PDF
In-Plane and Space Truss
Introduction
In the following example you first build and solve a simple 2D truss model using the 2D Truss interface. Later on, you analyze a 3D variant of the same problem using the 3D Truss interface. This model calculates the deformation and forces of a simple geometry. The example is based on problem 11.1 in Aircraft Structures for Engineering Students by T.H.G. Megson (Ref. 1). The results are compared with the analytical results given in Ref. 1.
Model Definition
The 2D geometry consists of a square symmetrical truss built up by five members. All members have the same cross-sectional area A. The side length is L, and the Young’s modulus is E.
Figure 1: The truss geometry.
In the 3D case, another copy of the diagonal bars are rotated 90° around the vertical axis, so that a cube-like structure with one diagonal member is generated. The figure above is thus applicable to a view in the zy-plane as well as in the xy-plane. The central bar is given twice the area of the other members. This creates a space truss which with equivalent symmetry, but twice the vertical stiffness.
GEOMETRY
•
Truss side length, L = 2 m
•
The truss members have a circular cross section with a radius of 0.05 m. In the 3D case, the area of the central bar is doubled.
Material
Aluminum: Young’s modulus, E = 70 GPa, Poisson’s ratio ν = 0.3.
Constraints
In the 2D case, displacements in both directions are constrained at vertices a and b. In the 3D case, the two new points are constrained in the same way.
Load
In the 2D case, a vertical force F of 50 kN is applied at the bottom corner. In the 3D case, the value 100 kN is used instead in order to get the same displacements.
Results and Discussion
The following table shows a comparison between the results calculated with the Structural Mechanics Module and the analytical results from Ref. 1.
Result
COMSOL Multiphysics
Ref. 1
Displacement at d
-5.14·10-4 m
-5.15·10-4 m
Displacement at c
-2.13·10-4 m
-2.13·10-4 m
Axial force in member ac=bc
-10.4 kN
-10.4 kN
Axial force in member ad=bd
25.0 kN
25.0 kN
Axial force in member cd
14.6 kN
14.6 kN
The results are in nearly perfect agreement.
Figure 2 and Figure 3 show the deformed geometry together with the axial forces in the truss members.
Figure 2: Deformed geometry and axial forces for the 2D case.
Figure 3: Deformed geometry and axial forces for the 3D case.
Notes About the COMSOL Implementation
In this example you build the 2D and the 3D truss as two different components within the same model file. This is not essential; you could equally well choose to create the components in two separate model files.
Reference
1. T.H.G. Megson, Aircraft Structures for Engineering Students, Edward Arnold, p. 404, 1985
Application Library path: Structural_Mechanics_Module/Verification_Examples/inplane_and_space_truss
Modeling Instructions
From the File menu, choose New.
New
In the New window, click  Model Wizard.
Model Wizard
1
In the Model Wizard window, click  2D.
2
In the Select Physics tree, select Structural Mechanics > Truss (truss).
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies > Stationary.
6
Click  Done.
Geometry 1
Square 1 (sq1)
1
In the Geometry toolbar, click  Square.
2
In the Settings window for Square, locate the Size section.
3
In the Side length text field, type 2.
4
Locate the Rotation Angle section. In the Rotation text field, type 45.
5
Locate the Object Type section. From the Type list, choose Curve.
6
Click  Build All Objects.
7
Click the  Zoom Extents button in the Graphics toolbar.
Line Segment 1 (ls1)
1
In the Geometry toolbar, click  More Primitives and choose Line Segment.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
From the Specify list, choose Coordinates.
4
Locate the Endpoint section. From the Specify list, choose Coordinates.
5
In the y text field, type sqrt(8).
6
Click  Build All Objects.
Truss (truss)
Cross-Section Data 1
1
In the Model Builder window, under Component 1 (comp1) > Truss (truss) click Cross-Section Data 1.
2
In the Settings window for Cross-Section Data, locate the Cross-Section Definition section.
3
From the Section type list, choose Circular.
4
In the do text field, type 0.05.
Pinned 1
1
In the Physics toolbar, click  Points and choose Pinned.
