Practical 7

Optimization of a plate with a hole.

Problem Statement:

Consider a square plate with a hole in its center. The plate is made out of "FEA Material", which
has a Young's Modulus of 29 e3 ksi and a Poisson's Ratio of 0.3. The length and width of the plate
are both 10 inches. The hole in the middle of the plate is subject to a uniform pressure of 1 x e6
psi in the outward radial direction. Due to the symmetry of this problem only one quarter of the
geometry is needed as shown below.

The radius of the hole is the design variable. Furthermore, the radius is constrained between a
minimum value of 1.0 inch and a maximum value of 2.5 inches.
Using ANSYS, minimize the volume of the plate by optimizing its radius, while staying
underneath a maximum Von Mises stress value of 32.5 ksi.

Pre-Analysis
  While the case of an infinite plate with a hole and a radially outward pressure within the
hole has an analytical solution, the case of a finite plate with a hole does not. The lack of
an analytical solution favors finite element analysis as a solution method.
 This Experiment will start out by using ANSYS to find the deformation and equivalent
Von Mises stress for a specific plate with a hole geometry. After the initial solution is
obtained, ANSYS will be told which variables the design variables and what results are
are the output parameters. These variables can be viewed as follow.
 Design Variables: Radius
 Objective function: Minimize volume
 Constraints: Equivalent Von-Mises stress <32.5 ksi from there, the optimization
procedures will run.

Start-Up: Open Files

 Open this project in Workbench by double-clicking on "Exp_2.wbpj" From manual files

folder.

Initial Solution
 To view the initial solution, select from the
main project window. The default units in Mechanical are Metric, so go to the top menu
bar
 Select Units and change from Metric to U.S. Customary (in). If you do not do this now
then you will likely have to start over so please change your units at this point. We will
begin by viewing the total deformation of the plate. Select Total Deformation from the
Solution tree in the Project Outline window on the left.

 The following images display the results for the initial case in which the radius of the hole
is 2 inches.

Total Deformation
  Let's compare the deformed shape of the plate to what we expect from the applied
boundary conditions. First, let's look at the radius of the hole.
 The radius of the hole has uniformly increased, which is consistent with the applied
boundary condition of uniform pressure at the radius. Next, let's examine the left and
bottom edges of the plate.
 Motion along these two edges has been parallel to these edges, which agrees with the
applied symmetry condition. Finally, let's look at the top and right edges. We can see that
both have deformed away from the hole, and the deformation is smallest at the top right
corner, which agree with our expectations.

Equivalent Stress

 Next, let's view the Equivalent Stress values calculated by ANSYS. Select Equivalent
(von-Mises) Stress from the tree in the left panel. We would now like to view the stresses
as colored contours. Select the Results>Contours >Contour Bands.

 The following image should now appear, representing the contour bands representation of
the von Mises Stress.
 Now let's do a quick mesh convergence study to make sure that our solution is good
enough. Remember that more elements in a mesh might give more accurate results but can
significantly increase the computational time.
 So, we want to refine our mesh (have more elements) until the solution changes so little
that we can deem it to be accurate enough for our purposes. In different words, we will
have ANSYS refine the mesh until the change in a chosen criteria is less than a specified
percent difference. In this example, the criteria we will examine is the maximum value of
the von Mises Stress. From the tree on the left, right-click Equivalent (von Mises) Stress
> Insert > Convergence. Set the Allowable Change to 5%, as seen below.

 Next, click Solve in the top toolbar. It turns out that ANSYS only needs one iteration to
reach the Allowable Change. After one iteration, we see that there is a change of around
0.10% in the maximum von Mises Stress in the plate. From this, we can conclude that our
solution is mesh converged.
 To see the final mesh that ANSYS has created during the "convergence" process, select
Mesh From right tree.
  Next, right click on Convergence in the tree on the left and choose Delete. This is done to
speed up the optimization process, which we will now move onto.

Input & Output Parameters

 To set up the input and output parameters for a geometry created in Workbench, simply
follow the steps below.

