COMSOL 6.3 - Linear Buckling Analysis of a Truss Tower with Dead Loads

Linear Buckling Analysis of a Truss Tower with Dead Loads

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 due to compressive loads that come from external vertical loading and from the self weight of the structure. Linear buckling analysis is a common way to calculate the critical buckling load. The calculated critical load factor is usually interpreted as a common multiplicative factor on all loads. Sometimes, you want to evaluate the critical value for a specific load, keeping some other loads constant. Distinguishing between constant (dead) loads and varying (live) loads makes it possible to get the critical load factor for only certain loads.

This example shows how to perform a linear bucking analysis with dead loads on a guyed truss tower where the pretension force in the guy wires and the gravity force are the dead loads. The vertical force at the top of the tower is the live 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. 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. Two sets of four guys are fixed at each corner of the tower, at two different heights. The tower and guys are fixed at the ground level, the guys are prestressed at 4 kN. Gravity is applied to the structure. A vertical load is applied at the four top points, one fourth of the unit load each. Hence, the critical load factor returned by the linear buckling analysis corresponds to the external load that would cause the collapse of the structure.

The guys are modeled using the Wire interface. As long as the guys are in tension, they act as bars, so it would also have been possible to model them in the Truss interface.

Figure 1: Geometry of the guyed truss tower.

In linear buckling theory the stiffness matrix K is separated into a linear part and a linearized nonlinear part which is proportional to the applied load

In the presence of dead loads, the loads are separated into constant dead loads Q0 and live loads P0

For a better linearization of nonlinear problems, the live loads are not calculated separately, but associated with the dead loads. Hence, an initial stationary solution is calculated with dead loads only. Then, a second solution is calculated with dead and live loads. The stiffness matrix is then

These two solutions are then selected as the linearization point and live load solution in the linear buckling study step.

Local Buckling

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:

In presence of dead loads, the aim is to find the multiplicative factor to live loads which is needed to reach the critical force:

Thus, the safety factor of the live load can be calculated from the live and dead load solutions:

Results and Discussion

The two first buckling modes, corresponding respectively to buckling in the depth direction (y direction) and width direction, are shown in Figure 2 and Figure 3. The prestressed guys make it possible to increase the critical load factor up to 92 kN and 117 kN, respectively.

Figure 2: First buckling mode.

Figure 3: Second buckling mode.

Figure 4 plots the local buckling index for live loads in the tower. The calculated minimal value for safety factor is 131 kN for the diagonal bars at the base of the tower.

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

Notes About the COMSOL Implementation

The study step has a section for setting the linearization point and the live load solutions. In the absence of dead loads, only one solution is needed, so the live load option must be kept at the default setting . When dead loads are present, two different solutions must be selected. They can come, for example, from two different study steps, from two different parameter values of an auxiliary sweep, or from two load cases. In this model, two stationary study steps are used, the first one with live load disabled.

Structural_Mechanics_Module/Buckling_and_Wrinkling/truss_tower_buckling_guys

Modeling Instructions

From the menu, choose .

New

In the window, click

Model Wizard

In the window, click

In the tree, select > .

Click .

In the tree, select > .

Click .

Click

In the tree, select > .

Click

Global Definitions

Tower Geometric Parameters

In the window, under click .

In the window for , type Tower 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.

Guy Geometric Parameters

In the toolbar, click

and choose > .

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

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


Name	Expression	Value	Description
gnd_attach_guy1	6[m]	6 m	Ground attachment distance of guy 1
gnd_attach_guy2	12[m]	12 m	Ground attachment distance of guy 2
guy_d	5[mm]	0.005 m	Diameter of guy 1 and guy 2
guy_height1	7[m]	7 m	Height of guy 1
guy_height2	12[m]	12 m	Height of guy 2
guy_area	pi/4*guy_d^2	1.9635E-5 m²	Area of guy 1 and guy 2
kA	3.927e6[N]	3.927E6 N	Axial stiffness
rhoL	0.15413[kg/m]	0.15413 kg/m	Mass per unit length

Geometry 1

In the toolbar, click and choose .

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

In the toolbar, click

In the window, under click .

Array 1 (arr1), Array 2 (arr2), Block 1 (blk1), Convert to Curve 1 (ccur1), Line Segment 1 (ls1), Line Segment 2 (ls2), Mirror 1 (mir1), Polygon 1 (pol1)

In the window, under > , Ctrl-click to select , , , , , , , and .

Right-click and choose .

Tower

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

Line Segment 3 (ls3)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

In the text field, type guy_height1-mod(guy_height1,height).

Locate the section. From the list, choose .

In the text field, type -gnd_attach_guy1*width/sqrt(width^2+depth^2).

In the text field, type -gnd_attach_guy1*depth/sqrt(width^2+depth^2).

Locate the section. Find the subsection. Click .

In the dialog, type Guy 1 in the text field.

Click .

In the window for , click

Line Segment 4 (ls4)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

In the text field, type guy_height2-mod(guy_height2,height).

