THERMAL ANALYSIS OF A COOLING FIN USING SHELL ELEMENTS

previous MODELING A CANTILEVERED BEAM’S VIBRATION USING 4 NODE SHELL ELEMENTS

I. THE PHYSICAL PROBLEM The problem you will model is a fin of aluminum alloy, 0.2 m long, 0.002 m thick and large width. This is the type of fin that might provide air-cooling on a motorcycle engine. For the finite element model, we consider a representative strip of the fin 0.01 m in depth (shown as the region between the dotted lines in the drawing). The 200-degree wall is representative of the hot temperature of the engine. Our goal is to find the temperature distribution down the fin. If the outside tip of the engine is too hot, it can be a safety concern. Heat is conducted down the fin (away from the heat source of the engine) and heat is also lost through convection from the top and bottom surfaces to the air. The ambient temperature of the air is known to be 25 C° and the convection coefficient (film coefficient) is known to be 30 (W/m²) . The fin itself is made of aluminum which has a conductivity of 177 (W/m² K).

II. THINKING ABOUT THE MECHANICS The analytic solution for the temperatures for this problem is readily available. Any Heat Transfer text will provide equations for the temperature distribution of a fin considering conduction away from the heat source and convection from the top and bottom surfaces. These results can be used to give basic analytic comparison solutions for certain sections of the structure. Note that we assume no radiation occurs and that only the top and bottom surfaces have significant convection heat transfer (the convection from the edges of the fin is neglected). These assumptions are normal for a first level analysis where the temperatures are in the ranges used in this problem.

III. GEOMETRIC AND FINITE ELEMENT MODEL
As is the standard procedure for building MSC/Patran models, we will build the geometry first and then construct a finite element mesh on that geometry. The geometry will proceed from creation of curves to a surface for this simple model. Next, we will use 4 node 2-dimensional elements to model the fin. Next, the material and element properties will be entered. We will set the wall temperature and the convection characteristics for the top and bottom of the fin. Finally, the nodes must be equivalenced before the analysis is ready to run.

IV. FINITE ELEMENT THEORY
The exact details of the formulation of the 4 node 2-d elements in MSC/Nastran is rather complicated. However, the basic formulation of the 2-d thermal element is not extremely difficult and will provide us with sufficient background information to begin to understand the general application areas and convergence of these elements. This basic formulation for the 2-d thermal, linear, quasistatic element can be found in most any Finite Element Analysis text (see for example Finite Elements for Stress Analysis, by R.D. Cook, John Wiley & Sons, 1995.).

V. INSTRUCTIONS FOR MODELING THE FIN USING MSC/PATRAN & MSC/NASTRAN

Preliminaries for using PATRAN include:
a) Log on to the computer
b) Click START (lower left corner of the Windows Desktop), go to Programs, Select MSC (common), Select MSC Patran9.0.

The instructions below give details for modeling the thermal fin problem discussed above. The instructions are NOT as detailed as have been given in other problems as it is expected that you have begun to get a feel for how to do certain tasks in Patran.

In the instructions below, the following abbreviations and terms will be used:
TM = Top Menu. This refers to the horizontal menu options residing at the top of the screen after PATRAN has been initiated.
RM = Right Menu. This refers to the menus that pop up after an option has been chosen from the top menu. These menus reside on the far right side of the PATRAN desktop.
SM = Subordinate Menu. This referees to the menus that pop up from options selected in the right menu.
Click = Unless otherwise stated, this indicates a click with the left mouse button.
Boldface will indicate text that occurs in the PATRAN menus.
Italics text will indicate text that you must enter into text boxes in the PATRAN menus or text that you choose in a menu scroll box.
1. Our first step is to create a new database:
From the TM choose File In the resulting pull down menu choose New
A SM called New Database pops up
Turn on (checked) Modify Preferences
Under File Name enter fin.db
Click OK
2. Next set the analysis preference:
A New Model Preferences window will appear as a RM
Under Tolerance choose Based on Model Set Model Dimension to 0.2
Under Analysis Code choose MSC/NASTRAN
Choose Analysis Type = Thermal
click OK
3. The geometry of the beam will be determined next: Select Geometry from TM.
On RM, select Action= Create, Object= Curve, Method= XYZ
Note Curve ID List has a 1.
Refer. Coordinate Frame should be Coord 0
Set Vector Coordinates List to 0.2 0 0 (You will be drawing lines (vectors) with these xyz components.)
Origin Coordinates List = 0 0 0 Click APPLY. (A line from origin to point 0.2,0,0 should appear on screen.)
Make second curve: With same vector, set Origin Coordinates List to 0 0.01 0.
Click Apply. (A second curve appears on the screen.)
Now create a surface between the curves.
On the Geometry RM, choose Action= Create; Object= Surface; Method= Curve.
Set Option to 2 Curve.
Note there is a Starting Curve List and Ending Curve List.
Click in the Starting Curve List box. .Select the first curve by using the mouse.
Click the small box on curve 1 on the screen. Click in the Ending Curve List box. Then click on curve 2. Note a surface is created.
4. Create the finite elements. On the TM select Elements and get a RM.
Choose Action= Create; Object=Mesh; Type= Surface
Choose the size of the elements. Type in Global Edge Length: 0.01
Select Isomesh. Click in Surface List box. Select the Surface 1 with the cursor.
Click Apply. Note the model has 20 elements.
5. Create Boundary conditions
At TM, select Load/BC’s. Get RM.
Now create the convection characteristics for the bottom of the fin
Chose Action=create, Object=convection, type=element uniform
Name the convection BC. In New Set Name, type top-convec Select Target Element Type = 2D
Click Input Data. Get submenu. Type 30 for convection coefficient (w/m²c) for top surface convection. Type 25 for ambient temp. Click OK. Back in Load/ BC menu, click Select Application Region box
Select FEM as the Geometry Filter.
Click in Select 2D Elements or Edges box
Using mouse, click on all the elements. (Hold shift down for multiple selections.) Click Add.
The application region box should list the elements 1:20. Click OK Back in Load/BC menu click Apply.
Now create the convection characteristics for the bottom of the fin
Chose Action=create, Object=convection, type=element uniform
Name the convection BC. In New Set Name, type bot-convec Select Target Element Type = 2D
Click Input Data. Get submenu. Type 30 for convection coefficient (w/m²c) for bottom surface convection. Type 25 for ambient temp. Click OK.
Back in Load/ BC menu, click Select Application Region box
Select FEM as the Geometry Filter.
Click in Select 2D Elements or Edges box
Using mouse, click on all the elements. (Hold shift down for multiple selections.) Click Add.
The application region box should list the elements 1:20. Click OK
Back in Load/BC menu click Apply.
Now create the base temperature BC.
In Load/BC RM Action=create, Object=Temp, type=nodal
In New Set Name type Basetemp. Click on Input Data.
In submenu Input Data, type 200 in Temperature box. Click OK.
Back in Load/BC SM, click on Select Application Region.
In submenu, select FEM as Geometry Filter.
Click on Select Nodes.
Using mouse, select the nodes 1 and 22 at the extreme left of the model. Click Add. Click OK.
Back in Load/BC menu, click Apply. (The screen should show 200 at nodes 1 and 22.)
6. Create and select material
On TM select Materials.
In submenu, Action=create, Object=isotropic, method=manual input.
In Material Name box, type aluminum. Click Input Properties.
In submenu, Input Options, enter thermal conductivity as 177. (w/m²k).
Click OK. If SM does not disappear, Click Cancel.
Back in the RM , Click Apply
In TM, select Properties
In submenu Action=create, Object=2D, Type=shell.
In Property Set Name type shell_prop.
Click on Input Properties In submenu, click on Aluminum in the Material Property Sets box.
M: Aluminum appears in the Material Name box at the top of the form.
Set Thickness= 0.002 Click OK.
Back in Element Properties, click Select members.
Use mouse to select the entire model. (You can click and draw a box around the entire model to select it.) Click Add. Click Apply.
7. Load Boundary Conditions
In order to have both the convection on top and on the bottom as well as the and base temperature
BC on the model, all 3 boundary conditions must be combined into a single load case.
In TM, select Load Cases.
In SM, Action=Create, Load case name, type fin_case.
In Description, type: h=30 on fin with base= 200C. and ambient=25C.
Click on Assign/Prioritize BC under the Select Individual Loads/BC Click on conve_bot-convec and then on conve_top-convec and then on temp_basetemp
As you click on these each of the 3 is added to the Assigned Load/BC
At the bottom of the menu, click OK Back in the Load Case RM, click Apply
8. Analyze (solve) for temperature.
In TM select Analysis. In SM, Action= Analysis, Object = entire model, Method = Full Run, Job name = fin Click translation Parameters and set output to Op2 & Print
Click, OK Back in the Analysis RM, click Solution Type
Choose Steady State Analysis
Click OK
Back in the Analysis RM, choose Subcase Create
Under Available Subcases, select fin_case
Under Available Loadcases, select fin_case
Click Apply
Click Cancel
Back in the Analysis RM, click Subcase Select Under Subcases for Solution Sequence 153, select fin_case
Under Subcases Selected, click on Default (this removes default from the list)
Click OK Back in Analysis SM Click Apply

