NAS120 Training

1
WORKSHOP 6 BRIDGE TRUSS
NAS120, Workshop 6, November 2003
WS6-1
2
(No Transcript)
3

• Problem Description
• The preliminary design of a steel truss bridge
  has just been finished. You are asked to
  evaluate the structural integrity of this bridge.
• The truss is made from steel with E 30 x 106
  psi and n 0.3
• The truss members are I-beams with H 18 in, W
  12 in, Tf 0.5 in, and Tw 0.5 in
• The bridge needs to be able to support a 23,000
  lb truck traveling over it. The truck weight is
  supported by two planar trusses. Model one
  planar truss with half the truck weight applied
  to it.
• One end of the truss is pinned while the other
  end is free to slide horizontally.

4
y
x
11,500 lb (Subcase 1)
11,500 lb (Subcase 2)
5

• Workshop Objectives
• Learn to mesh line geometry to generate CBAR
  elements
• Become familiar with setting up the CBAR
  orientation vector and section properties
• Learn to set up multiple load cases
• Learn to view the different CBAR stress
  components in Patran

6

• Suggested Exercise Steps
• Create a new database.
• Create a geometry model of the truss using the
  table on the previous page.
• Use Mesh Seeds to define the mesh density.
• Create a finite element mesh.
• Define material properties.
• Create Physical Properties using the beam
  library.
• Create boundary conditions.
• Create loads.
• Set up load cases.
• Run the finite element analysis using
  MSC.Nastran.
• Plot displacements and stresses.

7
Step 1. Create New Database
a
a

• Create a new database called bridge_truss.db
• File / New.
• Enter bridge_truss as the file name.
• Click OK.
• Choose Default Tolerance.
• Select MSC.Nastran as the Analysis Code.
• Select Structural as the Analysis Type.
• Click OK.

d
e
f
b
c
g
8
Step 2. Create Geometry
d

• Create the first point
• Geometry Create / Point / XYZ.
• Enter 0 0 0 for the Point Coordinate List.
• Click Apply.
• Turn Point size on.

a
b
c
9
Step 2. Create Geometry

• Finish creating all 12 points.

10
Step 2. Create Geometry

• Create curves to represent the truss members
• Geometry Create / Curve / Point.
• Screen pick the bottom left point as shown.
• Screen pick the top left point. A curve is
  automatically created because Auto Execute is
  checked.

a
c
b
11
Step 2. Create Geometry

• Finish creating all 21 curves.

12
Step 3. Create Mesh Seeds

• Create a uniform mesh seed
• Elements Create / Mesh Seed / Uniform.
• Enter 6 for the Number of Elements.
• Click in the Curve List box.
• Rectangular pick the bottom of the truss.

a
d
b
c
13
Step 3. Create Mesh Seeds

• Create another mesh seed
• Elements Create / Mesh Seed / Uniform.
• Enter 2 for the Number of Elements.
• Click in the Curve List box.
• Rectangular pick the rest of the truss, as shown.
  

a
d
b
c
14
Step 4. Create Mesh

• Create a finite element mesh
• Elements Create / Mesh / Curve.
• Set Topology to Bar2.
• Click in the Curve List box.
• Rectangular pick all of the curves as shown.
• Click Apply.

a
b
d
c
e
15
Step 4. Create Mesh

• Equivalence the model
• Elements Equivalence / All / Tolerance Cube.
• Click Apply.

a
b
16
Step 5. Create Material Properties

• Create an isotropic material
• Materials Create / Isotropic / Manual Input.
• Enter steel as the Material Name.
• Click Input Properties.
• Enter 30e6 for the elastic modulus and 0.3 for
  the Poisson Ratio.
• Click OK.
• Click Apply.

a
d
b
c
f
e
17
Step 6. Create Physical Properties

• Create element properties
• Properties Create / 1D / Beam.
• Enter i_beam as the Property Set Name.
• Click Input Properties.
• Click on the Select Material Icon.
• Select steel as the material.
• Click on the Beam Library button.

a
d
b
c
f
e
18
Step 6. Create Physical Properties

• Define the beam section
• Enter i_section for the New Section Name.
• Enter the appropriate values to define the beams
  dimensions .
• Click Calculate/Display to view the beam section
  and its section properties.
• After verifying that the section is correct,
  Click OK.

b
a
c
d
19
Step 6. Create Physical Properties

• Define the bar orientation
• Enter lt1 2 0gt for the Bar Orientation.
• Click OK.

