Using Nastran to perform analysis of bearing stress

1. 1
3D Bearing Support
Estimated time required: ~30 min
Experience level: Lower
MD Patran/Nastran

2. 2
Topics Covered
• Creating 3D geometry using primitive solids in Patran
• Using Boolean geometry to merge and subtract geometries from part
• Transforming solid geometry by mirroring using 3 points along a plane
• Using Tetmesher with Tet10 elements for meshing solid geometry
•Applying uniform pressure load to a surface

3. 3
Problem Description
The structure shown below is designed to support a bearing on its right
(curved) surface. For this example, the left end is cantilevered. This means
that both the translational and the rotational are held to zero along this
surface. A pressure of 100 psi is applied normal to the surface curvature
where the bearing resides.
10 in
0.25 in
6 in
5 in
4 in
Radius 1.0 in
Radius 2.75 in
Modulus of Elasticity = 10e6 psi
Poisson’s ratio = 0.3
Thickness = 3 in

4. 4
Goal
• Use the 3D geometric modeling kernel of Patran to build the model
•Mesh the solid geometry using Tetmesh using Tet10 topology
• Determine the von Mises stress of the model of the bearing support
• Determine the displacement of the model of the bearing support

5. 5
Expected Results
von Mises Stress Displacement
Maximum stress = 1.65e3 psi @ Nd 3025
Minimum stress = 2.85e1 psi @ Nd 276
Maximum displacement = 1.83e-3 in. @ Nd 6
Minimum displacement = 0 in. @ Nd 1598

6. 6
Animation

7. 7
Starting MSC.Patran from Windows
a. Click on start menu
b. Roll mouse over All Programs
c. Roll mouse over MSC.Software
d. Roll mouse over MSC.Patran
2005 r2
e. Click on MSC.Patran 2005 r2
To start MSC.Patran from a
windows computer you will have to:

8. 8
Creating a New Database
a
a. Click File menu / Select New.
b. In the File name text field enter
bearing_support
c. Click OK button
d. Under Tolerance select Default.
e. For Analysis Code select MSC.Nastran
from the drop down menu
f. For Analysis Type select Structural from
the drop down menu
g. Click OK button
Note: MSC.Patran defaults the working folder to C:/windows/temp. Make sure the folder content is
deleted or backed up before starting a new database to avoid confusing among files.
b c
e
f
g
d

9. 9
a
Creating Solid Geometry with Block Primitive
a. Click on Geometry icon
b. Select Create / Solid /
Primitive from the drop
down menus
c. Click on the Block icon
d. In the X Length List text
field enter 10
e. In the Y Length List text
field enter 2
f. In the Z Length List text
field enter 3
g. Click on Auto Execute box
to turn it Off
h. In the Base Origin Point
List text field enter [0, 0, 0]
i. Click Apply button
j. Click on the Iso 1 View icon
k. Click on Hidden Line icon
b
c
d
e
f
g
h
i
j
k

10. 10
Creating Additional Solid Geometry with Block Primitive
a. Select Create / Solid /
Primitive from the drop
down menu
b. Click on Block icon
c. In X Length List text field
enter 1
d. In Y Length List text field
enter 3
e. In Z Length List text field
enter 3
f. Click on Auto Execute
check box to turn it Off
g. In Base Origin Point List
text field enter [10, -1, 0].
Note that the y coordinate
is negative because it
starts off below the origin.
h. Click Apply button
a
b
c
e
f
g
h
d

11. 11
Creating Additional Solid Geometry with Block Primitive
a. Select Create / Solid /
Primitive from the drop
down menu
b. Click on Block icon
c. In X Length List text field
enter 1
d. In Y Length List text field
enter 3
e. In Z Length List text field
enter 3
f. Click on Auto Execute
check box to turn it Off
g. In Base Origin Point List
text field enter [10, -1, 0].
h. Click Apply button
a
b
c
e
f
g
h
d

12. 12
Creating Solid Geometry with Cylinder Primitive
a. Select Create / Solid /
Primitive from the drop
down menus
b. Click on Cylinder icon
c. In the Height List text field
enter -3. This is because we
are selecting the orange
point as illustrated in the
viewport. Thus the negative
sign identifies that we are
going to extrude in the
negative z direction
d. For Radius List text field
enter 1
e. In the Thickness List text
field enter 1
f. Click on Auto Execute
check box to turn it Off.
g. For the Base Center Point
List select the orange
corner illustrated on the
viewport (point 10)
h. Click Apply button
a
b
c
d
e
f
g
h

