PDF
Pratt Truss Bridge
Introduction
This example is inspired by a classic bridge type called a Pratt truss bridge. You can identify a Pratt truss by its diagonal members, which (except for the very end ones) all slant down and in toward the center of the span. All the diagonal members are subject to tension forces only, while the shorter vertical members handle the compressive forces. Since the tension removes the buckling risk, this allows for thinner diagonal members resulting in a more economic design.
A truss structure supports only tension and compression forces in its members and you would normally model it using bars, but as this model uses 3D beams it also includes bending moments to some extent in a frame structure. In the model, shell elements represent the roadway.
Model Definition
BASIC DIMENSIONS
The length of the bridge is 40 m, and the width of the roadway is 7 m. The main distance between the truss members is 5 m.
Analysis Types
The model includes two different analyses of the bridge:
•
The goal of the first analysis is to evaluate the stress and deflection fields of the bridge when exposed to a pure gravity load and also when a load corresponding to one or two trucks cross the bridge.
•
Finally, an eigenfrequency analysis shows the eigenfrequencies and eigenmodes of the bridge.
Loads and Constraints
To prevent rigid body motion of the bridge, it is important to constrain it properly. All translational degrees of freedom are constrained at the leftmost horizontal edge. Constraints at the right-most horizontal edge prevent it from moving in the vertical and transversal directions but allow the bridge to expand or contract in the axial direction. This difference would however only be important if thermal expansion was studied.
Figure 1 shows the bridge geometry.
Figure 1: The geometry of the bridge
The first study uses several load cases. In the first load case the effects of self-weight are analyzed. The following load cases compute the solution when two trucks are moving over the bridge. The weight of each truck is 12,000 kg, the wheelbase is 6 m, the axle track is 2 m, and the weight is distributed with one third on the front axle and two thirds on the rear axle. The right side wheels of the truck are 1 m from the edge of the bridge.
In the second study the natural frequencies of the bridge are computed.
Material Properties and cross section data
The material in the frame structure is structural steel. The roadway material is concrete; the effect of reinforcement is ignored. The frame members have different cross sections:
•
The main beams along the bridge have square box profiles with height 200 mm and thickness 16 mm. This is also true for the outermost diagonal members.
•
The diagonal and vertical members have a rectangular box section 200 mm-by-100 mm and a thickness of 12.5 mm. The large dimension is in the transverse direction of the bridge.
•
The transverse horizontal members supporting the roadway (floor beams) are standard HEA100 profiles.
•
The transverse horizontal members at the top of the truss (struts) are made from solid rectangular sections with dimension 100 mm-by-25 mm. The large dimension is in the horizontal direction.
Results and Discussion
Figure 2 and Figure 3 illustrate the result. Figure 2 shows the displacements, and it can be seen that the maximum deflection amounts to 3 cm on the roadway. The distribution of axial forces (Figure 3) demonstrates the function of the frame: The interplay of members in tension and compression contribute to the load carrying function. The upper horizontal members are in compression and the lower in tension. The force in the lower members is much smaller, since the load is also shared by the roadway in this example. The diagonal members are subject to tension forces only, while the shorter vertical members handle the compressive forces.
Figure 2: Deformation under self-weight.
Figure 3: The axial forces in the beams. Red is tension and blue is compression.
To study the effects of trucks moving over the bridge, several load cases represent the position of the trucks. The trucks are moved 3 m along the bridge for each load case. Figure 4 shows the stress distribution in the roadway when the first truck has passed the bridge center and the second truck has entered the bridge deck.
Figure 4: Truck load analysis: Stresses in the bridge deck with two trucks on the bridge.
The study of eigenfrequencies is important with respect to the excitation and frequency content from various loads such as wind loads and earthquakes.
Figure 5 shows the 10th eigenmode of the bridge, which is the fundamental mode for the roadway. The first eight eigenmodes only involve displacements of the weak struts at the top of the truss.
Figure 5: The 10th eigenmode.
Notes About the COMSOL Implementation
You can define load cases to activate and deactivate loads within a study. All the loads need to be defined in the Model Builder. Under the Stationary Study node, you can then select which load or constraint to activate for a specific load case. Moreover for each load case you can modify the value of the applied load by changing its weight factor.
When combining two different physics interfaces, each have individual sets of degrees of freedom as a default. In structural mechanics, you usually want these to be equal. You can set such connections across various structural mechanics interfaces using built in multiphysics connection features. In this particular model, the Shell-Beam Connection features under the Multiphysics node are used to set up the connection between the two physics.
