LESSON 8
Linear Static Analysis of a
Simply-Supported Truss
Objectives:
■ Create a finite element model by explicitly defining node
locations and element connectivities.
■ Define a MSC/NASTRAN analysis model comprised of
CROD elements.
■ Prepare a MSC/NASTRAN input file for a linear static
analysis.
■ Visualize analysis results.
MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
8-2 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
LESSON 8 Simply-Supported Truss (Sol 101)
Model Description:
Below is a finite element representation of the truss structure shown on page
8-1. The nodal coordinates provided are defined in the global cartesian coordi-
nate system (MSC/NASTRAN Basic system).
The structure is comprised of truss segments connected by smooth pins such
that each segment is either in tension or compression. The structure is pinned
at node 1 and supported by a roller at node 7. Point forces are applied at nodes
2, 4, and 6.
Grid Coordinates and Element Connectivities
[288,144,0]
4
2 3
[144,72,0] [432,72,0]
2 6
6 7
1 5 8 4
1 9 3 10 5 11 7
[0,0,0] [192,0,0] [384,0,0] [576,0,0]
Y
Z X
Loads and Boundary Conditions
1500.
1500. 1300. 1500.
3456
1300. 1300.
3456 3456
123456 3456 3456 23456
Z X
Cross-Sectional Area 5.25 in2
Elastic Modulus 1.76E6 psi
Tension Stress Limit 1900 psi
Compression Stress Limit 1900 psi
MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5) 8-3
Suggested Exercise Steps:
■ Open a new database.
■ Explicitly generate a finite element representation of the
truss structure without defining any geometry, i.e., the nodes
(GRID) and element connectivities (CROD) should be
defined manually.
■ Define material (MAT1) and element (PROD) properties.
■ Apply simply-supported boundary constraints (SPC1) and
point forces (FORCE).
■ Use the load and boundary condition sets to define a
loadcase (SUBCASE).
■ Prepare the model for a linear static analysis (SOL 101 and
PARAMs).
■ Generate an input file and submit it to the MSC/NASTRAN
solver.
■ Post-process results.
■ Quit MSC/PATRAN.
Exercise Procedure:
1. Create a new database called truss.db.
File/New...
New Database Name: Truss
OK
In the New Model Preferences form set the following:
Tolerance: ◆ Default
Analysis Code: MSC/NASTRAN
Analysis Type: Structural
OK
8-4 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
LESSON 8 Simply-Supported Truss (Sol 101)
Activate the entity labels by selecting the Show Labels button on
the toolbar.
Show Labels
2. Create the nodes by manually defining their respective
coordinates:
◆ Finite Elements
Action: Create
Object: Node
Method: Edit
❑ Associate with Geometry
❑ Auto Execute
Node Location List: [ 0, 0, 0 ]
Apply
Repeat the previous operation to create the remaining nodes. Refer to
the figure on page 8-3 for the nodal coordinates.
Node Location List: [ 140, 72, 0 ]
Apply
Node Location List: [ 192, 0, 0 ]
Apply
Node Location List: [ 288, 144, 0 ]
Apply
Node Location List: [ 384, 0, 0 ]
Apply
Node Location List: [ 432, 72, 0 ]
Apply
MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5) 8-5
Node Location List: [ 576, 0, 0 ]
Apply
Next, manually define the truss segment connectivites with BAR2 ele-
ments using our newly created nodes. Again, refer to page 8-3 for con-
nectivity information.
◆ Finite Elements
Action: Create
Object: Element
Method: Edit
Shape: Bar
Topology: Bar2
❑ Auto Execute
Node 1 = Node 1
Node 2 = Node 2
Apply
Repeat the previous operation until all the truss segments have been cre-
ated .
Node 1 = Node 1
Node 2 = Node 2
Apply
Node 1 = Node 2
Node 2 = Node 4
Apply
Node 1 = Node 4
Node 2 = Node 6
Apply
8-6 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
LESSON 8 Simply-Supported Truss (Sol 101)
Node 1 = Node 6
Node 2 = Node 7
Apply
Node 1 = Node 2
Node 2 = Node 3
Apply
Node 1 = Node 3
Node 2 = Node 4
Apply
Node 1 = Node 4
Node 2 = Node 5
Apply
Node 1 = Node 5
Node 2 = Node 6
Apply
Node 1 = Node 1
Node 2 = Node 3
Apply
Node 1 = Node 3
Node 2 = Node 5
Apply
Node 1 = Node 5
Node 2 = Node 7
Apply
MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5) 8-7
The completed model should appear as follows:
4
2 3
2 6 7 6
1 5 8 4
1 9 3 10 5 11 7
Z X
3. Next, define a material using the specified modulus of
elasticity and allowable stresses.
