Plate with a Hole - In-class Example
A 12" x 12" x 1" aluminum plate has a 1" diameter hole at the center. This plate experiences a tensile (distributed) load of 1000 psi 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"
(OPTIONAL) In Workbench 11.0: From the Project TAB -> Tools -> Options... -> Common Settings -> User Interface, you may want to set the "Show Beta Options" switch to "Yes" (to see and use beta features)
On the left side of the WB Project TAB, pick "New Geometry" to start the DesignModeler®, then 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.
Use "Dimensions" in the Sketching Toolbox to dimension the width and height of the rectangle.
In the Details View (lower left), set 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 WBE 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 90o form the bottom horizontal edge to the left vertical edge of the rectangle.
Under "Modify" in the Sketching Toolbox on the left side, use Trim to cut the lines of the rectangle at the intersection with the arc.
Use "Dimensions" in the Sketching Toolbox to dimension the radius of the arc.
In the Details View (lower left), set the proper value for the radius of the arc.
At the top of the DesignModeler® panel:
choose "Concept"
then choose "Surfaces from Sketches"
Pick the 5 lines in your sketch (or you can pick "Sketch1" from the Tree Outline)
Apply Sketch1 as the Base Object,
choose "Add Material" for the Operation
orient with Plane Normal - yes
then ADD the thickness of the part
Click on "Generate" above the Tree Outline and the surface body is created.
Return to the Workbench Project TAB:
Under File -> Save All -> use the same file name "plate1.agdb" and save in the same folder on your permanent (P:\) storage space.
Click on the DesignModeler geometry icon for your new model on the right side of the page
On the left side, expand Advanced Geometry Defaults and change the Analysis Type to 2-D
Under Design Modeler Tasks pick "New Simulation" to start DesignSimulation®. The geometry created in DesignModeler® is automatically transferred to DesignSimulation®.
Immediately, 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), expand the Geometry branch and click on Surface Body. In the Details area, click on Structural Steel and then Edit Structural Steel, to open the Engineering Data TAB. Rename (use right mouse button) "Structural Steel" to " Aluminum"
Click on Add/Remove Properties in the Engineering Data Tab and Remove ALL the properties we won't need for this simulation. Edit the Property Data you wish to include for this simulation (Young's Modulus and Poisson's ratio, then enter the data values of 10E6 psi and 0.32, respectively). ALT: Import a material, find Aluminum Alloy in the "Workbench_Samples"
Return to DesignSimulation® by clicking on its TAB at the top of the WBE screen. Notice that in the Details area you can check dimensions of your model in "Bounding Box" and "Properties"
Click on "Mesh" in the Outline, then in the Details area, set "Relevance": 100; then under "Advanced" set Element Size: 0.25 in; and Shape Checking: Aggressive Mechanical. Then, click RIGHT mouse on Mesh in the Outline and "Generate Mesh"
Click RIGHT mouse on Mesh, then Insert, Sizing. Pick the arc on the hole in the plate, then in the Details area, click on Apply next to "Geometry" under "Scope". Set the element size to 0.05 in and generate the mesh again.
From the top menu: click on "New Analysis" and insert "Static Structural" environment in the tree menu.
Click RIGHT mouse on Static Structural, then Insert, Frictionless Support (for symmetry). Pick one of the straight edges which split the model for symmetry, then in the Details area under "Scope", Apply that edge to this boundary condition. Repeat (make a 2nd Frictionless Support for the other symmetry edge. (WHY make two objects for Frictionless Support ?)
Click RIGHT mouse on Static Structural, then Insert, Force. Pick the straight edge on the right. Then, in the Details areaunder "Scope", Apply that edge to this boundary condition. Use "Components" to define the force, then enter the x-component: 6000 lbf. (WHY use a Force when we used Pressure load before ?)
Click on Analysis Settings, then in the
Details area, set Weak Springs: Off
(a properly constrained model does NOT need weak springs)
Click RIGHT mouse on Solution, then Insert, Stress, Normal Stress. In the Details area, request X Axis Orientation
Click RIGHT mouse on Solution, then Insert, Stress, Equivalent (vonMises) Stress.
Click RIGHT mouse on Solution, then Insert, Deformation, Total
Click RIGHT mouse on Solution, then Insert, Stress, Error
Click RIGHT mouse on Solution, then Insert, Commands:
/SHOW,PNG ! send plots to PNG file350 ! plot file resolution
/GFILE,
Return to the Workbench Project TAB:
Under File -> Save All -> use the same file name "plate1.dsdb" and save in the same folder on your permanent (P:\) storage space.
Return to the Workbench Simulation TAB:
In the Outline, click RIGHT mouse on Solution, then SOLVE
Examine the normal stress, equivalent stress, total deformation, and structural error results.
Click RIGHT mouse 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)
Click RIGHT mouse on Solution, then Insert, Probe, Force Reaction, and scope it to the vertical symmetry plane, frictionless support boundary condition.
Insert FIGURES (in the Tree Outline) for the Geometry, Mesh, Static Structural Environment, and for EACH Solution result. These figure 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.
Below the Graphics area, click on the Report Preview TAB. The report generates automatically. You then fill in your name as author, subject: Plate with a Hole 2D FEA Model, and prepared for: MET 415, "this semester". Then leave the Report Preview TAB and return to force a new generation of the report.
Above the Graphics area, click on Send to > Microsoft Word, save the report as a Word document (change file type to *.doc) on your P:\ drive.
Format it so it will print nicely (don't let figure size push captions onto the next page). Add important information about your analysis.
Add comments regarding the element types used, the overall mesh error, and the local mesh error plot
TURN IN:
this report
Answers to the two BOLD, embedded questions (above)
REMEMBER: On the Engr. PC Network, only the files you save on or move to the P:\ drive are permanent ! Files left on the local drives, C:\ TEMP, will be automatically deleted. You may wish to keep copies of your model for another day. We use the local drives to avoid exceeding the allowable limit on the P:\ drive during a solution (with temporary, scratch files), and for better performance when solving.
Keep the WBE database files: name.wbdb, name.eddb, name.agdb, name.dsdb. These files are: project page, engr. data, geometry, and simulation databases, respectively.
You may also wish to reduce storage required - if so, before saving the simulation database (.dsdb), click right mouse on Solution, then pick "Clean" before saving. (This deletes the solution results and makes a much smaller .dsdb file, but you do have to solve again to look at results during the next session).