9. To read in the results for post-processing
.In the RM=Analysis
Set Action = Read Output2; Object = Results Entities; Method = Translate
Click Select Results File
A SM appears called Select File Click the file fin.op2 (You may need to look in your home or root directory to find the file. If this file does not exist, then you have made a mistake in constructing your model. Go to Explorer (right-click on Start and choose Explore) and find the file fin.log and fin .f06. Open these files by double clicking on them and search for the word “error” or “fatal” to determine what your mistake is).
fin.op2 then appears in the File Name box
Click OK
(back in the Analysis menu)
Click Apply

10. Select the TM Results
A RM will appear called Results
Set Action = Create
        Object = Quick Plot
You can display different results, but the main focus will be on the temperatures.
11. Next you will end your MSC/PATRAN session by saving your database and exiting.
On the TM select File From the pull down menu select Save
On the TM select File From the pull down menu select Quit

MODELING A CANTILEVERED BEAM’S VIBRATION USING 4 NODE SHELL ELEMENTS

previous MODELING A STABELIZATION FIXTURE WITH END PRESSURE USING SOLID ELEMENTS

MSC/PATRAN TUTORIAL # 6
MODELING A CANTILEVERED BEAM’S VIBRATION USING 4 NODE SHELL ELEMENTS

I. THE PHYSICAL PROBLEM
The beam below is cantilevered or "built in" on the left edge. This means that both the translations and the rotations are held to zero along this edge. The material properties for the beam are E= 70 x 10⁹ Pascals (typical for Aluminum) and n = 0.3 . The beam has a solid rectangular cross section with thickness in the Z-direction t = 0.01 meters and height in the Y-direction h = 0.1 meters. We wish to find the mode shapes and associated vibration frequencies for this beam.

II. THINKING ABOUT THE MECHANICS
The analytic solution (modes shapes and natural frequencies) for this problem is readily available. Any vibrations text will provide equations for the mode shapes (eigenvectors) and the natural frequencies (eigenvalues). These equations are given below. For the cantilevered beam with bending moment of inertia “I”, Elastic (Young’s) modulus “E”, mass per unit length “m” and Length “L”, the first 3 natural frequencies W_1-3 (rad/sec) are given by:

Note that these correspond to the following 3 mode shapes which are all bending modes in the plane of the smallest value of “I”.

Modeshape 1:

Modeshape 2:

Modeshape 3:

Some basic questions to consider before creating the computational model are:

1. Are there any other types of mode shapes that might occur (torsional, axial or bending in a different plane)?
2. What would be a reasonable frequency for the first mode shape?
3. Are there any constraint force checks that will help me validate the accuracy of my model?

Answering these questions qualitatively, along with the quantitative analytical solutions for the mode shapes and their associated natural frequencies will provide reinforcement that your computational model is correctly constructed.

III. GEOMETRIC AND FINITE ELEMENT MODEL As is the standard procedure for building MSC/Patran models, we will build the geometry first and then construct a finite element mesh on that geometry. The geometry will proceed from creation of points to curves to surfaces for this simple model. Next, we will use 4 node shell elements to model the beam. Next, the material and element properties will be entered. We will constrain the 3 displacement and 3 rotational degrees of freedom on the left edge (for all nodes). This creates the cantilevered or built-in, end condition. Finally, the nodes must be equivalenced before the analysis is ready to run.

IV. FINITE ELEMENT THEORY The exact details of the formulation of the 4 node shell elements in MSC/Nastran is rather complicated. However, the basic formulation of an isoparametric 4 node membrane element is not extremely difficult and will provide us with sufficient background information to begin to understand the vibration model studies. This basic form is constructed as follows:

Isoparametric Formulation of a 2-D Membrane Element [K] Matrix
Assume the element has the configuration shown below:

The physical and natural coordinate locations of the 4 nodes are:

Our goal is to find the element stiffness matrix

ASSUME: 2 displacement degrees of freedom (dof) per node With :
[B] = the strain - displacement matrix such that [B]{u} = {ε}
where: {u} is the dof vector and {ε} is the strain vector
[E] = the constitutive matrix such that [E]{ε} = {σ}
where {σ} is the stress vector and V = volume.

Step 2: Find the [B] matrix:

Step 3: Use the Jacobian to find derivatives:

i.e. the isoparametric assumption is that geometry can be interpolated using the same interpolation functions as the displacements.

This allows us to find the entries in [B]
Step 4: Perform the numerical integration:

where |J| is the determinant of the Jacobian matrix.

Gaussian numerical integration is then used to find the final numbers for the element stiffness.

Where ng_j and ngi are the number of gaussian integration points in the “j” and “i” directions respectively and w_j and w_i are the associated gaussian weighting factors.

Understanding the Computational Vibration Analysis :
The elements as formed above must be assembled into a global stiffness matrix. In the same manner, element mass matrices are formed using the equation

[M] = ρʃ[N]T [N] J dx dh . A similar form exists for the Rayleigh damping matrix . A similar form exists for the Rayleigh damping matrix [C]. The stiffness, mass and damping matrices are then used in the dynamics equilibrium relationship where the over-dots indicated derivatives with respect to time and {f} is the forcing function. This set of equations can be solved for the time history of the motion (transient dynamics) or for the eigenvalues and eigenvectors. For the vibration analysis, the damping and the forcing function are assumed to be zero. The resulting eigenvalue problem of the second kind is : [M] {w} + [K] {d} = {0} where eigenvalues are the natural frequencies w and the eigenvectors {d} give the node shapes.

V. STEP BY STEP INSTRUCTIONS FOR MODELING THE VIBRATION OF THE CANTILEVERED BEAM USING MSC/PATRAN

Preliminaries for using PATRAN include:
a) Log on to the computer
b) Click START (lower left corner of the Windows Desktop), go to Programs, Select MSC (common), Select MSC Patran9.0.

In the instructions below, the following abbreviations and terms will be used:
TM = Top Menu. This refers to the horizontal menu options residing at the top of the screen after PATRAN has been initiated.

RM = Right Menu. This refers to the menus that pop up after an option has been chosen from the top menu. These menus reside on the far right side of the PATRAN desktop.

