COMSOL 6.4 - Bracket — Linear Buckling Analysis

Buckling analysis is an important study type in structural mechanics because it provides an estimate of the critical load that can cause sudden collapse of the structure. In this example, you first learn how to perform a linear buckling analysis to find the critical buckling load. In a second study, you will compute the nonlinear deformation while increasing the applied load until buckling occurs.

It is recommended you review the Introduction to the Structural Mechanics Module, which includes background information and discusses the bracket_basic.mph model relevant to this example.

In the Structural Mechanics Modeling chapter of the Structural Mechanics Module User’s Guide:

•

Linearized Buckling Analysis

•

Buckling Analysis

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 load is applied to the pin hole in the left arm, and has a resultant oriented in the positive y direction, as shown in Figure 1.

Figure 1: Load distribution.

Results and Discussion

Figure 2 shows the first buckling mode for the bracket geometry. The critical load factor is about 6·104, which corresponds to the critical buckling load 60 kN since the static load used is 1 N.

Figure 2: First buckling mode and critical load factor value.

Figure 3 shows the solution from the nonlinear analysis. The variation of the displacement in the right arm of the bracket is plotted as function of increasing applied load (blue). You can see how the displacement deviates strongly from the linear response as the applied load approaches the critical buckling load from the linear buckling analysis. A deviation of 20% from linearity is obtained at an applied force of 57 kN.

Figure 3: Bracket right arm y-displacement versus applied load.

In a linearized buckling analysis, it is important to check that the stresses at the buckling load not are so large that material nonlinearities become important. If that is the case, a nonlinear analysis of the type shown here must be performed, but with a suitable material model.

In Figure 4, the von Mises equivalent stress is shown for the last load step in the nonlinear analysis. At some locations, the stress are well above the yield stress, which can be assumed to be 350 MPa for this type of steel. This may invalidate the analysis.

In Figure 5, a damage index is shown. In the regions where the value is 1, the yield stress is exceeded. Given this result, it would be good practice to also include plasticity in the nonlinear analysis. If you do that (all that is needed is to add a subnode under , and run again) you will find that the failure load is reduced by about 50%.

Figure 4: The von Mises stress at the last load step.

Figure 5: Regions where the stress exceeds the yield stress at the last load step.

Notes About the COMSOL Implementation

In a linear buckling analysis, you perform the following operations:

•

Run a linear static analysis using a load of arbitrary magnitude.

•

Compute the eigenvalue problem including the stresses from the static load. The first eigenvalue corresponds to the value of the critical buckling load.

COMSOL Multiphysics automatically runs the sequence described above and then returns the value of the critical buckling load.

To perform a nonlinear buckling analysis, use the continuation solver to ramp up the load smoothly. You can use a stop condition to automatically stop the solver once a certain criterion is reached. In this example, the stop criterion is the deviation from linearity of the y-displacement in the right arm. The linear displacement response is predicted by using the solution computed under a unit load case for the linear buckling.

Structural_Mechanics_Module/Tutorials/bracket_linear_buckling

Modeling Instructions

Application Libraries

From the menu, choose .

In the window, select > > in the tree.

Click

Global Definitions

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	1[N]	1 N	Force per hole

Definitions

Change reference orientation of the cylindrical system so that the load is pointing inward.

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	-sign(X)	0

Solid Mechanics (solid)

Boundary Load 1

In the toolbar, click

and choose .

Apply a boundary load to the bracket holes. Since the entire circumference of each hole is selected, the expression for the pressure must be truncated so that it acts only on the intended 180 degrees

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


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

Add Study

In the toolbar, click

to open the window.

Go to the window.

Find the subsection. In the tree, select > .

Click the button in the window toolbar.

In the toolbar, click

to close the window.

Study 1

In the toolbar, click

Results

Mode Shape (solid)

Click the

button in the toolbar.

Click the

button in the toolbar.

The default plot shows the mode shape of the first buckling mode.

Evaluate the y-direction displacement corresponding to the applied unit load.

Point Evaluation 1

In the toolbar, click

In the window for , locate the section.

From the list, choose .

Select Point 5 only.

Locate the section. In the table, enter the following settings:


Expression	Unit	Description
v	mm	Displacement field, Y-component

Click

You can now determine the linear relation between displacement and applied load. This can be used in the later analysis to determine when the nonlinear solution deviates from the linear one.

Definitions

Integration 1 (intop1)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Select Point 5 only.

Add Study

In the toolbar, click

to open the window.

Go to the window.

Find the subsection. In the tree, select > .

Click the button in the window toolbar.

In the toolbar, click

to close the window.

Study 2

Step 1: Stationary

In the window for , locate the section.

Select the checkbox.

Click to expand the section. Select the checkbox.

Click

In the table, enter the following settings:


Parameter name	Parameter value list
Fh (Force per hole)	1 1e3 5e3 1e4 2e4 5.924e4*log10(({range(2,1,10)}+1)/1.1)^(1/5)

Solution 3 (sol3)

In the toolbar, click

In the window, expand the node.

In the window, expand the > > > node.

Right-click > > > > and choose .

In the window for , locate the section.

Click

In the table, enter the following settings:


Stop expression	Stop if	Active	Description
comp1.intop1(comp1.v)/(Fh*1.12E-8)/1.2	True (>=1)	√	Stop expression 1

Locate the section. From the list, choose .

Clear the checkbox.

In the toolbar, click

Results

Stress (solid)

Click the

button in the toolbar.

Follow the instructions below to reproduce Figure 3.

1D Plot Group 3

In the toolbar, click

In the window for , locate the section.

From the list, choose .

Point Graph 1

Right-click and choose .

Select Point 5 only.

In the window for , locate the section.

In the text field, type v.

Displacement

In the window, under click .

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

Locate the section.

Select the checkbox. In the associated text field, type Applied force [N].

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

Point Graph 2

Right-click and choose .

Select Point 5 only.

In the window for , locate the section.

In the text field, type Fh*1.12E-8[m/N].

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

Displacement

In the window, click .

In the window for , click to expand the section.

From the list, choose .

In the toolbar, click

Solid Mechanics (solid)

Linear Elastic Material 1

In the window, under > click .

Safety 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the σts list, choose . In the associated text field, type 350[MPa].

A feature does not affect the solution, it only defines variables. You will thus not need to solve the study again. It is sufficient to update it so that the new variables are accessible.

Study 2

In the toolbar, click