MSC/PATRAN TUTORIAL # 1
MODELING A BAR PROBLEM
I. THE PHYSICAL PROBLEM
In the simple bar problem below, there are three separate sections of the bar. Each section has different properties. The following properties apply, Al → Aluminum, St → Steel, E for Steel = 200 E9 Pa, E for Al = 70 E9 Pa All Bars have square cross section and the right and left ends of the bar are built in. The force "F" = 9000 Newtons
In the simple bar problem below, there are three separate sections of the bar. Each section has different properties. The following properties apply, Al → Aluminum, St → Steel, E for Steel = 200 E9 Pa, E for Al = 70 E9 Pa All Bars have square cross section and the right and left ends of the bar are built in. The force "F" = 9000 Newtons
The 2-d model of the problem is shown below.
The analytic solution for stresses and displacements for this problem is readily available. Any Mechanics of Materials text will provide equations for the displacements and stresses throughout the bar. The problem is indeterminant because there are two reactions (one at each wall) and only one relevant equilibrium equation (∑Fx = 0 ).
Therefore, it is necessary to use the Mechanics of materials (stress and or displacement) equations as well as the force equilibrium equations to solve the problem.
The normal stress due to axial loading is given by :
σxx = P/A , where P is the internal force in the axial direction and A is the cross
sectional area of the bar. The displacements are computed from 
here L is the bar’s length and E is the Elastic (Young’s) modulus.
here L is the bar’s length and E is the Elastic (Young’s) modulus.
Some basic questions to consider before creating the computational model are:
- Where will the stresses be tensile and where will they be compressive?
- What will be the magnitude and direction of the reaction forces?
- Where will the displacements be greatest?
- How do the displacements vary along the length (linear, quadratic etc.)?
- What will the local effect of the concentrated load be on the stresses?
- Is the model fully constrained from rigid body rotations and displacements?
Answering these questions qualitatively, along with the quantitative analytical solutions for the stresses and displacements, will provide reinforcement that your computational model is correctly constructed.
III. GEOMETRIC AND FINITE ELEMENT MODEL Some general notes on PATRAN:
A general finite element analysis can be broken down into 3 principle tasks; preprocessing, analysis and post processing. The preprocessing task includes building the geometric model, building the finite element model, giving these elements the correct properties, setting the boundary conditions and loading conditions and finally, assembling these elements into a connected structure for analysis. The analysis stage simply solves for the unknown degrees of freedom, as well as reactions and stresses. In the postprocessing stage, the results are evaluated and displayed. The accuracy of these results is postulated during this postprocessing task.
The Patran and Nastran software together perform all 3 of the principle tasks of a finite element analysis. The pre and post processors are unique to PATRAN itself. However, this package allows the user to do the actual solution analysis on a variety of different packages. At many sites you have the option of using the MSC/Nastran package, which is probably the most widely used solver in industry. Many of the other packages commonly used in industrial settings (ABAQUAS, ANSYS, MARC) are also compatible with PATRAN.
IV. FINITE ELEMENT THEORY
The exact details of the formulation of the rod elements in MSC/Nastran is given in the MSC/Nastran manuals and is somewhat lengthy. However, the basic formulation of an isoparametric 2 node rod element is not difficult and will provide us with sufficient background information to begin to understand the convergence and other accuracy studies. This basic form can be found in any standard text of finite element analysis. For Example see Finite Element Modeling for Stress Analysis, by R.D. Cook, John Wiley & Sons, 1995.
V. STEP BY STEP INSTRUCTIONS FOR MODELING THE BAR PROBLEM USING MSC/PATRAN
Unless you have used the PATRAN software numerous times in the past, the steps shown below should be followed exactly. However, in order to prepare you to do independent finite element work using PATRAN in the future, you are encouraged to go back after you have completed the assignment and investigate modeling options using different PATRAN selections. Also, I encourage you to take notes as you go through this exercise in order to prepare for the time when you will be asked "build a certain geometric structure" or "apply a certain type of boundary condition" with out being given the specific steps for carrying out this task.
