal stress along the fillet with the highest stress.

Figure 7: First principal stress along the fillet with the highest stress. No averaging between adjacent elements.

If the bracket would have been made from cast iron, rather than steel, the von Mises stress as shown in Figure 3 is a less suitable criterion, since cast iron is more sensitive to tension than compression. In COMSOL, you can find many failure criteria, suitable for materials with more sophisticated failure modes.

For a cast iron, it is possible to use the Rankine criterion. In this case, the largest principal stress in each point is checked against the allowed tensile stress, while the smallest principal stress is checked against the allowed compressive stress. Here it is assumed that the allowed values are

•

Maximum tensile stress: 100 MPa

•

Maximum compressive stress: -400 MPa

In Figure 8, the failure index for the Rankine criterion is shown. Values above 1 indicate failure. This happens around the bolt holes, there the stresses are unrealistic anyway.

Figure 8: Failure in using a Rankine criterion.

It can be noted that with the Rankine criterion, the risk of failure is no longer symmetric between the right and left sides of the bracket.

Notes About the COMSOL Implementation

In this model, the possibility to add comments to nodes in the Model Builder is utilized. This can be useful when some expressions in the settings are not obvious to someone else using your model, or even when you yourself revisit it later. An example is shown in Figure 9.

Figure 9: The Settings tab for the Parameters node with an explanatory comment added.

You add and modify comments in the tab for a certain node. This tab is not shown by default. To open the tab, right-click on the current node, and select . You can now enter a text, and there are also a number of formatting tools as shown in Figure 10. Once you have added a comment for a node in the model, this comment will be visible in the tab.

Figure 10: The Properties tab for the Parameters node, where the comment text is maintained.

Note that the complex expressions in Figure 10 is not the way you typically enter comments. It is an effect of applying formatting tools from the toolbars.

Structural_Mechanics_Module/Tutorials/bracket_static

Modeling Instructions

This example is the same as described in the Introduction to the Structural Mechanics Module document. If you are new to COMSOL Multiphysics, that may be a better starting point, since it contains a more detailed description.

Note that part of the instructions below are not essential for performing the analysis. Rather, they are intended to showcase some useful tools. Examples of such instructions are the assignments of colors to geometrical parts, as well as many adjustments to the plots.

The first step to build a model is to open COMSOL and then specify the type of analysis you want to do - in this case, a stationary, solid mechanics analysis.

From the menu, choose .

New

In the window, click

Model Wizard

In the window, click

In the tree, select > .

Click .

Click

In the tree, select > .

Click

Global Definitions

It is good modeling practice to gather constants and parameters in one place so that you can change them easily. Using parameters will also improve the readability of your input data.

Parameters 1

In the window, under click .

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Value	Description
Fh	800[N]	800 N	Force per hole
dHole	50[mm]	0.05 m	Hole diameter
tArm	8[mm]	0.008 m	Thickness of arm
p0	Fh/(dHoletArmpi/4)	2.5465E6 N/m²	Peak load intensity

In any node in the Model Builder, you can add comments to explain the settings. In this example, you may want to explain the expression for the peak load intensity. How to do that is shown in Figure 9 and Figure 10.

Geometry 1

The next step is to create your geometry, which also can be imported from an external program. COMSOL Multiphysics supports a multitude of CAD programs and file formats. In this example, import a file in the COMSOL Multiphysics geometry file format (.mphbin).

Import 1 (imp1)

In the toolbar, click

In the window for , locate the section.

From the list, choose .

Click

Browse to the model’s Application Libraries folder and double-click the file bracket.mphbin.

Click

Block 1 (blk1)

It is possible to create a free tetrahedral mesh covering the whole component. Such a strategy is however not optimal for the large flat regions. For this reason, you will partition the geometry, so that you can create a better mesh.

In the toolbar, click

In the window for , locate the section.

Find the subsection. Click .

In the dialog, type Partition Block in the text field.

Click .

In the window for , locate the section.

In the text field, type 0.025.

In the text field, type 0.13.

In the text field, type 0.04.

Locate the section. In the text field, type -0.11.

In the text field, type -0.12.

In the text field, type 0.025.

Click

In the window, click .

Mirror 1 (mir1)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Select the checkbox.

Locate the section. Find the subsection. From the list, choose .

Click

Mirror 2 (mir2)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Select the checkbox.

Locate the section. In the text field, type 1.

In the text field, type 0.

Locate the section. Find the subsection. From the list, choose .

Click

Partition Objects 1 (par1)

In the toolbar, click

and choose .

Select the object only.

In the window for , locate the section.

Click to select the

toggle button for .

From the list, choose .

Click

Form Union (fin)

In the toolbar, click

Click the

button in the toolbar.

Definitions

Bolt 1

In the toolbar, click

In the window for , type Bolt 1 in the text field.

Click the

button in the toolbar.

Locate the section. From the list, choose .

Select Boundary 41 only.

Select the checkbox.