SM = Subordinate Menu. This referees to the menus that pop up from options selected in the right menu.
Click = Unless otherwise stated, this indicates a click with the left mouse button.
Boldface will indicate text that occurs in the PATRAN menus.
Italics text will indicate text that you must enter into text boxes in the PATRAN menus or text that you choose in a menu scroll box.
1. Our first step is to create a new database:
From the TM choose File In the resulting pull down menu choose New
A SM called New Database pops up
Turn on (checked) Modify Preferences Under File Name enter beam-vib.db
Click OK
2. Next set the analysis preference:
A New Model Preferences window will appear as a RM
Under Tolerance choose Based on Model
Set Model Dimension to10.0
Under Analysis Code choose MSC/NASTRAN
Choose Analysis Type = Structural
click OK
3. The geometry of the beam will be determined next: From the TM choose Geometry A RM called Geometry will result
Set Action = Create
        Object = Point
        Method = XYZ
Set the Point ID list to 1
Set Reference Coordinate Frame to Coord 0
Turn off the Auto Execute button
Enter the following into the Point Coordinates list:
[0,0,0] (note that PATRAN will accept either commas or blanks as separators between coordinates)
Click Apply
A point will appear in the main viewport at coordinates [0,0,0]
Use this same procedure to create points at coordinates [1,0,0], [1,0.1,0] and [0,0.1,0]
Back at the top of the RM called Geometry
Set Action = Create
        Object = Curve
        Method = Point Set the Curve ID list to 1
Turn Autoexecute off
Set Starting Point List = Point 1
Set Ending Point List = Point 2
Click Apply
Back at the top of the RM called Geometry
Set Action = Create
        Object = Curve
        Method = Point
Set the Curve ID list to 2
Turn Autoexecute off
Set Starting Point List = Point 3 Set Ending Point List = Point 4
Click Apply
Back at the top of the RM called Geometry
Set Action = Create         Object = Surface
        Method = Curve
Set the Surface ID list to 1
Set Patran 2 Convention off Option = 2 Curve
Set Manifold off (not checked)
Set Starting Curve List = Curve 1 Set Ending Curve List = Curve 2
Click Apply
2. The finite element mesh is specified next:
From the TM choose Elements
A RM appears called Elements
Set Action = Create         Object = Mesh
        Type = Surface
Set Node Id = 1
Set Element Id List = 1 Set Global Edge Length = 0.025
Set Element Topology = Quad4
Set Mesher = Isomesh
Click in the Surface List box
Click and drag to select the entire structure
The Words "Surface 1" should appear in the Surface List Click Apply

Set Action = Equivalence
        Object = All
        Type = Tolerance Cube
(The purpose here is to tie the nodes together that lie on top of one another)
Set the Equivalencing Tolerance to .003
Click Apply (The command window at the bottom of the PATRAN desktop will tell you that 0 nodes were deleted. This step will become critical if, in more complicated models, you are attempting to join portions of a model which have been meshed separately.)

3. The boundary conditions are specified next:
From the TM choose Load/BC's A RM called Load/Boundary Conditions will appear
Set Action = Create
        Object = Displacement
        Type = Nodal
Set Current Load Case = Default Enter New Set Name as l_cant ( The name can be whatever name you wish. The name l_cant is chosen as this is for the cantilever of the left most nodes)
Click Input Data... a SM called Input Data appears
Set Load/BC Scale factor = 1
Set Translations to <0,0,0> Set Rotations to <0,0,0> Be sure Analysis Coordinate Frame is Coord0
Click OK
(back in the Load/Boundary Conditions RM)
Click Select Application Region A SM called Select Application Region appears
Turn on the FEM (button down)
Click in box under Select Nodes
Use the cursor to highlight the set of nodes along the left vertical edge of the beam. There should be 5 nodes there.
Click OK
(The Load / Boundary Condition RM appears again)
Click Apply

(3 displacement constraint arrows and 3 rotation constraint arrows should now appear on each node in the main viewport window on the extreme left edge of the beam. Numbers 1,2,3,4,5,6 will appear with the arrows to show that all 6 of the dof are constrained there)

4. The materials are specified next:
On the TM select Materials a RM will appear called Materials
Set Action = Create
        Object = Isotropic
        Method = Manual Input
Click Material Name box
Input the name to be aluminum Click Input Properties box
SM called Input Options appears
Input Elastic Modulus =70.0E9 Input Poisson = 0.3
Input the Density to be 2700
Click OK Back in the Materials RM
Click Apply
5. The properties for each element are assigned next: On the TM select Properties
a RM will appear called Element Properties
Set Action = Create         Dimension = 2d
        Type = Shell
Click Property Set Name box
Enter beam_prop
Click Input Properties
a SM appears called Input Properties
Click in the Material Name box
Click on the word "aluminum" in the Material Property Sets box at the bottom of the SM
( the words m:aluminum will appear in the Material Name box at the top of the SM)
Click in the Thickness box
Enter 0.01
Click OK
(Back in the Element Properties RM)
Click Select Members box
a Patran Select menu will appear on the left edge of the RM
Click on the icon which contains the surface or face icon

Move the cursor arrow to a point to the left and above the highest, leftmost point on the beam. Click and hold down the left mouse button. Drag the cursor (while holding down the mouse button) to a point to the right of and below the right-most bottom node. A "selection box" is formed while you drag. Release the button.

(The words Surface 1 will appear in the Select Members box)
Click Add
(The words Surface 1 appears in the Application Region box)
Click Apply in the Element Properties menu
(beam_prop will be added to the Existing Property Sets box)
6. The analysis is to be done is specified next:
On the TM select Analysis
a RM will appear called Analysis Set Action = Analyze
        Object = Entire Model
        Method = Full Run
Click Translation Parameters
In the SM that appears, set Data Output = Op2 and Print Click OK Back in the RM Analysis Set Solution Type = Normal Modes (button down)
Click OK
Click Apply (The analysis will take a few seconds to run. A SM indicating that MSC/Nastran is working may appear)

7. A graphical representation of the mode shapes can be produced. A graphical representation of the mode shapes provides an easy way to begin to determine if you have constructed your model correctly.
On the TM select Analysis
Set Action = Read Output2
        Object = Results Entities
        Method = Translate
Click Select Results File
A SM appears called Select File Click the file beam-vib.op2
(You may need to look in your home or root directory to find the file. If this file does not exist, then you have made a mistake in constructing your model. Go to Explorer (right-click on Start and choose Explore) and find the file beam- vib.log and beam.f06. Open these files by double clicking on them and search for the word “error” to determine what your mistake is).
Beam-vib.op2 then appears in the File Name box
Click OK (back in the Analysis menu)
Click Apply

On the TM select Results
A RM will appear called Results Set Action = Create
        Object = Quick Plot
In the Select Result Case box click Default, Mode 1…
In the Select Fringe Result box click Eigenvectors, translational
In the Apply Fringe Result box click Eigenvectors, translational Set Quantity = Magnitude
Turn on the animation button (so it displays a check)
Click Apply (This will create the animation of the first mode)

Investigate other, higher order mode shapes. Be sure to record data and screen captures needed to answer the questions below.

8. Next you will end your MSC/PATRAN session by saving your database and exiting.
On the TM select File
From the pull down menu select Save
On the TM select File From the pull down menu select Quit
next THERMAL ANALYSIS OF A COOLING FIN USING SHELL ELEMENTS

MODELING A STABELIZATION FIXTURE WITH END PRESSURE USING SOLID ELEMENTS

previous MODELING A FRAME STRUCTURE (WEIGHT BENCH) USING BEAM ELEMENTS

MSC/PATRAN TUTORIAL # 5
MODELING A STABELIZATION FIXTURE WITH END PRESSURE USING SOLID ELEMENTS

I. THE PHYSICAL PROBLEM
The structure below is designed to support a bearing on its right, curved edge. A similar part exists to hold the bearing on the other side. The left edge is cantilevered or "built in". This means that both the translations and the rotations are held to zero along this edge. A pressure load of magnitude 100 lb/in2 in the negative X direction results from the bearing reaction. The material properties for the beam are E= 10 x 106 psi (typical for aluminum) and n = 0.3 . The part has a solid cross section with thickness in the Zdirection t = 3 in.

II. THINKING ABOUT THE MECHANICS
The analytic solution for stresses and displacements for this problem is not readily available. However, any Mechanics of Materials text will provide equations for the max stress and the max displacement of simple problems that will provide upper or lower bounds for stresses and displacements. These analytic verifications will be discussed below.

Some basic questions to consider before creating the computational model are:

1. Where will the stresses be tensile and where will they be compressive?
2. What will be the magnitude and direction of the reaction forces/moments?
3. Where will the stresses be zero?
4. How do the displacements vary along the length (linear, quadratic etc.)?
5. What will the local effect of the pressure load be on the stresses?
6. Is the model fully constrained from rigid body rotations and displacements?

