CATIA V5 FEA Tutorial.pdf

CATIA V5 FEA
Tutorials
Release 21
Nader G. Zamani
®
www.SDCpublications.com
Better Textbooks. Lower Prices.
SDC
P U B L I C A T I O N S
Schroff Development Corporation

Visit the following websites to learn more about this book:

CATIA V5 FEA Tutorials 2-1
Chapter 2
Analysis of a Bent Rod with Solid
Elements

2-2 CATIA V5 FEA Tutorials
Clamped end
loaded end
Clamped end
loaded end
Introduction
In this tutorial, a solid FEA model of a bent rod experiencing a combined load is created.
No planes of symmetry exist and therefore model simplifications cannot be made.
Finally, the significance of the von Mises stress in design equation is discussed.
1 Problem Statement
The bent rod, shown to the right, is clamped at one end and
subjected to a load of 2000 lb as displayed. The steel rod has a
Young’s modulus of 30E+6 psi and Poisson ratio 0.3.
The nominal dimensions of the rod are also displayed below.
Although this problem is more efficiently handled with beam
elements, we propose to use solid elements.
There are two main types of solid elements available in CATIA
V5, linear and parabolic. Both are referred to as tetrahedron
elements and shown below.
The linear tetrahedron elements are faster computationally but less accurate. On the other
hand, the parabolic elements require more computational resources but lead to more
accurate results. Another important feature of parabolic elements is that they can fit
curved surfaces better. In general, the analysis of bulky objects requires the use of solid
elements. Hexahedral elements are also available on a limited basis in recent releases of
CATIA. These elements will be discussed in a later chapter.
2 Creation of the Part in Mechanical Design Solutions
Enter the Part Design workbench which can be
achieved by different means depending on your CATIA
customization. For example, from the standard Windows
toolbar, select File > New . From the box shown on
the right, select Part. This moves you to the Part Design
workbench and creates a part with the default name Part.1.
See Note#1 in Appendix I.
5 in
8 in
1 in
Cross sectional
Radius is 1 in
Tetrahedron Elements
linear parabolic
Tetrahedron Elements
linear parabolic

Analysis of a Bent Rod with Solid Elements 2-3
In order to change the default name, move the cursor to Part.1 in the tree, right-click and
select Properties from the menu list.
From the Properties box, select the Product tab
and in Part Number type wrench. This will be
the new part name throughout the chapter. The tree
on the top left corner of the screen should look as
displayed below.
From the tree, select the xy plane and enter the Sketcher . In the Sketcher, draw a
circle , and dimension it . In order to change the dimension, double-click on the
dimension on the screen and in the resulting box enter radius 1. Your simple sketch and
the Constraint Definition box used to enter the correct radius are shown below.
Leave the Sketcher .
From the tree, select the yz plane and enter the Sketcher . Draw the spine of the
bent rod by using Profile and dimension it to meet the geometric specs. In the
Sketcher, the spine should match the figure shown next. Upon leaving the Sketcher
, the screen and the tree should resemble the following figures.

You will now use the ribbing operation to extrude the
circle along the spine (path). Upon selecting the rib
icon , the Rib Definition box opens. For Profile
select the circle (Sketch.1) and for the Center Curve
select (Sketch.2) as indicated. The result is the final
part shown below.
The next step is to apply material properties on the part created.
Use the Apply Material icon from the bottom row of toolbars. The use of this icon
opens the material database box shown next.

Choose the Metal tab on the top; select Steel. Use your cursor to pick the part on the
screen at which time the OK and Apply Material buttons can be selected.
Close the box.
The material property is now reflected in the tree.
In order to inspect the values of the material properties assigned, double-click on Steel
in the tree. It may take a minute before the database is searched. You will notice that the
Properties box shown below opens. Choose the Analysis tab from this box, and the
values will be displayed. Note that these values can be edited.
Since your Young’s modulus and Poisson ratio are different from what is shown, in
appropriate boxes, type Young’s modulus = 3E+7 and Poisson ratio =.3. Press OK.

