To bottom

MENG 421 Assignment 9

Ansys in graphical mode: Stressed plate with hole

Prev Lesson   MENG 421 | Class assignments | 1 2 3 4 5 6 8 9 10 11 12   Next Lesson

Lecture notes -- Milestones, 1, Failure, Plane42, Plane55, Plane82,
End support, Full support, Correct, Wrong, Capture, Mesh size  

In this lesson, you use Ansys in graphics mode to model a square plate with a hole. You will use the 8-node Plane82 element that is similar to the 4-node Plane42 element that you used for Assignment 4. You can use Plane82 in axisymmetric mode to create rods and pipes like you did with Plane42 for Assignment 4. Because there are eight nodes, the element sides are parabolas rather than straight lines. For previous labs, you ran Ansys with a batch file, only occasionally typing in commands. By contrast, for today's assignment, you work entirely with the keyboard and mouse rather than using a batch file. You will define the Element Type, Real Constants, and Material Properties as you have done previously in batch mode. But you will select these items from menus.

In the next lesson, Assignment 10, you will apply a load to this model and determine the deformation and stresses. Because of symmetry, we will only model one quarter of the plate. This will save computer time and show more detail. Be careful however to properly support the lower and left edges of our quarter mode.

Original plate with hole Model of one-quarter of plate

That is, we take the plate shown in left figure and cut out the upper-right quarter for our model shown in the right figure. Then we will load the quarter model on the right edge and constrain the model on the left and lower edges where the model meet the remainder of the original plate. The lower edge can move right but not down. Similarly, the left edge can move up but not to the left. You must be careful to chose one-dimensional (roller) supports not only at the ends but also at each node. If the supports are incorrect, the edges will not be straight.

First, you will let Ansys automatically create the mesh. Then you will refine that mesh around the hole. Finally, you will print a graphic of the meshed plate.

You will create the first figure below in today's lesson and the others in the next lesson. Click the figures to enlarge them.

If you find the lower part of a window off the screen, hold the Alt key while pressing the Space Bar. Release both keys and press the M key. Now you can move the window by pressing the cursor arrows. For example, press the up arrow to raise the window. Press Enter when the window is in the new position or press the Esc key to cancel this action.

Constraints for plate, click to enlarge Deflection in plate, click to enlarge Stress in plate, click to enlarge

  1. Before starting Ansys be sure that your directory has at least 1.5 MB of free space. Otherwise, you will not be able to save your work for next week.
  2. You learned how to change the screen resolution in Assignment 1. Check that the screen resolution is 1024x768x16 (High Color).
  3. Point a copy of Explorer to C:\WINDOWS\Temp and clear all files. Today you will make frequent copies of the Ansys file named file.log because this is where Ansys keeps a copy of all the keyboard commands you type. Then you can easily rerun your work from the resulting batch file.
  4. Start Ansys
  5. Utility Menu: File | Change Jobname | Plate82 | OK
  6. Utility Menu: File | Change Title | (Put the usual here -- Plate 82 with hole, your name, and the date) | OK
    Your file.log now looks like this
  7. Notice that the Ansys Main Menu has the familiar items Preprocessor, Solution, and General Postsproc. We will use these items to define the element type, reals, material properties, nodes, elements, etc, as we have done previously in batch mode.
  8. Main Menu: Preferences | Structural | OK
  9. Main Menu: Preprocessor | Element Type | Add/Edit/Delete
  10. Element Types: Add
  11. Structural Solid -- Quad 8Node 82 (notice that there is a 4Node 42) | OK
  12. Element Types: (Check that Element Type 1 is defined as Plane 82) Options
  13. Element behavior K3 -- click dropdown and select Plane strs w/thk | OK
  14. Element Types: Close
  15. Preprocessor: Real Constants | Add/Edit/Delete | Add
  16. Check for Type 1 Plane 82 | OK
  17. Set Thickness THK to 0.25 | Apply
  18. To learn more about Element 82 click Help. You can see the curving sides of the elements. File | Exit
  19. Real Constant Set: OK
  20. Real Constants: Close
  21. Preprocessor: Material Props |Material Models to get the Define Material Model Behavior dialog box. On left side check for Material Model Number 1.
  22. On right side, double-click structural to expand it like this.
  23. Double-click Linear to expand it.
  24. Double-click Elastic to expand it.
  25. Double-click Isotropic to get the dialog box.
  26. For EX (elastic modulus) enter the value 29e6.
  27. For PRXY (Poisson's ratio) enter the value 0.3.
  28. Click OK
  29. Close Define Material ... by clicking Material, Exit.
  30. Close Material Properties window.
  31. First, save a batch file of your commands so far
  32. Ansys Toolbar: SAVE_DB to save a binaray copy your work so far. There is now a 1-MB file named Plate82.db at C:\WINDOWS\Temp (or where ever set you Ansys workspace). You can quit now and continue later with this file.

  33. Now that you have defined the element type, real, and material properties, you can define the nodes and elements.
  34. Preprocessor: Modeling -- Create
  35. Utility Menu: PlotCtrls | Pan, Zoom, Rotate | (click small dot to zoom out)
  36. Utility Menu: PlotCtrls | Numbering | Area numbers ON (click white box next to Off) | OK
  37. Utility Menu: Plot | Lines (Figure shows lines)
  38. Preprocessor: -Modeling- Create
  39. Now we have to subtract the circle from the square --
  40. Make another copy of file.log and name it Plate40.a
  41. Ansys Toolbar: SAVE_DB to save your work in binary
  42. Preprocessor: MeshTool
  43. MeshTool: Size controls: Global Set
  44. Global Element Sizes: SIZE 1.5 | OK
  45. MeshTool: (4th section down) Mesh: Areas | Mesh
  46. Mesh Area menu: Pick All
    Your meshed plate should look like this.
    As you know, the stresses are greatest around the hole, so there should be smaller elements there. But, as you can see, the elements are all about the same size. Therefore, let us refine the mesh.
  47. MeshTool: Refine -- at Nodes | Refine
  48. Watch Refine mesh menu while you pick the three nodes around the hole | check for Count = 3 | OK |
  49. Refine Mesh at Node: Choose refinement level 2 | OK
    Your meshed plate should look like the second one. Notice how the elements are now smaller around the hole.
  50. MeshTool: Close
  51. Make the background black by typing the Ansys command
    Then click the Plot menu and pick Replot.
  52. Make copy of file.log that has all your typed commands, name it Plate52.a, and print it.
  53. Save your work in binary for next time. It will take about 900 KB of space.
    Utility Menu: File | Save as | Plate82.db |
    Be sure to save your file on the Ansys directory of Drive U. Otherwise, your work is saved on the local PC you are currently working on OK
  54. Capture and print your meshed plate.
  55. You went through a lot of material today. Therefore, you might want to clear Ansys and redo the above lesson.
    Utility Menu: File | Clear & Start New
  56. When you are finished, Toolbar: Quit | Quit - no save | OK

  57. Assignment
    Create a cover sheet describing what you did and discuss stress concentration. Include a graphic of your meshed plate and your list of commands from the log file. Compare this lab with the previous ones where you used a batch file and typed lines of keyboard input. Do not combine with Lesson 10. Turn in the package as specified at the lab.

 To top

Prev Lesson   MENG 421 | Ansys | Lectures | Class assignments | 1 2 3 4 5 6 8 9 10 11 12   Next Lesson

Revised: March 31, 2004 -- Copyright 1997-2004 ARMiller