Answering these questions qualitatively, along with the quantitative analytical solutions for the max stress and displacement will provide reinforcement that your computational model is correctly constructed.

III. CREATING THE GEOMETRIC AND FINITE ELEMENT MODEL
1. Create the Geometry
Create the 3-d object below according to the following steps:
Create the points shown with coordinates as in the table

Next create curves between points 1 and 2, 3 and another curve between 4, 6 and another curve between 7, 8 and 9, 2 and another curve between 8, 3 and 7.

Create the curve between points 2 and 3 and between points 7and 8 using the 2-d arc 2point using a radius of 1.
Create the arc between points 4, 5 and 6 using the 2d arc3point option.
Now create 3 surfaces. The instructions will use the curve numbers in the picture below.
Please substitute the curve numbers form the curves you created.

Create the first surface between the curves 1,2,5 and 10 using the Create/Surface/Edge command.
Create the 2nd surface between the curves 7, 10, 6 and 9 and the 3rd surface between the curves 3, 9, 4, and 8.

Now create solids of thickness 3 (in the Z direction) from each of the 3 surfaces using the Create/Solid/Extrude command. The translation vector will need to be <0,0,3>.

When you are done, the part will look like this.

2. Create the Finite Element Mesh The first task is to seed the mesh. This is critical in this model as the model contains 3 separate solids which will need to be meshes separately. Then the nodes will need to be equivalenced so that the 3 solids are “attached” computationally. If this equivalencing is to work correctly, nodes along the interface between 2 solids will need to be coincident. The mesh seed will ensure this. Using the Create/Mesh Seed/Uniform option in the Element menu, create mesh seeds as shown below. Note that is your mesh seeds are a little different than the ones shown below, it will simply mean that you end up with a slightly different number and placement of elements. This should NOT affect the results of your analysis substantially except in one case. The distribution of elements in the Y direction must be constant across the part. For example if you have 6 elements across the far left edge, then you need to have 6 elements across the right curved edge and across other X=constant planes in the part. The reason this is important is that if the element pattern is not symmetric in the in the Y direction, the part will experience a nonsymmetric distribution of loads in the Y direction, resulting in non-physical displacements in the Y direction and also resulting in non-physical bending stresses.

Next place the actual mesh on the solids using the Create/Mesh/Solid. If the mesh seeds are done as shown, it will not matter what the global edge length is. Use the Hex8 elements. Use the isomesh mesh generator.

Next equivalence the nodes using the Equivalence/All/Tolerance cube command. The defaults tolerance is fine. This should indicate approximately 64 nodes were deleted. The graphics will show these nodes along the interface between the 3 solids.

The completed mesh should look approximately as shown below.

3. Create the BC and Loads
To clamp the left edge (edge away from the rounded bearing surface) use the Create/Displacement/Nodal command in the Loads/BC menu. Set all 3 displacements and all 3 rotations to zero and select apply to the left edge.

Next create the pressure load on the bearing surface by using the Create/Pressure/element Uniform command. Make sure the element target type is 3d. Choose a pressure of 100. To select the application surface (in the Select Application Surface) turn on the geometry button and then select the icon for “Face of a Solid” and choose the curved surface shown highlighted below. The BC and loads graphics will appear as shown.

The BC on the left and the pressure load on the right might look different on your part depending on whether you have applied the BC or pressure to the geometry.

4. Create the Material and Property
The material for the part is aluminum which has a E of 10e6 psi and a Poisson’s ratio of 0.3. Using the Materials menu create an isotropic homogeneous material with these properties.

The properties set is made using the command Create/3D/Solid in the properties menu. Input the properties simply as the material you just created. Select the entire part to have these properties.

5. Do the Analysis In the analysis menu, use the command Analyze/Entire Model/Full Run . Set the Translation Parameters to output the *.op2 file. Read in the analysis results Using the command Read Output2/Result Entities/ Translate. Select the appropriate results (*.op2) file.

6. View the Results
In the results menu, use the command Create/Quick Plot. Make plots of the displacements ad the appropriate stresses.

next MODELING A CANTILEVERED BEAM’S VIBRATION USING 4 NODE SHELL ELEMENTS

MODELING A FRAME STRUCTURE (WEIGHT BENCH) USING BEAM ELEMENTS

previous MODELING A CANTILEVERED BEAM WITH END LOAD USING 4 NODE SHELL ELEMENTS

MSC/PATRAN TUTORIAL# 4
MODELING A FRAME STRUCTURE (WEIGHT BENCH) USING BEAM ELEMENTS

I. THE PHYSICAL PROBLEM
The frame structure (weight lifting bench) below has the 4 legs that are attached to the floor. The weight of a user is assumed to be distributed across the rectangular box which sits in the horizontal plane. The weight of this user and accompanying weights is accounted for by a 8 lb per inch load distributed across the 108 inches of the horizontal rectangle. The weight on the uprights is assumed to be 500 lb max on each upright. This accounts for some impact load as well as the static force of a fully loaded bar. In addition to the vertical force, there is a 100 lb per upright force in the horizontal direction. This is intended to model the physics of someone pushing the bar horizontally (in the Y direction) against the cradle supports as they remove the bar to begin the bench press exercise.

II. THINKING ABOUT THE MECHANICS The analytic solution for stresses and displacements for this problem is readily available if we think about the problem in sections. Any Mechanics of Materials text will provide equations for the stress and the displacements for built in and simply supported beams as well as axial loads. These results can be used to give basic analytic comparison solutions for certain sections of the structure.

III. GEOMETRIC AND FINITE ELEMENT MODEL
As is the standard procedure for building MSC/Patran models, we will build the geometry first and then construct a finite element mesh on that geometry. The geometry will proceed from creation of points to curves for this simple model. Next, we will use 2 node beam elements to model the frame. Next, the material and element properties will be entered. We will constrain the 3 displacement and 3 rotational degrees of freedom on the 4 legs. This creates the cantilevered or built-in, end conditions for these sections of the frame. Then we will place a point load of magnitude 500 in the –Y direction on the top nodes of each of the uprights (where the weight bar would rest). A 100 lb load in the horizontal direction is also placed at that same node. A vertical load of 8 lb per inch is placed on the horizontal bench section (rectangle in the XY plane). Finally, the nodes must be equivalenced before the analysis is ready to run.

As can be seen in the step by step instructions below, Patran has a library of beam cross sections that can be used for frame analysis. These properties include various cross sections and wall thickness. One particular feature of note is the manner in which the orientation of the cross section is specified. The menu that allows you to pick the properties of the beam cross section requires a value for “Beam Orientation” . This value determines how the cross section will oriented. In particular, imagine that the graphic of the cross section (which is shown on the library menu) has a local coordinate system with X_L being the horizontal and Y_L being the vertical coordinates respectively (see figure below). Obviously, this means that Z_L is the coordinate down the long axis of the beam. If we label the “Beam Orientation” vector {bo}, then the following relationship can be used to specify our values for the components of {bo}.

{bo} X {Z_L} = {X_L}.

An Example is shown below:

Consider the following cross section and the orientation of the cross section on the 2 beams in the picture.

For the section of the beam that has its long axis down the global X axis, the Beam Orientation vector {bo} is set to {0,1,0} This results in the orientation of the cross section as shown because

{bo} X {Z_L} = {X_L} à {0,1,0} X {1,0,0} = {0,0,1}. So the choice of {bo} = {0,1,0} results in the global Z axis (i.e. {0,0,1}) being the local X-axis as seen in the graphic of the cross section. Note that this same choice for {bo} will result in the orientation for the section of the beam that has its long axis in the {1,1,0} direction above. This is because, for that case {bo} X {Z_L} = {X_L}. = {0,1,0} X {1,1,0} = {0,0,1}.

This procedure is used below, in the step-by-step procedure, to determine the choice of {bo} in the beam library menu.

