A 12" x 12" x 1" aluminum plate has a 1" diameter hole at the center.  This plate experiences a tensile load of 12,000 lbf in the horizontal direction.  This model exhibits two planes of symmetry.   Determine the stress near the hole. Determine the deflection of the plate.

CONCEPTS:

• 2D modeling

• Planes of Symmetry

• Stress Concentration

• Geometric Construction: Primitive Shapes, Boolean Operations

• Finite Element Meshing / Mesh Controls

RUN ANSYS Workbench.  Create a new "Empty Project"

On the left side of the “Schematic Page”, double-click on “Static Structural (ANSYS)” to create a new project

Double-click on "Geometry" to start (DM) DesignModeler® (or right-click and pick New Geometry)

Select the length units you want to use for modeling.  [It seems you get ONE chance to select the desired length unit when entering DM - if you get it wrong, delete what you have done and start over]

To sketch on the XY plane, click on "XYplane" in the Tree Outline, then click the Sketching Tab below the tree outline.

To view the sketching plane head-on, click the Z-axis on the XYZ triad at the lower right corner of the Graphics window. -OR- there is a "Look At" button in the top toolbar which sets your view to look at the plane you are sketching on.

Create a 1/4-symmetry planar (2D) model for the plate with a hole:

Under "Draw" in the Sketching Toolbox on the left side, create a rectangle with one corner at the origin and the other corner to the right and above the first.

Notice that the cursor changes when you touch an axis or the origin – this is DM’s “design intent” anticipating what you might want to do.

Use "Dimensions" in the Sketching Toolbox to dimension the width (6”) and height (6”) of the rectangle.

In the Details View (lower left), enter the proper value for each dimension.

 To rescale the Graphics display, use the right mouse button (find “Zoom to Fit”) or use the Zoom to Fit button at the top of the WB window.

Under "Draw" in the Sketching Toolbox on the left side, create an Arc by Center with the center at the origin (on the lower left corner of the rectangle) and have the arc span 90^o form the bottom horizontal edge to the left vertical edge of the rectangle.

Watch prompts from WB at the bottom of the window.

Under "Modify" in the Sketching Toolbox on the left side, use Trim to cut the lines of the rectangle INSIDE the intersection with the arc.

Use "Dimensions" in the Sketching Toolbox to dimension the radius of the arc.
In the Details View (lower left), enter the proper value (0.5”) for the radius of the arc.

At the top of the DesignModeler® window:

• choose "Concept" 

• then choose "Surfaces from Sketches"  (we are making a “surface body”)

• Pick the 5 lines in your sketch (or you can pick "Sketch1" from the Tree Outline)

• In the Details Area: Apply Sketch1 as the Base Object, 

• choose "Add Material" for the Operation

• orient with Plane Normal - yes

• then ADD the thickness of the part (1")

• Click on "Generate" above the Tree Outline and the "surface body" is created.

Return to the Project Schematic:

Under File -> Save As -> use the same file name "plate1" and save it on C:\TEMP [or in a folder on your permanent (P:\) storage space].

Enter or Select Material Data:

Double-click on the Engineering Data line of you project:

• Click the last button on the top row of buttons, “Engineering Data Sources”

• In the Outline Filter (at top), click on “General Materials”

• Find "Aluminum Alloy" and click the plus sign to add this material to your project

• Next, under “Units,” switch to “US Engineering” and “Display Values in Project Units”

• Finally, at the top of the page, click on “Return to Project”

Prepare to do a 2D model simulation:

In your project schematic, select Geometry by clicking ONCE on it

If the Properties panel is not visible, at the top of the page, click on “View” then click on Properties

In the Properties Panel, find “Advanced Geometry Options” and change the Analysis Type to 2D

Take the model to DS (DesignSimulation®)

Double-click on "Model" to start DesignSimulation® (or right-click and pick Edit)

The geometry created in DesignModeler® is automatically transferred to DesignSimulation®.

 Recommended: check Units to make sure you are going to operate in the proper system of dimensions, properties, and loads.

In the DesignSimulation® Outline (left side):

Click on “Geometry” (top of Outline) and VERIFY the 2D Behavior: Plane Stress is defined.

Also, you may check volume, mass, area, and bounding box dimensions to check model import.

 Expand the Geometry branch and click on Surface Body. 

In the Details area, the Material Assignment is Structural Steel (incorrect).  
Assign the Aluminum Alloy material to the body

Click on "Mesh" in the Outline

In the Details area, set "Relevance": 100

under "Advanced"  set Shape Checking: Aggressive Mechanical

RIGHT click on “Mesh” in the Outline and 

• “Insert” a “Sizing”

• Pick the Body and in the Details Area under Scope "Apply" it as the Geometry for the Sizing

• Enter the Element Size: 0.50 in
  

• “Insert” a “Sizing”

• Change Cursor Mode to Line picking:  buttons at top – OR – right mouse in graphics area

• Pick the circular arc of the hole in the plate and

• In the Details Area under Scope, "Apply" it as the Geometry for the Sizing

• In the Details Area, enter the Element Size: 0.05 in

RIGHT click on “Mesh” in the Outline and "Generate Mesh"

In the Details area, check “Statistics” to see how many nodes and elements were created

In the Tree Outline, under Static Structural,

Right-click to Insert, Frictionless Support (or use the “Loads” menu above the Outline)

Pick one of the straight edges which split the model for symmetry

In the Details area under "Scope", Apply that edge to this boundary condition. 