The MSC/Patran program is menu driven much in the same way that most Windows programs are driven. Selecting a category from a menu may result in a pull down set of options or in a subordinate menu. Selections in menus may be in the form of buttons to turn on or off, or in the form of boxes which require text. Text entered into boxes may be changed by positioning the cursor at the point of text insertion and either typing the new text or erasing the incorrect text. A standard finite element analysis normally proceeds across the top menus starting with Geometry and ending with Results. Selecting one of these top menus results in a set of menus which allow you to complete that task in the analysis process. Generally, it is best to attempt to proceed from the top of these menus toward the bottom, answering questions as you go.
Preliminaries for using MSC Patran and Nastran normally include: - Log in to the machine.
- Change to the directory that you wish to contain your results.
- To start the program MSC/Patran, click on Start/Programs/MSC(common) and choose MSC Patran 90.
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.
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 off (no check) Modify Preferences
If the new database for has come up showing a directory on a remote computer (as opposed to a directory on the local machine), then switch the directory to the local directory c:\MSC
Under New Database Name enter bar.db
Click OK
The geometry of the structure 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] [.05,0,0] [.10,0,0] [.20,0,0]
(note that PATRAN will accept either commas or blanks as separators between coordinates) Click Apply
(At this point 4 points should appear on your "bar.db - default_viewport - default_group - entity" main viewport)
The next job is to connect these points to form 3 lines:
While still in the Geometry RM,
Set Action = Create While still in the Geometry RM,
Object = Curve
Method = Point
Turn off the Auto Execute button if it is on
(for the following, it is assumed that you have created points 1,2,3,4 numbered from left to right in the main viewport. If the numbers are not in that order, follow the procedure below from left to right regardless of point numbers)
Click in the Starting Point List box Click on node 1 in the main viewport.
Click in the Ending Point List box
Click on the point 2 in the main viewport
Click on Apply
(A line will be drawn from point 1 to point 2. This line should be named line 1)
Click in the Starting Point List box
Click on point 2 in the main viewport.
Click in the Ending Point List box
Click on the point 3 in the main viewport
Click on Apply
(A line will be drawn from point 2 to point 3. This line should be named line 2)
Click in the Starting Point List box
Click on node 3 in the main viewport
Click in the Ending Point List box
Click on the point 4 in the main viewport
Click on Apply
(A line will be drawn from point 3 to point 4. This line should be named line 3)
The finite element mesh is specified next: From the TM choose Elements
A RM appears called Finite Elements
Set Action = Create
Object = Mesh Seed
Type = Uniform
Select Number of Elements (button down)
Number = 1
Turn off the Auto Execute (button up)
Click in Curves List box
Click on the left most curve in the main viewport
(The words "Curve 1" will be added to the Curve List)
Click Apply
(circles which represent finite element nodes will appear on ends of the curve)
Click Curve List box
Click on the center curve in the main viewport
(the words "Curve 2" will be added to the Curve List)
Click Apply
(circles which represent finite element nodes will appear on ends of the curve)
Click Curve List box
Click on right most curve in the main viewport
(the words "Curve 3" will be added to the Curve List)
Click Apply
(circles which represent finite element nodes will appear on ends of the curve)
(The nodes created above must now be tied together with element s)
(up at the top of the RM)
Set Action = Create
Object = Mesh
Type = Curve
Click on Bar2 under Element Topology
Click Curve List Box
Click the left most curve in the main viewport (should be curve 1)
Click Apply
Click Curve List Box
Click the middle curve in the main viewport (should be curve 2)
Click Apply
Click Curve List Box
Click the right most curve in the main viewport (should be curve 3)
Click Apply
(numbers for the nodes will appear over the geometry points)
(up at the top of the RM)
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 .005
Click Apply (at the bottom of the RM)
(The command window at the bottom of the PATRAN desktop will tell you that 2 nodes were deleted. In addition circles will appear over the ends of the middle curve to indicate the equivalencing of the "overlapping" nodes)
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 .005
Click Apply (at the bottom of the RM)
(The command window at the bottom of the PATRAN desktop will tell you that 2 nodes were deleted. In addition circles will appear over the ends of the middle curve to indicate the equivalencing of the "overlapping" nodes)
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
RLClamp
( This is for the right and left clamping of the bar structure)
Click Input Data...