IV. FINITE ELEMENT THEORY
The exact details of the formulation of the 2 node beam elements in MSC/Nastran is rather complicated. However, the basic formulation of an isoparametric 2 node beam element is not extremely difficult and will provide us with sufficient background information to begin to understand the general application areas and “h” convergence of these elements. This basic formulation for the 2 node isoparametric beam can be found in the almost any Finite Elements text (see for example Finite Elements for Stress Analysis, R.D. Cook, John Wiley & Sons, 1995) .

V. STEP BY STEP INSTRUCTIONS FOR MODELING THE FRAME USING MSC/PATRAN & MSC/NASTRAN
Preliminaries for using PATRAN include:
a) Log on to the computer
b) Click START (lower left corner of the Windows Desktop), go to Programs, Select MSC (common), Select MSC Patran9.0.

The instructions below give details for modeling the beam problem discussed above. The instructions are NOT as detailed as I have given in other problems as I expect that you have begun to get a feel for how to do certain tasks in Patran.

In the instructions below, the following abbreviations and terms will be used: TM = Top Menu. This refers to the horizontal menu options residing at the top of the screen after PATRAN has been initiated.

RM = Right Menu. This refers to the menus that pop up after an option has been chosen from the top menu. These menus reside on the far right side of the PATRAN desktop.

SM = Subordinate Menu. This referees to the menus that pop up from options selected in the right menu.

Click = Unless otherwise stated, this indicates a click with the left mouse button.

Boldface will indicate text that occurs in the PATRAN menus.

Italics text will indicate text that you must enter into text boxes in the PATRAN menus or text that you choose in a menu scroll box.
1. Our first step is to create a new database:
From the TM choose File In the resulting pull down menu choose New A SM called New Database pops up
Turn on (checked) Modify Preferences Under File Name enter bench.db
Click OK
2. Next set the analysis preference:
A New Model Preferences window will appear as a RM
Under Tolerance choose Based on Model
Set Model Dimension to 40.0
Under Analysis Code choose MSC/NASTRAN
Choose Analysis Type = Structural click OK
3. The geometry of the beam will be determined next:
From the TM choose Geometry A RM called Geometry will result
Set Action = Create         Object = Point
        Method = XYZ Set the Point ID list to 1
Set Reference Coordinate Frame to Coord 0
Turn off the Auto Execute button
Enter the following into the Point Coordinates list:
[2,0,0] (note that PATRAN will accept either commas or blanks as separators between coordinates)
Click Apply A point will appear in the main viewport at coordinates [2,0,0]
Using the same approach, create each of the other points in this table

Back at the top of the RM called Geometry
Set Action = Create
        Object = Curve
        Method = Point
Set the Curve ID list to 1
Turn Autoexecute off
Set Starting Point List = Point 1
Set Ending Point List = Point 3
Click Apply
Using the same approach, create each of the other curves in this table

4. The boundary conditions are specified next:
From the TM choose Load/BC's A RM called Load/Boundary Conditions will appear
Set Action = Create
        Object = Displacement
        Type = Nodal
Set Current Load Case = Default Enter New Set Name as cant
( The name can be whatever name you wish. The name cant is chosen as this is for the cantilever of the leg ends which contact the floor)
Click Input Data... a SM called Input Data appears
Set Load/BC Scale factor =1
Set Translations to <0,0,0>
Set Rotations to <0,0,0>
Be sure Analysis Coordinate Frame is Coord0
Click OK
(back in the Load/Boundary Conditions RM)
Click Select Application Region
A SM called Select Application Region appears
Turn on the Geometry (button down)
Click in box under Select Geometric Entities
A Selection Choices SM appears
Choose points 1,2,5,6
Click on Add just below this box
Click OK
(The Load / Boundary Condition RM appears again)
Click Apply

(3 displacement constraint arrows and 3 rotation constraint arrows should now appear on each point in the main viewport window on the extreme lower edge of the bench’s legs. Numbers 1,2,3,4,5,6 will appear with the arrows to show that all 6 of the dof are constrained there)

5. The finite element mesh is specified next:
From the TM choose Elements
A RM appears called Elements
Set Action = Create         Object = Mesh Seed
        Type = Uniform
Choose the Number of Elements option
Set the number of elements to 4
We want each of the 12 curves to have 4 elements. To ensure this, in the Curve List Box enter Curve 1:12
Click APPLY
A set of mesh seeds will appear to show the density of nodes.
Back at the top of the RM called Elements
Set Action = Create
        Object = Mesh
        Type = Curve
Set Node Id = 1
Set Element Id List = 1 Set Global Edge Length = 1.0
Set Element Topology = Bar 2
Click in the Curve List box
Click and drag to select the entire structure
Click Apply
Four elements will appear on each of the curves in the structure.

Back at the top of the RM called Elements
Set Action = Equivalence
        Object = All
        Type = Tolerance Cube
(The purpose here is to tie the nodes together that lie on top of one another)
Set the Equivalencing Tolerance to .02
Click Apply
(The command window at the bottom of the PATRAN desktop will tell you that some nodes were deleted. This step is CRITICAL as it “attaches” the nodes together at the frame junctions)

6. The materials are specified next: On the TM select Materials
a RM will appear called Materials
Set Action = Create
        Object = Isotropic
        Method = Manual Input
Click Material Name box
Input the name to be beam_matl Click Input Properties box
SM called Input Options appears
Input Elastic Modulus 30.0E6
Input Poisson = 0.3
Click OK
Back in the Materials RM
Click Apply

7. The properties for each element are assigned next:
On the TM select Properties a RM will appear called Element Properties Set Action = Create
        Dimension = 1d         Type = Beam Click Property Set Name box
Enter square_prop We will now create the cross sectional properties for the parts of the bench that have square cross sections. These parts are the 4 legs and the 2 uprights(which would hold the actual weight bar)
Click Input Properties
a SM appears called Input Properties Click in the Material Name box
Click on the word "beam_matl" in the Material Property Sets box at the bottom of the SM
( the words m:beam_matl will appear in the Material Name box at the top of the SM)
Just to the right of the Section Name box, set the option to Dimensions
Click in the Section name box and input square_sect Just to the right of the Bar Orientation box, set the option to Vector
Click in the Bar Orientation box and enter the vector <1,0,0>
Click on the ICLBeam Library button

A SM appears called Beam Library
Set Action = Create
        Dimension = Standard Shape         Type = Nastran Standard
Set the New Section Name to Square1
Scroll through the various possible cross sections using the < and > buttons (under the 3x3 set of cross section pictures) until you find the hollow rectangular picture with constant wall thickness (on the lowest row). Click this graphic.
In the upper right part of the window:
Set W = 1.0
Set H = 1.0
Set t1 = .125
Set t2 = .125 If you want to see the information on the cross sectional properties (which will come in handy when doing the analytical comparison calculation later) click on the Calculate/Display button.
Click Apply Click OK (if a menu asks if you wish to over write say YES)
Click Cancel
Back in the Input Properties Menu, click OK Back in the Properties RM
Click in the Select Members box
Choose the 4 legs and the 2 uprights (this is 6 curves and all the vertical members)
Click Add
Click Apply

Now we’ll create the properties for the horizontal members. These members will have a 2 in x 1 in hollow cross section with .125 wall thickness. In this case it is critical that the large dimension of the cross section be oriented to provide the max bending moment of inertia “I” , so the larger (2 in) dimension must be the vertical dimension of the cross section.