Application Library path: Structural_Mechanics_Module/Beams_and_Shells/pratt_truss_bridge
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  3D.
2
In the Select Physics tree, select Structural Mechanics>Shell (shell).
3
Click Add.
4
In the Select Physics tree, select Structural Mechanics>Beam (beam).
5
Click Add.
6
Click  Study.
7
In the Select Study tree, select General Studies>Stationary.
8
Click  Done.
Global Definitions
Load Groups
1
In the Model Builder window, right-click Global Definitions and choose Node Group.
2
In the Settings window for Group, type Load Groups in the Label text field.
Load Group 1
1
Right-click Load Groups and choose Load and Constraint Groups>Load Group.
2
Repeat this nine times so that you get ten load groups.
Geometry 1
The geometry sequence for the model (see Figure 1) is available in a file. If you want to create it from scratch yourself, you can follow the instructions in the Appendix — Geometry Modeling Instructions section. Otherwise, insert the geometry sequence as follows:
1
In the Geometry toolbar, click  Insert Sequence.
2
Browse to the model’s Application Libraries folder and double-click the file pratt_truss_bridge_geom_sequence.mph.
3
In the Geometry toolbar, click  Build All.
Global Definitions
Parameters 1
Add the non geometrical parameters.
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
truck_weight
12000[kg]
12000 kg
Total truck weight
Definitions
Create groups for the different beam sections.
BeamsTransvBelow
1
In the Definitions toolbar, click  Box.
2
In the Settings window for Box, type BeamsTransvBelow in the Label text field.
3
Locate the Geometric Entity Level section. From the Level list, choose Edge.
4
Locate the Box Limits section. In the x minimum text field, type -(length/2+1).
5
In the x maximum text field, type length/2+1.
6
In the y minimum text field, type 1.
7
In the y maximum text field, type width-1.
8
In the z minimum text field, type -1.
9
In the z maximum text field, type 1.
BeamsAllBelow
1
Right-click BeamsTransvBelow and choose Duplicate.
2
In the Settings window for Box, type BeamsAllBelow in the Label text field.
3
Locate the Box Limits section. In the y minimum text field, type -1.
4
In the y maximum text field, type width+1.
5
Locate the Output Entities section. From the Include entity if list, choose Entity inside box.
BeamsTransvAbove
1
In the Definitions toolbar, click  Box.
2
In the Settings window for Box, type BeamsTransvAbove in the Label text field.
3
Locate the Geometric Entity Level section. From the Level list, choose Edge.
4
Locate the Box Limits section. In the x minimum text field, type -(length/2+1).
5
In the x maximum text field, type length/2+1.
6
In the y minimum text field, type 1.
7
In the y maximum text field, type width-1.
8
In the z minimum text field, type height-1.
9
In the z maximum text field, type height+1.
BeamsDiag
1
In the Definitions toolbar, click  Box.
2
In the Settings window for Box, type BeamsDiag in the Label text field.
3
Locate the Geometric Entity Level section. From the Level list, choose Edge.
4
Locate the Box Limits section. In the x minimum text field, type -(length/2-spacing+1).
5
In the x maximum text field, type length/2-spacing+1.
6
In the y minimum text field, type -1.
7
In the y maximum text field, type width+1.
8
In the z minimum text field, type 1.
9
In the z maximum text field, type 2.
AllBeams
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type AllBeams in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Edge.
4
Select the All edges check box.
BeamsMain
1
In the Definitions toolbar, click  Difference.
2
In the Settings window for Difference, type BeamsMain in the Label text field.
3
Locate the Geometric Entity Level section. From the Level list, choose Edge.
4
Locate the Input Entities section. Under Selections to add, click  Add.
5
In the Add dialog box, select AllBeams in the Selections to add list.
6
Click OK.
7
In the Settings window for Difference, locate the Input Entities section.
8
Under Selections to subtract, click  Add.
9
In the Add dialog box, in the Selections to subtract list, choose BeamsTransvBelow, BeamsTransvAbove, and BeamsDiag.
10
Click OK.
Add the materials.
Add Material
1
In the Home toolbar, click  Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select Built-in>Concrete.
4
Click Add to Component in the window toolbar.
5
In the tree, select Built-in>Structural steel.
6
Click Add to Component in the window toolbar.