If the part is still “gray”, one can change the rendering style. From the View toolbar
, select the View mode toolbar
.
Next choose the Shading with Material
The part now appears shaded as shown on the right.
3 Entering the Analysis Solutions
From the standard Windows toolbar, select
Start > Analysis & Simulation > Generative Structural Analysis
There is a second workbench known as the Advanced Meshing Tools which will be
discussed later.
The New Analysis Case box pops up. The default choice is Static Analysis which is
precisely what we intend to use. Therefore, close the box by clicking on OK.
Note that the tree structure gets considerably longer.
The bottom branches of the tree are presently
“unfilled”, and as we proceed in this workbench,
assign loads and restraints, the branches gradually
get “filled”.
Another point that cannot be missed is the
appearance of an icon close to the part that reflects
a representative “size” and “sag”. This is displayed
in the next figure.

The concept of element size is self-explanatory. A smaller element size leads to more
accurate results at the expense of a larger computation time. The “sag” terminology is
unique to CATIA. In FEA, the geometry of a part is approximated with the elements. The
surface of the part and the FEA approximation of a part do not coincide. The “sag”
parameter controls the deviation between the two. Therefore, a smaller “sag” value could
lead to better results. There is a relationship between these parameters that one does not
have to be concerned with at this point.
The physical sizes of the representative “size”
and “sag” on the screen, which also limit the
coarseness of the mesh can be changed by the
user. There are two ways to change these
parameters:
The first method is to double-click on the
representative icons on the screen which
forces the OCTREE Tetrahedron Mesh
box to open as shown to the right. Change the
default values to match the numbers in the
box.
Notice that the type of the elements used (linear/parabolic) is also set in this box. Close
the box by selecting OK.
The second method of reaching this box is through the tree.
By double-clicking on the branch labeled OCTREE Tetrahedron Mesh shown below,
the same box opens allowing the user to modify the values.
In order to view the generated mesh, you can point the cursor to the branch Nodes and
Elements, right-click and select Mesh Visualization. This step may be slightly
different in some UNIX machines. Upon performing this operation a Warning box
appears which can be ignored by selecting OK. For the mesh parameters used, the
following mesh is displayed on the screen. See Note #2 in Appendix I.
Representative sag
Representative size
Representative sag
Representative size

The representative “size” and “sag” icons can be removed from the display by simply
pointing to them right-click and select Hide. This is the standard process for hiding any
entity in CATIA V5.
Before proceeding with the rest of the model, a few more points regarding the mesh size
are discussed. As indicated earlier, a smaller mesh could result in a more accurate
solution; however, this cannot be done indiscriminately. The elements must be small in
the regions of high stress gradient such as stress concentrations. These are areas where
the geometry changes rapidly such as bends, fillets, and keyways.
Uniformly reducing the element size for the whole part is a poor strategy.
CONGRATULATIONS! You now have a mesh with the correct material properties.
Regularly save your work.
Applying Restraints:
CATIA’s FEA module is geometrically based. This means that
the boundary conditions cannot be applied to nodes and
elements. The boundary conditions can only be applied at the
part level. As soon as you enter the Generative Structural
Analysis workbench, the part is automatically hidden.
Therefore, before boundary conditions are applied, the part
must be brought to the unhide mode. This can be carried out by
pointing the cursor to the top of the tree, the Links
Manager.1 branch, right-click, select Show. At this point, the
part and the mesh are superimposed as shown to the right and
you have access to the part.
If, the presence of the mesh is annoying, you can always hide it. Point the cursor to
Nodes and Elements, right-click, Hide.
Instead of hiding the mesh as indicated above, one can point the cursor to the Mesh.1
item in the tree, right-click, and select Activate/Deactivate. The result is that the mesh
is hidden and the part is displayed. The steps are graphically in the next figure.

In FEA, restraints refer to applying displacement boundary conditions which is achieved
through the Restraint toolbar . In the present
problem, you can assume that the base of the longer section is
clamped. The Clamp condition means that the displacements
in all three directions are zero. Select the Clamp icon and
pick the bottom face of the rod. Be careful not to pick the
circumference (edge) of the circle instead of the face. In that
case, only two restraint symbols will be shown attached to the circumference.
Applying Loads:
In FEA, loads refer to forces. The Loads toolbar is used
for this purpose. Select the Distributed Force icon , and with the cursor pick the
other face of the rod which is loaded. The Distributed Force box shown below opens.
A visual inspection of the global axis on your screen indicates that the force of magnitude
2000 lb should be applied in the negative x-direction.