◆ Materials
Action: Create
Object: Isotropic
Method: Manual Input
Material Name: mat_1
Input Properties...
Constitutive Model: Linear Elastic
Elastic Modulus = 1.76e6
Apply
Constitutive Model: Failure
Tension Stress Limit = ??? (Enter material limit)
Compression Stress Limit = ??? (Enter material Limit)
Apply
8-8 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
LESSON 8 Simply-Supported Truss (Sol 101)
Current Constitutive Models:
Failure - [n/a,,,,] - [Active]
Linear Elastic - [,,,,] - [Active]
Cancel
4. Next, reference the material that was created in the previous step.
Define the properties of the truss segments using the specified cross-
sectional data.
◆ Properties
Action: Create
Object: 1D
Method: Rod
Property Set Name: rod
Input Properties...
Material Name: m:mat_1
Area: ??? (Enter cross-sectional area)
OK
Select Members: Elm 1:11
Add
Apply
5. Shrink the elements by 10% for clarity; this allows us to easily
assess the element connectivities. Use the Display/Finite Ele-
ments... option.
Display/Finite Elements...
FEM Shrink: 0.10
Apply
Cancel
MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5) 8-9
6. Create two displacement constraints and apply them to the analysis
model. These boundary conditions represent the simply-supported
ends of the truss.
6a. The left-hand support is defined as follows:
◆ Loads/BCs
Action: Create
Object: Displacement
Method: Nodal
New Set Name: pin
Input Data...
Translation < T1 T2 T3 > < 0, 0, >
OK
Select Application Region...
Geometry Filter: ◆ FEM
Select Nodes: Node 1
Add
OK
Apply
6b. The right-hand constraint is located at the opposite end of the truss.
◆ Loads/BCs
Action: Create
Object: Displacement
Method: Nodal
New Set Name: roller
Input Data...
Translation < T1 T2 T3 > < , 0, >
OK
8-10 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
LESSON 8 Simply-Supported Truss (Sol 101)
Select Application Region...
Geometry Filter: ◆ FEM
Select Nodes: Node 7
Add
OK
Apply
The displacement constraints are shown below:
4
2 3
2 6 7 6
1 5 8 4
1 9 3 10 5 11 7
12 2
Y
Z X
7. Apply forces to the upper joints of the truss as shown on page 8-3.
Vertical forces of 1500 lbs and horizontal forces of 1300 lbs should
be applied at the proper nodes.
7a. First, define the vertical forces.
◆ Loads/BCs
Action: Create
Object: Force
Method: Nodal
New Set Name: force_1
Input Data...
MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5) 8-11
Force < F1 F2 F3 > < , -1500, >
OK
Select Application Region...
Geometry Filter: ◆ FEM
Select Nodes: Node 2:6:2
Add
OK
Apply
The vertical forces should appear as follows:
1500.
4
1500. 2 3 1500.
2 6 7 6
1 5 8 4
1 9 3 10 5 11 7
Y
Z X
7b. Next, define the horizontal forces.
◆ Loads/BCs
Action: Create
Object: Force
Method: Nodal
New Set Name: Force_2
Input Data...
Force < F1 F2 F3 > < -1300, , >
8-12 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
LESSON 8 Simply-Supported Truss (Sol 101)
OK
Select Application Region...
Geometry Filter: ◆ FEM
Select Nodes: Node 2:6:2
Add
OK
Apply
When you are done, resultant forces will be displayed as follows:
1985.
4
1985. 2 3 1985.
2 6 7 6
1 5 8 4
1 9 3 10 5 11 7
Z X
7c. Reset the display by selecting the broom icon on the Top Menu Bar.
Reset Graphics
To display only the horizontal forces, change the Action on the Load/
BCs form to Plot Markers.
◆ Loads/BCs
MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5) 8-13
Action: Plot Markers
Select the Force_force_2 set in the Assigned Load/BC Sets box by high-
lighting it. Also apply the markers to the current group default_group.
Assigned Load/BC Sets: Force_force_2
Select Groups: default_group
Apply
The display should appear as follows:
4
1300.
2 3
2 6 7 6
1300. 1300.
1 5 8 4
1 9 3 10 5 11 7
Y
Z X
8. Create a load case that references the forces and boundary condi-
tions that have already been defined.