2
Select Points 1 and 4 only.
Point Load 1
1
In the Physics toolbar, click  Points and choose Point Load.
2
Select Point 2 only.
3
In the Settings window for Point Load, locate the Force section.
4
Specify the FP vector as
0
x
-50e3
y
Global Definitions
In this example, the same material data will be referenced from two different components, so it is convenient to define a global material.
Material 1 (mat1)
1
In the Model Builder window, under Global Definitions right-click Materials and choose Blank Material.
2
In the Settings window for Material, click to expand the Material Properties section.
3
In the Material properties tree, select Basic Properties > Density.
4
Click  Add to Material.
5
In the Material properties tree, select Solid Mechanics > Linear Elastic Material > Young’s Modulus and Poisson’s Ratio.
6
Click  Add to Material.
7
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Density
rho
2900
kg/m³
Basic
Young’s modulus
E
70e9
Pa
Young’s modulus and Poisson’s ratio
Poisson’s ratio
nu
0.3
1
Young’s modulus and Poisson’s ratio
Materials
Material Link 1 (matlnk1)
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose More Materials > Material Link.
Study 1
In the Study toolbar, click  Compute.
Result Templates
1
In the Results toolbar, click  Result Templates to open the Result Templates window.
2
Go to the Result Templates window.
3
In the tree, select Study 1/Solution 1 (sol1) > Truss > Force (truss).
4
Click the Add Result Template button in the window toolbar.
5
In the Results toolbar, click  Result Templates to close the Result Templates window.
Results
Force (truss)
1
In the Model Builder window, expand the Results > Force (truss) node, then click Force (truss).
2
In the Settings window for 2D Plot Group, locate the Color Legend section.
3
Select the Show maximum and minimum values checkbox.
Line 1
1
In the Model Builder window, click Line 1.
2
In the Settings window for Line, locate the Expression section.
3
From the Unit list, choose kN.
4
Click the  Zoom Extents button in the Graphics toolbar.
Next, compute the displacements at d (Vertex 2) and c (Vertex 3).
Displacement of Vertices (2D)
1
In the Results toolbar, click  Evaluation Group.
2
In the Settings window for Evaluation Group, type Displacement of Vertices (2D) in the Label text field.
Point Evaluation 1
1
Right-click Displacement of Vertices (2D) and choose Point Evaluation.
2
Select Points 2 and 3 only.
3
In the Settings window for Point Evaluation, locate the Expressions section.
4
In the table, enter the following settings:
Expression
Unit
Description
v
m
Displacement field, Y component
5
In the Displacement of Vertices (2D) toolbar, click  Evaluate.
Although you can read off the values of the local axial force in the members ac and ad from the max and min values for the color legend for the plot in the Graphics window, it is instructive to see how you can compute such values more generally.
Definitions
Add nonlocal average couplings for the members ac, ad, and cd. You will use these for defining variables that evaluate the axial forces in these members.
Average 1 (aveop1)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Average.
2
In the Settings window for Average, type aveop_ac in the Operator name text field.
3
Locate the Source Selection section. From the Geometric entity level list, choose Boundary.
4
Select Boundary 5 only.
Average 2 (aveop2)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Average.
2
In the Settings window for Average, type aveop_ad in the Operator name text field.
3
Locate the Source Selection section. From the Geometric entity level list, choose Boundary.
4
Select Boundary 4 only.
Average 3 (aveop3)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Average.
2
In the Settings window for Average, type aveop_cd in the Operator name text field.
3
Locate the Source Selection section. From the Geometric entity level list, choose Boundary.
4
Select Boundary 3 only.
Variables 1
1
In the Definitions toolbar, click  Local Variables.
2
In the Settings window for Variables, locate the Variables section.
3
In the table, enter the following settings:
Name
Expression
Unit
Description
F_ac
aveop_ac(truss.Nxl)
N
Axial force, member ac
F_ad
aveop_ad(truss.Nxl)
N
Axial force, member ad
F_cd
aveop_cd(truss.Nxl)
N
Axial force, member cd
Study 1
Update the solution to evaluate the variables you just defined.
