2.3. Example: Static Analysis (GUI Method)

Following is an example static analysis of an Allen wrench.

 

2.3.1. Problem Description

An Allen wrench (10 mm across the flats) is torqued by means of a 100 N force at its end. Later, a 20 N downward force is applied at the same end, at the same time retaining the original 100 N torquing force. The objective is to determine the stress intensity in the wrench under these two loading conditions.

 

2.3.2. Problem Specifications

The following dimensions are used for this problem:

Width across flats = 10 mm

Configuration = hexagonal

Length of shank = 7.5 cm

Length of handle = 20 cm

Bend radius = 1 cm

Modulus of elasticity = 2.07 x 1011 Pa

Applied torquing force = 100 N

Applied downward force = 20 N

 

2.3.3. Problem Sketch

Figure 2.1: Diagram of Allen Wrench

Diagram of Allen Wrench

 

2.3.3.1. Set the Analysis Title

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

  2. Type Static Analysis of an Allen Wrench and click OK.

 

2.3.3.2. Set the System of Units

  1. Click once in the Input Window to make it active for text entry.

  2. Type the command /UNITS,SI and press ENTER. Notice that the command is stored in the history buffer, which can be accessed by clicking on the down arrow at the right of the input window.

  3. Select menu path Utility Menu> Parameters> Angular Units. The Angular Units for Parametric Functions dialog box appears.

  4. In the drop-down menu for Units for angular parametric functions, select Degrees DEG.

  5. Click OK.

 

2.3.3.3. Define Parameters

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

  2. Type the following parameters and their values in the Selection field. Click Accept after you define each parameter. For example, first type "exx = 2.07e11" in the Selection field and then click Accept. Continue entering the remaining parameters and values in the same way.

    Parameter Value Description
    EXX2.07E11Young's modulus is 2.07E11 Pa
    W_HEX.01Width of hex across flats = .01 m
    W_FLAT W_HEX* TAN(30)Width of flat = .0058 m
    L_SHANK.075Length of shank (short end) .075 m
    L_HANDLE.2Length of handle (long end) .2 m
    BENDRAD.01Bend radius .01 m
    L_ELEM.0075 Element length .0075 m
    NO_D_HEX2Number of divisions along hex flat = 2
    TOL25E-6Tolerance for selecting node = 25E-6 m

    Note:  You can type the labels in upper- or lowercase; Mechanical APDL always displays the labels in uppercase.

  3. Click Close.

  4. Click SAVE_DB on the Toolbar.

 

2.3.3.4. Define the Element Types

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

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

  3. In the scroll box on the left, click Structural Solid.

  4. In the scroll box on the right, click Brick 8node 185.

  5. Click OK to define it as element type 1. The Library of Element Types dialog box closes.

  6. Click Options. The SOLID185 element type options dialog box appears.

  7. In the element technology scroll box, scroll to Simple Enhanced Str and select it.

  8. Click OK. The element type options dialog box closes. Click Add in the element types box.

  9. Scroll up the list on the right to Quad 4node 182. Click once to select it.

  10. Click OK to define Quad 4node182 as element type 2. The Library of Element Types dialog box closes.

  11. Click Options. The PLANE182 element type options dialog box appears.

  12. In the scroll box for element technology, scroll to Simple Enhanced Str and select it.

  13. Click Close in the Element Types dialog box.

 

2.3.3.5. Define Material Properties

  1. Select 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 the following options: Structural, Linear, Elastic, Isotropic. A dialog box appears.

  3. Type the text EXX in the EX field (for Young's modulus), and .3 for PRXY.

    Click OK. This sets Young's modulus to the parameter specified above. Material Model Number 1 appears in the Material Models Defined window on the left.

  4. Select menu path Material> Exit to remove the Define Material Model Behavior dialog box.

 

2.3.3.6. Create Hexagonal Area as Cross-Section

  1. Select menu path Main Menu> Preprocessor> Modeling> Create> Areas> Polygon> By Side Length. The Polygon by Side Length dialog box appears.