Repeat the steps above to add three more explicit selections, with the following properties:


Default node label	New node label	Select this boundary
Explicit 2	Bolt 2	43
Explicit 3	Bolt 3	55
Explicit 4	Bolt 4	57

Bolt Holes

In the toolbar, click

In the window for , type Bolt Holes in the text field.

Locate the section. From the list, choose .

Locate the Color section. On Windows, select the eighth color in the first row of the palette (a pink color). On other platforms, choose Color 8 from the Color list.

Locate the section. Under , click

In the dialog, in the list, choose , , , and .

Click .

Create selections for the two holes carrying the load.

Left Pin Hole

In the toolbar, click

In the window for , type Left Pin Hole in the text field.

Locate the section. From the list, choose .

Select Boundary 4 only.

Locate the Color section. On Windows, select the ninth color in the first row of the palette (a light blue-gray color). On other platforms, choose Color 9 from the Color list.

Right Pin Hole

In the toolbar, click

In the window for , type Right Pin Hole in the text field.

Locate the section. From the list, choose .

Select Boundary 76 only.

Locate the Color section. On Windows, select the second color in the second row of the palette (a light brown color). On other platforms, choose Color 12 from the Color list.

Pin Holes

In the toolbar, click

In the window for , type Pin Holes in the text field.

Locate the section. From the list, choose .

Locate the section. Under , click

In the dialog, in the list, choose and .

Click .

Add a selection to be used during mesh generation.

Bolt Hole Edges

In the toolbar, click

In the window for , type Bolt Hole Edges in the text field.

Locate the section. From the list, choose .

Locate the section. Under , click

In the dialog, select in the list.

Click .

Click the

button in the toolbar.

Materials

COMSOL Multiphysics is equipped with built-in material properties for a number of common materials. Here, choose structural steel. The material is automatically assigned to all domains.

Add Material

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.

Solid Mechanics (solid)

By default, the Solid Mechanics interface assumes that the participating material models are linear elastic, which is appropriate for this example. All that is left to do is to define the constraints and loads.

Fixed Constraint 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Geometry 1

Apply pressure loads to the bracket holes. Start by adding a cylindrical coordinate system, so that it is easy to generate the sinusoidal distribution of the pressure from the pin.

Centroid Measurement 1 (cm1)

In the toolbar, click

and choose .

On the object , select Points 2 and 5 only.

In the window for , click

Locate the section. In the text field, type PinHoleX.

In the text field, type PinHoleY.

In the text field, type PinHoleZ.

Definitions

Cylindrical System 2 (sys2)

In the toolbar, click

and choose .

In the window for , locate the section.

Find the subsection. In the table, enter the following settings:


x (m)	y (m)	z (m)
0	PinHoleY	PinHoleZ

Find the subsection. In the table, enter the following settings:


x	y	z
1	0	0

Find the ϕ subsection. In the table, enter the following settings:


x	y	z
0	0	sign(X)

Note how two cylindrical systems with different reference orientations are created by making the orientation dependent on in which arm the system is referenced.

Locate the section. From the list, choose .

Solid Mechanics (solid)

Boundary Load 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

Locate the section. Specify the fA vector as


-p0*cos(sys2.phi)	n

There are several different ways in which this load could have been described without making use of a position dependence when defining the coordinate system. You could, for example, use two separate nodes with different signs in front of the load. Alternatively, you could still use a single node, but with the expression p0*abs(cos(sys2.phi)) or p0*cos(sys2.phi)*sign(X)

Definitions

Boundary System 1 (sys1)

Make sure that the coordinate system in which the loads are applied does not change with deformation. This does not matter here, but if the model is used later on for geometrically nonlinear analysis, the distinction can matter.

In the window, under > click .

In the window for , locate the section.

From the list, choose .

Mesh 1

Start by creating an edge mesh around the bolt holes to make sure that they are properly resolved.

Edge 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Distribution 1

Right-click and choose .

In the window for , locate the section.

In the text field, type 8.

Create a mesh which is swept through the thin flat parts, and then use a free tetrahedral mesh in the parts with a more complex geometry. Note that the transition between the two types of elements is automatic. A layer of pyramid elements will be generated there.

Swept 1

In the toolbar, click

In the window for , locate the section.

From the list, choose .

Select Domains 1, 4–6, and 9 only.

Size 1

Right-click and choose .

In the window for , locate the section.

Click the button.

Locate the section.

Select the checkbox. In the associated text field, type 6[mm].

Click

You are going to use the element size later in the modeling. It is then a good idea to convert it into a parameter. It is possible to add new parameters on the fly from any input field that supports parameters. You can right-click in an empty text field to do that, but you can also convert an existing value into a parameter.

In the text field, select all text. Right-click and choose .

In the dialog, type elSize in the text field.

In the text field, type Element size.

Click .

The value in the expression for the element size is now automatically substituted by the new parameter name.

The parameter was added to the list in the node, and can later be modified there if necessary. You can also select any parameter in a text field, right-click it, and immediately modify its value or description.

Size

In the window, under > click .

