WORKSHOP 10

Linear Static Analysis

of a Simply-Supported
Stiffened Plate

Objectives:
■ Create a geometric representation of a stiffened plate.

■ Use the geometry model to define a MSC.Nastran analysis

model comprised of CQUAD4 & CBAR elements.

■ Prepare a MSC.Nastran input file for a Linear Static

analysis.

■ Visualize analysis results.

MSC.Nastran 120 Exercise Workbook 10-1

10-2 MSC.Nastran 120 Exercise Workbook
WORKSHOP 10 Stiffened Plate (Sol 101)

Model Description:
Figure 10.1 is a finite element representation of the stiffened plate
shown on the title page. Since the plate is 0.1 inches thick, thin-shell
theory applies. I-beam stiffeners are mounted as shown. The
structure is simply supported on its four corners and a uniform
pressure of 0.5 psi is applied to the surface of the plate.

NOTE: Because the centroidal axes of the stiffeners do not

coincide with the mid-plane of the plate, it will be
necessary to account for this when defining the element
properties for the stiffeners.

Figure 10.1 - Model Schematics

0.5 psi
ye
5.0 (typ) 0.1
Stiffener b
C D

A 2.0
a a ze
A 0.1
20.0 F E

View A-A b
20.0 Z 1.0
X
Y

Table 10.1 - Model Properties

Elastic Modulus: 10.3E+06 psi

Poisson Ratio: 0.3
Density: 0.101 lbs/in3
Plate Thickness: 0.1 in
Bar Cross-Sectional Area: 0.38 in2
Iaa: 0.2293 in4
Ibb: 0.0168 in4
J: 0.0013 in4

MSC.Nastran 120 Exercise Workbook 10-3

Suggested Exercise Steps:
■ Open a new database.

■ Define a geometric representation of the stiffened plate

using a surface.

■ Define an analysis model by meshing the geometry model

with shell (CQUAD4) and bar (CBAR) elements.

■ Define material (MAT1) and element properties (PSHELL

and PBAR).

■ Verify XY-orientation and offset vectors for the bar

elements.

■ Define simply-supported boundary constraints (SPC1) and

apply a uniform pressure load to the plate (PLOAD4).

■ Use the load and boundary condition sets to define a load

case (SUBCASE).

■ Prepare the model for a Linear Static analysis (SOL 101 and
PARAMs).

■ Generate and submit input file for MSC.Nastran.

■ Post-process results.

■ Quit MSC.Patran.

10-4 MSC.Nastran 120 Exercise Workbook

WORKSHOP 10 Stiffened Plate (Sol 101)

Exercise Procedure:
1. Create a new database called workshop10.db.

File/New...
New Database Name: workshop10
OK

In the New Model Preference form set the following:

Tolerance: ◆ Default
Analysis Code: MSC/NASTRAN
Analysis Type: Structural
OK

NOTE:Whenever possible, toggle off the ❑ Auto Execute option by

left clicking the check box.

2. Create a 20x20 surface.

◆ Geometry
Action: Create
Object: Surface
Method: XYZ
Vector Coordinates List: <20, 20, 0>
Apply

2a. For clarity, turn on the Show Parametric Direction. Use the
Display/Geometry... option.

Display/Geometry...
■ Show Parametric Direction
Apply
Cancel

MSC.Nastran 120 Exercise Workbook 10-5

 3. Edit the surface by breaking it into two halves. To control how the
surface is to be divided, use the Break Direction Parameter;
Constant u Direction corresponds to Parametric direction 1 as
displayed on the Surface created in Step 2.

◆ Geometry
Action: Edit
Object: Surface
Method: Break
Option: Parametric
Break Direction: ◆ Constant u Direction
Break curve: 0.5
■ Delete Original Surfaces
Surface List: Surface 1
Apply

Answer Yes when the question, "Do you wish to delete the original
surfaces?" comes up on the screen.

After this step, the display should resemble Figure 15.2.

Figure 10.2

2 3

2
5 1 6

2
Y

Z X 2
1 1 4

3a. Repeat the last operation to break the two new surfaces to yield a
total of four new surfaces, each having the same dimensions as the
other.

10-6 MSC.Nastran 120 Exercise Workbook

WORKSHOP 10 Stiffened Plate (Sol 101)

Recall that surfaces can be selected by using the keyboard to specify

the ids of the desired surfaces explicitly in the Surface List databox
using the proper pick-list syntax, OR

Specifying the desired surface with the mouse by first clicking in the
Surface List databox and then clicking desired surface in the
default_viewport.

Surface List: Surface 2

Apply

Answer Yes when the question, "Do you wish to delete the original
surfaces?" comes up on the screen.

Surface List: Surface 3

Apply

Answer Yes when the question, "Do you wish to delete the original
surfaces?" comes up on the screen.