Back in the RM called Element Properties Set Action = Create
        Dimension = 1d
        Type = Beam Click Property Set Name box
Enter rectY_prop
We will now create the cross sectional properties for the parts of the bench that have rectangular cross sections and run in the Y direction
Click Input Properties
a SM appears called Input Properties

Click in the Material Name box
Click on the word "beam_matl" in the Material Property Sets box at the bottom of the SM
( the words m:beam_matl will appear in the Material Name box at the top of the SM)
Just to the right of the Section Name box, set the option to Dimensions
Click in the Section name box and input rectY_sect
Just to the right of the Bar Orientation box, set the option to Vector Click in the Bar Orientation box and enter the vector <1,0,0>
Click on the ICLBeam Library button
A SM appears called Beam Library
Set Action = Create
        Dimension = Standard Shape
        Type = Nastran Standard
Set the New Section Name to RectY Scroll through the various possible cross sections using the < and > buttons (under the 3x3 set of cross section pictures) until you find the hollow rectangular picture with constant wall thickness (on the lowest row). Click this graphic
Set W = 2.0
Set H = 1.0
Set t1 = .125
Set t2 = .125
If you want to see the information on the cross sectional properties (which will come in handy when doing the analytical comparison calculation later) click on the Calculate/Display button.
Click Apply
Click OK (if a menu asks if you wish to over write say YES)
Click Cancel
Back in the Input Properties Menu, click OK
Back in the Properties RM
Click in the Select Members box
Choose the 2 horizontal members that have their long axis in the Y direction (curves 3 & 12)
Click Add Click Apply
Back in the RM called Element Properties
Set Action = Create
        Dimension = 1d         Type = Beam
Click Property Set Name box
Enter rectX_prop
We will now create the cross sectional properties for the parts of the bench that have rectangular cross sections and run in the X direction
Click Input Properties
a SM appears called Input Properties
Click in the Material Name box
Click on the word "beam_matl" in the Material Property Sets box at the bottom of the SM
(the words m:beam_matl will appear in the Material Name box at the top of the SM)
Just to the right of the Section Name box, set the option to Dimensions Click in the Section name box and input rectX_sect Just to the right of the Bar Orientation box, set the option to Vector
Click in the Bar Orientation box and enter the vector <0,1,0>
Click on the ICLBeam Library button
A SM appears called Beam Library
Dimension = Standard Shape
Type = Nastran Standard Set the New Section Name to RectX
Scroll through the various possible cross sections using the < and > buttons (under the 3x3 set of cross section pictures) until you find the hollow rectangular picture with constant wall thickness (on the lowest row). Click this graphic
Set W = 2.0
Set H = 1.0
Set t1 = .125
Set t2 = .125
If you want to see the information on the cross sectional properties (which will come in handy when doing the analytical comparison calculation later) click on the Calculate button.
Click Apply
Click OK ( if you are asked to overwrite, say YES)
Click Cancel
Back in the Input Properties Menu, click OK
Back in the Properties RM
Click in the Select Members box
Choose the 4 horizontal members that have their long axis in the X direction (curves 4,7,8,9)
Note that there are 4 members that have their long axis aligned with the X axis; not just 2. These 4 include 2 curves that attach the uprights to the rectangular horizontal supports.
Click Add
Click Apply

In order to see if the cross sections are correctly aligned, go to the TM = Display, then select Load/BC/Elem Props… in the RM that appears, Under Beam Display, change the default 1-D Line to 3-D Full Span and hit Apply (at the bottom of the SM ). This will turn on display of the cross sections. If you wish to see the cross sections shaded, you can use the TM shading icon (solid shaded box, just to the right of the little wire frame icons)

8. The loads are specified next:
Click the TM = Loads/BC The RM Loads/BC pops up. Set
Action = Create Object = Force
Type = Nodal
Change the New Set Name to weights
Click Input Data... a SM appears
Enter the force vector <0, 100 , -500 >
Leave the moments < > (i.e. blank)
Click OK
(Continuing on in the Load/BC's RM)
Click Select Application Region
a small Patran select menu appears close to the RM
Click in this Patran select menu on the point icon In the main viewport, click on the points 7 & 8 (top of the uprights on the bench)
Add these points to the application region
Click OK (Load/BC's menu now reappears)
Click Apply
(A vector with the 510 unit downward and backward load should appear on points 7 & 8 in the main viewport)

Back in the main RM Loads/BC
Action = Create
Object = Distributed Load
Type = Element Uniform
Set NewSet Name = d-load
Set Target Element Type = 1-d
Click Input Data
In the resulting SM
Set the forces to <0,0,8>
Leave the moments blank
Click OK
Back in the Loads/BC RM
Click Select Application Region
In the resulting RM
Turn on FEM as the Geometry filter
Select all the elements along the curves 3,4,8,12 (these are the 4 beams in the XY plane that form the rectangle)
Click Add Click OK
Back in the RM click Apply
Note: if the forces that appear on the main view screen are not in the correct direction, then you probably flipped one of the curve beginning/ending points. The easiest way to fix this is to remove the distributed load from those elements where it is in the wrong directions and create a second distributed force set that has the values <0,0,-8> and apply it to these elements.

9. The analysis is to be done is specified next:
On the TM select Analysis a RM will appear called Analysis
Set Action = Analyze         Object = Entire Model
        Method = Full Run
Click Translation Parameters
In the SM that appears, set Data Output = Op2 and Print
Click OK
Back in the RM Analysis
Set Solution Type = Linear Static (button down)
Click OK Click Apply (The analysis will take a few seconds to run. A SM indicating that MSC/Nastran is working may appear)

10. A graphical representation of the deformation can be produced.
A graphical representation of the deformation provides an easy way to help determine if you have constructed your model correctly.
On the TM select Analysis Set Action = Read Output2
        Object = Results Entities
        Method = Translate
Click Select Results File
A SM appears called Select File
Click the file bench.op2
(You may need to look in your home or root directory to find the file. If this file does not exist, then you have made a mistake in constructing your model. Go to Explorer (right-click on Start and choose Explore) and find the file bench.log and bench.f06. Open these files by double clicking on them and search for the word “error” or “fatal” to determine what your mistake is).
beam.op2 then appears in the File Name box
Click OK
(back in the Analysis menu)
Click Apply

Select the TM Results
A RM will appear called Results
Set Action = Create         Object = Quick Plot
In the Select Fringe Result box click Displacements, translational
In the Apply Displacement Result box click Displacements, translational
Set Quantity = magnitude
Click Apply (This will create the deformed plot)
Note that stresses can also be plotted from the Results menu by specifying them in the Select Fringe Result section. You will want to use the VonMises stresses in this case as the X, Y or Z based stresses are, by default, in the local coordinate system for that beam and are not in the global (Coord 0) frame.

11. Next you will end your MSC/PATRAN session by saving your database and exiting.
On the TM select File
From the pull down menu select Save
On the TM select File From the pull down menu select Quit
next MODELING A STABELIZATION FIXTURE WITH END PRESSURE USING SOLID ELEMENTS

MODELING A CANTILEVERED BEAM WITH END LOAD USING 4 NODE SHELL ELEMENTS

previous Modeling of a Truss

MSC/PATRAN TUTORIAL # 3
MODELING A CANTILEVERED BEAM WITH END LOAD USING 4 NODE SHELL ELEMENTS

I. THE PHYSICAL PROBLEM
The beam below is cantilevered or "built in" on the left edge. This means that both the translations and the rotations are held to zero along this edge. A point or concentrated load of magnitude 1000 N (approximately 225 lb) in the negative Y direction is found at the tip of the beam. This problem is part of a standard set of test cases for finite elements published in a paper by MacNeal and Harder (MacNeal founded the company that makes the FEA code MSC/NASTRAN and MSC/PATRAN). The set of problems is called "The MacNeal - Harder Test Cases". The material properties for the beam are E= 200 x 10⁹ Pascals (typical for steel) and ν = 0.0 (as the analytic beam theory we use below does not take Poison’s ration effects into account). The beam has a solid rectangular cross section with thickness in the Z-direction t = 0.1 meters and height in the Y-direction h = 0.2 meters.

II. THINKING ABOUT THE MECHANICS
The analytic solution for stresses and displacements for this problem is readily available. Any Mechanics of Materials text will provide equations for the max stress (located at the built in edge and on either the top fiber for max tensile stress or the bottom fiber for max compressive stress) and the max displacement (located, of course, at the free tip where the load is applied). These equations are given below.
For the normal stress due to bending:

Some basic questions to consider before creating the computational model are:

1. Where will the stresses be tensile and where will they be compressive?
2. What will be the magnitude and direction of the reaction forces/moments?
3. Where will the stresses be zero?
4. How do the displacements vary along the length (linear, quadratic etc.)?
5. What will the local effect of the concentrated load be on the stresses?
6. Is the model fully constrained from rigid body rotations and displacements?

