Buckling Analysis of a Truss Tower

Trusses are commonly used to create light structures that can support heavy loads. When designing such a structure, it is important to ensure its safety. For a tower made of bars, buckling can cause the structure to collapse. This example shows how to compute the critical buckling load using a linear buckling analysis. The solution is compared with an analytical expression for critical load estimation for Euler buckling.

Then a slight prescribed deformation is applied to the structure, and a stationary study with load increasing up to critical buckling load is performed. This study puts in evidence the singularity at critical buckling load.

Model Definition

The model geometry consists of a 19 m tall truss tower with a rectangular section. The critical buckling load is computed using the linear buckling analysis available in the Truss interface.

The geometry is the periodic structure represented in Figure 1 below. It consists of 19 blocks of trusses. Each block has a width of 0.45 m, a depth of 0.40 m and a height of 1.0 m. The trusses that are perpendicular to the ground are thicker and have an outer radius of 15 mm and an inner radius of 10 mm. The remaining trusses have an outer radius of 10 mm and an inner radius of 7 mm. The tower is made out of structural steel, which is one of the predefined materials in the material library.

Figure 1: Geometry of the truss tower.

The tower is fixed at the ground level and a vertical load is applied at the top.

One fourth of the unit load is applied at each point of the tower top so that the critical load factor returned by the linear buckling analysis corresponds to the load that would cause the collapse of the structure.

A second study is performed to put in evidence the singularity at critical buckling load. To do so, the geometry is slightly deformed according to the first mode shape to initiate the buckling deformation. The load is then increased above the calculated critical buckling load in a stationary study using an auxiliary sweep.

Results and Discussion

For a simple column the critical buckling load is given by the Euler buckling formula

where E is the Young’s modulus, I is the area moment of inertia, L is the unsupported length of the column and K is the column effective length factor.

For a column with one end fixed and the other end free to move laterally, K = 2.

For a tower like the one in this example with 4 main bars in the axial direction, the area of moment of inertia of the section can be computed as:

where h is the distance between the vertical bars, and S the cross section area of the bars.

As the section is rectangular with different depth and width values, the tower has one weak direction. Here the depth is 40 cm and the width is 45 cm. This means that the first critical buckling load is expected to be about 86 kN in the depth direction (y direction). In the width direction, which is expected to be stiffer, the critical buckling load is estimated to be about 110 kN.

The results obtained with the linear buckling analysis agree well with these values. Note that the approximation given for the Euler buckling critical load is suitable for a tower structure when the height is significantly larger than the width or the depth.

Figure 2 shows the value of the first critical buckling load and the deformation shape.

Figure 2: Deformation shape at the first critical buckling load.

Figure 3 shows the value of the second critical buckling load and the deformation shape.

Figure 3: Deformation shape at the second critical buckling load.

In addition to the buckling of the whole structure, the safety against buckling of individual truss members must be studied. The critical compressive load for an individual bar can be calculated from material properties and the geometry of the bar:

Here, Imin is the moment of inertia in the weakest direction, based on the cross section data, and Lbar is the length of the bar. In this case the effective length factor Kbar is kept to its default value of 1, which corresponds to a pinned-pinned configuration. From this critical force and the compressive axial force N, the failure index fi and the local buckling safety factor sf can be calculated:

Based on the stationary step with unit loading it appears that the maximum buckling failure index is reached for some diagonal bars near the top of the tower (Figure 4), which undergo less compressive force than vertical bars, but are longer and thinner. The calculated minimal value of safety factor leads to a critical load of about 150 kN, which is significantly higher than the critical load of the two first modes for global buckling. Hence the global buckling will occur before the collapse of the individual truss members.

Figure 4: Maximum local buckling index, with value of minimal safety factor.

The plot of the force in post buckling analysis (Figure 5) shows that the higher forces are located at the base of the tower, while the points at the top of the tower have the maximum horizontal displacement. The displacement plot shows a sudden increase around the critical load, see Figure 6. The stress plot (Figure 7) also shows a sudden increase of the stress at critical load. The stress value becomes very high, probably higher than the physical limits of the material, which may cause a total collapse of the structure.

Figure 5: Force in truss at critical load.

Figure 6: Displacement of the top of the tower in post buckling study.

Figure 7: Stress in the truss at critical load.

Notes About the COMSOL Implementation

The settings of the post buckling analysis are made easier by the node.

It contains a section that enables to choose the buckling solution and modes that will defined the prescribed displacements. The button generates one node for each structural mechanics physics interface involved, and sets the prescribed deformations with the variables defined by the node. The prescribed deformations are those computed in the linear buckling study, multiplied by the scale factor. Low values of scale factor make the buckling effect sharper, but lead to more difficult convergence.

The section enables to select an existing study or choose to create a new one, and choose a parameter used to increase the loads in an auxiliary sweep. The button then creates a new stationary study if required, then checks on, and applies an auxiliary sweep with the selected parameter. The parameters values are filled based on the calculated critical buckling factor, with a logarithmic increase to capture accurately the behavior near the singularity.