Locate the section. From the list, choose .

In the text field, type -gnd_attach_guy2*width/sqrt(width^2+depth^2).

In the text field, type -gnd_attach_guy2*depth/sqrt(width^2+depth^2).

Locate the section. Find the subsection. Click .

In the dialog, type Guy 2 in the text field.

Click .

In the window for , click

Mirror 2 (mir2)

In the toolbar, click

and choose .

Select the objects and only.

In the window for , locate the section.

Select the checkbox.

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

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

In the text field, type 0.

Click

Mirror 3 (mir3)

In the toolbar, click

and choose .

Select the objects , , , and only.

In the window for , locate the section.

Select the checkbox.

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

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

In the text field, type 0.

Click

Click the

button in the toolbar.

Line Segment 3 (ls3), Line Segment 4 (ls4), Mirror 2 (mir2), Mirror 3 (mir3)

In the window, under > , Ctrl-click to select , , , and .

Right-click and choose .

Guys

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

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 5, 112, 180, and 240 only.

Select the checkbox.

Transversal Truss Edges

In the toolbar, click

In the window for , type Transversal Truss Edges 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 .

Tower

In the toolbar, click

In the window for , type Tower 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 .

Guys

In the toolbar, click

In the window for , type Guys 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 .

Truss (truss)

In the window, under click .

In the window for , locate the section.

From the list, choose .

Cross-Section Data (Vertical Edges)

In the window, under > click .

In the window for , type Cross-Section Data (Vertical Edges) in the text field.

Locate the section. From the list, choose .

In the do text field, type do1.

In the di text field, type di1.

Cross-Section Data (Other Truss Edges)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

In the do text field, type do2.

In the di text field, type di2.

In the text field, type Cross-Section Data (Other Truss Edges).

Pinned 1

In the toolbar, click

and choose .

Select Points 1–5, 25, 45, 65, and 85–88 only.

Gravity 1

In the toolbar, click

and choose .

Point Load 1

In the toolbar, click

and choose .

Select Points 24, 44, 64, and 84 only.

In the window for , locate the section.

From the list, choose .

Specify the Ftot vector as


0	x
0	y
-1[N]	z

Wire (wire)

In the window, under click .

In the window for , locate the section.

From the list, choose .

Use the same dependent variable in both physics interfaces in order to share the displacement where the guys are attached to the tower.

Click to expand the section. In the text field, type u.

Elastic Wire 1

In the window, under > click .

In the window for , locate the section.

In the A text field, type guy_area.

Initial Stress and Strain 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. In the Ni text field, type 4[kN].

Pinned 1

In the toolbar, click

and choose .

Select Points 1–4 and 85–88 only.

Gravity 1

In the toolbar, click

and choose .

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.

Materials

Structural steel (mat1)

In the window for , locate the section.

From the list, choose .

Wire material

In the window, right-click and choose .

In the window for , type Wire material in the text field.

Locate the section. From the list, choose .

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


Property	Variable	Value	Unit	Property group
Axial stiffness	k_A	kA	N	Elastic wire
Mass per unit length	rho_L	rhoL	kg/m	Elastic wire

Mesh 1

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.

From the list, choose .

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

Distribution 2

In the window, right-click and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. In the text field, type 10.

Distribution 3

Right-click and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. In the text field, type 10.

Click

The buckling study requires two stationary study steps to compute live and dead load solutions.

Study 1

Step 3: Stationary 2

In the toolbar, click

and choose > .

Right-click and choose .

Use the first stationary study step to solve for the dead loads only.

Stationary, Dead Loads Only

In the window, click .

In the window for , type Stationary, Dead Loads Only in the text field.

Locate the section. Select the checkbox.

In the tree, select > > .

Click

In the second stationary study step, both live and dead loads are applied.

Stationary, Dead + Live Loads

In the window, under click .

In the window for , type Stationary, Dead + Live Loads in the text field.

You need to generate the solver sequence to enable the selection of solutions in the linear buckling steps.

Solution 1 (sol1)

In the toolbar, click

Step 3: Linear Buckling

In the window, under click .

In the window for , locate the section.

In the text field, type 2.

Locate the section. From the list, choose .

From the list, choose .

Locate the section. From the list, choose .

In the toolbar, click

Results

Line 1

In the window, expand the node, then click .

In the window for , locate the section.

In the text field, type 6.

Line 1

In the window, expand the > node.

Right-click and choose .

Line 2

In the window, right-click and choose .

In the window for , click to expand the section.

From the list, choose .

Mode Shape (truss)

In the window, click .

In the toolbar, click

Add variables to assess the risk of local buckling.

Definitions

Variables 1

In the window, under right-click and choose .

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Unit	Description
lbs_f	(1-withsol('sol2',truss.lbf_i))/(withsol('sol3',truss.lbf_i)-withsol('sol2',truss.lbf_i))		Local buckling safety factor
lbf_i	1/lbs_f		Local buckling failure index