Solution 1 (sol1)
1
In the Model Builder window, expand the Study 1 > Solver Configurations node.
2
Right-click Study 1 > Solver Configurations > Solution 1 (sol1) and choose Solution > Update.
Results
Axial Force in Members (2D)
1
In the Results toolbar, click  Evaluation Group.
2
In the Settings window for Evaluation Group, type Axial Force in Members (2D) in the Label text field.
Global Evaluation 1
1
Right-click Axial Force in Members (2D) and choose Global Evaluation.
2
In the Settings window for Global Evaluation, locate the Expressions section.
3
In the table, enter the following settings:
Expression
Unit
Description
F_ac
N
Axial force, member ac
F_ad
N
Axial force, member ad
F_cd
N
Axial force, member cd
4
In the Axial Force in Members (2D) toolbar, click  Evaluate.
The values in the evaluation group agree with those of the analytical reference solution.
Root
Now create the 3D truss as a new model.
Add Component
In the Model Builder window, right-click the root node and choose Add Component > 3D.
Add Physics
1
In the Home toolbar, click  Add Physics to open the Add Physics window.
2
Go to the Add Physics window.
3
In the tree, select Recently Used > Truss (truss).
4
Find the Physics interfaces in study subsection. In the table, clear the Solve checkbox for Study 1.
5
Click the Add to Component 2 button in the window toolbar.
6
In the Home toolbar, click  Add Physics to close the Add Physics window.
Add Study
1
In the Home toolbar, click  Add Study to open the Add Study window.
2
Go to the Add Study window.
3
Find the Studies subsection. In the Select Study tree, select General Studies > Stationary.
Switch off the 2D truss physics in this study.
4
Find the Physics interfaces in study subsection. In the table, clear the Solve checkbox for Truss (truss).
5
Click the Add Study button in the window toolbar.
6
In the Home toolbar, click  Add Study to close the Add Study window.
Geometry 2
Work Plane 1 (wp1)
1
In the Geometry toolbar, click  Work Plane.
2
In the Model Builder window, click Work Plane 1 (wp1).
3
In the Settings window for Work Plane, click  Go to Plane Geometry.
Work Plane 1 (wp1) > Square 1 (sq1)
1
In the Work Plane toolbar, click  Square.
2
In the Settings window for Square, locate the Size section.
3
In the Side length text field, type 2.
4
Locate the Rotation Angle section. In the Rotation text field, type 45.
5
Locate the Object Type section. From the Type list, choose Curve.
6
In the Work Plane toolbar, click  Build All.
Rotate 1 (rot1)
1
In the Model Builder window, right-click Geometry 2 and choose Transforms > Rotate.
2
In the Settings window for Rotate, locate the Input section.
3
Select the Keep input objects checkbox.
4
Select the object wp1 only.
5
Locate the Rotation section. From the Axis type list, choose Cartesian.
6
In the y text field, type 1.
7
In the z text field, type 0.
8
In the Angle text field, type 90.
9
Click  Build All Objects.
Line Segment 1 (ls1)
1
In the Geometry toolbar, click  More Primitives and choose Line Segment.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
From the Specify list, choose Coordinates.
4
Locate the Endpoint section. From the Specify list, choose Coordinates.
5
In the y text field, type sqrt(8).
6
Click  Build All Objects.
Definitions (comp2)
Add nonlocal average couplings for the members ac, ad, and cd and corresponding axial force variables.
Average 4 (aveop4)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Average.
2
In the Settings window for Average, type aveop_ac in the Operator name text field.
3
Locate the Source Selection section. From the Geometric entity level list, choose Edge.
4
Select Edge 8 only.
Average 5 (aveop5)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Average.
2
In the Settings window for Average, type aveop_ad in the Operator name text field.
3
Locate the Source Selection section. From the Geometric entity level list, choose Edge.
4
Select Edge 4 only.
Average 6 (aveop6)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Average.
2
In the Settings window for Average, type aveop_cd in the Operator name text field.
3
Locate the Source Selection section. From the Geometric entity level list, choose Edge.
