ANSYS 5.6 Tutorials Lecture # 2 - Static Structural Analysis Example 1 – Static Analysis of a Bracket 1. Problem Description: The objective of the problem is to demonstrate the basic ANSYS procedures for performing a simple analysis. This problem is a simple 2 dimensional static structural problem of a simple bracket as shown in the figure. This bracket is made of a 20 mm thick steel plate. The material properties of steel are given below: Young’ s modulus or Elastic Modulus, E Poisson’ s ratio, γ Density, ρ
200x109 Pascals 0.3 7860 kg/m3
R5 0
PLATE THICKNESS: 20 mm ALL DIM IN mm
60
R1 0( TY P)
= = =
P=1000N
R2 0( TY P)
0 R3
80
Loading and Boundary conditions: The plate is to be welded at the two smaller weld holes and a point load of 1000 N has to be applied along the y-axis as shown. The welded holes restrain the model in both x and y directions. 2. Approach and Assumptions: We assume this problem to be a 2 dimensional problem as the applied loads and the boundary conditions are in the x-y plane only. The thickness can be taken into account into the calculations in ANSYS without actually modeling in 3D. The approach is to model the bracket as a 2D solid model and generate the elements and mesh automatically. We can also create the nodes and elements separately. But such an approach would be a waste of time for a simple model as given in the example.
3. Summary of Steps: a) Preprocessing: - Create the solid model. - Choose the element type. - Assign real constants for the chosen element type - Assign material properties. - Mesh the model. b) Solution: - Apply the displacement boundary conditions - Apply the loads - Solve the model c) Post processing: - Read the results. - Plot the deformed shape. Compare with the undeformed shape. - Plot the von Mises stress. - Animate the stress output and study the trend - List the reaction solution - Exit ANSYS 5.6 4. Outline of Hand-out Conventions: Before entering ANSYS 5.6, here is an outline of the layout of the tutorial handout. • The handout starts from, “How to enter ANSYS 5.6?” to “How to end session?” However, the user may find some problems due to the version of ANSYS or some lack of continuity in the handout or due to a different operating system. The user may contact the instructor for clarifications. • This tutorial is designed for use on ANSYS 5.6 operating on Windows 95/97/2000 or Windows NT. Also the tutorials follows the GUI mode (Graphic User Interface). • Whenever the handout has commands in ITALICS, it means that the user should follow the menu options as directed. • There would also be a description of the operation performed to help the user to understand what he is doing. • The handout will also provide with pictures, tables and menus as it appears on the ANSYS window for more clarity. • The Analysis procedure described in the handout may not be the only procedure to do the analysis. Neither is it the easiest procedure. But it has been designed such that the user gets exposed to as much options as possible. 5. Starting ANSYS 5.6: • Start -> Programs -> Engineering Programs -> ANSYS 5.6 -> Interactive • In the opened window, change the working directory to C:\temp • Run You have now entered the ANSYS workspace. You can find that the main menu of ANSYS is open. If not, go to MenuCtrls -> Main Menu
6. File Operations: 6.1 Title of Analysis: In the Utility menu bar (the menu bar on the top of the screen), go to File -> Change Title. You can give a title name of your choice. Say, “Static Analysis of a Bracket”. 6.2 Analysis File Name: It is a good practice to give a file name even before you start the analysis. File -> Save As One more word of caution. ANSYS does not save the analysis into your file name when you give File -> Save. Instead it saves it into the default filename “file.db”. So every time to save a file, we have to say File -> Save As and overwrite the existing file. 7. Creating the Model: This is the first step of preprocessing. Preprocessing is the ANSYS analysis phase where you provide data regarding the geometry, element type, material properties and meshing. It would be referred in ANSYS as PREP7. The model can be created in many different ways. One of the easiest ways is to use the Rectangle and Circle Primitives – Primitives are simple predefined geometric shapes ANSYS provides - as effectively as possible. So the geometry is to be viewed as an assemblage of circles and rectangles. a) Define the Rectangle: The first step is to create a base rectangle to which circles and other rectangles are to be added upon or subtracted from. Let us consider the lower left corner of the bracket as the origin. • Main Menu –> Preprocessor -> (-Modeling-) Create -> (-Areas-) Rectangle -> By 2 Corners
CAUTION: It is the responsibility of the user to ensure that the consistency of units be maintained throughout the analysis. It is best to first solve a simple problem as given in the assignment for which the analytical results are available. • Close the Rectangle Menu after creating it. b) Create the Circle: • Main Menu –> Preprocessor -> (-Modeling-) Create -> (-Areas-) Circle -> Solid Circle • The area plot shows both rectangle and circle, which are areas, in the same color. To more clearly distinguish between areas, turn on area numbers and colors. The "Plot Numbering Controls" dialog box on the Utility Menu controls how items are displayed in the Graphics Window. By default, a "replot" is automatically performed upon execution of the dialog box. The replot operation will repeat the last plotting operation that occurred (in this case, an area plot). Utility Menu -> PlotCtrls -> Numbering -> Area numbering ON