In the window for , locate the section.

From the list, choose .

Free Tetrahedral 1

In the toolbar, click

Size 1

Right-click and choose .

In the window for , locate the section.

Click the button.

Locate the section.

Select the checkbox. In the associated text field, type elSize.

Size 2

In the window, right-click and choose .

Use a finer mesh in the fillets where high stresses can be anticipated.

In the window for , locate the section.

From the list, choose .

Select Boundaries 24, 28, 63, and 70 only.

Locate the section. From the list, choose .

Click

The steps below show how to visualize the load distribution in the current geometry before computing the solution.

Study 1

In the toolbar, click

Note that the Study node automatically defines a solver sequence for the simulation based on the selected physics (Solid Mechanics) and study type (Stationary).

The generation of initial values also creates any default plots. For this study type, it is a stress plot. You can now add an arrow plot of the loads from a list of result templates.

Result Templates

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.

Results

Boundary Load 1

In the window, expand the node, then click .

In the window for , locate the section.

Select the checkbox. In the associated text field, type 1E-8.

From the list, choose .

In the toolbar, click

Now that you have verified the load distribution, solve the model.

Study 1

In the toolbar, click

The default plot shows the von Mises stress distribution, together with an exaggerated (automatically scaled) picture of the deformation.

Set default units for result presentation.

Results

Preferred Units 1

In the toolbar, click

and choose .

In the window for , locate the section.

Click

In the dialog, select > in the tree.

Click .

In the window for , locate the section.

In the table, enter the following settings:


Quantity	Unit	Preferred unit
Displacement	m	mm

Click

In the dialog, select > in the tree.

Click .

In the window for , locate the section.

In the table, enter the following settings:


Quantity	Unit	Preferred unit
Stress tensor	N/m^2	MPa

Click

Volume 1

In structural mechanics models, it is common with high stresses at singular boundary conditions. Here, this is the case at the bolt holes. In order to visualize the interesting parts of the stress distribution better, it is often useful to truncate the value range in plots.

In the window, expand the > node, then click .

In the window for , click to expand the section.

Select the checkbox.

In the text field, type 70.

In the window toolbar, click

next to

, then choose .

Combine the stress plot with the load arrows.

Boundary Load 1

In the window, under > right-click and choose .

Boundary Load 1

In the window, right-click and choose .

In the window for , click to expand the section.

From the list, choose .

Clear the checkbox.

Color Expression

In the window, expand the node, then click .

In the window for , locate the section.

Clear the checkbox.

Click the

button in the toolbar.

Click the

button in the toolbar.

Stress (solid)

In the window, under click .

In the window for , click to expand the section.

From the list, choose .

Find the subsection. Clear the checkbox.

Clear the checkbox.

Locate the section. Select the checkbox.

In the toolbar, click

Add a plot showing the displacement of the bracket. This is another one of the result templates.

Result Templates

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.

Results

Marker 1

In the window, expand the > node.

Right-click and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. In the text field, type 2.

Displacement (solid)

In the window, under click .

In the window for , locate the section.

From the list, choose .

In the toolbar, click

Create another plot to display the principal stresses.

Principal Stress

In the toolbar, click

In the window for , type Principal Stress in the text field.

Click to expand the section. From the list, choose .

Select Domains 1–4 only.

Select the checkbox.

Click the

button in the toolbar.

Principal Stress Volume 1

In the toolbar, click

and choose .

In the window for , locate the section.

Find the subsection. In the text field, type 20.

Find the subsection. In the text field, type 40.

Find the subsection. In the text field, type 10.

Locate the section. From the list, choose .

In the toolbar, click

Plot the stress distribution along the fillet having high stress levels.

Stress Along Fillet

In the toolbar, click

In the window for , type Stress Along Fillet in the text field.

Line Graph 1

Right-click and choose .

Select Edge 48 only.

In the window for , click in the upper-right corner of the section. From the menu, choose > > > > .

In the toolbar, click

Graph Marker 1

Right-click and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. Select the checkbox.

In the text field, type 2.

Click to expand the section. From the list, choose .

In the toolbar, click

You can get an indication of the discretization errors by switching off the averaging between adjacent elements.

Line Graph 1

In the window, click .

In the window for , click to expand the section.

From the list, choose .

In the toolbar, click

Now, assume that the bracket is made from cast iron, a material that is much stronger in compression than in tension. The von Mises criterion, which is isotropic with respect to the stress direction is not suitable in this case. By adding a node, it is possible to check the margins against failure for many different types of materials.

Solid Mechanics (solid)

Linear Elastic Material 1

In the window, under > click .

Safety 1

In the toolbar, click

and choose .

The Rankine criterion is suitable for materials where the failure is governed by either the most positive or most negative stress.

In the window for , locate the section.

From the list, choose .

Here, you can choose to either augment the node under or enter the strength values directly in the node. When a single material is used, it does not matter. When there are several materials in a model, it is a good practice to use the option.

From the σts list, choose . In the associated text field, type 100[MPa].