◆ Load Cases
Action: Create
Load Case Name: truss_lbcs
Load Case Type: Static
Assign/Prioritize Loads/BCs
Displ_pin
(Click each selection until all
Displ_roller
Loads/BCs have one entry in the
Force_force_1
spreadsheet)*
Force_force_2
8-14 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
LESSON 8 Simply-Supported Truss (Sol 101)
OK
Apply
* NOTE: Be sure not to enter any load more than one time into the
spreadsheet. Doing so will result in increasing the load by a
factor equal to the number of times the load is entered into
the spreadsheet. The increase in factor can be shown in two
different manners. First, the LBC Scale Factor may show a
value greater than one, or second, the spreadsheet may con-
tain repeated entries of the same load. Either condition will
result in erroneous loading conditions.
Reset the display by selecting the broom icon on the Top Menu Bar.
Reset Graphics
Plot the Load/BCs markers and post them to the current group.
◆ Loads/BCs
Action: Plot Markers
Select all the Load/BC sets in the Assigned Load/BC Sets box by high-
lighting all of them. Post the markers to the current group.
Displ_pin
Assigned Load/BCs Sets: Displ_roller
Force_force_1
Force_force_2
Select Groups: default_group
Apply
MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5) 8-15
Here is how the display should appear:
1985.
4
1985. 2 3 1985.
2 6 7 6
1 5 8 4
1 9 3 10 5 11 7
12 2
Y
Z X
9. Deactivate the entity labels by using the Display/Entity Color/
Label/Render... option.
Display/Entity Color/Label/Render...
Hide All Entity Labels
Apply
Cancel
Reset the display by selecting the broom icon on the Top Menu Bar.
Reset Graphics
Display your model in its unshrunken state using the Display/Finite
Elements... option.
Display/Finite Elements...
FEM Shrink: 0.0
Apply
Cancel
8-16 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
LESSON 8 Simply-Supported Truss (Sol 101)
10. Now you are ready to generate an input file for analysis.
Click on the Analysis radio button on the Top Menu Bar and complete
the entries as shown here.
◆ Analysis
Action: Analyze
Object: Entire Model
Method: Analysis Deck
Job Name: Truss
Translation Parameters...
OUTPUT2 Format: Binary
MSC/NASTRAN Version: ??? Set accordingly, here it is 70
OK
Solution Type...
Solution Type: ◆ Linear Static
Solution Parameters...
■ Database Run
■ Automatic Constraints
Data Deck Echo: Sorted
Wt.- Mass Conversion = 0.00259 (For English units)
OK
OK
Subcase Select...
Subcases For Solution Sequence: truss_lbcs
Subcases Selected: Default (Click on this to deselect)
OK
MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5) 8-17
Apply
An MSC/NASTRAN input file called Truss.bdf will be generated. This
process of translating your model into an input file is called the Forward
Translation. The Forward Translation is complete when the Heartbeat
turns green.
Submit the input file to MSC/NASTRAN for analysis. To do this, find
an available UNIX shell window and at the command prompt enter:
nastran Truss.bdf scr=yes
Monitor the run using the UNIX ps command.
10a. When the run is completed, edit the Truss.f06 file and search for the
word FATAL. If no matches exist, search for the word WARNING.
Determine whether existing WARNING messages indicate modeling
errors.
10b. While still editing Truss.f06, search for the word:
D I S P L A C E (spaces are necessary).
What are the components of the displacement vector for GRID 7 (trans-
lation only)?
Disp. X =
Disp. Y =
Disp. Z =
Search for the word:
S I N G L E (spaces are necessary).
What are the components of the reaction force at GRID 1?
Force X =
Force Y =
Force Z =
Search for the word:
S T R E S S (spaces are necessary).
What is the margin of safety for CROD 2?
M.S. =
8-18 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
LESSON 8 Simply-Supported Truss (Sol 101)
What is the Axial Stress for CROD 7?
Axial Stress =
11. Proceed with the Reverse Translation process, that is, importing the
Truss.op2 results file into MSC/PATRAN. To do this, return to the
Analysis form and proceed as follows:
◆ Analysis
Action: Read Output2
Object: Result Entities
Method: Translate
Select Results File...
Filter
Selected Results File select the desired .op2 file
OK
Apply
When the translation is complete and the Heartbeat turns green,
bring up the Results form.
◆ Results
Action: Create
Object: Quick Plot
Choose the desired result case in the Select Result Cases list and
select the result(s) in the Select Fringe Result list and/or in the
Select Deformation Result list. And hit Apply to view the
result(s) in the viewport.
If you wish to reset your display graphics to the state it was in
before you began post-processing your model, remember to select
the broom icon.
Reset Graphics
Quit MSC/PATRAN when you have completed this exercise.
MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5) 8-19
8-20 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