  2. Enter 6 for number of sides.

  3. Enter W_FLAT for length of each side.

  4. Click OK. A hexagon appears in the Graphics window.

 

2.3.3.7. Create Keypoints Along a Path

  1. Select menu path Main Menu> Preprocessor> Modeling> Create> Keypoints> In Active CS. The Create Keypoints in Active Coordinate System dialog box appears.

  2. Enter 7 for keypoint number. Type a 0 in each of the X, Y, Z location fields.

  3. Click Apply.

  4. Enter 8 for keypoint number.

  5. Enter 0,0,-L_SHANK for the X, Y, Z location, and click Apply.

  6. Enter 9 for keypoint number.

  7. Enter 0,L_HANDLE,-L_SHANK for the X, Y, Z location, and click OK.

 

2.3.3.8. Create Lines Along a Path

  1. Select menu path Utility Menu> PlotCtrls> Window Controls> Window Options. The Window Options dialog box appears.

  2. In the Location of triad drop-down menu, select "At top left."

  3. Click OK.

  4. Select menu path Utility Menu> PlotCtrls> Pan/Zoom/Rotate. The Pan-Zoom-Rotate dialog box appears.

  5. Click Iso to generate an isometric view and click Close.

  6. Select menu path Utility Menu> PlotCtrls> View Settings> Angle of Rotation. The Angle of Rotation dialog box appears.

  7. Enter 90 for angle in degrees.

  8. In the Axis of rotation drop-down menu, select Global Cartes X.

  9. Click OK.

  10. Select menu path Utility Menu> PlotCtrls> Numbering. The Plot Numbering Controls dialog box appears.

  11. Click the Keypoint numbers radio button to turn keypoint numbering on.

  12. Click the Line numbers radio button to turn line numbering on.

  13. Click OK.

  14. Select menu path Main Menu> Preprocessor> Modeling> Create> Lines> Lines> Straight Line. The Create Straight Line picking menu appears.

  15. Click once on keypoints 4 and 1 to create a line between keypoints 1 and 4. (If you have trouble reading the keypoint numbers in the Graphics window, use the controls on the Pan-Zoom-Rotate dialog box (Utility Menu> PlotCtrls> Pan/Zoom/Rotate) to zoom in.)

  16. Click once on keypoints 7 and 8 to create a line between keypoints 7 and 8.

  17. Click once on keypoints 8 and 9 to create a line between keypoints 8 and 9.

  18. Click OK.

 

2.3.3.9. Create Line from Shank to Handle

  1. Select menu path Main Menu> Preprocessor> Modeling> Create> Lines> Line Fillet. The Line Fillet picking menu appears.

  2. Click once on lines 8 and 9.

  3. Click OK in the picking menu. The Line Fillet dialog box appears.

  4. Enter BENDRAD for Fillet radius and click OK.

  5. Click SAVE_DB on the Toolbar.

 

2.3.3.10. Cut Hex Section

In this step, you cut the hex section into two quadrilaterals. This step is required to satisfy mapped meshing.

  1. Select menu path Utility Menu> PlotCtrls> Numbering. The Plot Numbering Controls dialog box appears.

  2. Click the Keypoint numbers radio button to Off.

  3. Click OK.

  4. Select menu path Utility Menu> Plot> Areas.

  5. Select menu path Main Menu> Preprocessor> Modeling> Operate> Booleans> Divide> With Options> Area by Line. The Divide Area by Line picking menu appears.

  6. Click once on the shaded area, and click OK.

  7. Select menu path Utility Menu> Plot> Lines.

  8. Click once on line 7. (If you have trouble reading the line numbers in the Graphics window, use the controls on the Pan-Zoom-Rotate dialog box (Utility Menu> PlotCtrls> Pan/Zoom/Rotate) to zoom in.)

  9. Click OK. The Divide Area by Line with Options dialog box appears. In the Subtracted lines will be drop-down menu, select Kept. Click OK.

  10. Select menu path Utility Menu> Select> Comp/Assembly> Create Component. The Create Component dialog box appears.

  11. Enter BOTAREA for component name.

  12. In the Component is made of drop-down menu, select Areas.

  13. Click OK.

 

2.3.3.11. Set Meshing Density

  1. Select menu path Main Menu> Preprocessor> Meshing> Size Cntrls> Lines> Picked Lines. The Element Size on Picked Lines picking menu appears.