Repeat (make a 2nd Frictionless Support for the other symmetry edge.

1) How does a “frictionless support” work for a symmetry condition ?

2) WHY make two objects for Frictionless Support ?

 In the Tree Outline, under Static Structural,

Right-click to Insert, Force (or use the “Loads” menu above the Outline)

Pick the straight edge on the right.

In the Details area under "Scope", Apply that edge to this boundary condition.

"Define by" "Components" (instead of "Vector”)  to define the force,

Enter the  x-component: 6000 lbf. 

3) WHY is 6000 lbf the proper value ?

4) WHY use a Force when we used Pressure load before ?

 In the Tree Outline, under Static Structural, click on Analysis Settings,

In the Details area, set Weak Springs: Off

(WHY ?  Because a properly constrained model does NOT need weak springs)

5) What are "weak springs" ?

In the Tree Outline, under Solution,

Right-click on Solution, then Insert, Stress, Normal Stress.  In the Details area, request X Axis Orientation

Right-click on Solution, then Insert, Stress, Equivalent (vonMises) Stress. 

Right-click on Solution, then Insert, Deformation, Total

Right-click on Solution, then Insert, Stress, Error

Right-click on Solution, then Insert, Commands (you may cut/paste commands from web page):

Under File -> Save Project.  (It will save where you did the last save.)

When you solve, where will the large, scratch files be created ?

Solution files are written in a folder below the directory where you saved the project.  If this is your P:\ drive, you may experience quota problems.

 In the Tree Outline, under Static Structural, click on Analysis Settings, then expand the Analysis Data Management branch in the Details Area.  This lists the Solver Files Directory.

To change the Solver Files Directory, return to the Project Schematic and File > Save As and resave your project on a different drive (like C:\TEMP)

In the Outline,

ALL items should have green check mark (ready to go) or yellow lightning bolt (not solved yet)

Right-click on Solution, then select SOLVE (or use the Solve button, at top)

 Examine the normal stress, equivalent stress, total deformation, and structural error results.

 Right-click on Solution, then Insert, Deformation, Directional. In the Details area, request X Axis Orientation.  RIGHT mouse on Solution, Evaluate Results (a full SOLVE is not necessary)

 Right-click on Solution, then Insert, Probe, Force Reaction, and scope it to the vertical symmetry plane, frictionless support boundary condition. 

 Right-click on Solution, then Insert, Stress, Normal Stress.  In the Details area, request X Axis Orientation, then change the “Scope” to be only the circular arc of the hole in the plate

 Insert FIGURES (in the Tree Outline) for the Geometry, Mesh, Static Structural Environment, and for EACH Solution result.  These figures will be added to the WB Report, when it is generated.  There is a button on the top, far right end of the button toolbar that will allow you to insert figures for each item in the Tree Outline. It can also be used to capture Images in files on the hard drive.

Below Solution in the Outline, click on “Solution Information”

  This is the ANSYS Output Window with all responses from ANSYS as the model was solved.  It is often necessary to look at Solution Information to discover:

• Error or Warning messages

• Element types used for the model

• Responses to operations in your Command Object

• The system of UNITS used for the solution [6) copy and save the lines which define the project units]

• Other useful information

At the top of the Outline, click on Project. In the Details enter, your name (or team) as author, subject: Plate with a Hole 2D FEA Model, and prepared for: MET 415, HW-5, "this semester".

Below the Graphics area, click on the Report Preview TAB.  The report generates automatically. 

Above the Outline, click on Send to > Microsoft Word,

WARNING: The figures are linked to the report. If you clean and save the project, the figure files are lost.  To make the figures embedded images in the MS-Work document:

1. With your Word 10 document open, click the File button, top-left of the window.
2. Select: Edit Links to Files (lower right)
3. Select and highlight the images you want to convert from the list.
4. Select the option to Save picture in document.
5. Click the Break Link button.
6. Click Yes to confirm.
7. Save the MS-Word document with embedded images.

• Format it so it will print nicely (don't let figure size push captions onto the next page; adjust figures).   Add important information about the analysis (from the Solution Information object) as comments*: the total mass reported during solution (is it correct ?), ALL element types used, the overall mesh error, and interpret the local mesh error plot.

TURN IN: 

1. This report,

   • formatted properly and

   • with comments* (above) added to it.  (Add comments to the end of the report)

2. At the end of the report, add answers to the six BOLD, embedded questions (above) [ 1) – 6) ]