13. 13
Creating Additional Solid Geometry with Cylinder Primitive
a. Select Create / Solid /
Primitive from the drop
down menus
b. Click on Cylinder icon
c. In the Height List text field
enter -3. This is because we
are selecting the orange
point as illustrated in the
viewport. Thus the negative
sign identifies that we are
going to extrude in the
negative z direction
d. For Radius List text field
enter 2.75
e. In the Thickness List text
field enter 2.75
f. Click on Auto Execute
check box to turn it Off.
g. For the Base Center Point
List select the orange
corner illustrated on the
viewport (point 19)
h. Click Apply button
h
g
e
d
b
a
c
f

14. 14
Using Boolean Subtraction of Solids
a. Select Edit / Solid /
Boolean form the drop
down menu
b. Click on the Subtract Icon
c. Click on Auto Execute
check box to turn it Off
d. For Target Solid click on
the small rectangle
illustrated on the viewport
(Solid 2)
e. For the Subtracting Solid
List text field click on the
small circle illustrated on
the viewport (solid 4)
f. Click Apply button
a
b
d
c
e
f

15. 15
Using Boolean Subtraction of Solids
a. Select Edit / Solid /
Boolean form the drop
down menu
b. Click on the Subtract Icon
c. Click on Auto Execute
check box to turn it Off
d. For Target Solid click on
the large rectangle
illustrated on the viewport
(solid 3)
e. For the Subtracting Solid
List text field click on the
large circle illustrated on
the viewport (solid 5)
f. Click Apply button
a
b
d
c
e
f

16. 16
Using Boolean Addition of Solids
Note from the previous slide that there are three solids parts. With this step we are
going to add all three solids to make only one solid geometry
a. Select Edit / Solid / Boolean
from the drop down menus
b. Click on the Add icon
c. In the Solid List text field
select all three solids by click
and dragging a rectangular
box over all three solids.
d. Click Apply button
This step is conducted before mirroring to decrease the total number of steps. If you were to not do this
first, you will have to mirror each solid individually and then adding all the solids together.
a
b
c
d

17. 17
Mirroring the Solid Geometry
a. Select Transforms / Solid /
Mirror from the drop down
menu
b. Click on the Define Mirror
Plane Normal text field with
out entering anything.
c. In the Picking Filter toolbar click
on 3 Point for the Plane
d. Click on the three corner
orange points as illustrated on
the viewport. Note nothing will
appear in the Desired Mirror
Plane Normal text field until all
three points are clicked
e. Click on Auto Execute check
box to turn Off
f. In the Solid List text field
select the entire solid at the
bottom
g. Click Apply button
h. The resulting view of the
viewport. Might need to refresh
and redraw the part.
a
b
c
d
e
f
g
h

18. 18
Using Boolean Addition of Solids
a. Select Edit / Solid /
Boolean from the drop
down menus
b. Click on Add icon
c. In the Solid List text field
select both solids by
dragging a square over
them.
d. Click Apply button
a
c
b
d

19. 19
Creating the Mesh using Tet Mesher
a. Click on Elements icon
b. Select Create / Mesh /
Solid from the drop down
menu
c. Under Element Shape
select Tet
d. Under Mesher select
TetMesh
e. Under Topology select
Tet10
f. In the Input List text field
select the entire geometry
(Solid 1)
g. For the Global Edge
Length Value text field
enter 0.5
h. Click Apply button
a
c
b
d
e
f
g
h
Note: Equivalencing the nodes is not required since there was a
single solid object and therefore no sharing of nodes
between objects

20. 20
Creating Boundary Condition for Left-End (Cantilevered)
a
a. Click on Load/BCs icon
b. Select Create / Displacement / Nodal from the
drop down menus
c. For the New Set Name text field enter left_end
d. Click on Input Data button
e. Under Translational text field enter <0, 0, 0>
f. Under Rotational text field enter <0, 0, 0>
g. Click Ok button
h. Click Select Application Region button
i. Make sure the radio button for Geometry Filter is
on Geometry
j. Click on the text field of Select Geometry
Entities
k. From the Picking Filter toolbar click on Surface
or Face
l. Click on Iso 2 View and select the left end.
m. Click Add button
n. Click Ok button
o. Click Apply button
Note:Recall from the notation that Solid 1.8 means that it is
from solid 1 and surface 8
b
c
d
e
f
g
h
i
j
k
l
m
n
o