Design Variables: Hole Radius (Design Modeler)

 You can also use Design Modeler to specify your parameters. In order to do so, open
Design Modeler by double-clicking on
from the Project Schematic window. Then expand XY Plane. Next, highlight Sketch1.
 Now, check the box to the left of "R3", which will be in the "Dimensions: 3" part of the
"Details View" table. When you check the box an uppercase "D" will appear within the
box and you will be asked what to call the parameter. Call the parameter "DS_R".
Design Modeler can now be closed.

Objective Function: Minimize Volume (& Mass)

 This particular optimization problem has two output parameters: the volume of the quarter
plate and the maximum Von Mises stress. In order to specify the volume output
parameters, first (Open) Results > (Expand) Geometry > (Highlight) Surface Body. In
the "Details of "Surface Body"" table expand Properties then check the box to the left of
Volume. A "P" should now be located within the box.
 Additionally, if mass is also a desired parameter, check the box to the left of Mass.
Constraints: Maximum Von Mises Stress < 32.5 ksi

 Now, the maximum Von Mises Stress will be specified as an output parameter. In order to
do so, (Expand) Solution > (Highlight) Equivalent Stress. In the "Details of "Equivalent
Stress"" window, underneath Results, check the box to the left of Maximum. Once again,
a "P" should appear to the left of the box to illustrate to the user that the maximum Von
Mises stress has been designated as an output parameter. Also Click Solve if results are
not updated.
 At this point the Results window can be closed and you should save the project.
 Let's review the input and output parameters that will be used in the optimization process.
In the main Project Schematic window, double click on Parameter Set.

 After doing so, we can see that DS_R is the input parameter, and the volume and max.
value of the von Mises Stress are the output parameters. Now, return to the main window
by clicking on the Project tab.
  Note: Make sure your parameters are using the correct units! If they are not, you will need
to go back into Mechanical and change the units before unchecking and rechecking the
box next to the parameters of interest. This should reset the units on the parameters in the
Parameter Set window, but beware that this may cause the entire optimization process to
need updated and repeated.

Design of Experiments
 This step samples specific points in the design space. It uses statistical techniques to
minimize the number of sampling points since a separate FEA calculation (and associated
stiffness matrix inversion) is required for each sampling point. This is the most time-
consuming step in the optimization process.

Response Surface Optimization

 First, Goal Driven Optimization needs to be placed in the Project Schematic. In the left-
hand menu called "toolbox" expand Design Exploration. Next, drag Response Surface
Optimization and drop it right underneath the Parameter Set. Your project schematic
window, should look comparable to the one below. Note that all the systems are connected.
 Next, double-click Design of Experiments. Again, we can see our input and output
parameters but this time under the Design of Experiments step.

 Highlight P1-DS_R and change the Lower Bound to 1 inch and the Upper Bound to 2.5
inches.
Now, that the radius of the hole is properly
constrained click on . ANSYS just
picked what it thinks are the best sampling
points according to an algorithm.

 Note that these sampling points are not necessarily linearly spaced. To get a numerical
solution for each of these radii, click Update.

 If you get the following error, click Yes.

  After the update has completed, click on Return To Project. You may want to save again
at this point.

Response Surface

 In this step, ANSYS builds a surface by interpolating the discrete sampling points selected
in the previous step. This can be thought of as building a model of the terrain in the design
space.
 Start by double clicking on Response Surface in the Project Schematic window.

 Once the Response Surface window opens click Update. After, the update has completed
click on Response to see a plot of the volume as a function of hole radius.
Volume

 The relation between radius and volume is quite trivial to compute. It will simply be the
area of the surface multiplied by the thickness of the surface.

Maximum Von Mises Stress

 In order to display a plot of the maximum von Mises stress as a function of the hole radius,
change the value assigned to Y axis to P3-Equivalent (von-Mises) Stress Maximum.
The plot below shows the maximum Von Mises stress as a function of the hole radius.

 As expected, the maximum Von Mises Stress increases as the radius increases. You can
use this graph to get an idea of what radius might constitute the upper limit in accordance
with our constraint of 32.5 ksi. Remember that to minimize volume, you want the greatest
radius possible that still creates an equivalent Von Mises stress under our constraint.
Taking a close look will tell you that you should expect an optimal radius of around 1.5
inches.
 At this point, click Return To Project and then save the project.

