COMSOL 6.4 - 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 directions.

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

Model Definition

This example is an extension of the one 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 twisting 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 twisting 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 significantly lower in this case..

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°.

The reaction forces at the first bolt location are shown in Figure 5. It should be noted that for a pretensioned bolt connection, this cannot be directly interpreted as the bolt force. In such a case, the force distribution in the bolts is far more complex. Only if the bracket is connected to its surrounding by rivets, or loosely tightened bolts, this result reflects the actual forces in the joint element.

Figure 5: Forces at the first attachment point as function of the load angle

Finally, the variation of the stress with the load angle in some points is studied in Figure 6. It is clear that the load angles that induce a bending/twisting state cause higher stresses than those which give predominantly tension and compression.

Figure 6: von Mises stress as function of the load angle for three different high stress locations.

Notes About the COMSOL Implementation

In COMSOL Multiphysics, you have 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.

It can be noted that the stiffness matrix in this case is only inverted once. The solver automatically recognizes the fact that it is only the loads, and thus the right hand side of the system of equations, that are changing between the parameter steps.

Structural_Mechanics_Module/Tutorials/bracket_parametric

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

Application Libraries

From the menu, choose .

In the window, select > > in the tree.

Click

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

Component 1 (comp1)

Let the reference orientation of the cylindrical system rotate with the load orientation

In the window, expand the node.

Definitions

Cylindrical System 2 (sys2)

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

In the window for , locate the section.

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


x	y	z
0	sin(theta0)*sign(X)	cos(theta0)*sign(X)

Left Pin Hole

Since the load is rotating inside the holes, it is no longer sufficient that half of the holes are selected.

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

In the window for , locate the section.

Select the checkbox.

Right Pin Hole

In the window, click .

In the window for , locate the section.

Select the checkbox.

Solid Mechanics (solid)

Since the entire circumference of each hole is now selected, the expression for the pressure must be truncated so that it acts only on the intended 180 degrees.

Boundary Load 1

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

In the window for , locate the section.

Specify the fA vector as


if(abs(sys2.phi)<pi/2,-p0*cos(sys2.phi),0)	n

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 checkbox.

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.

In the window for , click