Note Any vector in the XY plane that is not
parallel to any truss member would work as well.
a
b
20
Step 6. Create Physical Properties

• Select application region
• Click in the Select Members box.
• Rectangular pick the entire truss as shown.
• Click Add.
• Click Apply.

b
a
c
d
21
Step 6. Create Physical Properties
c
e
a

• Verify the beam section
• Display- Load/BC/Element Props.
• Set Beam Display to 3DFull-Span.
• Shade the model.
• Rotate the model and zoom in to verify that the
  I-beams are oriented correctly.
• Return to the front view.
• Set Beam Display back to 1DLine.

d
b
f
22
Step 7. Create Boundary Conditions

• Create a boundary condition
• Loads/BCs Create / Displacement / Nodal.
• Enter left_side as the New Set Name.
• Click Input Data.
• Enter lt0 0 0gt for Translations and lt0,0, gt for
  Rotations.
• Click OK.

a
d
b
c
e
23
Step 7. Create Boundary Conditions
a

• Apply the boundary condition
• Reset graphics.
• Click Select Application Region.
• Select the bottom left point as the application
  region.
• Click Add.
• Click OK.
• Click Apply.

d
c
b
e
f
24
Step 7. Create Boundary Conditions

• Create another boundary condition
• Loads/BCs Create / Displacement / Nodal.
• Enter right_side as the New Set Name.
• Click Input Data.
• Enter lt ,0,0gt for Translations and lt0,0, gt for
  Rotations.
• Click OK.

a
d
b
c
e
25
Step 7. Create Boundary Conditions

• Apply the boundary condition
• Click Select Application Region.
• Select the bottom right point as the application
  region.
• Click Add.
• Click OK.
• Click Apply.

c
b
d
a
e
26
Step 8. Create Loads

• Create the mid span load
• Loads/BCs Create / Force / Nodal.
• Enter mid_span_load as the New Set Name.
• Click Input Data.
• Enter lt0 11500 0gt for the Force.
• Click OK.

a
d
b
c
e
27
Step 8. Create Loads

• Apply the mid span load
• Click Select Application Region.
• Set the geometry filter to FEM.
• For the application region select the node in the
  middle of the span to the right of the center, as
  shown.
• Click Add.
• Click OK.
• Click Apply.

b
d
c
a
e
f
28
Step 8. Create Loads

• Create the truss joint load
• Loads/BCs Create / Force / Nodal.
• Enter truss_joint_load as the New Set Name.
• Click Input Data.
• Enter lt0 11500 0gt for the Force.
• Click OK.

a
d
b
c
e
29
Step 8. Create Loads

• Apply the load
• Click Select Application Region.
• Set the geometry filter to Geometry.
• For the application region select the point at
  the center of the bridge, as shown.
• Click Add.
• Click OK.
• Click Apply.

b
d
c
a
e
f
30
Step 9. Set Up Load Cases

• Create a load case
• Load Cases Create.
• Enter mid_span as the Load Case Name.
• Click Assign/Prioritize Loads/BCs.
• Click on Displ_left_side, Displ_right_side, and
  Force_mid_span_load to add them to the Load Case.
• Click OK.
• Click Apply.

a
d
b
c
f
e
31
Step 9. Set Up Load Cases

• Create another load case
• Load Cases Create.
• Enter truss_joint as the Load Case Name.
• Click Assign/Prioritize Loads/BCs.
• Click on Displ_left_side, Displ_right_side, and
  Force_truss_joint_load to add them to the Load
  Case.
• Click OK.
• Click Apply.