7
In the Home toolbar, click  Add Material to close the Add Material window.
Materials
Structural steel (mat2)
1
In the Settings window for Material, locate the Geometric Entity Selection section.
2
From the Geometric entity level list, choose Edge.
3
From the Selection list, choose All edges.
Shell (shell)
Thickness and Offset 1
1
In the Model Builder window, under Component 1 (comp1)>Shell (shell) click Thickness and Offset 1.
2
In the Settings window for Thickness and Offset, locate the Thickness and Offset section.
3
In the d text field, type 0.25.
Add self-weight for the bridge deck.
Gravity 1
1
In the Physics toolbar, click  Boundaries and choose Gravity.
2
In the Settings window for Gravity, locate the Boundary Selection section.
3
From the Selection list, choose All boundaries.
Pinned 1
1
In the Physics toolbar, click  Edges and choose Pinned.
2
Select Edge 1 only.
Prescribed Displacement/Rotation 1
1
In the Physics toolbar, click  Edges and choose Prescribed Displacement/Rotation.
2
Select Edge 78 only.
3
In the Settings window for Prescribed Displacement/Rotation, locate the Prescribed Displacement section.
4
Select the Prescribed in y direction check box.
5
Select the Prescribed in z direction check box.
Add the possible loads from the truck wheels.
Point Loads
1
In the Model Builder window, right-click Shell (shell) and choose Node Group.
2
In the Settings window for Group, type Point Loads in the Label text field.
Point Load 1
1
In the Physics toolbar, click  Points and choose Point Load.
2
Click  Load Group and choose Gravity Load.
3
Select Points 3 and 4 only.
4
In the Settings window for Point Load, locate the Force section.
5
Specify the FP vector as
0
x
0
y
-truck_weight*g_const/6
z
Point Load 2
1
Right-click Point Load 1 and choose Duplicate.
2
In the Physics toolbar, click  Load Group and choose Load Group 2.
3
In the Model Builder window, click Point Load 2.
4
In the Settings window for Point Load, locate the Point Selection section.
5
Click  Clear Selection.
6
Select Points 5 and 6 only.
7
Repeat this duplication procedure so that you get ten Point Load features. The loaded points and corresponding load groups are summarized in the table below:
Point load
Points
Load goup
Point Load 3
11, 12
Load Group 3
Point Load 4
15, 16
Load Group 4
Point Load 5
19, 20
Load Group 5
Point Load 6
25, 26
Load Group 6
Point Load 7
27, 28
Load Group 7
Point Load 8
33, 34
Load Group 8
Point Load 9
37, 38
Load Group 9
Point Load 10
41, 42
Load Group 10
Beam (beam)
Set the cross-section data of the different beam types.
Cross Section Main
1
In the Model Builder window, under Component 1 (comp1)>Beam (beam) click Cross-Section Data 1.
2
In the Settings window for Cross-Section Data, type Cross Section Main in the Label text field.
3
Locate the Cross-Section Definition section. From the list, choose Common sections.
4
From the Section type list, choose Box.
5
In the hy text field, type 200[mm].
6
In the hz text field, type 200[mm].
7
In the ty text field, type 16[mm].
8
In the tz text field, type 16[mm].
Section Orientation 1
1
In the Model Builder window, click Section Orientation 1.
2
In the Settings window for Section Orientation, locate the Section Orientation section.
3
From the Orientation method list, choose Orientation vector.
4
Specify the V vector as
0
X
1
Y
0
Z
Cross Section Diagonals
1
In the Physics toolbar, click  Edges and choose Cross-Section Data.
2
In the Settings window for Cross-Section Data, type Cross Section Diagonals in the Label text field.
3
Locate the Edge Selection section. From the Selection list, choose BeamsDiag.
4
Locate the Cross-Section Definition section. From the list, choose Common sections.
5
From the Section type list, choose Box.
6
In the hy text field, type 200[mm].
7
In the hz text field, type 100[mm].
8
In the ty text field, type 12.5[mm].
9
In the tz text field, type 12.5[mm].
Section Orientation 1
1
In the Model Builder window, expand the Cross Section Diagonals node, then click Section Orientation 1.
2
In the Settings window for Section Orientation, locate the Section Orientation section.
3
From the Orientation method list, choose Orientation vector.
4
Specify the V vector as
0
X
1
Y
0
Z
Cross Section Transv Below
1
In the Physics toolbar, click  Edges and choose Cross-Section Data.