Show Labels

The completed geometry model should resemble Figure 10.3

Figure 10.3

2 3

7
2
9 1 10

6
2
5 1 6

5
2
7 1 8
Y
4
Z X 2
1 1 4

MSC.Nastran 120 Exercise Workbook 10-7

 4. For clarity, shrink the elements by 20%; this facilitates verification
of the element connectivities.

Display/Finite Elements...
FEM Shrink: 0.20

To better visualize the connectivities, increase the node display size

using Display/Finite Element.... Deactivate the labels for the
surfaces and the points to minimize the model information in the
display.

Node Sizes: 5
Hide All FEM Labels
Apply
Cancel

Display/Geometry...
❑ Show Parametric Direction
Show All Geometry Labels
Colors and Labels:
Point: ❑ Label
Surface: ❑ Label
Apply
Cancel

5. Mesh the geometry model.

5a. First, discretize the surface into quad4 elements:

◆ Finite Elements
Action: Create
Object: Mesh
Type: Surface
Global Edge Length: 2
Element Topology: Quad4

10-8 MSC.Nastran 120 Exercise Workbook

WORKSHOP 10 Stiffened Plate (Sol 101)

Mesher: ◆ IsoMesh
Surface List: Surface 4:7
OK

Apply

5b. To model the stiffeners, generate bar elements along the longitudinal
edges of the surfaces. There is no need to specify a Global Edge
Length since the mesher will utilize existing nodes from the quad
elements on the plate geometry.

NOTE: The stiffener centroidal offsets are NOT taken into account
during the discretization step. These offsets are specified
when defining the Element Properties for the bar
elements.

◆ Finite Elements
Action: Create
Object: Mesh
Type: Curve
Element Topology: Bar2
Curve List: Surface 4.4, 4:7.2

NOTE: The curve list may be different since there are edges from
two different surfaces that occupy the same location.

Apply

6. Equivalence the model to remove duplicate nodes at common

surface edges.

◆ Finite Elements
Action: Equivalence
Object: All
Method: Tolerance Cube
Apply

MSC.Nastran 120 Exercise Workbook 10-9

 Refresh the screen as needed using the brush icon on the Top Menu
Bar.

Refresh Graphics

For clarity, hide the entity labels by selecting the Hide Labels icon
on the Top Menu Bar.

Hide Labels

The completed model with all entity labels hidden should appear as
follows:

Figure 10.4

Z X

7. Define a material using the specified Modulus of Elasticity, Poisson

Ratio & Density.

◆ Materials
Action: Create
Object: Isotropic
Method: Manual Input
Material Name: alum
Input Properties...
Constitutive Model: Linear Elastic

10-10 MSC.Nastran 120 Exercise Workbook

WORKSHOP 10 Stiffened Plate (Sol 101)

Elastic Modulus = 10.3E6

Poisson Ratio = .3
Density = .101
OK
Apply

8. Define element properties for the analysis model.

◆ Properties
Action: Create
Dimension: 2D
Type: Shell
Property Set Name: plate
Input Properties...
Material Name: m:alum
Thickness: ???
(Enter the plate thickness)

OK
Select Members: Surface 4:7
Add
Apply

9. Next, define properties for the bar2 elements which represent the
stiffeners. For this model, in addition to bar orientation, area, area
moments of inertia, torsional constant and appropriate stress
recovery coefficients, offsets must be defined (See NOTE on page
10-3).

◆ Properties
Action: Create
Object: 1D
Method: Beam

MSC.Nastran 120 Exercise Workbook 10-11

 Property Set Name: bar
Input Properties...

Material Name: m:alum

Bar Orientation: <0, 0, 1>
[Offset @ Node 1] <0, 0, 1.05>
[Offset @ Node 2] <0, 0, 1.05>
Area: 0.38
[Inertia 1,1] ???
(Enter Inertia about 1-1)

[Inertia 2,2] ???

(Enter Inertia about 2-2)

[Torsional Constant] 0.0013

[Y of Point C] 1.
[Z of Point C] -0.5
[Y of Point D] ???
(Enter Y of Point D)

[Z of Point D] ???
(Enter Z of Point D)

[Y of Point E] -1.
[Z of Point E] 0.5
[Y of Point F] -1.
[Z of Point F] -0.5
OK
Select Members: Surface 4.4, 4:7.2
Add
Apply

10. Use the Viewing/Angles... option to change the view. Also erase all
geometry using the Display/Plot/Erase... option.

Viewing/ Angles...
Method: ◆ Model Absolute

10-12 MSC.Nastran 120 Exercise Workbook

WORKSHOP 10 Stiffened Plate (Sol 101)

Angles: 23.0, 34.0, 0.0

Apply
Cancel

Display/Plot/Erase...
Erase All Geometry
OK

10a. Graphically assess the orientation vectors that are required on the
CBAR entries in the MSC.Nastran input file.

