Header Background
Release 11.0 Documentation for ANSYS
Prev Next

Structural Guide | Chapter 15. p-Method Structural Static Analysis |

15.3. Sample p-Method Analysis (GUI Method)

www.kxcad.net Home > CAE Index > ANSYS Index > Release 11.0 Documentation for ANSYS


Your Ad Here

Follow the steps below to perform a p-method analysis using the GUI.

15.3.1. Problem Description

In this sample problem, you will perform a p-method analysis on a steel plate with a hole.

15.3.2. Problem Specifications

For this problem, you will use symmetry boundary conditions to constrain the left side and bottom of the model.

This problem uses element type PLANE145. The material is 1/4" thick steel.

Loading for this problem is: P = (100) (10) (.25) = 250 lbs (total force applied on the right side).

15.3.3. Problem Diagram

Figure 15.8  Steel Plate With a Hole

15.3.3.1. Set the Analysis Title

After you enter the ANSYS program, follow these steps to set the title.

  1. Choose menu path Utility Menu> File> Change Title.

  2. Type the text "p-Method Plate with Hole" and click on OK.

15.3.3.2. Select p-Method

  1. Choose menu path Main Menu> Preferences. The Preferences for GUI Filtering dialog box appears.

  2. Click the Structural method on. Click the p-Method Struct. option on.

  3. Click on OK.

15.3.3.3. Define the Element Type and Options

  1. Choose menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete.

  2. Click on Add. The Library of Element Types dialog box appears.

  3. Click on OK to accept the default of "2D Quad 145."

  4. Click on Options. The PLANE145 element type options dialog box appears.

  5. In the scroll box for Analysis type, scroll down to "Plane Stress+TK" to select it.

  6. Click on OK.

  7. Click on Close in the Element Types dialog box.

15.3.3.4. Define the Real Constants

  1. Choose menu path Main Menu> Preprocessor> Real Constants> Add/Edit/Delete.

  2. Click on Add. The Element Type for Real Constants dialog box appears.

  3. Click on OK. The Real Constants for PLANE145 dialog box appears.

  4. Enter .25 for thickness and click on OK.

  5. Click on Close to close the Real Constants dialog box.

15.3.3.5. Define Material Properties

  1. Choose menu path Main Menu> Preprocessor> Material Props> Material Models. The Define Material Model Behavior dialog box appears.

  2. In the Material Models Available window, double-click on the icons next to the following options: Structural, Linear, Elastic, Isotropic. A dialog box appears.

  3. Enter 30e6 for EX (Young's modulus).

  4. Enter 0.29 for PRXY and click on OK. Material Model Number 1 appears in the Material Models Defined window on the left.

  5. Choose menu path Material> Exit to remove the Define Material Model Behavior dialog box.

15.3.3.6. Create Plate with Hole

  1. Choose menu path Main Menu> Preprocessor> Modeling> Create> Areas> Rectangle> By Dimensions. The Create Rectangle by Dimensions dialog box appears.

  2. Enter 0,20 for the X-coordinates and 0,10 for the Y-coordinates. Use the TAB key to move between fields.

  3. Click on OK. The rectangle appears in the ANSYS Graphics window.

  4. Choose menu path Main Menu> Preprocessor> Modeling> Create> Areas> Circle> By Dimensions. The Circular Area by Dimensions dialog box appears.

  5. Enter 5 for outer radius.

  6. Click on OK. The circle appears on the ANSYS Graphics window, on the lower left corner of the rectangle.

  7. Choose menu path Main Menu> Preprocessor> Modeling> Operate> Booleans> Subtract> Areas. The Subtract Areas picking menu appears.

  8. Click once on the rectangle to select it.

  9. Click on OK in the picking menu. Another Subtract Areas picking menu appears.

  10. Click once on the circle to select it.

  11. Click on OK in the picking menu. A semicircle is removed from the lower left-hand corner of the plate.

15.3.3.7. Mesh the Areas

  1. Choose menu path Main Menu> Preprocessor> Meshing> MeshTool. The MeshTool appears.

  2. Click the SmartSize check box on. Set the SmartSize slider to 5.

  3. In the Mesh section of the MeshTool, choose Areas and Free. Then click the MESH button. The Mesh Areas picking menu appears.

  4. Click on Pick All. A mesh for the plate is created.

  5. Click Close to close the MeshTool.

  6. Click on SAVE_DB on the ANSYS Toolbar.

15.3.3.8. Define Symmetry Boundary Conditions

  1. Choose menu path Utility Menu> Select> Entities.

  2. In the top two menus, pick "Nodes" and "By Location."

  3. Enter 0 for Min, Max and click on OK.

  4. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> Symmetry B.C.> On Nodes. The Apply SYMM on Nodes dialog box appears.

  5. Click on OK to accept the default of symmetric surface normal to X-axis. The displacement symbols appear down the left edge of the drawing.

  6. Choose menu path Utility Menu> Select> Entities.

  7. Click the "Y coordinates" option on. Click OK.

  8. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> Symmetry B.C.> On Nodes. The Apply SYMM on Nodes dialog box appears.

  9. In the drop down menu for Symm surface is normal to, select "Y-axis."

  10. Click OK. The displacement symbols appear along the bottom of the drawing.

15.3.3.9. Define Pressure Load along Right Edge.

  1. Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears.

  2. Click the "X coordinates" option on.

  3. Enter 20 for Min, Max and click on OK.

  4. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Pressure> On Nodes. The Apply PRES on Nodes picking menu appears.

  5. Click on Pick All. The Apply PRES on Nodes dialog box appears.

  6. Enter 100 for pressure value and click on OK.

  7. Choose menu path Utility Menu> Select> Everything.

15.3.3.10. Define Convergence Criteria

  1. Choose menu path Utility Menu> Parameters> Scalar Parameters. The Scalar Parameters dialog box appears.

  2. In the Selection field, enter NCVG = NODE(0,5,0) and click on Accept.

  3. Click on Close.

  4. In the ANSYS Input window, enter PCONV,1,S,X,NCVG and press ENTER.

15.3.3.11. Solve the Problem

  1. Choose menu path Main Menu> Solution> Solve> Current LS.

  2. Carefully review the information in the status window, and then close it.

  3. Click on OK in the Solve Current Load Step dialog box to begin the solution.

  4. Click on Close when the Solution is done window appears.

15.3.3.12. Review the Results and Exit ANSYS

In this step, you will review results as deformed shape and SX contour plot.

  1. Choose menu path Main Menu> General Postproc> Read Results> First Set.

  2. Choose menu path Main Menu> General Postproc> Plot Results> Deformed Shape. The Plot Deformed Shape dialog box appears.

  3. Click the "Def + undeformed" option on. Click on OK. The deformed and undeformed shapes appear in the ANSYS Graphics window.

  4. Choose menu path Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu. The Contour Nodal Solution Data dialog box appears.

  5. In the scroll box on the left, click once on "Stress" to select it. In the scroll box on the right, click once on "X-direction SX" to select it.

  6. Click on OK. Review the graphic using the legend in the graphics window. Expected results are: Max displacement = .97x10-4 in, and Max stress in X direction = 437 psi.

  7. Click on QUIT on the ANSYS Toolbar.

  8. Choose a save option and click on OK.

Prev
15.2. Using the p-Method		Up / HomeNext
15.4. Sample p-Method Analysis (Command or Batch Method)
Your Ad Here