2
In the Settings window for Cross-Section Data, type Cross Section Transv Below in the Label text field.
3
Locate the Edge Selection section. From the Selection list, choose BeamsTransvBelow.
4
Locate the Cross-Section Definition section. From the list, choose Common sections.
5
From the Section type list, choose H-profile.
6
In the hy text field, type 96[mm].
7
In the hz text field, type 100[mm].
8
In the ty text field, type 8[mm].
9
In the tz text field, type 5[mm].
Section Orientation 1
1
In the Model Builder window, expand the Cross Section Transv Below node, then click Section Orientation 1.
2
In the Settings window for Section Orientation, locate the Section Orientation section.
3
From the Orientation method list, choose Orientation vector.
4
Specify the V vector as
0
X
0
Y
1
Z
Cross Section Transv Above
1
In the Physics toolbar, click  Edges and choose Cross-Section Data.
2
In the Settings window for Cross-Section Data, type Cross Section Transv Above in the Label text field.
3
Locate the Edge Selection section. From the Selection list, choose BeamsTransvAbove.
4
Locate the Cross-Section Definition section. From the list, choose Common sections.
5
In the hy text field, type 100[mm].
6
In the hz text field, type 25[mm].
Section Orientation 1
1
In the Model Builder window, expand the Cross Section Transv Above node, then click Section Orientation 1.
2
In the Settings window for Section Orientation, locate the Section Orientation section.
3
From the Orientation method list, choose Orientation vector.
4
Specify the V vector as
1
X
0
Y
0
Z
Add the self-weight of the beams.
Gravity 1
1
In the Physics toolbar, click  Edges and choose Gravity.
2
In the Settings window for Gravity, locate the Edge Selection section.
3
From the Selection list, choose All edges.
Create connections between beams and shells.
Multiphysics
Shell-Beam Connection 1 (shbc1)
1
In the Physics toolbar, click  Multiphysics Couplings and choose Global>Shell-Beam Connection.
2
In the Settings window for Shell-Beam Connection, locate the Connection Settings section.
3
From the Connection type list, choose Shared edges.
4
Select the Manual control of selections check box.
5
Locate the Edge Selection section. Click  Clear Selection.
6
Select Edges 2, 8, 18, 30, 40, 50, 62, and 72 only.
7
Locate the Connection Settings section. From the Offset definition list, choose Offset vector.
8
Specify the d0 vector as
0
X
beam.hy_box/2
Y
-beam.hz_box/2
Z
Shell-Beam Connection 2 (shbc2)
1
Right-click Shell-Beam Connection 1 (shbc1) and choose Duplicate.
2
In the Settings window for Shell-Beam Connection, locate the Edge Selection section.
3
Click  Clear Selection.
4
Select Edges 4, 13, 25, 35, 45, 57, 67, and 76 only.
5
Locate the Connection Settings section. Specify the d0 vector as
0
X
-beam.hy_box/2
Y
-beam.hz_box/2
Z
Shell-Beam Connection 3 (shbc3)
1
In the Physics toolbar, click  Multiphysics Couplings and choose Global>Shell-Beam Connection.
2
In the Settings window for Shell-Beam Connection, locate the Connection Settings section.
3
From the Connection type list, choose Shared edges.
4
Select the Manual control of selections check box.
5
Locate the Edge Selection section. From the Selection list, choose BeamsTransvBelow.
6
Locate the Connection Settings section. From the Offset definition list, choose Offset vector.
7
Specify the d0 vector as
0
X
0
Y
-beam.hy_H/2
Z
Mesh 1
1
In the Model Builder window, under Component 1 (comp1) click Mesh 1.
2
In the Settings window for Mesh, locate the Physics-Controlled Mesh section.
3
From the Element size list, choose Extremely fine.
4
Locate the Mesh Settings section. From the Sequence type list, choose User-controlled mesh.
Distribution 1
1
In the Model Builder window, right-click Edge 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
In the Number of elements text field, type 2.
4
Click  Build All.
5
Click the  Zoom Extents button in the Graphics toolbar.
Study 1
Step 1: Stationary
1
In the Model Builder window, under Study 1 click Step 1: Stationary.
2
In the Settings window for Stationary, click to expand the Study Extensions section.
3
Select the Define load cases check box.
4
Click  Add nine times.