c) Adding the Circle and Rectangle: • Main Menu –> Preprocessor -> (-Modeling-) Operate -> (-Boolean-) Add -> Areas • The Select window opens. Select both the areas and press OK. • Now you can see that the areas are merged into a single area and the area number and color is also single. d) Creating the R30 bigger hole: • As in the previous case, we have to first draw the circle and then perform the Boolean operation to subtract that area from the original area • Main Menu –> Preprocessor -> (-Modeling-) Create -> (-Areas-) Circle -> Solid Circle Main menu –> Preprocessor -> (-Modeling-) Operate -> (-Boolean-) Subtract -> Areas
CIRCLE CREATION MENU
BOOLEAN (Subtraction) MENU
• During the Boolean Subtraction - Pick the area from which subtraction is going to take place(the bigger area, A3), PRESS OK. Then Pick area which is being subtracted (smaller area, A1), PRESS OK. e) To create the Fillet: • To create the Fillet, we have to first create the Line Fillet. Then an area is created by the enclosure formed by the line fillet and then performing the Boolean Subtraction to subtract the fillet area from the main area. • It is better to operate with lines when we create a line fillet. • Utility Menu -> Plot -> Lines • Main Menu -> Preprocessor ->(-Modeling-) Create -> (-Lines-)Line Fillet • As shown in the adjoining figure, the lines that are to be filleted are selected and the fillet radius is given as 20. This creates the line fillet over the already existing area. So we have to create an area by the lines encompassing this fillet and subtract it from the bracket area.
• Main Menu –> Preprocessor -> (-Modeling-) Create -> (-Areas-) Arbitrary -> By Lines • In the select window, select the 3 lines that make the area of the first fillet and click apply. Then select the area which form the second fillet and select OK
• Main menu –> Preprocessor -> (-Modeling-) Operate -> (-Boolean-) Subtract -> Areas • Now pick the bracket area (Base area from which subtraction is done) and press OK in the Pick Window. Then pick the Fillet areas (Areas to be subtracted) and press OK. f) To create the Weld Holes: • Similar to the R 30 hole which we created in step (b), we can create the two weld holes with the following parameters. Parameter Weld Hole 1 Weld Hole 2 WP X 20 20 WP Y 20 80 Radius 10 10 • Main Menu –> Preprocessor -> (-Modeling-) Create -> (-Areas-) Circle -> Solid Circle • Main menu –> Preprocessor -> (-Modeling-) Operate -> (-Boolean-) Subtract -> Areas • The completed geometry would look like the figure below
SAVE AS..
Ur Filename.db
8. Element Type, Real Constants and Material Properties: a) Element Types - Indicates the element types used in the problem; over 100 element types are available in ANSYS. You choose an element type which characterizes, among other things, the degree-of-freedom set (displacements and/or rotations, temperatures, etc.) the characteristic shape of the element (line, quadrilateral, brick, etc.), whether the element lies in 2-D space or 3-D space, the response of your system, and the accuracy level you're interested in. For this analysis, we can use a 8 noded structural solid element called PLANE82. Since our system is of relatively simple geometry and loading, PLANE82 is sufficient. Results can be made accurate by having a very fine mesh. • Main Menu -> Preprocessor -> Element type -> Add/Edit/Delete -> • Structural Family of Elements -> Solid -> Quad 8 node 82 -> OK • To account for the thickness of the bracket, the element options is selected to include calculation of stress including the thickness of the bracket. • Defined Element type Window -> Options -> (Pull down Menu) Element Behavior K3 -> Plane strs w/thk . ELEMENT DEFINITION ELEMENT OPTION DEFINITION
b) Real Constants: Real constants provide additional geometry information for element types whose geometry is not fully defined by its node locations. Typical real constants include shell thickness for shell elements and cross-sectional properties for beam elements. All properties required as input for a particular element type are entered as one set of real constants. • Main Menu -> Preprocessing -> Real constants -> Add ->Real Constant Set Number -> THK 20
c) Material Properties: Physical properties of a material such as modulus of elasticity or density that are independent of geometry. Although they are not necessarily tied to the element type, the material properties required to solve the element matrices are listed for each element type for your convenience. Depending on the application, material properties may be linear, nonlinear, and/or anisotropic. As with element types and real constants, you may have multiple material property sets (to correspond with multiple materials) within one analysis. Each set is given a reference number. • Main Menu -> Preprocessing -> MaterialProps -> (-Constant-) Isotropic • Give the material a number label and press OK. • Input the material properties in the Material property window. ANSYS provides us with a library of materials also. For accessing this library, we have to find the path name under the ANSYS directory for MATLIB directory. • Main Menu -> Preprocessing -> MaterialProps -> Material Library -> Library path • The Library path typically would be something like this, c:\ansys56\matlib • Once you have entered the library, you can select from the list of materials available in ANSYS. • Main Menu -> Preprocessing -> MaterialProps -> Material Library -> Import Library
