ANSYS AIM Tutorial Structural Analysis of a Plate with Hole Author(s): Sebastian Vecchi, ANSYS Created using ANSYS AIM 18.1 Problem Specification Pre-Analysis & Start Up Analytical vs. Numerical Approaches Analytical Results Displacement, σr, σθ, τrθ, σx Start-Up Geometry Draw Geometry Mesh Set Mesh Size Generate Mesh Physics Set-Up Specify Material Boundary Conditions / Forces Solution/Result Verification
Problem Specification Consider the classic example of a circular hole in a rectangular plate of constant thickness. The plate is A514 steel with a modulus of elasticity of 29e6 psi and a Poisson ratio of 0.3. The thickness of the plate is 0.2 in., the diameter of the hole is 0.5 in., the length of the plate is 10 in. and the width of the plate 5 in., as the figure below indicates. This tutorial will show you how to use ANSYS AIM to find the displacement and the stresses in the plate.
Pre-Analysis & Start Up Analytical vs. Numerical Approaches We can either assume the geometry as an infinite plate and solve the problem analytically, or approximate the geometry as a collection of "finite elements", and solve the problem numerically. The following flow chart compares the two approaches. Let's first review the analytical results for the infinite plate. We'll then use these results to check the numerical solution from ANSYS. Analytical Results Displacement Let's estimate the expected displacement of the right edge relative to the center of the hole. We can get a reasonable estimate by neglecting the hole and approximating the entire plate as being in uniaxial tension. Dividing the applied tensile stress by the Young's modulus gives the uniform strain in the x direction.
Multiplying this by the half-width (5 in) gives the expected displacement of the right edge as ~ 0.1724 in. We'll check this against ANSYS AIM. σ r Let's consider the expected trends for σ r, the radial stress, in the vicinity of the hole and far from the hole. The analytical solution for σ r in an infinite plate is: where a is the hole radius and σ o is the applied uniform stress (denoted P in the problem specification). At the hole (r=a), this reduces to This result can be understood by looking at a vanishingly small element at the hole as shown schematically below. We see that σ r at the hole is the normal stress at the hole. Since the hole is a free surface, this has to be zero. For r >> a, Far from the hole, σ r is a function of θ only. At θ = 0, σ r ~ σ o. This makes sense since r is aligned with x when θ = 0. At θ = 90 deg., σ r ~ 0 which also makes sense since r is now aligned with y. We'll check these trends in the ANSYS AIM results.
σ θ Let's next consider the expected trends for σ θ, the circumferential stress, in the vicinity of the hole and far from the hole. The analytical solution for σ θ in an infinite plate is: At r = a, this reduces to At θ = 90 deg., σ θ = 3*σ o for an infinite plate. This leads to a stress concentration factor of 3 for an infinite plate. For r >> a, At θ = 0 and θ = 90 deg., we get Far from the hole, σ θ is a function of θ only but its variation is the opposite of σ r (which is not surprising since r and θ are orthogonal coordinates; when r is aligned with x, θ is aligned with y and vice-versa). As one goes around the hole from θ = 0 to θ = 90 deg., σ θ increases from 0 to σ o. More trends to check in the ANSYS AIM results! τ r θ The analytical solution for the shear stress, τ r θ, in an infinite plate is: At r = a, By looking at a vanishingly small element at the hole, we see that τ r θ is the shear stress on a stress surface, so it has to be zero.
For r >> a, We can deduce that, far from the hole, τ rθ = 0 both at θ = 0 and θ = 90 deg. Even more trends to check in ANSYS AIM! σ x First, let's begin by finding the average stress, the nominal area stress, and the maximum stress with a concentration factor. The concentration factor for an infinite plate with a hole is K = 3. The maximum stress for an infinite plate with a hole is: Although there is no analytical solution for a finite plate with a hole, there is empirical data available to find a concentration factor. Using a Concentration Factor Chart (Cornell 3250 Students: See Figure 4.22 on page 158 in Deformable Bodies and Their Material Behavior), we find that d/w = 1 and thus K ~ 2.73. Now, we can find the maximum stress using the nominal stress and the concentration factor:
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 18.1. Once you are at the start page of AIM, select the Structural template in the top left corner as shown below. 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. For this problem we will be using static calculation type. Press Finish on the next panel. The Model Editor will launch automatically. Geometry Since the problem given to us represents a 2D state of stress, there are several simplifications that must be made due to the fact that AIM model will be 3D. Since the geometry is symmetric, when we draw the shape we want to create a one-quarter model. By taking advantage of symmetry, we can simplify the problem and also ensure that the model is not over constrained.
Draw Geometry In order to use the units given to us in the problem, press the Project button in the top left corner and select Units > U.S.Engineering. 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 and choose Select New Sketch Plane, then 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. Select the origin, then drag up and to the right until the rectangle is the correct size, or enter the dimensions directly into the highlighted boxes as pictured below. The height should be 5 inches while the length is 10 inches. After the rectangle has been drawn, make a circle at the origin with a radius of 0.25 inches. Using the Trim Away tool in the Sketch subgroup of the Design tab, remove the outside of the circle and the ends of the box to look like the picture below.
Rotate the model slightly out of the XY-plane, then extrude the face using the Pull tool in the Edit section of the toolbar. The problem specifies that the thickness of the plate must be 0.2 inches.
Mesh Close 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 all the way to the right, to give us the most accurate data. Under Global Sizing, change the Size function method to Curvature. The Curvature option allows the mesh to become more refined closer to the circle. 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.
Physics Set-Up Specify Material Select the Physics task in the workflow, then press Material Assignmentss under Physics Definition. AIM has automatically assigned Structural Steel as the default material. We could assign a different material here, if needed. The entire object is made of structural steel, so we can add our other constraints. Boundary Conditions / Forces The pressure acting on both ends of the plate can now be added. Return to the Physics task, then go to Structural Conditions > Add > Pressure. Select the end of the plate face without the cut-out and apply the appropriate pressure. The problem specifies that the pressure be 1 E 6 psi, but since AIM defaults pressure to compressive, it must be negated in order to have a tensile pressure. Return to the Physics task, then press Structural Conditions > Add > Support, select the back side of the plate as the Location, and change the Type to User specified. Change Translation X and Translation Y to Free. There should now be only one arrow pointing from the back of the plate to the front, constraining the direction normal to the surface. This symmetric boundary condition implies that there is zero translation normal to the symmetry surface, and there is zero rotation about the two axes orthogonal to the symmetry surface. Constraining the normal direction to the symmetry surface prevents both translation normal to
the surface and rotation about the two orthogonal axes. In our problem, we will set up three symmetry surfaces by constraining the normal directions for the three surfaces as shown in the image below. Repeat this process for the remaining symmetry surfaces, setting the appropriate Translation values to Free for each.
Solution/Result Press the Results button in the Workflow to extract information from the simulation. In order to compute the solution and find information that can be readily, used first press Evaluate Results. 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.
Verification In the pre-analysis, the maximum stress was calculated. In order to verify that our simulation was accurate, a comparison must be made. To calculate the maximum stress of the simulation, return to the Results panel, click on Add next to Results, and select Calculated Value. In the Function drop down menu, select Maximum. In the Variable drop down menu, select Stress XX in the Stress category. Next, press the Evaluate button. Very quickly, the maximum stress of the plate with a hole is calculated and displayed. The table below compares the calculated and simulated values for maximum stress in the plate with a hole. With a difference of less than 5%, we can consider our simulation to be accurate. This small difference in results may be caused by not using enough mesh refinement. Simulated Value Calculated Value Difference 3.089 E 6 psi 3.033 E 6 psi 1.81%