5
In the table, select the load cases and set the related weight according to the table:
Load case
Active load groups and weights
Self-weight
 
1 truck, position 1
lg1: 2.0; lg3: 1.0
1 truck, position 2
lg2: 2.0; lg4: 1.0
1 truck, position 3
lg3: 2.0; lg5: 1.0
1 truck, position 4
lg4: 2.0; lg6: 1.0
2 trucks, position 1
lg1: 1.0; lg5: 2.0; lg7: 1.0
2 trucks, position 2
lg2: 1.0; lg6: 2.0; lg8: 1.0
2 trucks, position 3
lg1: 2.0; lg3: 1.0; lg7: 2.0; lg9: 1.0
2 trucks, position 4
lg2: 2.0; lg4: 1.0; lg8: 2.0; lg10: 1.0
6
In the Home toolbar, click  Compute.
Results
Stress (shell)
The default plot is the stress plot for the shells using the last load case, see Figure 4.
Surface 1
1
In the Model Builder window, expand the Stress (shell) node, then click Surface 1.
2
In the Settings window for Surface, locate the Expression section.
3
From the Unit list, choose MPa.
4
Click the  Zoom Extents button in the Graphics toolbar.
5
In the Stress (shell) toolbar, click  Plot.
Add a new plot containing both shell and beam results, and examine the self-weight load case to reproduce Figure 2.
Displacement
1
In the Home toolbar, click  Add Plot Group and choose 3D Plot Group.
2
In the Settings window for 3D Plot Group, type Displacement in the Label text field.
3
Locate the Data section. From the Load case list, choose Self-weight.
Surface 1
Right-click Displacement and choose Surface.
Deformation 1
In the Model Builder window, right-click Surface 1 and choose Deformation.
Line 1
1
In the Model Builder window, right-click Displacement and choose Line.
2
In the Settings window for Line, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1)>Beam>Displacement>beam.disp - Displacement magnitude - m.
You can indicate the dimensions of the beams by drawing them with a size depending on the radius of gyration.
1
Locate the Coloring and Style section. From the Line type list, choose Tube.
2
In the Tube radius expression text field, type comp1.beam.re.
3
Click to expand the Inherit Style section. From the Plot list, choose Surface 1.
Surface 1
1
In the Model Builder window, click Surface 1.
2
In the Settings window for Surface, click to expand the Range section.
3
Select the Manual color range check box.
4
In the Maximum text field, type 0.05.
Deformation 1
In the Model Builder window, right-click Line 1 and choose Deformation.
Now plot the axial force in beams like in Figure 3.
1
In the Settings window for Deformation, locate the Expression section.
2
In the X component text field, type u2.
3
In the Y component text field, type v2.
4
In the Z component text field, type w2.
5
In the Displacement toolbar, click  Plot.
Displacement
1
In the Model Builder window, click Displacement.
2
In the Settings window for 3D Plot Group, locate the Plot Settings section.
3
Clear the Plot dataset edges check box.
4
Click the  Zoom Extents button in the Graphics toolbar.
5
In the Displacement toolbar, click  Plot.
Investigate the forces in the beams.
Axial Force (beam)
1
Click the  Zoom Extents button in the Graphics toolbar.
2
In the Model Builder window, expand the Results>Section Forces (beam) node, then click Axial Force (beam).
3
In the Axial Force (beam) toolbar, click  Plot.
Stress (shell)
1
In the Model Builder window, click Stress (shell).
2
In the Stress (shell) toolbar, click  Plot.
Create an animation of the trucks passing the bridge.
Animation 1
1
In the Results toolbar, click  Animation and choose Player.
2
In the Settings window for Animation, locate the Frames section.
3
In the Number of frames text field, type 9.
4
In the Frame number text field, type 9.
You can easily remove unused plots to clean up the structure in the Results tree. An alternative could have been to clear Generate default plots in the Study feature, but then you would have needed to create the current plot manually.
In the Model Builder window, select Results>Stress Bottom (shell) 1, hold down the Shift key, and then select Results>Torsion Moment (beam) 1. Right-click and choose Delete.
Before adding a new study you can group all current plots. First ungroup the load plots and section forces plots created by default.
Applied Loads (beam), Applied Loads (shell), Section Forces (beam)
1
In the Model Builder window, under Results, Ctrl-click to select Applied Loads (shell), Section Forces (beam), and Applied Loads (beam).
2
Right-click and choose Ungroup.