  2. Enter 1,2,6 in the picker, then press ENTER.

  3. Click OK in the picking menu. The Element Sizes on Picked Lines dialog box appears.

  4. Enter NO_D_HEX for number of element divisions and click OK.

 

2.3.3.12. Set Element Type for Area Mesh

In this step, set the element type to PLANE182, all quadrilaterals for the area mesh.

  1. Select menu path Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes. The Element Attributes dialog box appears.

  2. In the Element type number drop-down menu, select "2 PLANE182" and click OK.

  3. Select menu path Main Menu> Preprocessor> Meshing> Mesher Opts. The Mesher Options dialog box appears.

  4. In the Mesher Type field, click the Mapped radio button and then click OK. The Set Element Shape dialog box appears.

  5. Click OK to accept the default of Quad for 2D shape key.

  6. Click SAVE_DB on the Toolbar.

 

2.3.3.13. Generate Area Mesh

In this step, generate the area mesh you will later drag.

  1. Select menu path Main Menu> Preprocessor> Meshing> Mesh> Areas> Mapped> 3 or 4 sided. The Mesh Areas picking box appears.

  2. Click Pick All.

  3. Select menu path Utility Menu> Plot> Elements.

 

2.3.3.14. Drag the 2D Mesh to Produce 3D Elements

  1. Select menu path Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes. The Element Attributes dialog box appears.

  2. In the Element type number drop-down menu, select "1 SOLID185" and click OK.

  3. Select menu path Main Menu> Preprocessor> Meshing> Size Cntrls> Global> Size. The Global Element Sizes dialog box appears.

  4. Enter L_ELEM for element edge length and click OK.

  5. Select menu path Utility Menu> PlotCtrls> Numbering.

  6. Click the Line numbers radio button to on if it is not already selected.

  7. Click OK.

  8. Select menu path Utility Menu> Plot> Lines.

  9. Select menu path Main Menu> Preprocessor> Modeling> Operate> Extrude> Areas> Along Lines. The Sweep Areas along Lines picking box appears.

  10. Click Pick All. A second picking box appears.

  11. Click once on lines 8, 10, and 9 (in that order).

  12. Click OK. The 3D model appears in the Graphics window.

  13. Select menu path Utility Menu> Plot> Elements.

  14. Click SAVE_DB on the Toolbar.

 

2.3.3.15. Select BOTAREA Component and Delete 2D Elements

  1. Select menu path Utility Menu> Select> Comp/Assembly> Select Comp/Assembly. The Select Component or Assembly dialog appears.

  2. Click OK to accept the default of select BOTAREA component.

  3. Select menu path Main Menu> Preprocessor> Meshing> Clear> Areas. The Clear Areas picking menu appears.

  4. Click Pick All.

  5. Select menu path Utility Menu> Select> Everything.

  6. Select menu path Utility Menu> Plot> Elements.

 

2.3.3.16. Apply Displacement Boundary Condition at End of Wrench

  1. Select menu path Utility Menu> Select> Comp/Assembly> Select Comp/Assembly. The Select Component or Assembly dialog appears.

  2. Click OK to accept the default of select BOTAREA component.

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

  4. In the top drop-down menu, select Lines.

  5. In the second drop-down menu, select Exterior.

  6. Click Apply.

  7. In the top drop-down menu, select Nodes.

  8. In the second drop-down menu, select "Attached to."

  9. Click the "Lines, all" radio button to select it.

  10. Click OK.

  11. Select menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. The Apply U,ROT on Nodes picking menu appears.

  12. Click Pick All. The Apply U,ROT on Nodes dialog box appears.

  13. In the scroll list for degrees of freedom to be constrained, click ALL DOF.

  14. Click OK.

  15. Select menu path Utility Menu> Select> Entities.

  16. In the top drop-down menu, select Lines.

  17. Click the Sele All button, then click Cancel.

 

2.3.3.17. Display Boundary Conditions

  1. Select menu path Utility Menu> PlotCtrls> Symbols. The Symbols dialog box appears.

  2. Click the All Applied BCs radio button for Boundary condition symbol.

  3. In the Surface Load Symbols drop-down menu, select Pressures.

  4. In the "Show pres and convect as" drop-down menu, select Arrows.

  5. Click OK.

 

2.3.3.18. Apply Pressure on Handle

In this step, apply pressure on the handle to represent 100 N finger force.