Although in our problem the 2000 lb force is applied in
the global direction x, it is possible to apply forces in
the local direction specified by the user. Upon selection
of the appropriate face, the force symbols will appear
as shown below.
If the circumference of the circle is accidentally picked,
only two arrows attached to the circle will appear.
Although in our present problem there may be small
differences in the results, one should apply the loads and restraints as intended.
The portion of the tree which reports the restraints and loads is shown below.
Launching the Solver:
To run the analysis, you need to use the Compute
toolbar by selecting the Compute icon . This leads to the Compute box
shown above. Leave the defaults as All which means everything is computed.
Upon closing this box, after a brief pause, the second box shown below appears. This box
provides information on the resources needed
to complete the analysis.
If the estimates are zero in the listing, then
there is a problem in the previous step and
should be looked into. If all the numbers are
zero in the box, the program may run but
would not produce any useful results.
The tree has been changed to reflect the
location of the Results and Computations as
shown below.

The user can change these locations by
double-clicking on the branch. The box,
shown on the right, will open and can be
modified.
Postprocessing:
The main postprocessing toolbar is called Image . To view the deformed
shape you have to use the Deformation icon . The resulting deformed shape is
displayed below.
The deformation image can be very deceiving because one could
have the impression that the wrench actually displaces to that
extent. Keep in mind that the displacements are scaled
considerably so that one can observe the deformed shape.
Although the scale factor is set automatically, one can change
this value with the Deformation Scale Factor icon in the
Analysis Tools toolbar .
Clicking on the above icon leads to the box shown on
the right where the desired scale factor can be typed.
The deformed shape displayed corresponds to a scale
factor of 46.017. The displayed value on the screen is
46.017 times the actual maximum displacement.

In order to see the displacement field, the
Displacement icon in the Image toolbar
should be used. The default display is in terms of
displacement arrows as shown on the right. The
color and the length of arrows represent the size
of the displacement. The contour legend indicates
a maximum displacement of .0353 in.
The arrow plot is not particularly useful. In order
to view the contour plot of the displacement field,
position the cursor on the arrow field and double-
click. The Image Edition box shown below opens.
Note that the default is to draw the contour on the
deformed shape. If this is not desired, uncheck the
box On deformed mesh. Next, select
AVERAGE-ISO and press OK.
The contour of the displacement field as shown is
plotted.
It is difficult to read the contour lines from the above
figure. You can change the render style by using
Shading with Material icon in the
View Mode toolbar
.
Note that the elements are not showing in this plot. If
you prefer that the elements are displayed at the same
time, you need to go through the following step.
Select the Custom View Mode icon from the above toolbar. In the resulting pop
up box, make sure that Edges and points is checked.

Ignoring the fillet radius of the bend, the beam bending solution of this problem can be
obtained using Castigliano’s theorem. This approximate value is .044 in which is in the
same ball park as the FEA solution of .0392 in. The discrepancy is primarily due to the
large bend radius.
Clearly, the maximum displacement is at the point of the application of the load, in the
negative x-direction. (Note: The color map has been changed; otherwise everything looks
black in the figure.)
The next step in the postprocessing is to
plot the contours of the von Mises stress
using the von Mises Stress icon
in the Image toolbar.
The von Mises stress is displayed to the
right.
The maximum stress is at the support
with a value of 2.06E+4 psi which is
below the yield strength of most steels.

Double-clicking on the contour legend leads to the Color Map box displayed on the
right.
The contour can be plotted as Smooth or Stepped. The
number of color bands is also specified in this box. Finally,
the user can describe the range of stresses to be plotted.
Occasionally, you may be interested in plotting the von
Mises stress contour in either the load area or the support
section. In order to achieve this, double-click on the
contour levels on the screen to open the image edition box. Next use the Selections tab
as shown below. Here, you have the choice of selecting different areas.
The contours on the right display the von Mises stress at Distributed Force.1 and
Clamp.1 sections.
Unfortunately in the current release of CATIA this
contour is rather useless. In a later chapter, you will
be shown how to use the Group concept to generate
a better contour plot as indicated below.

