2.4. A Sample Static Analysis (GUI Method)

Students Hands-On: Static Analysis of an Allen Wrench

In this example, you will learn how to do the following:

How to define a scalar parameter and simple computations?
How to use Select/Entities to select subregions with combined constraints?
How to automatically calculate a coordinate range (minyval,maxyval)?
How to create 3D mesh by dragging a 2D mesh along lines?
How to display pressure load by PlotCtrls?
How to define multiple load steps by Write LS File?

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.

Problem Sketch

Figure 1. Diagram of Allen wrench

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

Step 1. Set the Analysis Title

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

2. Type the text "Static Analysis of an Allen Wrench" and click on OK.

Step 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. The command appears in the upper text block of the ANSYS Input window.

3. Choose 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 on OK.

Step 3. Define Parameters

1. Choose 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 on Accept after you define each parameter. For example, first type “exx = 2.07e11” in the Selection field and then click on Accept. Continue entering the remaining parameters and values in the same way.

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

Note: You can type the labels in upper- or lower-case; ANSYS always displays the labels in upper-case.

3. Click on Close.

4. Click on SAVE_DB on the ANSYS Toolbar.

Step 4. Define the Element Types

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. In the scroll box on the left, click once on "Structural Solid."

4. In the scroll box on the right, click once on "Brick 8node 45."

5. Click on Apply to define it as element type 1.

6. Scroll up the list on the right to "Quad 4node 42." Click once to select it.

7. Click on OK to define Quad 4node42 as element type 2. The Library of Element Types dialog box closes.

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

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

Step 6. Create Hexagonal Area as Cross-Section

1. Choose 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 on OK. A hexagon appears in the ANSYS Graphics window.

Step 7. Create Keypoints Along a Path

1. Choose 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 on Apply.

4. Enter 8 for keypoint number.

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

6. Enter 9 for keypoint number.

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

Step 8. Create Lines Along a Path

1. Choose 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 on OK.

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

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

6. Choose 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 on OK.

10. Choose 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 on OK.

14. Choose 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 ANSYS 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 on OK.

Step 9. Create Line from Shank to Handle

1. Choose 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 on OK in the picking menu. The Line Fillet dialog box appears.

4. Enter BENDRAD for Fillet radius and click on OK.

5. Click on SAVE_DB on the ANSYS Toolbar.

Step 10. Cut Hex Section

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

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

2. Click the Keypoint numbers radio button to Off.

3. Click on OK.

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

5. Choose 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 on OK.

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

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

9. Click on 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. Choose 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 on OK.

Step 11. Set Meshing Density

1. Choose 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 on 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 on OK.

Step 12. Set Element Type for Area Mesh

In this step, set the element type to PLANE42, all quadrilaterals for the area mesh.

1. Choose 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 PLANE42” and click on OK.

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

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

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

6. Click on SAVE_DB on the ANSYS Toolbar.

Step 13. Generate Area Mesh

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

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

2. Click on Pick All.

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

Step 14. Drag the 2D Mesh to Produce 3D Elements

1. Choose 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 SOLID45” and click on OK.

3. Choose 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 on OK.

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

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

7. Click on OK.

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

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

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

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

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

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

14. Click on SAVE_DB on the ANSYS Toolbar.

Step 15. Select BOTAREA Component and Delete 2D Elements

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

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

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

4. Click on Pick All.

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

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

Step 16. Apply Displacement Boundary Condition at End of Wrench

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

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

3. Choose 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 on Apply.

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

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

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

10. Click on OK.

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

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

13. In the scroll list for DOFs to be constrained, click on "ALL DOF."

14. Click on OK.

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

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

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

Step 17. Display Boundary Conditions

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

2. Click on 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 on OK.

Step 18. Apply Pressure on Handle

In this step, apply pressure on the handle to represent 100 N finger force. Note that the nodes where the pressure is applied are selected by the following steps: a) Select the handle surface; b) select the front side of the handle surface; c) select the nodes on that side; d) finally narrow down to just those nodes covering 3-element length at the end of the handle. The magnitude of the pressure is calculated by the total force divided by the effective normal area.

1. Choose 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 on the "Y coordinates" radio button to select it.

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

6. Click on "X coordinates" to select it.

7. Click on Reselect.

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

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

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

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

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

13. Click on Apply.

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

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

16. Click on the "Reselect" radio button.

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

18. Click on OK.

19. Choose 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 on 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 on Apply.

27. Click on 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 on OK.

32. Choose 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 on Accept.

34. Click on Close.

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

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

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

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

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

40. Click on SAVE_DB on the ANSYS Toolbar.

Step 19. Write the First Load Step

1. Choose 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 on OK.

Step 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. Choose 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 on Accept.

3. Click on Close.

4. Choose 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 on the "Z coordinates" radio button to select it.

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

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

10. Click on Apply.

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

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

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

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

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

16. Click on the "Reselect" radio button.

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

18. Click on OK.

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

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

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

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

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

Step 21. Write Second Load Step

1. Choose 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 on OK.

3. Click on SAVE_DB on the ANSYS Toolbar.

Step 22. Solve from Load Step Files

1. Choose 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 on OK.

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

Step 23. Read First Load Step and Review Results

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

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

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

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

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

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

7. Choose 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 on OK.

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

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

12. Choose 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 on OK.

14. Choose 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 on OK.

19. Choose 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 on "Stress." In the scroll box on the right, click on "Intensity SINT." (For stress intensity)

21. Click on OK.

22. Choose 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 on OK.

Step 24. Read the Next Load Step and Review Results

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

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

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

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

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

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

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

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

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

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

11. Choose 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 on "Stress." In the scroll box on the right, scroll to "Intensity SINT" and select it.

13. Click on OK.

Step 25. Zoom in on Cross-Section

1. Choose 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 on OK.

3. Choose 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 on OK.

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

8. Click on "WP."

9. Drag the Rate slider bar to 10.

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

Step 26. Exit ANSYS

1. Choose QUIT from the ANSYS Toolbar.

2. Choose Quit - No Save!

3. Click on OK.

The ANSYS Log file for this problem may be found here.