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

  2. In the top drop-down menu, select Areas.

  3. In the second drop-down menu, select By Location.

  4. Click the "Y coordinates" radio button to select it.

  5. Enter BENDRAD,L_HANDLE for Min, Max, and click Apply.

  6. Click "X coordinates" to select it.

  7. Click Reselect.

  8. Enter W_FLAT/2,W_FLAT for Min, Max, and click Apply.

  9. In the top drop-down menu, select Nodes.

  10. In the second drop-down menu, select "Attached to."

  11. Click the "Areas, all" radio button to select it.

  12. Click the "From Full" radio button to select it.

  13. Click Apply.

  14. In the second drop-down menu, select By Location.

  15. Click the "Y coordinates" radio button to select it.

  16. Click the "Reselect" radio button.

  17. Enter L_HANDLE+TOL,L_HANDLE-(3.0*L_ELEM)-TOL for Min, Max.

  18. Click OK.

  19. Select menu path Utility Menu> Parameters> Get Scalar Data. The Get Scalar Data dialog box appears.

  20. In the scroll box on the left, scroll to Model Data and select it.

  21. In the scroll box on the right, scroll to "For selected set" and select it.

  22. Click OK. The Get Data for Selected Entity Set dialog box appears.

  23. Enter minyval for the name of the parameter to be defined.

  24. In the scroll box on the left, click once on "Current node set" to select it.

  25. In the scroll box on the right, click once on "Min Y coordinate" to select it.

  26. Click Apply.

  27. Click OK again to select the default settings. The Get Data for Selected Entity Set dialog box appears.

  28. Enter maxyval for the name of the parameter to be defined.

  29. In the scroll box on the left, click once on "Current node set" to select it.

  30. In the scroll box on the right, click once on "Max Y coordinate" to select it.

  31. Click OK.

  32. Select menu path Utility Menu> Parameters> Scalar Parameters. The Scalar Parameters dialog box appears.

  33. Type the text PTORQ=100/(W_HEX*(MAXYVAL-MINYVAL)) in the Selection text box and click Accept.

  34. Click Close.

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

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

  37. Enter PTORQ for Load PRES value and click OK.

  38. Select menu path Utility Menu> Select> Everything.

  39. Select menu path Utility Menu> Plot> Nodes.

  40. Click SAVE_DB on the Toolbar.

 

2.3.3.19. Write the First Load Step

  1. Select menu path Main Menu> Solution> Load Step Opts> Write LS File. The Write Load Step File dialog appears.

  2. Enter 1 for load step file number n.

  3. Click OK.

 

2.3.3.20. Define Downward Pressure

In this step, you define the downward pressure on top of the handle, representing 20N (4.5 lb) of force.

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

  2. Type the text PDOWN=20/(W_FLAT*(MAXYVAL-MINYVAL)) in the Selection text box and click Accept.

  3. Click Close.

  4. Select menu path Utility Menu> Select> Entities. The Select Entities dialog appears.

  5. In the top drop-down menu, select Areas.

  6. In the second drop-down menu, select By Location.

  7. Click the "Z coordinates" radio button to select it.

  8. Click the "From Full" radio button to select it.

  9. Enter -(L_SHANK+(W_HEX/2)) for Min, Max.

  10. Click Apply.

  11. In the top drop-down menu, select Nodes.

  12. In the second drop-down menu, select "Attached to."

  13. Click the Areas, all radio button to select it, and click Apply.

  14. In the second drop-down menu, select By Location.

  15. Click the "Y coordinates" radio button to select it.

  16. Click the "Reselect" radio button.

  17. Enter L_HANDLE+TOL,L_HANDLE-(3.0*L_ELEM)-TOL for Min, Max.

  18. Click OK.

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

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

  21. Enter PDOWN for Load PRES value and click OK.

  22. Select menu path Utility Menu> Select> Everything.

  23. Select menu path Utility Menu> Plot> Nodes.

 