As the postprocessing proceeds and we
generate different plots, they are recorded in
the tree as shown. Each plot generated
deactivates the previous one on the screen.
By pointing to a desired plot in the tree and
right-clicking, you can activate the plot.
Clearly any plot can be deleted from the tree
in the usual way (right-click, Delete).
The location and magnitude of the extremum values of a contour (e.g. von Mises stress)
can be identified in a plot. This is achieved by using the Image Extrema icon in the
Image Analysis toolbar .
Before the plot is generated, the Extrema Creation box
pops up as shown to the right. If the default values are
maintained, the global maximum and minimum are found
and their location pin-pointed in a contour plot as displayed
below.
At this point we have generated two plots. The displacement and the von Mises stress
contours which can be displayed individually. However, CATIA also allows you to show
both plots side by side.
First make sure that both images to be plotted are active in the tree. If not, point to the
graph in the tree, right-click, select Active.
Click the Image Layout icon from the
Image Analysis toolbar. The Images box,
shown to the right, asks you to specify the direction
along which the two plots are expected to be
aligned.

The outcome is side-by-side plots shown below. (Note: The color map has been changed
otherwise everything looks black.)
Before describing how the principal stresses are plotted, we like to elaborate on the
significance of the von Mises stress plot.
The state of stress is described by the six Cauchy stresses { }
yz
xz
xy
z
y
x ,
,
,
,
, τ
τ
τ
σ
σ
σ which
vary from point to point. The von Mises stress is a combination of these according to the
following expression:
( )
[ ]
)
(
6
)
(
)
(
2
1 2
yz
2
xz
2
xy
2
z
y
2
z
x
2
y
x
VM τ
+
τ
+
τ
+
σ
−
σ
+
σ
−
σ
+
σ
−
σ
=
σ
For an obvious reason, this is also known as the effective stress. Note that by definition,
the von Mises is always a positive number. In terms of principal stresses, VM
σ can also
be written as
[ ]
2
3
2
2
3
1
2
2
1
VM )
(
)
(
)
(
2
1
σ
−
σ
+
σ
−
σ
+
σ
−
σ
=
σ
For many ductile materials, the onset of yielding (permanent plastic deformation) takes
place when Y
VM σ
=
σ where Y
σ is the yield strength of the material. For design purposes,
a factor of safety “N” is introduced leading to the condition
N
Y
VM
σ
=
σ .
Therefore, a safe design is considered to be one where
N
Y
VM
σ
<
σ . The von Mises stress
contour plot allows you to check the above condition.

The Cutting Plane icon from the Analysis tools toolbar
can be used to make a cut
through the part at a desired location and inspect the stresses
inside of the part. The Cut Plane box allows you to keep
the plane or to remove it for display purposes. A typical
cutting plane is shown below.
The principal stresses are postprocessed next.
The principal directions are three mutually
perpendicular directions along which only normal
stresses act. These normal stresses are known as the
principal stresses. The figure to the right displays the
principal directions x1, x2, and x3, together with the
principal directions 1
σ , 2
σ , and 3
σ . The standard
convention in stress analysis is to label the stresses
according to 3
2
1 σ
≥
σ
≥
σ . The principal stresses are important for both theoretical
reasons and practical ones. In experimental stress analysis, the positioning of strain
gauges relies on the principal directions on the surface of a part.
From the Image toolbar ,
select the Principal Stress icon . The
result is the principal stress directions in the
vector form as displayed to the right. Due
to the large number of arrows, the
interpretation of this plot is difficult.
A zoomed view of the tip is also shown
below.
σ2
σ1
σ3
σ2
σ1
σ3

You can improve on the display of principal
stresses by selecting a specific stress component to
be plotted. To do so, double-click on the arrows on
the screen which causes the Image Edition,
shown to the right to open. Click on the More
button to expand the window as shown below.
Choose the Component C11. In CATIA, C11
represents 1
σ , the largest principal stress.
At this point the vector plot displays only the directions associated with 1
σ as shown in
the plot below.
An alternative to the vector plot of the principal stress
is the contour plot of 1
σ . This can be achieved
through the Image Edition box, under the Visu tab.
You should select AVERAGE-ISO instead of
Symbol. The resulting contour plot is shown below.

