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
(OPTIONAL) Utility Menu: File -> you may change jobname and working directory after you start ANSYS
Main Menu: Preprocessor -> Element Type -> Add/Edit/Delete -> Add
-> Structural Solid, Quad 8node 183 -> OK -> Close
Material Props -> Material Library -> Import Library -> Units: BIN -> OK
Read Into Material: 1
Browse for the ANSYS "MATLIB" - in the ANSYS installation directory
Use: Aluminum 6061-T6 -> OK
Close the listing of properties, AFTER YOU EXAMINE THEM !
Modeling -> Create -> -Area- Rectangle -> By Dimensions
Enter dimensions of x= 0 & 6 and y= 0 & 6 -> OK
(what is the difference btw. OK and APPLY ?) ______________________
Modeling -> Create -> -Area- Circle -> By Dimensions
Create a solid circle with radius = 0.5 in. -> OK
Utility Menu: Plot -> Lines
(where did "lines" come from ?) ___________________Toolbar: SAVE_DB
(Where does the DB file get saved ?) ___________________Modeling -> Operate -> Booleans -> Subtract -> Areas
Subtract the circle from the square
- BE CAREFUL - Read the prompts in the ANSYS Input Window
In the Preprocessor menu, -> Meshing -> MeshTool ...
Under "Size Controls", "Global", click on: SET
Enter an "Element edge length" of 0.75 -> OK
(We are setting the overall maximum finite element edge size at 0.75")
Under "Size Controls", "Keypts", click on: SET
Pick the points at both ends of the arc, then -> OK
Set the element edge length at picked keypoints: 0.1 -> OK
(Near the hole, we are requesting smaller elements, higher accuracy)
Toolbar: SAVE_DB
(Where does the DB file get saved ?)In the MeshTool: Set it to mesh: Areas, Quad, Free
then click the Mesh button -> Pick All -> OK
Close the MeshTool
Utility Menu: Plot -> Nodes
Note:
Pan-Zoom & Rotate buttons on the right side of the ANSYS window.
ALSO, use the right mouse button for EITHER a Box Zoom - OR - for a view menu.
Use Zoom or Box Zoom to get a close-up view of the nodes around the hole.
Use the Fit button to
restore the view of the whole model.
Main Menu: Solution
Define Loads -> Apply -> Structural -> Displacement -> Symmetry B.C. -> On Lines
Pick the left edge and the bottom edge -> OK
(why do we pick only 2 edges to define symmetry ?) _____________________________
Define Loads -> Apply -> Structural -> Pressure -> On Lines
Pick the right edge -> OK
Enter a pressure (VALUE) of -1000 (yes, that is minus 1000) -> OK
(a negative pressure acts OUTWARD from elem. faces, i.e. surface traction)
Utility Menu: PlotCtrls -> Symbols ...
Under Boundary Condition Symbols: All Applied B.C.'s = ON
Under Surface Load Symbols: Pressure, As Arrows (instead of Face Outlines)
Utility Menu: Plot -> Lines
Examine the symbols !
Utility Menu: Plot -> Nodes
Define Loads -> Operate -> Transfer to FE -> All Solid Loads -> OK
Examine the symbols (They have changed. Why ?) _________________
Toolbar: SAVE_DB
Solve -> Current LS -> OK
When you see "Solution is Done,"
Close the info box & the /STAT Command box
Main Menu: General Postproc
List Results -> Reaction Solu ... All Items -> OK
Scroll to the Totals. Does the total reaction make sense ?
Plot Results -> Deformed Shape -> Def + undef edge -> OK
Do the observed deformations make sense ? How big is the total deflection ?
Plot Results -> Contour Plot -> Nodal Solu -> Stress, X-direction SX -> OK
OPTIONAL: Utility Menu: PlotCtrls -> Window Controls -> Window Options -> change "Multi Legend" to "Legend ON"
Toolbar: POWRGRPH, and turn off PowerGraphics
(in order to see mesh error quantities)
List Results -> Percent Error
if error quantities are not available, go to "Options for Outp" in the Main Menu and make sure "Error estimation calcs" are ON, then hit "OK"
Plot Results -> Deformed Shape -> Def + undef edge -> OK
(Notice the percent error, SEPC, in the plot legend)
Utility Menu: Plot Ctrls -> Style -> Edge Options ...
change the "All / Edge Only" to "Edge Only / All" -> OK
Utility Menu: Plot -> Replot (what was the effect of changing the edge option setting ?)
Go back to the plot of Stress, X-direction SX, restore the Edge Option setting to "All / Edge Only" then Use Pan-Zoom & Rotate buttons on the right side of the ANSYS window. Zoom up to see the maximum stress. Does this agree with stress concentration theory from Strength of Materials class ?
Plot Results -> Contour Plot -> Element Solu -> Error Estimation, SERR -> OK
(Consider which elements are creating the most error)
Plot Ctrls -> Style -> Symmetry Expansion ->
Periodic/Cyclic Symmetry -> 1/4 Dihedral Symmetry
(to see the entire structure)
Plot Results -> Contour Plot -> Nodal Solu -> Stress, X-direction SX -> OK
Plot Results -> Contour Plot -> Nodal Solu -> Stress, vonMises SEQV -> OK
Toolbar: QUIT, Exit with No Save -> OK
REMEMBER: On the Engr. PC Network, only the files you move to the P:\ drive are permanent ! Files left on the local drives, C:\ and 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.
As a minimum keep the database file (jobname.db). You may also wish to keep the results file (jobname.rst) and the session log file (jobname.log)
Large file can be compressed (zipped) to conserve space. ANSYS binary DB files may compress up to 90% or more. The results file RST can compress as much as 40-50%.