2.3.3.21. Write Second Load Step

  1. Select menu path Main Menu> Solution> Load Step Opts> Write LS File. The Write Load Step File dialog box appears.

  2. Enter 2 for Load step file number n, and click OK.

  3. Click SAVE_DB on the Toolbar.

 

2.3.3.22. Solve from Load Step Files

  1. Select menu path Main Menu> Solution> Solve> From LS Files. The Solve Load Step Files dialog box appears.

  2. Enter 1 for Starting LS file number.

  3. Enter 2 for Ending LS file number, and click OK.

  4. Click the Close button after the Solution is done! window appears.

 

2.3.3.23. Read First Load Step and Review Results

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

  2. Select menu path Main Menu> General Postproc> List Results> Reaction Solu. The List Reaction Solution dialog box appears.

  3. Click OK to accept the default of All Items.

  4. Review the information in the status window, and click Close.

  5. Select menu path Utility Menu> PlotCtrls> Symbols. The Symbols dialog box appears.

  6. Click the "None" radio button for Boundary condition symbol, and click OK.

  7. Select menu path Utility Menu> PlotCtrls> Style> Edge Options. The Edge Options dialog box appears.

  8. In the Element outlines for non-contour/contour plots drop-down menu, select Edge Only/All.

  9. Click OK.

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

  11. Click the "Def + undeformed" radio button and click OK.

  12. Select menu path Utility Menu> PlotCtrls> Save Plot Ctrls. The Save Plot Controls dialog box appears.

  13. Type pldisp.gsa in the Selection box, and click OK.

  14. Select menu path Utility Menu> PlotCtrls> View Settings> Angle of Rotation. The Angle of Rotation dialog box appears.

  15. Enter 120 for Angle in degrees.

  16. In the Relative/absolute drop-down menu, select "Relative angle."

  17. In the Axis of rotation drop-down menu, select Global Cartes Y.

  18. Click OK.

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

  20. In the scroll box on the left, click Stress. In the scroll box on the right, click Intensity SINT.

  21. Click OK.

  22. Select menu path Utility Menu> PlotCtrls> Save Plot Ctrls. The Save Plot Controls dialog box appears.

  23. Type plnsol.gsa in the Selection box, and click OK.

 

2.3.3.24. Read the Next Load Step and Review Results

  1. Select menu path Main Menu> General Postproc> Read Results> Next Set.

  2. Select menu path Main Menu> General Postproc> List Results> Reaction Solu. The List Reaction Solution dialog box appears.

  3. Click OK to accept the default of All Items.

  4. Review the information in the status window, and click Close.

  5. Select menu path Utility Menu> PlotCtrls> Restore Plot Ctrls.

  6. Type pldisp.gsa in the Selection box, and click OK.

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

  8. Click the "Def + undeformed" radio button if it is not already selected and click OK.

  9. Select menu path Utility Menu> PlotCtrls> Restore Plot Ctrls.

  10. Type plnsol.gsa in the Selection box, and click OK.

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

  12. In the scroll box on the left, click Stress. In the scroll box on the right, scroll to Intensity SINT and select it.

  13. Click OK.

 

2.3.3.25. Zoom in on Cross-Section

  1. Select menu path Utility Menu> WorkPlane> Offset WP by Increments. The Offset WP tool box appears.

  2. Enter 0,0,-0.067 for X, Y, Z Offsets and click OK.

  3. Select menu path Utility Menu> PlotCtrls> Style> Hidden Line Options. The Hidden-Line Options dialog box appears.

  4. In the drop-down menu for Type of Plot, select "Capped hidden."

  5. In the drop-down menu for Cutting plane is, select "Working plane."

  6. Click OK.

  7. Select menu path Utility Menu> PlotCtrls> Pan-Zoom-Rotate. The Pan-Zoom-Rotate tool box appears.

  8. Click WP.

  9. Drag the Rate slider bar to 10.

  10. On the Pan-Zoom-Rotate dialog box, click the large round dot several times to zoom in on the cross section.

 

2.3.3.26. Exit Mechanical APDL

  1. Select QUIT from the Toolbar.

  2. Select Quit - No Save!

  3. Select OK.