ANSYS AIM Tutorial Stepped Shaft in Axial Tension

Transcription

1 ANSYS AIM Tutorial Stepped Shaft in Axial Tension Author(s): Sebastian Vecchi, ANSYS Created using ANSYS AIM 18.1 Contents: Problem Specification 3 Learning Goals 4 Pre-Analysis & Start Up 5 Calculation 5 Start-Up 5 Geometry 7 Draw Geometry 7 Mesh 12 Set Mesh Size 13 Generate Mesh 13 Physics Set-Up 15 Boundary Conditions / Forces 15 Solution/Result 17 Verification 19 Page 1 of 19

2 Problem Specification This problem is taken from: Prantil, V. C., Papadopoulos, C. and Gessler, P. D., Lying by Approximation: The Truth About Finite Element Analysis, Morgan and Claypool (2013). Consider a stepped shaft under an applied axial load, P. A stress concentration is apparent at the step where the cross-sectional area is discontinuous. The cross section is circular. So the problem becomes amenable, let s consider a relatively small fillet placed at the step to reduce the stress concentration to a finite value. The pressure load on the smaller cross-section is 1000 psi. Calculate the axial stress concentration factor and compare it to the formula provided in Roark s Formulas for Stress and Strain, Warren C. Young and Richard G. Budynas, Page 2 of 19

3 Learning Goals The purpose of this tutorial is to showcase the simplest stress concentration and demonstrate that it can be resolved in 2 or 3 dimensions. Simple one-dimensional elements (i.e. simple axial bar elements) that capture constant stress within an element are insufficient to capture stress concentrations, even when many elements are used. That is to say, when the necessary physics is not contained in the element formulation, so-called h-convergence or using more elements captures no more of the solution than does a coarse(r) discretization. This tutorial is meant to highlight where it is relatively straightforward to apply FEA and resolve a solution correctly that belies analytical treatment with uniaxial formulae (such as axial_stress = P/A). A few words on the formatting on the following instructions: 1) Notes that require you to perform an action will be colored in blue 2) General information will be colored in black, but do not require any action 3) Words that are bolded are labels for items found in ANSYS AIM 4) Most important notes will be colored in red Page 3 of 19

4 Pre-Analysis & Start Up Calculation It is recommended that you make some back-of-the-envelope estimates of expected results before launching into your computer solution. Here: for which the following formula for the axial stress concentration factor, K, holds ( Roark s Formulas for Stress and Strain, Warren C. Young and Richard G. Budynas, 2002): We'll compare the above axial stress concentration factor to the value obtained from ANSYS AIM. Start-Up Now that we have the pre-calculations, we are ready begin simulating in ANSYS AIM. Open ANSYS AIM by going to Start > All Apps > ANSYS 18.1 > ANSYS AIM Once you are at the starting page of AIM, select the Structural template in the top left corner as shown below. Page 4 of 19

5 You will be prompted by the Structural Template to either Define new geometry, Import geometry file, or Connect to active CAD session. Select Define new geometry and press Next, then press Finish on the next panel. For this problem, we will be using the static calculation type. The Model Editor will launch automatically. In order to use the units given to us in the problem, press the Home button in the top left corner and select Units > U.S.Engineering. Page 5 of 19

6 Geometry This problem could be simulated in either 2D or 3D by employing the proper geometric assumptions and boundary conditions. Since AIM provides a 3D capability, there are several simplifications that must be made to the geometry. When the shape is drawn, we want to create a quarter symmetric model of the geometry so that proper supports can be added to the model that do not over constrain the model. By creating these one dimensional supports, we allow the body to be subjected to the forces of the problem while preventing any rigid body translation and/or rotation of the body in space. Draw Geometry Click the Z-axis on the compass in the bottom left corner of the screen to look at only the XY-plane. Right click in the empty white space and choose Select New Sketch Plane so that the plane we are sketching on will be on the XY-plane, then click on the grid that appears. Next, select the Line tool and, beginning at the origin, make a 8-inch line going in the positive Y direction. Then, starting at the top of the newly-created line, create another line in the positive X direction for 1 inch. You can enter the dimensions directly by pressing the spacebar and typing the numbers. Make another line on the positive X axis, starting from the origin, for 4 inches, and then another 4 inches in the positive Y direction from the right end of the previous line. Page 6 of 19