4
Select Edge 5 only.
Variables 2
1
In the Definitions toolbar, click  Local Variables.
2
In the Settings window for Variables, locate the Variables section.
3
In the table, enter the following settings:
Name
Expression
Unit
Description
F_ac
aveop_ac(truss2.Nxl)
N
Axial force, member ac
F_ad
aveop_ad(truss2.Nxl)
N
Axial force, member ad
F_cd
aveop_cd(truss2.Nxl)
N
Axial force, member cd
Truss 2 (truss2)
Cross-Section Data 1
1
In the Model Builder window, under Component 2 (comp2) > Truss 2 (truss2) click Cross-Section Data 1.
2
In the Settings window for Cross-Section Data, locate the Cross-Section Definition section.
3
In the A text field, type pi/4*0.05^2.
Cross-Section Data 2
1
In the Physics toolbar, click  Edges and choose Cross-Section Data.
2
Select Edge 5 only.
3
In the Settings window for Cross-Section Data, locate the Cross-Section Definition section.
4
In the A text field, type 2*pi/4*0.05^2.
Pinned 1
1
In the Physics toolbar, click  Points and choose Pinned.
2
Select Points 1, 3, 4, and 6 only.
Point Load 1
1
In the Physics toolbar, click  Points and choose Point Load.
2
Select Point 2 only.
3
In the Settings window for Point Load, locate the Force section.
4
Specify the FP vector as
0
x
-100e3
y
0
z
Materials
Material Link 2 (matlnk2)
In the Model Builder window, under Component 2 (comp2) right-click Materials and choose More Materials > Material Link.
Study 2
In the Study toolbar, click  Compute.
Result Templates
1
In the Results toolbar, click  Result Templates to open the Result Templates window.
2
Go to the Result Templates window.
3
In the tree, select Study 2/Solution 2 (3) (sol2) > Truss 2 > Force (truss2).
4
Click the Add Result Template button in the window toolbar.
5
In the Results toolbar, click  Result Templates to close the Result Templates window.
Results
Force (truss2)
1
In the Model Builder window, click Force (truss2).
2
In the Settings window for 3D Plot Group, locate the Color Legend section.
3
Select the Show maximum and minimum values checkbox.
Line 1
1
In the Model Builder window, click Line 1.
2
In the Settings window for Line, locate the Expression section.
3
From the Unit list, choose kN.
Proceed to compute the displacements at d (Vertex 2) and c (Vertex 5).
Displacement of Vertices (3D)
1
In the Model Builder window, right-click Displacement of Vertices (2D) and choose Duplicate.
2
In the Settings window for Evaluation Group, type Displacement of Vertices (3D) in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study 2/Solution 2 (3) (sol2).
Point Evaluation 1
1
In the Model Builder window, expand the Displacement of Vertices (3D) node, then click Point Evaluation 1.
2
Select Points 2 and 5 only.
3
In the Settings window for Point Evaluation, locate the Expressions section.
4
In the table, enter the following settings:
Expression
Unit
Description
v2
m
Displacement field, Y component
5
In the Displacement of Vertices (3D) toolbar, click  Evaluate.
The results are nearly identical to those of the 2D case.
Finally, compute the axial force values.
Axial Force in Members (3D)
1
In the Model Builder window, right-click Axial Force in Members (2D) and choose Duplicate.
2
In the Settings window for Evaluation Group, type Axial Force in Members (3D) in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study 2/Solution 2 (3) (sol2).
Global Evaluation 1
Because the applied force was doubled to get the same displacement as in the 2D case, you need to divide the value of the axial force in member cd by 2 to get a value comparable to that of the 2D case.
1
In the Model Builder window, expand the Axial Force in Members (3D) node, then click Global Evaluation 1.
2
In the Settings window for Global Evaluation, locate the Expressions section.
3
In the table, enter the following settings:
Expression
Unit
Description
F_cd/2
N
 
4
In the Axial Force in Members (3D) toolbar, click  Evaluate.
Again, the values in the evaluation group agree very well with the reference solution.