a SM appears
Set Input Translations to <0,0,0>
Be sure Analysis Coordinate Frame is Coord0
Click OK
(back in the Load/Boundary Conditions RM)
Click Select Application Region
Turn on the Geometry (button down)
Click in box under Select Geometric Entities
A Patran item menu appears (just to the left of the RM)
Click on the picture with a point in this menu
In the main view port, click on the left most point on the line
A SM called Selection Choices appears
Choose Point 1
( This will cause the words "Point 1" (assuming point 1 is the leftmost point on the line) to appear in the Select Geometric Entities box in the RM)
Click on Add just below this box
( This will remove the words "Point 1" from the Select Geometric Entities box and add them to the Application Region box)
Click in the Select Geometric Entities box again.
Next Click point 2 in the main view port (assuming point 2 is the right most point in the bar structure)
A SM called Selection Choices appears
Choose Point 2
Click Add (The Application Region box should now have the words
"Point1 2" in it and the Select Geometric Entities box should be empty)
Click OK
(The Load / Boundary Condition RM appears again)
Click Apply
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
RLClamp
( This is for the right and left clamping of the bar structure)
Click Input Data...
a SM appears
Set Input Translations to <0,0,0>
Be sure Analysis Coordinate Frame is Coord0
Click OK
(back in the Load/Boundary Conditions RM)
Click Select Application Region
Turn on the Geometry (button down)
Click in box under Select Geometric Entities
A Patran item menu appears (just to the left of the RM)
Click on the picture with a point in this menu
In the main view port, click on the left most point on the line
A SM called Selection Choices appears
Choose Point 1
( This will cause the words "Point 1" (assuming point 1 is the leftmost point on the line) to appear in the Select Geometric Entities box in the RM)
Click on Add just below this box
( This will remove the words "Point 1" from the Select Geometric Entities box and add them to the Application Region box)
Click in the Select Geometric Entities box again.
Next Click point 2 in the main view port (assuming point 2 is the right most point in the bar structure)
A SM called Selection Choices appears
Choose Point 2
Click Add (The Application Region box should now have the words
"Point1 2" in it and the Select Geometric Entities box should be empty)
Click OK
(The Load / Boundary Condition RM appears again)
Click Apply
(3 displacement constraint arrows should now appear in the main viewport window on the extreme right and on the extreme left points in the bar structure)
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 axial3
Click Input Data...
a SM appears
Enter the force vector <1.8E4,0,0>
leave the moments < > (i.e. blank)
Click OK
(Continuing on in the Load/BC's RM)
Click Select Application Region
a Select Application menu appears as well as a small Patran item menu
In the Select Applications menu, turn on the Geometry Filter
Next, click in the box labeled Select Geometric Entities
Click in the Patran item menu (just to the left of the RM)
on the point icon
In the main viewport, click on the 3rd point from the left (its number (should be Point 4) will be added to the Select Geometric Entities list)
Click Add
(the point’s number will be added to the Application Region list)
Click OK
(Load/BC's menu now reappears)
Click Apply (bottom of the RM)
(A vector with the load should appear on the 3rd point from the left in the main viewport)
The materials are specified next: Click Select Application Region
a Select Application menu appears as well as a small Patran item menu
In the Select Applications menu, turn on the Geometry Filter
Next, click in the box labeled Select Geometric Entities
Click in the Patran item menu (just to the left of the RM)
on the point icon
In the main viewport, click on the 3rd point from the left (its number (should be Point 4) will be added to the Select Geometric Entities list)
Click Add
(the point’s number will be added to the Application Region list)
Click OK
(Load/BC's menu now reappears)
Click Apply (bottom of the RM)
(A vector with the load should appear on the 3rd point from the left in the main viewport)
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 Steel
Click Input Properties
SM called Input Options appears
Input Elastic Modulus = 2.0E11