7 Page 7 of 19

8 In order to get a fillet edge where these two lines intersect, first we need to intersect them. Create lines starting from the open points of the sketch and allow them to intersect ; the lengths the lines are arbitrary as long as they cross. Next, trim the extra lines using the Trim Away tool. Lastly, use the Create Rounded Corner tool to make a fillet edge between the new corner. Click the vertical line and hover the mouse of the horizontal line then press 1 to create the radius of 1 inch. The Model Editor will display 2.0 in while in sketch mode but when 3D will truly be 1.0 in. The problem specified its radius to be 1 inch. The Create Rounded Corner tool is selected in the Sketch section of the toolbar in the picture below. Page 8 of 19

9 In order to convert this sketch into the stepped shaft that is required, it must be rotated around the Y axis. Since the sketch is now complete, select the Pull tool in the Edit section of the toolbar. Utilize the Revolve feature by picking the Y axis to rotate about. Rotate the view slightly to see the yellow, curved arrow, then drag with your mouse to pull the sketch around the Y axis. Press the spacebar and enter 90deg to achieve the precise rotation needed. It should look like the object in the picture below. Page 9 of 19

10 Click in a blank spot of the model window, or press the Esc key on your keyboard, to complete the Pull operation. Page 10 of 19

11 Mesh Close the Model Editor, then initiate the meshing process by clicking on Mesh in the workflow. Set Mesh Size Uncheck the Use predefined settings to access a greater depth of control over the mesh. Under Global Sizing, change the Size function method to Curvature. Input 0.05 [in] as the Minimum size and set the Curvature normal angle to 5 [degrees]. Page 11 of 19

12 Under Objects select the Add drop down menu next to Mesh Controls, add an Element Shape control. Use the Body Selection tool to add the entire shaft volume as the Location and change the Shape to Hexahedrons. Page 12 of 19

13 Under Objects, select the Add drop down menu next to Size Controls and add a Face Sizing. As the Location select either of the flat sides of the stepped shaft and input 0.2 [in] as the Element size. Generate Mesh Click Generate Mesh under Output or at the top of the screen by the status window for Mesh. AIM should detect you are ready to generate the mesh and highlight the buttons in blue. Below is an example of what the mesh should look like. Page 13 of 19

14 Page 14 of 19

15 Physics Set-Up The entire object is made of structural steel, which is the default material in AIM. We can immediately add our other constraints. Boundary Conditions / Forces Select the Physics task in the workflow. The first conditions that need to be specified for a structural simulation are supports. In this case, the supports will exist on the symmetry planes where we cut the model into quarters. Next to Structural Conditions press Add > Support, select one of the cut sides as the location, and change the Type to User specified. Edit the Translation drop down menus until there is only one arrow going into our model, then repeat for the other side and the large quarter circle at one end. This creates a symmetrical constraint support for the shaft, which allows it to deform while also not translating or rotating from its location. Next, the pressure is added to the outermost face of the shaft by selecting the Pressure option in the Add drop down menu. It was given to us as 1000 Psi, but since AIM defaults pressures as compressive, the correct value to input is Psi. Page 15 of 19

16 Page 16 of 19

17 Solution/Result Press the Results button in the Workflow, then press Evaluate Results to extract the information. Once the evaluation is complete, AIM will automatically output two contours in the Results section under Objects. They should be Equivalent Stress and Displacement Magnitude, which are shown below, respectively. Page 17 of 19

18 Page 18 of 19

19 Verification In the pre-analysis, the maximum stress was calculated. To verify that our simulation was accurate, a comparison must be made. In order to view the maximum stress of the simulation, in the Add drop down menu select Calculated Value, change Function to Maximum and the Variable to Stress YY. The table below compares the calculated and simulated values for maximum stress in the stepped shaft. There is a negligible difference between the finite element calculation and the simulation result. Calculated Value Simulated Value Percent Difference 1376 psi 1311 psi 0.20% Page 19 of 19