Bracket — Parametric 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 example includes computing the solution to a case where the direction of the load is changed using a parametric sweep over a set of angles.

It is recommended you review the Introduction to the Structural Mechanics Module, which includes background information.

Model Definition

This model is an extension of the example described in the section “The Fundamentals: A Static Linear Analysis” in the Introduction to the Structural Mechanics Module. The same model is also available as a standalone model in the Application Libraries as Bracket - Static Analysis.

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. To model the external load from the pin, you specify a surface load p with a trigonometric distribution on the inner surfaces of the two holes:

where P0 is the peak load intensity. The main direction of the load is defined by θ0, the angle from the y-axis. The load on the two holes acts in opposite directions. The orientation of the load is controlled by a local coordinate system with axis directions generated using the sweep parameter theta0.

Results

Figure 2 shows the von Mises stress distribution corresponding to a bending load case, where the load acts in the positive z direction in the left arm and in the negative z direction in the right arm.

Figure 2: Von Mises stress in a bending load case (parameter theta0 = 0°).

Figure 3 shows the von Mises stress distribution corresponding of a tensile load in the right arm and a compressive load in the left arm. The maximum von Mises stress value is lower in this case. A stress concentration can be seen also around the hole in the arm which is in tension.

Figure 3: Von Mises stress in a tensile and compressive load case (parameter theta0 = 90°).

Figure 4 shows the von Mises stress distribution corresponding to a load orientation of 130°.

Figure 4: Von Mises stress for parameter theta0 = 130°.

Figure 5 shows that the x-component of the reaction force in all bolts for all load cases.

Figure 5: Reaction forces (x-component) as a function of angle.

Figure 6 shows the y-component and Figure 7 shows the z-component of the reaction force in all bolts for all load cases.

Figure 6: Reaction forces (y-component) as a function of angle.

Figure 7: Reaction forces (z-component) as a function of load angle.

Notes About the COMSOL Implementation

COMSOL Multiphysics has two ways to perform parametric studies — using either a node or the from the node. In this example, either method can be used. An is used here, but the continuation solver is not used. The continuation solver uses the solution from the previous parameter as an initial guess to calculate the current parameter value, which is the preferred option for nonlinear problems. Using the node is necessary for applications requiring, for example, geometric parameterization.

Structural_Mechanics_Module/Tutorials/bracket_parametric

Parametric studies can be set up from scratch or, as in this example, added to an existing study.

From the menu, choose .

Browse to the model’s Application Libraries folder and double-click the file bracket_static.mph.

Results

Stress (solid)

Click the

button in the toolbar.

Global Definitions

In this model, the stress in the bracket is computed for different load orientations. First add a parameter to set the load direction angle.

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
theta0	0[deg]	0 rad	Load direction angle

Definitions

You will now create a local coordinate system that will rotate with the load orientation.

Cylindrical System 2 (sys2)

In the window, expand the node.

Right-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	YC	0

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	sin(theta0)	cos(theta0)

Analytic 1 (load)

Change the expression for the load distribution.

In the window, click .

In the window for , locate the section.

In the text field, type F*cos(p).

In the text field, type F, p.

Locate the section. In the text field, type Pa, rad.

Solid Mechanics (solid)

Change the boundary loads to consider the parameterized direction.

Boundary Load 1

In the window, expand the node, then click .

In the window for , locate the section.

From the list, choose .

Locate the section. Specify the FA vector as


load(P0sign(X),sys2.phi)(sign(X)*(abs(sys2.phi)-pi/2)<0)	r
0	phi
0	a

Study 1

Add an auxiliary sweep parameter, and compute the results.

Step 1: Stationary

In the window, expand the node, then click .

In the window for , click to expand the section.

Select the check box.

Click

In the table, enter the following settings:


Parameter name	Parameter value list	Parameter unit
theta0 (Load direction angle)	range(0,10,160)	deg

From the list, choose .

In the toolbar, click

Results

Stress (solid)

The default plot shows the solution for the last parameter value (160[deg]). You can easily change the parameter value to display the plot and then compare solutions for different load cases.

The following instructions reproduce Figure 2 to Figure 4.