Answering these questions qualitatively, along with the quantitative analytical solutions for the max stress and displacement will provide reinforcement that your computational model is correctly constructed.

III. GEOMETRIC AND FINITE ELEMENT MODEL As is the standard procedure for building MSC/Patran models, we will build the geometry first and then construct a finite element mesh on that geometry. The geometry will proceed from creation of points to lines to surfaces for this simple model. Next, we will use 4 node shell elements deforming in their membrane mode to model the beam. In this exercise, we will vary the exact number and configuration of these elements. This is discussed in detail in the next paragraph. Next, the material and element properties will be entered. We will constrain the 3 displacement and 3 rotational degrees of freedom on the left edge (for both nodes). This creates the cantilevered or built-in, end condition. Then we will, place a point load of magnitude 1000 on the top right node of the tip (or right-most) element. This load will be in the negative Y direction. Finally, the nodes must be equivalenced before the analysis is ready to run.

Below, we show 5 mesh configurations for the beam (labeled “a” through “e”). Comparison of results between mesh “a” and mesh “b” will indicate of how the number of elements affects the model’s ability to correctly model a beam problem. Increasing the number of elements in a mesh in order to increase the accuracy of the results is called “h” convergence. Meshes “b” – “e” all have 6 elements; but the elements have different orientations. Elements that have non-regular shapes are said to be distorted. Distorted elements can cause errors in the FEA results. This can be a significant problem in complex meshes as even the best automatic mesh generators often produce some distorted elements. The elements in MSC/Nastran have been specifically designed to minimize this unfortunate effect, but some sensitivity to element distortion may still remain. Different types of element distortion result in different levels of error. Evaluating results from the meshes “b” - “e” will provide you with some feel for how these elements perform when they are distorted.

Meshes for the “h” Convergence & Distortion Analysis

a) Rectangular 2 Element Mesh:

b) Rectangular 6 Element Mesh:

c) 10 Degree Parallelogram Mesh:

d) 45 Degree Parallelogram Mesh:

e) 45 Degree Trapezoid Mesh:

IV. FINITE ELEMENT THEORY
The exact details of the formulation of the 4 node shell elements in MSC/Nastran is rather complicated. However, the basic formulation of an isoparametric 4 node membrane element is not extremely difficult and will provide us with sufficient background information to begin to understand the “h” convergence and distortion sensitivity studies. This basic form is constructed as follows:

Isoparametric Formulation of a 2-D Membrane Element [K] Matrix Assume the element has the configuration shown below:

The physical and natural coordinate locations of the 4 nodes are:

Our goal is to find the element stiffness matrix

ASSUME: 2 displacement degrees of freedom (dof) per node
With : [B] = the strain - displacement matrix such that [B]{u} = {ε}
where: {u} is the dof vector and {ε} is the strain vector [E] = the constitutive matrix such that [E]{ε} = {σ}
where {σ} is the stress vector and V = volume.

and the rules for the shape functions are :
1) N_i must be =1 at node "i"
2) N_i must be =0 at any node not = "i"

Step 2: Find the [B] matrix:

So {ε} » [D][N]{u} = [B]{u} with [B] = [D][N]
Therefore,

the commas denote partial differentiation.

Step 3: Use the Jacobian to find derivatives:

i.e. the isoparametric assumption is that geometry can be interpolated using the same interpolation functions as the displacements.

This allows us to find the entries in [B]

Step 4: Perform the numerical integration:
Assume that the element has constant thickness = t implies
 

Which, according to the rules of calculus can be written:

where |J| is the determinant of the Jacobian matrix.

Gaussian numerical integration is then used to find the final numbers for the element stiffness.

Where ng_j and ng_i are the number of gaussian integration points in the “j” and “i” directions respectively and w_j and w_i are the associated gaussian weighting factors.

Understanding the “h” Convergence Experiment:

From step 1 above we gain insight into the “h” convergence study. Remember that the that the analytic formula for the displacements as a function X (distance from built-in edge) is:

where P is the load, L is the length, E is the Elastic Modulus and I is the bending moment in inertia. This equation shows that the displacement is a cubic function of the distance from the cantilever. As the bi-linear (linear in both x and h ) shape functions are used to interpolate the displacements for this 4 node element, the elements are attempting to capture a cubic behavior by using a series of linear approximations. The number of linear approximations is equal to the number of elements we use (the actual situation when using MSC/Nastran’s 4 node shell element is a little better than this due to the innovative element formulation, but this is a good way to conceptually grasp the idea of “h” convergence). This is the reason why 2 elements give a higher error than do 6 elements.

Understanding the Distortion Sensitivity Experiment:
When an element is rectangular, its Jacobian matrix (used in steps 3 and 4 above) is numerically exact. However, if the element becomes distorted, the bi-linear shape functions used to form [J] can no longer exactly capture the geometry and the Jacobian is no longer numerically exact. This introduces error into steps 3 and 4 above. The exact form of the element’s distortion determines the amount of error which is introduced. As mentioned previously, the elements in MSC/Nastran are intricately designed to remove as much of this distortion based error as possible. If the simple standard isoparametric formulation shown above is used, the trapaziodal elements (mesh “e” above) would actually “lock” (become very stiff) and the errors in the displacements would be huge (over 90%). For this reason, it is critical that sophisticated, well-tested finite element codes be used for any critical analysis. Even then, it is wise to inspect meshes for regions where elements are highly distorted and attempt to create a less distorted mesh in that area.

V. STEP BY STEP INSTRUCTIONS FOR MODELING THE CANTILEVERED BEAM USING MSC/PATRAN
Preliminaries for using PATRAN include:
a) Log on to the computer
b) Click START (lower left corner of the Windows Desktop), go to Programs, Select MSC (common), Select MSC Patran9.0.

The instructions below give details for modeling the beam problem discussed above. Specifically, the 6 rectangular elements (mesh “b” above) is constructed. If one wishes to create any of the other meshes, the mesh creation section must be adapted to fit that mesh.

In the instructions below, the following abbreviations and terms will be used:
TM = Top Menu. This refers to the horizontal menu options residing at the top of the screen after PATRAN has been initiated.
RM = Right Menu. This refers to the menus that pop up after an option has been chosen from the top menu. These menus reside on the far right side of the PATRAN desktop.
SM = Subordinate Menu. This referees to the menus that pop up from options selected in the right menu.

Click = Unless otherwise stated, this indicates a click with the left mouse button.

Boldface will indicate text that occurs in the PATRAN menus.

Italics text will indicate text that you must enter into text boxes in the PATRAN menus or text that you choose in a menu scroll box.
1. Our first step is to create a new database:
From the TM choose File In the resulting pull down menu choose New
A SM called New Database pops up
Turn on (checked) Modify Preferences
Under File Name enter beam.db
Click OK
2. Next set the analysis preference: A New Model Preferences window will appear as a RM
Under Tolerance choose Based on Model
Set Model Dimension to 6.0
Under Analysis Code choose MSC/NASTRAN
Choose Analysis Type = Structural
click OK
3. The geometry of the beam will be determined next:
From the TM choose Geometry A RM called Geometry will result
Set Action = Create         Object = Point         Method = XYZ Set the Point ID list to 1
Set Reference Coordinate Frame to Coord 0
Turn off the Auto Execute button
Enter the following into the Point Coordinates list:
[0,0,0] (note that PATRAN will accept either commas or blanks as separators between coordinates)
Click Apply
A point will appear in the main viewport at coordinates [0,0,0]

Back at the top of the RM called Geometry
Set Action = Create
        Object = Point
        Method = XYZ
Set the Point ID list to 2
Set Reference Coordinate Frame to Coord 0
Turn off the Auto Execute button
Enter the following into the Point Coordinates list:
[6,0,0]
(note that PATRAN will accept either commas or blanks as separators between coordinates)
Click Apply
A point will appear in the main viewport at coordinates [6,0,0]