Using the icon Generate Report in the Analysis Results toolbar
an HTML based report can be generated which summarizes the features
and results of the FEA model. The first page of this report is displayed below.
Finally, animation of the model can be achieved through the Animate icon in the
Analysis Tools toolbar and AVI files can easily be
generated.

Exercises for Chapter 2
Problem 1: Analysis of a Foot Pedal
The foot pedal shown below is made of steel with Young’s modulus 30E+6 psi and
Poisson ratio 0.3. The pedal is loaded with a normal force of 100 lb along the edge
shown. The other end of the pedal is clamped. The geometrical dimensions are provided
at the bottom of the page where all the dimensions are in inches.

Try running the model with the two different element “size” and “sag” with both the
linear and parabolic type of elements. Record the results in terms of the maximum
displacement and the maximum von Mises stress in a table and comment on the results.
The run time of the parabolic elements with element size of 0.1 could be substantial
depending on the type of processor used.
Partial Answer:
Size = .3, sag = .05
Element Type Linear Parabolic
Maximum
Displacement
.0158 in. .0227 in.
Maximum
von Mises
Stress
5.32E+3 psi 1.1E+4 psi
Size = .1, sag = .05
Element Type Linear Parabolic
Maximum
Displacement
.021 in. .0229 in.
Maximum
von Mises
Stress
9.43E+4 psi 1.6E+4 psi
The above tables reveal an extremely important fact about finite element analysis.
Making a single run and accepting the results at face value is a serious mistake. Note that
for linear elements as the mesh is refined, there is a significant change in both
displacement and von Mises stress. The user should not accept either value as being
correct and must refine the mesh further. The refinement should reach a point at which
the difference with the previous mesh is not deemed to be significant to user. This
process is referred to as a mesh convergence study.
Keep in mind that the refinement need not be uniform throughout the part. One should
perform the refinement in the critical areas only. It is clear that parabolic elements are
superior in accuracy to linear element. Furthermore, note that although the displacement
seems to have stabilized, the von Mises is still unreliable. It is well known that the
displacements in FEA are more accurate than stresses. The reason is that the stresses are
obtained by differentiating the displacement, a process which magnifies the error.

Problem 2: Analysis of a Cylindrical Bar under Torsion
The cylindrical bar shown below has a clamped end. The other end is subjected to a
couple caused by opposite forces on magnitude 1000 lb separated by 1.5 in. This is
equivalent to a torque of 1500 lb.in applied to the cylinder. The material is steel with
Young’s modulus 30E+6 and Poisson ratio of 0.3.
The diameter of the cylinder is 1 in. and the dimensions of the loaded end are shown
below. Although not showing, the length of the padded cylinder is 5 in. and the length of
the padded rectangle is 0.5 in. All sharp corners at the loaded end have surface fillet of
radius 0.1 in.

Model the part with linear solid elements with size = 0.1 and sag = 0.025 which results in
the mesh shown in the previous page. Compare the hoop stress (The hoop stress is the
largest principal stress “C11”) with the theoretical solution from strength of materials.
Partial Answer:
The strength of materials solution is based on
J
Tr
=
τ where T is the applied torque, r is
the radius of the cylinder and J is the polar moment of inertia. In terms of the diameter,
2
D
r = , and
32
D
J
4
π
= . The hoop stress “C1” which numerically equals τ is calculated
from 3
D
T
16
π
. For the present problem, 1500
T = lb.in and 1
D = in. Based on these
parameters, a value of 7643 psi for the hoop stress is predicted.
The FEA results can be assessed by plotting the contour of “C1” at the clamped section.
The resulting plot shown below agrees quite well with 7643 psi obtained earlier. The
circular fringe patterns are another qualitative check on the validity of the FEA results.

CATIA V5 FEA Tutorial.pdf

More Related Content

What's hot (20)

Similar to CATIA V5 FEA Tutorial.pdf (20)

Recently uploaded (20)

CATIA V5 FEA Tutorial.pdf