Home » , , , » MODELING A FRAME STRUCTURE (WEIGHT BENCH) USING BEAM 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.
MODELING A FRAME STRUCTURE (WEIGHT BENCH) USING BEAM ELEMENTS
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 XL being the horizontal and YL being the vertical coordinates respectively (see figure below). Obviously, this means that ZL 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 {ZL} = {XL}.
An Example is shown below:
Consider the following cross section and the orientation of the cross section on the 2 beams in the picture.
orientation of the cross section on the 2 beams
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 {ZL} = {XL} 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 {ZL} = {XL}. = {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
image
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
image

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
Share this article :

0 comments:

Post a Comment

Please wait for approval of your comment .......