a
d
b
c
f
e
32
Step 10. Run Linear Static Analysis

• Choose the analysis type
• Analysis Analyze / Entire Model / Full Run.
• Click Solution Type.
• Choose Linear Static.
• Click OK.

a
c
b
d
33
Step 10. Run Linear Static Analysis

• Analyze the model
• Analysis Analyze / Entire Model / Full Run.
• Click Subcase Select.
• Click Unselect All.
• Click on mid_span and truss_joint to add them to
  the Subcases Selected list.
• Click OK.
• Click Apply.

a
d
c
b
f
e
34
Step 11. Plot Displacements and Stresses

• Attach the results file
• Analysis Access Results / Attach XDB / Result
  Entities.
• Click Select Results File.
• Choose the results file bridge_truss.xdb.
• Click OK.
• Click Apply.

a
c
d
b
e
35
Step 11. Plot Displacements and Stresses

• Create a deformation plot for the mid span result
  case
• Results Create / Deformation.
• Select the Mid Span Result Case.
• Select Displacements, Translational as the
  Deformation Result.
• Check Animate.
• Click Apply.
• Record the maximum deformation.
• Click Stop Animation and Refresh Results Tools.
• Max Deformation
• ____________

a
b
c
d
e
36
Step 11. Plot Displacements and Stresses

• Create a Fringe Plot of X Component Axial Stress
• Results Create / Fringe.
• Select the Mid Span Result Case.
• Select Bar Stresses, Axial as the Fringe Result.
• Select X Component as the Fringe Result Quantity.
• Click on the Plot Options icon.
• Set the Averaging Definition Domain to None.
• Click Apply.

a
e
b
c
f
d
g
37
Step 11. Plot Displacements and Stresses

• View the results
• Record the maximum and minimum X component axial
  stress.
• Max X Axial Stress
• _________________
• Min X Axial Stress
• __________________

38
Step 11. Plot Displacements and Stresses

• Create Fringe Plots of maximum and minimum
  combined bar stresses
• Results Create / Fringe.
• Select the Mid Span Result Case.
• Select Bar Stresses, Maximum Combined as the
  Fringe Result.
• Click Apply.
• Record the Maximum combined stress.
  
  
  Max Stress _______
• Repeat the procedure with Bar Stresses, Minimum
  Combined as the Fringe Result and record the
  Minimum Stress. Min Stress
  _______

a
b
c
d
39
Step 11. Plot Displacements and Stresses
e

• Create a deformation plot for the truss joint
  result case
• Results Create / Deformation.
• Select the Truss Joint Result Case.
• Select Displacements, Translational as the
  Deformation Result.
• Check Animate.
• Reset Graphics.
• Click Apply.
• Record the maximum deformation.
• Click Stop Animation and Refresh Results Tools.
• Max Deformation
• ____________

a
b
c
d
f
40
Step 11. Plot Displacements and Stresses

• Create a Fringe Plot of X Component Axial Stress
• Results Create / Fringe.
• Select the Truss Joint Result Case.
• Select Bar Stresses, Axial as the Fringe Result.
• Select X Component as the Fringe Result Quantity.
• Click on the Plot Options icon.
• Set the Averaging Definition Domain to None.
• Click Apply.

a
e
b
c
f
d
g
41
Step 11. Plot Displacements and Stresses

• View the results
• Record the maximum and minimum X component axial
  stress.
• Max X Axial Stress
• _________________
• Min X Axial Stress
• __________________

42
Step 11. Plot Displacements and Stresses

• Create Fringe Plots of maximum and minimum
  combined bar stresses
• Results Create / Fringe.
• Select the Truss Joint Result Case.
• Select Bar Stresses, Maximum Combined as the
  Fringe Result.
• Click Apply.
• Record the Maximum combined stress.
  Max Stress _______
• Repeat the procedure with Bar Stresses, Minimum
  Combined as the Fringe Result and record the
  Minimum Stress.
• Min Stress _______

a
b
c
d