Structural_Mechanics_Module/Buckling_and_Wrinkling/truss_tower_buckling

Modeling Instructions

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

Geometric Parameters

In the window, under click .

In the window for , type Geometric Parameters in the text field.

Locate the section. Click

Browse to the model’s Application Libraries folder and double-click the file truss_tower_buckling_geometric_parameters.txt.

Loads

In the toolbar, click

and choose .

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

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


Name	Expression	Value	Description
I1	4A1(depth/2)^2	6.2832E-5 m4	Area moment of inertia weak direction
Fc1	pi^2200e9[Pa]I1/(2*L)^2	85890 N	First critical buckling load
I2	4A1(width/2)^2	7.9522E-5 m4	Area moment of inertia stiffer direction
Fc2	pi^2200e9[Pa]I2/(2*L)^2	1.087E5 N	Second critical buckling load
load	1[N]	1 N	Applied load

Geometry 1

Block 1 (blk1)

In the toolbar, click

In the window for , locate the section.

In the text field, type width.

In the text field, type depth.

In the text field, type height.

Polygon 1 (pol1)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

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


x (m)	y (m)	z (m)
0	depth	0
0	0	height
width	0	0
width	depth	height

Line Segment 1 (ls1)

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. In the text field, type depth.

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

Line Segment 2 (ls2)

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. In the text field, type height.

Locate the section. In the text field, type width, to depth, and to height.

Convert to Curve 1 (ccur1)

In the toolbar, click

and choose .

Click in the window and then press Ctrl+A to select all objects.

In the toolbar, click

Mirror 1 (mir1)

In the toolbar, click

and choose .

Select the object only.

In the window for , locate the section.

Select the check box.

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

In the toolbar, click

Array 1 (arr1)

In the toolbar, click

and choose .

Select the object only.

In the window for , locate the section.

In the text field, type n.

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

Array 2 (arr2)

In the toolbar, click

and choose .

Select the object only.

In the window for , locate the section.

In the text field, type n-1.

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

In the toolbar, click

Click the

button in the toolbar.

Create selections for vertical and transversal edges to make further modeling easier.

Definitions

Vertical Edges

In the toolbar, click

In the window for , type Vertical Edges in the text field.

Locate the section. From the list, choose .

Select Edges 1, 108, 176, and 234 only.

Select the check box.

Transversal Edges

In the toolbar, click

In the window for , type Transversal Edges in the text field.

Locate the section. From the list, choose .

Locate the section. Under , click

In the dialog box, select in the list.

Click .

Add Material

In the toolbar, click

to open the window.

Go to the window.

In the tree, select .

Click in the window toolbar.

In the toolbar, click

to close the window.

Truss (truss)

Cross-Section Data 1

In the window, under click .

In the window for , locate the section.

From the list, choose .

In the do text field, type do1.

In the di text field, type di1.

Cross-Section Data 2

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

From the list, choose .

In the do text field, type do2.

In the di text field, type di2.

Pinned 1

In the toolbar, click

and choose .

In the window for , locate the section.

Click

In the dialog box, type 1 21 41 61 in the text field.

Click .

Point Load 1

In the toolbar, click

and choose .

In the window for , locate the section.

Click

In the dialog box, type 20 40 60 80 in the text field.

Click .

In the window for , locate the section.

Specify the FP vector as


0	x
0	y
-load/4	z

Study 1

Step 2: Linear Buckling

In the window, under click .

In the window for , locate the section.

In the text field, type 2.

In the toolbar, click

Results

Line 1

In the window, expand the node, then click .

In the window for , click to expand the section.

From the list, choose .

Locate the section. In the text field, type 4.

Click the

button in the toolbar.

In the toolbar, click

Create a new plot to check that local buckling of truss members occurs at higher load than the global buckling.

Local Buckling

In the toolbar, click

and choose .

In the window for , type Local Buckling in the text field.

Locate the section. From the list, choose .

Line 1

Right-click and choose .

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

Locate the section. Clear the check box.

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

Locate the section. From the list, choose .

In the text field, type truss.re.

Select the check box. In the associated text field, type 2.

Local Buckling

In the window, click .

Max/Min Line 1

In the toolbar, click

and choose .

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

Locate the section. From the list, choose .

Locate the section. In the text field, type Safety factor .

In the toolbar, click

Now prescribe a deformation to the geometry from the calculated buckling mode to perform a post-buckling study.

Definitions

Buckling Imperfection 1 (bcki1)

In the toolbar, click

and choose .

In the window for , locate the section.

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


Mode	Scale factor
1	1e3

Click in the upper-right corner of the section.

This button creates a node with the requested deformation settings. The newly created is automatically disabled in the existing study steps to enable further computation without changes in the results.