Input Poisson = 0.3
Click OK
Back in the Materials RM, click Apply
Click Material Name box
Input the name to be Aluminum
Click Input Properties box
SM called Input Options appears
Input Elastic Modulus = 7.0E10
Input Poisson = 0.3
Click OK
Back in the Materials RM, click Apply
(The Existing Materials box should have Steel and Aluminum in it)
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 = rod
Click Property Set Name box
Enter bar1
Click Input Properties
a SM appears called Input Properties
Click in the Material Name box
Click on the word "Steel" in the Materials Property Set box
( the words m:Steel will appear in the Material Name box)
Click in the Area box
Enter 0.0004
Click OK
(note: If you just input the word Steel in the Material Name box, the element will not have the correct properties. The exact syntax m:Steel is necessary) (Back in the Element Properties RM)
Click Select Members box
a Patran item menu will appear to the left of the RM
In the item menu, click in the box which contains the element with end nodes (as opposed to the curve in the left box)
(This allows you to pick finite element entities as opposed to the geometric entities in the other box)
Click on element 1 in the main viewport
(element 1 is the left most element in the bar structure)
(The words Elm 1 will appear in the Select Members box)
Click Add
(The words Element 1 appear in the Application Region box)
Click Apply in the Element Properties menu
(Bar 1 will be added to the Existing Property Sets box)
Change Property Set Name to bar2 a RM will appear called Element Properties
Set Action = Create
Dimension = 1d
Type = rod
Click Property Set Name box
Enter bar1
Click Input Properties
a SM appears called Input Properties
Click in the Material Name box
Click on the word "Steel" in the Materials Property Set box
( the words m:Steel will appear in the Material Name box)
Click in the Area box
Enter 0.0004
Click OK
(note: If you just input the word Steel in the Material Name box, the element will not have the correct properties. The exact syntax m:Steel is necessary) (Back in the Element Properties RM)
Click Select Members box
a Patran item menu will appear to the left of the RM
In the item menu, click in the box which contains the element with end nodes (as opposed to the curve in the left box)
(This allows you to pick finite element entities as opposed to the geometric entities in the other box)
Click on element 1 in the main viewport
(element 1 is the left most element in the bar structure)
(The words Elm 1 will appear in the Select Members box)
Click Add
(The words Element 1 appear in the Application Region box)
Click Apply in the Element Properties menu
(Bar 1 will be added to the Existing Property Sets box)
Click Input Properties...
a SM called Input Properties will appear
Click the Material Name box
Click Aluminum in the Materials Property Sets box
(The words m:Aluminum will appear in the Materials Name box)
Change the Area to 0.0025
Click OK
(Back on the Element Properties Menu)
Click the Select Members box
A Patran item menu appears just to the left of the RM
In this item menu, click in the box which contains the element with end nodes (as opposed to the curve in the other box)
Click on element 2 in the main viewport
(Element 2 is the middle element in the bar structure)
(The words Elm 2 appears in the Select Members box)
Click Add
(The words Element 2 appear in the Application Region box)
( Note: If anything other than Element 2 is in the Application Region box, it must be deleted.)
Click Apply
(The words bar2 will be added to the Existing Properties Sets box)
Change Property Set Name to bar3
Click Input Properties...
a SM called Input Properties will appear
Click the Material Name box
Click Aluminum in the Materials Property Sets box
(The words m:Aluminum will appear in the Materials Name box)
Change the Area to 0.0001
Click OK
Click the Select Members box
A Patran item menu appears just to the left of the RM
In this item menu, click in the right box which contains the element with end nodes (as opposed to the curve in the other box)
Click on element 3 in the main viewport
(Element 3 is the right most element in the bar structure)
(The words Elm 3 appears in the Select Members box)
Click Add
(The words Element 3 appear in the Application Region box)
( Note: If anything other than Element 3 is in the Application Region box, it must be deleted.)