Back at the top of the RM called Geometry Set Action = Create         Object = Point
        Method = XYZ Set the Point ID list to 3
Set Reference Coordinate Frame to Coord 0
Turn off the Auto Execute button
Enter the following into the Point Coordinates list:
[0,0.2,0] (note that PATRAN will accept either commas or blanks as separators between coordinates)
Click Apply A point will appear in the main viewport at coordinates [0,0.2,0]
Back at the top of the RM called Geometry
Set Action = Create
        Object = Point
        Method = XYZ
Set the Point ID list to 4
Set Reference Coordinate Frame to Coord 0
Turn off the Auto Execute button
Enter the following into the Point Coordinates list:
[6,0.2,0]
(note that PATRAN will accept either commas or blanks as separators between coordinates)
Click Apply A point will appear in the main viewport at coordinates [6,0.2,0]
Back at the top of the RM called Geometry Set Action = Create
        Object = Curve
        Method = Point
Set the Curve ID list to 1
Turn Auto execute off
Set Starting Point List = Point 1
Set Ending Point List = Point 2
Click Apply
Back at the top of the RM called Geometry
Set Action = Create         Object = Curve
        Method = Point
Set the Curve ID list to 2
Turn Auto execute off
Set Starting Point List = Point 3 Set Ending Point List = Point 4 Click Apply
Back at the top of the RM called Geometry Set Action = Create
        Object = Surface
        Method = Curve
Set the Surface ID list to 1
Set Patran 2 Convention off
Option = 2 Curve
Set Manifold off (not checked)
Set Starting Curve List = Curve 1 Set Ending Curve List = Curve 2
Click Apply

4. The boundary conditions are specified next: From the TM choose Load/BC's
A RM called Load/Boundary Conditions will appear
Set Action = Create         Object = Displacement         Type = Nodal Set Current Load Case = Default Enter New Set Name as l_cant ( The name can be whatever name you wish. The name l_cant is chosen as this is for the cantilever of the left most nodes)
Click Input Data... a SM called Input Data appears
Set Load/BC Scale factor =1
Set Translations to <0,0,0>
Set Rotations to <0,0,0>
Be sure Analysis Coordinate Frame is Coord0
Click OK
(back in the Load/Boundary Conditions RM)
Click Select Application Region
A SM called Select Application Region appears
Turn on the Geometry (button down)
Click in box under Select Geometric Entities
In the Patran Select Menu (just to the left of the RM)
Click on the curve icon (just under the point icon)
In the main view port, select the left most vertical edge of the beam.
A Selection Choices SM appears
Choose Surface 1.1 ( This will cause the words "Surface 1.1" to appear in the Select Geometric Entities box in the RM)
Click on Add just below this box
( This will remove the words "Surface 1.1 " from the Select Geometric Entities box and adds them to the Application Region box)
Click OK
(The Load / Boundary Condition RM appears again)
Click Apply

(3 displacement constraint arrows and 3 rotation constraint arrows should now appear on each point in the main viewport window on the extreme left edge of the beam. Numbers 1,2,3,4,5,6 will appear with the arrows to show that all 6 of the dof are constrained there)

5. The loads are specified next:
(Continuing on in the Load/BC's RM)
change Action = Create
                Object = Force
                Type = Nodal
Change the New Set Name to r_point
Click Input Data...
a SM appears
Enter the force vector <0 , -1000 , 0>
leave the moments < > (i.e. blank)
Click OK
(Continuing on in the Load/BC's RM)
Click Select Application Region
a small Patran select menu appears to the left edge of the RM
Click in this Patran select menu on the point icon
In the main viewport, click on the point 4 (top right corner of the beam)
A SM called Selection Choices menu appears.
Choose the Point 4 option, not the Curve or Surface option)
(Point 4 will be added to the Select Geometric Entities list)
Click Add (Point 4 will be added to the Application Region list)
Click OK
(Load/BC's menu now reappears)
Click Apply
(A vector with the 1000 unit downward load should appear on point 4 in the main viewport)

6. The finite element mesh is specified next: From the TM choose Elements A RM appears called Elements
Set Action = Create
        Object = Mesh
        Type = Surface
Set Node Id = 1
Set Element Id List = 1
Set Global Edge Length = 1.0 (This will create 6 elements. If you want to create only 2 elements (as is needed to answer question #1 below) then set the Global edge length to 3.0)
Set Element Topology = Quad4
Set Mesher = Isomesh
Click in the Surface List box
Click and drag to select the entire structure
The Words "Surface 1" should appear in the Surface List Click Apply
Six elements will appear on the structure.

Set Action = Equivalence         Object = All
        Type = Tolerance Cube
(The purpose here is to tie the nodes together that lie on top of one another)
Set the Equivalencing Tolerance to .003
Click Apply
(The command window at the bottom of the PATRAN desktop will tell you that 0 nodes were deleted. This step will become critical if, in more complicated models, you are attempting to join portions of a model which have been meshed separately.)

7. The materials are specified next: On the TM select Materials a RM will appear called Materials
Set Action = Create
        Object = Isotropic
        Method = Manual Input
Click Material Name box
Input the name to be beam_matl Click Input Properties box
SM called Input Options appears
Input Elastic Modulus =200.0E9 Input Poisson = 0.0
Click OK
Back in the Materials RM
Click Apply
8. The properties for each element are assigned next:
On the TM select Properties a RM will appear called Element Properties Set Action = Create
        Dimension = 2d
        Type = Shell
Click Property Set Name box
Enter beam_prop Click Input Properties
a SM appears called Input Properties
Click in the Material Name box
Click on the word "beam_matl" in the Material Property Sets box at the bottom of the SM
( the words m:beam_matl will appear in the Material Name box at the top of the SM)
Click in the Thickness box
Enter 0.1
Click OK (Back in the Element Properties RM)
Click Select Members box
a Patran Select menu will appear on the left edge of the RM
Click on the icon which contains the surface or face icon

Move the cursor arrow to a point to the left and above the highest, leftmost point on the beam. Click and hold down the left mouse button. Drag the cursor (while holding down the mouse button) to a point to the right of and below the right-most bottom node. A "selection box" is formed while you drag. Release the button.

(The words Surface 1 will appear in the Select Members box)
Click Add
(The words Surface 1 appears in the Application Region box)
Click Apply in the Element Properties menu
(beam_prop will be added to the Existing Property Sets box)
9. The analysis is to be done is specified next: On the TM select Analysis
a RM will appear called Analysis Set Action = Analyze
        Object = Entire Model         Method = Full Run
Click Translation Parameters
In the SM that appears, set Data Output = Op2 and Print
Click OK
Back in the RM Analysis Set Solution Type = Linear Static (button down)
Click OK
Click Apply
(The analysis will take a few seconds to run. A SM indicating that MSC/Nastran is working may appear)

10. A graphical representation of the deformation can be produced. A graphical representation of the deformation provides an easy way to help determine if you have constructed your model correctly.
On the TM select Analysis
Set Action = Read Output2
        Object = Results Entities
        Method = Translate
Click Select Results File
A SM appears called Select File
Click the file beam.op2 (You may need to look in your home or root directory to find the file. If this file does not exist, then you have made a mistake in constructing your model. Go to Explorer (right-click on Start and choose Explore) and find the file beam.log and beam.f06. Open these files by double clicking on them and search for the word “error” to determine what your mistake is).
beam.op2 then appears in the File Name box
Click OK (back in the Analysis menu)
Click Apply

On the TM select Results A RM will appear called Results Set Action = Create
        Object = Quick Plot
In the Select Fringe Result box click Displacements, translational In the Apply Fringe Result box click Displacements, translational
Set Quantity = Y Component
Click Apply
(This will create the deformed plot)
Note that stresses can also be plotted from the Results menu by specifying them in the Select Fringe Result section.

11. Next you will end your MSC/PATRAN session by saving your database and exiting. On the TM select File From the pull down menu select Save
On the TM select File From the pull down menu select Quit
next MODELING A FRAME STRUCTURE (WEIGHT BENCH) USING BEAM ELEMENTS