These vectors define the local XY plane for each bar element. Since
the element property created was applied to the geometry model
instead of the analysis model, a graphical display of respective
attributes will appear on the geometry model by default.

In order to display attributes such as the orientation vectors on the

analysis model, change the option in Display/Load/BC/Elem.
Props..., since all geometry was erased from the Viewport. For
additional clarity, turn on bar element labels.

Display/Finite Elements...
Colors and Labels
Bar: ■ Label
Apply
Cancel

Display/Load/BC/Elem. Props...
■ Show on FEM Only
Apply
Cancel

10b. Change the Action in Properties form to Show.

◆ Properties
Action: Show
Existing Properties: Definition of XY Plane

MSC.Nastran 120 Exercise Workbook 10-13

 Display Method: Vector Plot
Select Group: default_group
Apply

The display in the viewport should resemble Figure 15.5.

Figure 10.5
170
169
168 1.000
167 1.000
166 1.000
165 1.000
164 1.000
163 1.000
162 1.000
161 1.000
1.000 160
1.000 159
158 1.000
157 1.000
156 1.000
155 1.000
154 1.000
153
152 1.000
151 1.000
1.000 150
1.000 149
1.000 148
147 1.000
146 1.000
145 1.000
144 1.000
143 1.000
142 1.000
141 1.000
1.000 140
1.000 139
1.000 138
137 1.000
136 1.000
135 1.000
134 1.000
133 1.000
132 1.000
131 1.000
1.000 130
1.000 129
1.000
Y 127
128
1.000
1.000
126 1.000
125
X 122
123
124
1.000
1.000
1.000
121 1.000
Z 1.000
1.000
1.000

10c. Display the offset vector at Node 2 of each bar element.

◆ Properties
Action: Show
Existing Properties: Offset @ Node 2
Display Method: Vector Plot
Select Group: default_group
Apply

The display should resemble Figure 10.6.

10-14 MSC.Nastran 120 Exercise Workbook

WORKSHOP 10 Stiffened Plate (Sol 101)

Figure 10.6

170
169 1.050
168 1.050
167 1.050
166 1.050
165 1.050
164 1.050
163 1.050
162 1.050
161 1.050
1.050 160
159 1.050
158 1.050
157 1.050
156 1.050
155 1.050
154 1.050
153 1.050
152 1.050
151 1.050
1.050 150
149 1.050
148 1.050
147 1.050
146 1.050
145 1.050
144 1.050
143 1.050
142 1.050
141 1.050
1.050 140
139 1.050
138 1.050
137 1.050
136 1.050
135 1.050
134 1.050
133 1.050
132 1.050
131 1.050
Y 1.050
129
130
1.050
128 1.050
127 1.050
X 124
125
126
1.050
1.050
123 1.050
Z 121
122
1.050
1.050
1.050
1.050

11. Before defining loads & boundary conditions, modify the display
and viewing settings as follows:

Display/Entity Color/Label/Render...

Entity Type Colors and Labels

Point: ■ Label
Surface: ■ Label
Bar: ❑ Label
Apply
Cancel

Display/Plot/Erase
Plot All Posted Geometry
Erase All FEM
OK

Display/Load/BC/Elem. Props...
❑ Show on FEM Only

MSC.Nastran 120 Exercise Workbook 10-15

 Apply
Cancel

Reset the display by selecting the broom icon on the Top Menu Bar
as needed before continuing.

Reset Graphics

11a. Define displacement constraints and apply them to the geometry

model. This boundary condition represents the simply supported
corners of the stiffened plate structure.

◆ Loads/BCs
Action: Create
Object: Displacement
Method: Nodal
New Set Name: simply_support
Input Data...
Translation < T1 T2 T3 > <0, 0, 0>
OK
Select Application Region...
Geometry Filter: ◆ Geometry
Select Geometry Entities: Point 1:4
Add
OK
Apply

The display should resemble Figure 10.7.

10-16 MSC.Nastran 120 Exercise Workbook

WORKSHOP 10 Stiffened Plate (Sol 101)

Figure 10.7

123
3

123 7 10
2

9 6 6

5 5 8

7 4 4
Y
123
X
Z 1
123

Reset the display by selecting the broom icon on the Top Menu Bar.

Reset Graphics

11b. Apply a uniform pressure load to the surface of the plate on which
the stiffeners are mounted.

