ANSYS AIM Tutorial Thermal Stresses in a Bar

Transcription

1 ANSYS AIM Tutorial Thermal Stresses in a Bar Author(s): Sebastian Vecchi, ANSYS Created using ANSYS AIM 18.1 Problem Specification Pre-Analysis & Start Up Pre-Analysis Start-Up Geometry Draw Geometry Create Bar Edit for 3D Accuracy Mesh Set Mesh Size Generate Mesh Physics Set-Up Add Structural Conditions Add Solid Thermal Conditions Solution/Result Validation

2

3 Problem Specification A steel bar ( E = 2.0E10 P a, ν = 0.3, α = 1.2E 5 ) with the dimensions shown below is placed between two walls. On one side, the bar is rigidly fixed to the wall and on the other, there is a 2 mm gap between the wall and the bar. What is the maximum stress in the bar after the temperature increases 100 degrees Celsius?

4 Pre-Analysis & Start Up Pre-Analysis First, we need to know if the expansion of the bar is greater than the free space between the bar and the wall, x = meters. Below are the equation and the calculated result used for the expansion of the bar. 1 δ T = α LΔT = ( 1.2E 5 C )(5m)(100 C) = 0.006m > 0.002m Now that we know that the deformation due to the change in temperature will be greater than the space between the bar and the wall, we know that there will be a stress on the bar. If the wall was not there, the bar would fully deform to the calculated value above. Since the wall does stop the deformation process, the following equation can be used. δ T = x + δ σ Where δ T is the strain contribution from the change in temperature and δ σ is the strain contribution from the force imparted by the wall on the bar. This equation can be combined with the first one to make the following. Substituting Solving for α LΔT P σ xx = A, we get the solvable equation σ, we find that α LΔT P L = x + EA σ L xx = x + E σ xx = αeδt xe L After substituting, we find 1 (0.002m)(2E11 P σ xx = ( 1.2E 5 C )(2E11 P a)(100 C) a) = 160 MP a (5m) A few words on the formatting on the following instructions: 1) Notes that require you to perform an action are colored in blue 2) General information is colored in black, but does not require any action 3) Words that are bolded are labels for items found in ANSYS AIM 4) Most important notes are colored in red 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 Thermal template.

5 You will be prompted by the Thermal template to either Define new geometry, Import geometry file, or Connect to active CAD session. Select Define new geometry and press Next. For this problem, we will be using the Steady/static calculation type and adding Structural as an additional physic. Select them in the menu and press Finish. The Model Editor will launch automatically.

6

7 Geometry Draw Geometry Click on 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, choose Select New Sketch Plane, and left click on the grid that appears, so that the plane we are sketching on will be on the XY-plane. Choose the Rectangle drawing tool in the Sketch subgroup of the Design Tab and click on Define rectangle from center at the left. Select the origin and drag out the rectangle until it is the correct size, or dimension the rectangle using the highlighted boxes, pictured below, that appear as you are making the rectangle. Create Bar Once the correct bar height and width are inputted as 0.1m, use the Pull feature in the Edit subgroup and extrude the bar to 5 meters.

8 Edit for 3D Efficiency Because the problem is symmetric, we can save computation time and memory by simulation a quarter cross-section. The easiest way to do this is to cut the bar into a quarter and further down the line set constraints on the cut sides. Select the top and bottom faces of the bar and press Plane in the Create section of the toolbar. Repeat with the sides of the bar. Use the Split Body tool to get rid of the the unwanted portions of the bar until we have a quarter. When using the Split Body tool, select the body in question, then the plane to split the body, then one side of the body to be deleted. Repeat this until there is only a quarter bar left.

9

10 Mesh Exit the modeling window, then initiate the meshing process by clicking on Mesh in the workflow. Set Mesh Size Using the Mesh resolution slider, we can edit how precise our mesh is for our calculations. Move the slider 2 notches to the right, slightly past halfway, to improve the accuracy of the solution. Under Global Sizing, select the Proximity option for the Size function method. Generate Mesh Click Generate Mesh under Output or at the top of the screen by the status window for Mesh. AIM should detect that you are ready to generate the mesh and highlight the buttons in blue.

11 Physics Set-Up Add Structural Conditions Once having entered the Physics task of the workflow, the wall support needs to be defined. This is done by selecting Add next to Structural Conditions. In the Add drop down menu, there is an option for Support. Click this to open the Support selection menu. Select the face which is going to be attached to the wall, then press the blue + button next to Location. Next, open the drop down menu below Type and choose User specified. Next, under Degrees of Freedom, set Translation X and Translation Y to be Free while Translation Z is set to Fixed. This allows the bar to expand in the X and Y directions while constraining Z. The other end of the bar needs a displacement constraint in order to keep it from clipping into the other wall. Return to the Physics task, select Add to the right of Structural Conditions, and choose Displacement. Select the appropriate face, press + next to Location, and input m in the Translation Z box. Then, type Free into the Translation X and Translation Y boxes. Using Free in these places will prevent the free end from being over constrained and calculate a more accurate stress distribution.

12 Next to Structural Conditions, pres s Add > Support, then select one of the cut sides as the Location and set the Type to User specified. Edit the Translation drop down menus until there is only one arrow going into our model. This creates a symmetrical constraint support for the shaft which allows it to deform while also not moving its location. Repeat this step for the other cut face. Add Solid Thermal Conditions Next, the temperature change needs to be added by selecting entire bar body, adding a Solid Thermal Condition > Temperature, and setting it to 122 degrees Celsius. Be sure to change to the Body selection mode using the toolbar at the top center of the model window. We know

13 that it needs to be set to 122 degrees Celsius because there needs to be a 100 degree increase. The original temperature can be found by going back to the Physics section via the workflow, and then selecting Material Assignments. In this menu, the Zero-thermal-strain reference temperature can be found and used as the starting temperature for the material. The material was automatically assigned to be structural steel, but if a different material was used, the zero-thermal-strain reference temperature would be different and so would the thermal condition for the free end of the bar.

14 Solution/Result Press the Results button in the Workflow to extract information from the simulation. In order to find information that can be readily used, first press Evaluate Results. Once the evaluation is complete, AIM will automatically output three contours in the Results section under Objects. They should be Temperature 1, Equivalent Stress 1 and Displacement Magnitude 1. The displacement magnitude contour is shown below. The end closest to the wall moved the least while the free end moved the maximum amount allowed. The movement can be viewed by pressing the Play button in the top of the model window after having selected the specific contour. Below is a close up of the free end of the bar while showing the equivalent stress contour. Both ends are identical because the fixed end needs to match the free end; otherwise, it wouldn t be fixed anymore, it would move through the wall.

15

16 Validation In the pre-analysis, the maximum stress was calculated. In order to verify that our simulation was accurate, a comparison must be made. In order to calculate the maximum stress of the simulation, click on Add next to Results, and select Calculated Value. In the function drop down menu, select Maximum. Under the Variable drop down menu, select Equivalent Stress then press Evaluate. Very quickly, the maximum stress of the heated bar is calculated and displayed. This maximum value can also be seen in the panel on the left when the Equivalent Stress 1 contour is displayed. The table below compares the calculated and simulated values for maximum stress in a heated bar. With a difference of much less than 5%, we can consider our simulation to be accurate. Calculated Value Simulated Value Difference Mpa 160 Mpa 0.018%