21. 21
Creating Boundary Condition for Pressure Due to Bearing
a. Select Create / Pressure / Element Uniform
from the drop down menus
b. For the New Set Name text field enter
bearing_pressure
c. In the Target Element Type drop down menu
select 3D
d. Click on Input Data button
e. Under Pressure text field enter 100
f. Click Ok button
g. Click Select Application Region button
h. Make sure the radio button for Geometry Filter is
on Geometry
i. Click on the text field of Select Solid Faces
j. From the Picking Filter toolbar click on Surface
or Face
k. Select the right end curved part of the fixture
(solid 1.5)
l. Click Add button
m. Click Ok button
n. Click Apply button
a
b
c
d
e
f
g
h
i
j
k
l
m
n

22. 22
Summery of Boundary Conditions
a. The left cantilevered en
should be constrained in
the 123456 directions as
illustrated in the viewport
b. The pressure load should
be 100 as illustrated in the
viewport a
b

23. 23
Creating Material Properties
a. Click on Materials icon
b. Select Create / Isotropic / Manual Input
from the drop down menus
c. In the Material Name text field enter
aluminum
d. Click on Input Properties button
e. From the Constitutive Model drop down
menu select Linear Elastic
f. In the Elastic Modulus text field enter 10e6
g. In the Poisson Ratio text field enter 0.3
h. Click on Ok button
i. Click on Apply button
b
c
d
e
f
g
h
a
i

24. 24
Applying Properties to the Solid
a
a. Click on Properties icon
b. Select Create / 3D / Solid from the
drop down menus
c. In the Property Set Name text field
enter bearing_clamp
d. Click on Input Properties button
e. Click on Mat. Prop. Name icon
f. Click on aluminum
g. Click Ok button
h. In the Select Member text field
select the part (solid 1)
i. Click Add button
j. Click Apply button
b
c
d
e
f
h
i
j

25. 25
Analyzing Bearing Support Model
a. Click on Analysis icon
b. Select Analysis / Entire Model / Full Run from the
drop down menu
c. Click on Solution Type button
d. Make sure Linear Static radio button is selected
e. Click Ok button
f. Click Apply button
a
b
c
d
e
f

26. 26
Loading Results
a
a. Select Access Results / Attach XDB
/ Result Entities from the drop down
menu
b. Click on Select Result File… button
c. Select bearing_support.xdb
d. Click Ok button
e. Click Apply button
b
c
d
e

27. 27
a
Loading Results
a. Click on Results icon
b. Select Create / Quick Plot from the
drop down menu
c. Select Default, A1: Static Subcase
d. Select Stress Tensor
e. In the Quantity drop down menu
select von Mises
f. Select Constraint Forces,
translational
g. Click Apply button
b
c
d
e
f
g
Note: The fringe plot will have uneven colors like if it was not displaying well. This is to be expected; the
next slide will show you how to correct it…

28. 28
Fixing Display of Viewport to Properly Display Fringe Plot
a. Click on Display menu and
Plot/Erase… from the main program
menus
b. Under Geometry click on the Erase
button
c. Click Ok button

29. 29
Summary of Results
von Mises Stress Displacement
Maximum stress = 1.65e3 psi @ Nd 3025
Minimum stress = 2.85e1 psi @ Nd 276
Maximum displacement = 1.83e-3 in. @ Nd 6
Minimum displacement = 0 in. @ Nd 1598

30. 30
Important Skills Acquired
• Creating 3D geometry using primitives in Patran (block and cylinder)
• Using Boolean geometry to merge and subtract geometries from part
• Transforming solid geometry by mirroring using 3 points on a plane
• Using Tetmesher with Tet10 elements for meshing solid geometry
•Applying uniform pressure load to a given surface

31. 31
Further Analysis (Optional)
• It can be clearly observed from the results that the stress will concentrate in the
edges furthest to the right where the bearing comes into contact with the
support. What will be a good method to reduce such stresses (use FEA analysis
to prove predictions)

32. 32
Best Practices
• When modeling a part that has symmetry along a plane,
take advantage of such characteristic to save time on
having to model unnecessary parts. Translating such
geometries will be much faster
•Using Boolean relations on primitive solid geometries is
easier and faster for simple parts than to drawing the
shape of the part and then extruding.