3
In the Model Builder window, hold down the Shift key to select all plot groups under Results, right-click the selected nodes and choose Group.
Stationary Results
1
In the Model Builder window, under Results click Group 3.
2
In the Settings window for Group, type Stationary Results in the Label text field.
Now add an eigenfrequency study.
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>Eigenfrequency.
4
Click Add Study in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Study 2
Step 1: Eigenfrequency
1
In the Settings window for Eigenfrequency, locate the Study Settings section.
2
Select the Desired number of eigenfrequencies check box.
3
In the associated text field, type 12.
4
In the Home toolbar, click  Compute.
Results
Mode Shape (shell)
Select the first mode involving the roadway, see Figure 5.
1
In the Settings window for 3D Plot Group, locate the Data section.
2
From the Eigenfrequency (Hz) list, choose 3.6086.
3
Locate the Plot Settings section. Clear the Plot dataset edges check box.
4
In the Model Builder window, expand the Mode Shape (shell) node.
Line 1
1
In the Model Builder window, expand the Results>Mode Shape (beam) node.
2
Right-click Line 1 and choose Copy.
Line 1
1
In the Model Builder window, right-click Mode Shape (shell) and choose Paste Line.
2
In the Settings window for Line, locate the Inherit Style section.
3
From the Plot list, choose Surface 1.
Deformation
1
In the Model Builder window, expand the Results>Mode Shape (shell)>Surface 1 node, then click Deformation.
2
In the Settings window for Deformation, locate the Scale section.
3
Select the Scale factor check box.
4
In the associated text field, type 0.2.
Surface 1
1
In the Model Builder window, click Surface 1.
2
In the Settings window for Surface, locate the Range section.
3
Select the Manual color range check box.
4
In the Maximum text field, type 4.
5
Click the  Zoom Extents button in the Graphics toolbar.
6
In the Mode Shape (shell) toolbar, click  Plot.
7
In the Model Builder window, hold down the shift key to select all the newly added plot groups under Results, right-click the selected nodes and choose Group.
Eigenfrequency Results
1
In the Model Builder window, under Results click Group 4.
2
In the Settings window for Group, type Eigenfrequency Results in the Label text field.
Prepare for an export to file of the beam section forces and stresses at element level for the main beams.
Study 1/Solution 1 (3) (sol1)
1
In the Model Builder window, expand the Results>Datasets node.
2
Right-click Results>Datasets>Study 1/Solution 1 (sol1) and choose Duplicate.
Selection
1
In the Results toolbar, click  Attributes and choose Selection.
2
In the Settings window for Selection, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Edge.
4
From the Selection list, choose BeamsMain.
Data 1
1
In the Model Builder window, under Results>Datasets right-click Study 1/Solution 1 (3) (sol1) and choose Add Data to Export.
2
In the Settings window for Data, locate the Data section.
3
From the Parameter selection (Load case) list, choose From list.
4
In the Load cases list, select Self-weight.
5
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
dom
 
Entity index
beam.Nxl
kN
Local axial force
beam.Myl
kN*m
Bending moment, local y direction
beam.Tzl
kN
Shear force, local z direction
beam.Mzl
kN*m
Bending moment, local z direction
beam.Tyl
kN
Shear force, local y direction
beam.Mxl
kN*m
Torsional moment, local x direction
beam.mises
MPa
von Mises stress
6
Locate the Output section. From the Geometry level list, choose Line.
7
Click to expand the Advanced section. Clear the Full precision check box.
Appendix — Geometry Modeling Instructions
If you want to create the geometry yourself, follow these steps.
Global Definitions
Parameters 1
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
width
7[m]
7 m
Width of bridge
height
5[m]
5 m
Height of bridge
spacing
5[m]
5 m
Spacing between members along the bridge
length
40[m]
40 m
Total bridge length
Geometry 1
Work Plane 1 (wp1)
1
In the Geometry toolbar, click  Work Plane.
2
In the Settings window for Work Plane, click  Show Work Plane.
Work Plane 1 (wp1)>Plane Geometry
1
In the Model Builder window, click Plane Geometry.
Create the bridge deck.
Work Plane 1 (wp1)>Rectangle 1 (r1)
1
In the Work Plane toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type spacing.
4
In the Height text field, type width.
5
Locate the Position section. In the xw text field, type -length/2.
6
In the Work Plane toolbar, click  Build All.