Click Apply
(The words bar3 will be added to the Existing Properties Sets box)
Click Input Properties...
a SM called Input Properties will appear
Click the Material Name box
Click Aluminum in the Materials Property Sets box
(The words m:Aluminum will appear in the Materials Name box)
Change the Area to 0.0001
Click OK
Click the Select Members box
A Patran item menu appears just to the left of the RM
In this item menu, click in the right box which contains the element with end nodes (as opposed to the curve in the other box)
Click on element 3 in the main viewport
(Element 3 is the right most element in the bar structure)
(The words Elm 3 appears in the Select Members box)
Click Add
(The words Element 3 appear in the Application Region box)
( Note: If anything other than Element 3 is in the Application Region box, it must be deleted.)
Click Apply
(The words bar3 will be added to the Existing Properties Sets box)
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 on Translation Parameters
a SM will appear
Change the Data Output to OP2 and Print
Click OK
Click on Solution Type
a SM will appear
Set Solution Type = Linear Static (button down)
Click OK
(back in the analysis menu)
Click Apply
(The analysis will take a few seconds [maybe 10] to run)
In the RM analysis
Set Action = Read Output 2
Object = Result Entities
Method = Translate
Click on Select Results File
a SM will appear
Find and select the file bar.op2
(You may need to use the “find” tools in Windows to locate the file. Occasionally Nastran will put the *.op2 file in a weird place. Occasionally it even puts the file on the hard drive of the license file server. If you cannot find the file on your local hard drive then look on the file servers hard drive. The file server for the NCL is DFELAB10. The file server for the library is HOPPER. You should be able to access either of these from your local machine over the network)
Click OK
Back in the Analysis RM
Click Apply
a SM will appear
Find and select the file bar.op2
(You may need to use the “find” tools in Windows to locate the file. Occasionally Nastran will put the *.op2 file in a weird place. Occasionally it even puts the file on the hard drive of the license file server. If you cannot find the file on your local hard drive then look on the file servers hard drive. The file server for the NCL is DFELAB10. The file server for the library is HOPPER. You should be able to access either of these from your local machine over the network)
Click OK
Back in the Analysis RM
Click Apply
Next you will post process the results by viewing and exporting them
On the TM select Results
a RM will appear called Results
Set Action = Create
Object = Quick Plot
A SM appears
Under Select Result Case
highlight the option Default, Static Subcase
Under Select Fringe Result
Highlight Displacements, Translational
Under Select Deformation Result
Highlight Displacements, Translational
Click Apply
A Colored picture displaying the displacement results will appear. It includes numeric results for max and min displacement as well as color-coded results for the entire beam.
a RM will appear called Results
Set Action = Create
Object = Quick Plot
A SM appears
Under Select Result Case
highlight the option Default, Static Subcase
Under Select Fringe Result
Highlight Displacements, Translational
Under Select Deformation Result
Highlight Displacements, Translational
Click Apply
A Colored picture displaying the displacement results will appear. It includes numeric results for max and min displacement as well as color-coded results for the entire beam.
To save this plot use the “copy to Clipboard” icon (usually just to the right of the print icon) to copy the viewport to the clipboard. Then paste the picture into a word processing document.
If you want to print the viewport directly, you can just use the normal Windows commands (File/Print)
Next, to see the stresses
Under Select Result Case
Highlight the option Default, Static Subcase Under Select Fringe Result
Highlight Stress, tensor
Change the Quantity to X Component
Under Select Deformation Result Highlight Displacements, Translational
Click Apply A Colored picture displaying the stresses results will appear. It includes numeric results for max and min Stresses as well as color-coded results for the entire beam.
Under Select Result Case
Highlight the option Default, Static Subcase Under Select Fringe Result
Highlight Stress, tensor
Change the Quantity to X Component
Under Select Deformation Result Highlight Displacements, Translational
Click Apply A Colored picture displaying the stresses results will appear. It includes numeric results for max and min Stresses as well as color-coded results for the entire beam.
To save this plot use the “copy to Clipboard” icon (usually just to the right of the print icon) to copy the viewport to the clipboard. Then paste the picture into a word document.
If you want to print the viewport directly, you can just use the normal Windows commands (File/Print)
Next you will end your 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 of a Truss
0 comments:
Post a Comment
Please wait for approval of your comment .......