Optimization

 Set-Up of Optimization
 Begin this step, by double clicking on Optimization.
 At this point, ANSYS must be told that the objective function(volume) is to be minimized
while staying below the 32.5 ksi Von Mises stress threshold. First, select “Objectives and
Constraints” in the outline window. Then, in the "Table of Schematic B4: Optimization"
window, select the parameter to be P2Surface Body Volume and change the objective type
to Minimize.

 Next, add in a second parameter which will be P3-Equivalent (von Mises) Stress
Maximum, change the constraint type to Values <= Upper Bound and enter 32500 for the
Upper Bound. Your table should now look like the one below.

 Now, execute the optimization by clicking on Update and click on Optimization from the
outline window to view the results. The optimization should yield similar results to the
table
 The optimization tool found three candidate points that matched our given constraints and
objectives. This computation was pretty fast because the optimization tool used the
response surface model (plots) that previously generated. It did not actually solve our
model by doing a matrix inversion. Remember that the response surface model is only an
approximation of the relationship between the parameters and so our results might not be
very accurate. Thankfully, we can solve our model using these candidate points to “verify”
that they really do satisfy our constraints.
 In the Properties of Schematic B4: Optimization window, insert a check to Verify
Candidate Points and click on Update once again. Notice how much longer it takes to
solve our model.

 The optimization should yield similar results to the following table. Surprise! Some
candidate points do not satisfy the maximum Von Mises stress constraint (now marked
with a red cross). This is why it is important to always verify the candidate points.
 By selecting candidate points under the results section of the Outline of Schematic B4:
Optimization window, you can also see how the results of each candidate points differ
 from the results of a specified reference candidate point. Additionally, you can even add
new candidate points.
 Output parameter values calculated from simulations (design point updates) are displayed
in black text, while output parameter values calculated from a response surface are dis-
played in blue.
 The number of gold stars or red crosses displayed next to each goal-driven parameter
indicate how well the parameter meets the stated goal, from three red crosses (the worst)
to three gold stars (the best).
Obtaining Deformation and Stress Results for Selected Design Point

 We will select candidate point 2 as the design point. It is a good idea to review the
deformation and stress plots at the chosen design point. To do this, let's set the radius from
Candidate Point 2 as the radius of the hole in Design Modeler. Select (Right Click)
Candidate Point 2 > Insert as Design Point.

 Next, click Return to Project and double click on Parameter Set. Selecting Insert as
Design Point created the design point DP1. Now in the "Table of Design Points" (Right
Click) Current > Duplicate design point.
 You have just duplicated the parameters from the original geometry into the new design
point DP2. Now (Right Click) DP1 > Copy Inputs to Current and click on Update All
Design Points in the toolbar.

 The radius of Candidate point 2 has been inserted as the radius in the Design Modeler.
Let’s now view the results of our model with our optimized radius of 1.4853. Click on
Return to Project and double click Results. The graphs below display the total
deformation and the equivalent Von Mises stress.
Total Deformation

Equivalent Von Mises Stress

Verification & Validation

 As with any numerical method verification and validation of great significance. As
mentioned earlier, there is no analytical solution for the finite plate with a hole. Thus, the
 results cannot be compared to theory. Thus, in this section other verification and
validations will be used. First, the solution will be examined as the mesh is refined to see
if it has converged. Additionally, the optimization results will be verified by using different
optimization methods and comparing results.

Mesh Refinement

 The convergence criteria which was inserted earlier was used to view the effect of mesh
refinement with a radius of 1.4853 inches.
Number of Elements Equivalent Von Mises Stress (PSI) Percent Change

244 32,495

775 32,712 0.6656

 As one can see from the data above, over the course of the mesh refinement, the equivalent
Von Mises Stress only changes by less than one percent. Thus, the solution has been
verified with respect to mesh refinement. However, notice how the equivalent Von Mises
Stress now lies above our constraint. While our optimization looked promising, we had
not taken into account the slight change in results from a finer mesh.

Optimization Methods

The optimization was carried using each of the four optimization methods offered in ANSYS
workbench. Note that the default optimization method in ANSYS was Screening but now is
MOGA.

Optimization Method Radius (In) Volume (In^3) Equivalent Von Mises Stress (PSI)

Screening 1.3278 9.8615 32,484

MOGA 1.3267 9.8618 32,500

NLPQL 1.3291 9.8613 32,503