◆ Loads/BCs
Action: Create
Object: Pressure
Method: Element Uniform
New Set Name: pressure
Target Element Type: 2D
Input Data...
Top Surf Pressure: 0.5
OK
Select Application Region...
Geometry Filter: ◆ Geometry
Select Geometry Entities: Surface 4:7

MSC.Nastran 120 Exercise Workbook 10-17

 Add
OK
Apply

Because the pressure loads are applied to the geometry model

instead of the analysis model, it may appear as if the load was not
applied correctly. The applied pressure will resemble Figure 10.8:

Figure 10.8
3
.5000

2 10
.5000 7 .5000

9 6
.5000 6 .5000

5 8
.5000 5 .5000

7 4
Y
.5000 4 .5000
X
Z
1
.5000

12. Create a new group called fem_only. This group will contain only
the analysis model.

Group/Create...
New Group Name: fem_only
■ Make Current
■ Unpost All Other Groups
Group Contents: Add All FEM
Apply
Cancel

10-18 MSC.Nastran 120 Exercise Workbook

WORKSHOP 10 Stiffened Plate (Sol 101)

12a. Enable the Show on FEM only button in Display/Load/BC/Elem

Props.... For clarity, disable the LBC/El. Prop. Values display for the
load & boundary condition sets.

Display/Load/BC/Elem. Props...
■ Show on FEM only
❑ Show LBC/El. Prop. Values
Apply
Cancel

Turn on markers for the loading conditions on the analysis model.

◆ Loads/BCs
Action: Plot Markers
Assigned Load/BCs Sets: Disp_simply_support
Press_pressure

Select Groups: fem_only

Apply

The model should resemble Figure 10.9.

Figure 10.9

Y
X
Z

MSC.Nastran 120 Exercise Workbook 10-19

 Reset the display by selecting the broom icon on the Top Menu Bar.

Reset Graphics

13. Create a load case which references the pressure and boundary
condition sets.

◆ Load Cases
Action: Create
Load Case Name: load_static
Load Case Type: Static
Assign/Prioritize Loads/BCs

(Click each selection until all Loads/BCs Disp_simply_support

have one entry in the spreadsheet)* Press_pressure

* REMINDER: Make sure that the LBC Scale Factor column shows
the proper value for each entry (= 1.0).

OK
Apply

14. Generate an input file for analysis.

◆ Analysis
Action: Analyze
Object: Entire Model
Method: Analysis Deck
Job Name: workshop10
Solution Type...
Solution Type: ◆ Linear Static
Solution Parameters...
■ Database Run
■ Automatic Constraints
Data Deck Echo: Sorted

10-20 MSC.Nastran 120 Exercise Workbook

WORKSHOP 10 Stiffened Plate (Sol 101)

Wt.- Mass Conversion = 0.00259

(For English unit)

OK
OK
Subcase Select...
Subcases For Solution Sequence: load_static
Subcases Selected: Default
(Click to deselect)

OK
Apply

An input file called workshop10.bdf will be generated. This process

of translating the model into an input file is called the Forward
Translation. The Forward Translation is complete when the
Heartbeat turns green.

MSC.Nastran 120 Exercise Workbook 10-21

Submitting the Input File for Analysis:
15. Submit the input file to MSC.Nastran for analysis.

15a. To submit the MSC.Patran .bdf file for analysis, find an

available UNIX shell window. At the command prompt
enter: nastran workshop10_work.bdf scr=yes.
Monitor the run using the UNIX ps command.

15b. When the run is completed, edit the workshop10.f06 file

and search for the word FATAL. If none exists, search
for the word WARNING. Determine whether or not
existing WARNING messages indicate modeling errors.

15c. While still editing workshop10.f06, search for the word:

D I S P L A C E (spaces are necessary)

Figure 10.10

CQUAD4 77

CBAR 146

GRID 83
Y

Z X

What are the components of the displacement vector for

GRID 83 (translation only)?

disp X =
disp Y =
disp Z =

10-22 MSC.Nastran 120 Exercise Workbook

WORKSHOP 10 Stiffened Plate (Sol 101)

Search for the word:

S T R E S S (spaces are necessary)

What is the axial stress for CBAR 146?

axial stress =

Search for the word:

Q U A D (spaces are necessary)

What are the centroidal Von Mises stresses for

CQUAD4 77?

-(thk/2): stress =

+(thk/2): stress =

MSC.Nastran 120 Exercise Workbook 10-23

 16. MSC.Nastran Users have finished this exercise.
MSC.Patran Users should proceed to the next step.
17. Proceed with the Reverse Translation process, that is attaching the
plate.xdb results file into MSC.Patran. To do this, return to the
Analysis form and proceed as follows.

◆ Analysis
Action: Attach XDB
Object: Result Entities
Method: Local
Select Results File...
Filter
Selected Results File: workshop10.xdb
OK
Apply

When translation is complete 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.

To reset the display graphics to the state it was in before post-

processing the model, remember to select the broom icon.

Reset Graphics

Quit MSC.Patran after completing this exercise.

10-24 MSC.Nastran 120 Exercise Workbook