Work Plane 1 (wp1)>Array 1 (arr1)
1
In the Work Plane toolbar, click  Transforms and choose Array.
2
In the Settings window for Array, locate the Size section.
3
From the Array type list, choose Linear.
4
Select the object r1 only.
5
In the Size text field, type length/spacing.
6
Locate the Displacement section. In the xw text field, type spacing.
7
In the Work Plane toolbar, click  Build All.
8
Click the  Zoom Extents button in the Graphics toolbar.
9
In the Model Builder window, right-click Geometry 1 and choose Build All.
10
Click the  Zoom Extents button in the Graphics toolbar.
Start creating the truss.
Work Plane 2 (wp2)
1
In the Geometry toolbar, click  Work Plane.
2
In the Settings window for Work Plane, locate the Plane Definition section.
3
From the Plane list, choose xz-plane.
4
Click  Show Work Plane.
Work Plane 2 (wp2)>Polygon 1 (pol1)
1
In the Work Plane toolbar, click  Polygon.
2
In the Settings window for Polygon, locate the Object Type section.
3
From the Type list, choose Open curve.
4
Locate the Coordinates section. From the Data source list, choose Vectors.
5
In the xw text field, type 0 spacing spacing spacing.
6
In the yw text field, type 0 height height 0.
Work Plane 2 (wp2)>Line Segment 1 (ls1)
1
In the Work Plane 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
Locate the Starting Point section. In the yw text field, type height.
6
Locate the Endpoint section. In the xw text field, type spacing and yw to height.
7
In the Work Plane toolbar, click  Build All.
Work Plane 2 (wp2)>Array 1 (arr1)
1
In the Work Plane toolbar, click  Transforms and choose Array.
2
In the Settings window for Array, locate the Size section.
3
From the Array type list, choose Linear.
4
Click in the Graphics window and then press Ctrl+A to select both objects.
5
In the Size text field, type length/(2*spacing)-1.
6
Locate the Displacement section. In the xw text field, type spacing.
7
In the Work Plane toolbar, click  Build All.
Work Plane 2 (wp2)>Line Segment 2 (ls2)
1
In the Work Plane 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
Locate the Starting Point section. In the xw text field, type length/2-spacing and yw to height.
6
Locate the Endpoint section. In the xw text field, type length/2.
7
In the Work Plane toolbar, click  Build All.
Work Plane 2 (wp2)>Mirror 1 (mir1)
1
In the Work Plane toolbar, click  Transforms and choose Mirror.
2
Click in the Graphics window and then press Ctrl+A to select all objects.
3
In the Settings window for Mirror, locate the Input section.
4
Select the Keep input objects check box.
5
In the Work Plane toolbar, click  Build All.
6
Click the  Zoom Extents button in the Graphics toolbar.
Work Plane 2 (wp2)>Line Segment 3 (ls3)
1
In the Work Plane 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 yw text field, type height.
6
In the Work Plane toolbar, click  Build All.
7
Right-click Geometry 1 and choose Build All.
Copy 1 (copy1)
1
In the Geometry toolbar, click  Transforms and choose Copy.
2
In the Settings window for Copy, locate the Displacement section.
3
In the y text field, type width.
4
Select the object wp2 only.
5
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
Locate the Starting Point section. In the x text field, type -length/2+spacing.
6
Locate the Endpoint section. In the x text field, type -length/2+spacing, y to width, and z to height.
7
Click  Build All Objects.
Array 1 (arr1)
1
In the Geometry toolbar, click  Transforms and choose Array.
2
Select the object ls1 only.
3
In the Settings window for Array, locate the Size section.
4
From the Array type list, choose Linear.
5
Locate the Displacement section. In the x text field, type spacing.
6
Locate the Size section. In the Size text field, type length/spacing-1.
Create points in the positions where the loads from the truck wheels are to be applied.
Point 1 (pt1)
1
In the Geometry toolbar, click  More Primitives and choose Point.
2
In the Settings window for Point, locate the Point section.
3
In the x text field, type -19.
4
In the y text field, type 1.
Array 2 (arr2)
1
In the Geometry toolbar, click  Transforms and choose Array.
2
Select the object pt1 only.
3
In the Settings window for Array, locate the Size section.
4
In the x size text field, type 10.
5
In the y size text field, type 2.
6
Locate the Displacement section. In the x text field, type 3.
7
In the y text field, type 2.
8
Click  Build All Objects.