9. The Meshing Process: Having defined the material properties, element type and the real constants, we can go ahead and mesh the model. One nice feature available in ANSYS is that we can generate the mesh automatically without breaking our heads to calculate the optimum mesh size. Depending on the degree of refinement required, we can choose either a course or a fine mesh size. Depending on the generated mesh, we can even refine it further. • Main menu -> Preprocessor -> (-Meshing-) Size Cntrls -> (-Manual Size-) (-Global-)Size • In the Size field, enter the number 5. This means that the element is to have a nominal size of 5x5 mm2. Press OK • Main menu -> Preprocessor -> (-Meshing-) Mesh -> (-Areas-) Free • Pick the area to be meshed and press OK. You should be getting a mesh close to the one shown below. • SAVE AS … … .. filename.db
10. Loads and Constraints: Now we have started the SOLUTION phase of the analysis. ANSYS analysis phase where you define analysis type and options, apply loads and load options, and initiate the finite element solution. A new, static analysis is the default. a) Application of Displacement Constraints: • As described in the problem description, the 2 smaller holes are to be welded from the inside. This means that the degrees of freedom (dofs) are zero in the x and y directions i.e. no displacements in the x and y directions. • Main Menu -> Solution -> (-Loads-) Apply ->(-Structural-) Displacement -> On Lines • Pick the lines that comprise the weld holes and press OK.
• Pick All DOF under Lab2 -> Enter 0 for Value. • This simulates the effect of a rigidly welded hole in actual practice. b) Application of a Point Load: As specified in the problem, a vertical load of 1000 N has to be applied on the larger hole at the bottom quadrant point. • • • • •
Main Menu -> Solution ->(-Loads-) Apply -> Force/Moment -> On Keypoints… … Pick the Keypoint in the lower quadrant and press OK. In the Load Window, Choose the direction of force to be Fy. The Apply as field is to be set at the default value of ‘Constant Value’ In the Force/Moment Value, Input force value as –1000 as the force is a downward (-ve y) acting force
. 11. SOLUTION: Now we have finished modeling, meshing and defining the loads of the model. Now we have to solve the model and get the results. The default setting for solution control holds good for such a model. We have to modify the solution controls for different types of analysis as the case demands. • Main Menu -> Solution -> (-Solve-) Current LS. • The above command indicates that we are solving for the current load step. Once you click on the OK button, a dialog box that shows the different input parameters appears. We need to review the parameters and when we find it to be satisfactory, we can start the solution by pressing OK after closing the dialog box. • If the model is good, a dialog box appears to say that the solution is done. • The solutions are stored in the results file “file.rst”as this is a structural analysis. If it had been a thermal analysis, the results file is “file.rth”. • SAVE_AS jobname.db
12. POST PROCESSING: The model has been solved and the user now has to invoke the POSTPROCESSING to view the results in a user-friendly manner. The postprocessor processes the results of the FEA, which is a huge 2n x 1 matrix of the displacements in the x and y directions, into user friendly plots. Also the post processor calculates other derived quantities like Stress, Strain, Strain energy etc. for the user to peruse. • Main Menu -> Postprocessing -> (-Read Results-) Last Set • The above command reads the final iteration result of the analysis. a) To plot the deformed shape: • Main Menu -> Postprocessing -> Plot Results -> Deformed Shape • Now we select Def + Undefrmed press OK. • We should get an output that should resemble something like the figure given below.
b) To plot the von Mises Stress field: • Main Menu -> Postprocessing -> Plot Results ->(-Contour Plot-) -> Nodal Solution • In the plot results window, click on the Stress field and on the right hand box, scroll down till we find von Mises SEQV. The dialogue box would look like this. Press OK.
The results would look something like the plot given below.
13. Modifying the loads and reviewing the results: This section is an extension of the previous model for the student to gain more insight into the analysis powers of ANSYS. The user has to go back to the solution and delete the point load and apply other types of loads. a) Try out with a pressure of 10000 N/m2 acting on the lower quadrant of the bigger hole. b) Include into the above model the effect of self-weight by including the gravitational loads – Gravitational loads are listed in Main Menu -> Solution ->(-Loads-) Apply ->Gravity c) Compare the results of the above two models. d) While solving the model with the gravity observe the solution status window before solving. The solution status window is the one given below.
14. Quitting ANSYS 5.6: • Utility Menu -> File -> Exit ->… … … … . On the window, pick on Quit, No Save References: 1. www.ansys.com 2. www.uni-karlsruhe.de/~ANSYS/ALBERT/bracket/bracket.html 3. ANSYS Structural Analysis Command Guide
