Following is an example static analysis of an Allen wrench.
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.
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
Select menu path .
Type the text "Static Analysis of an Allen Wrench" and click on OK.
Click once in the Input Window to make it active for text entry.
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.
Select menu path . The Angular Units for Parametric Functions dialog box appears.
In the drop down menu for Units for angular parametric functions, select "Degrees DEG."
Click on OK.
Select menu path . The Scalar Parameters dialog box appears.
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 lowercase; Mechanical APDL always displays the labels in uppercase.
Click on Close.
Click on SAVE_DB on the Toolbar.
Select menu path .
Click on Add. The Library of Element Types dialog box appears.
In the scroll box on the left, click once on "Structural Solid."
In the scroll box on the right, click once on "Brick 8node 185."
Click on OK to define it as element type 1. The Library of Element Types dialog box closes.
Click on Options. The SOLID185 element type options dialog box appears.
In the element technology scroll box, scroll to "Simple Enhanced Str" and select it.
Click OK. The element type options dialog box closes. Click on Add in the element types box.
Scroll up the list on the right to "Quad 4node 182." Click once to select it.
Click on OK to define Quad 4node182 as element type 2. The Library of Element Types dialog box closes.
Click on Options. The PLANE182 element type options dialog box appears.
In the scroll box for element technology, scroll to "Simple Enhanced Str" and select it.
Click on Close in the Element Types dialog box.
Select menu path . The Define Material Model Behavior dialog box appears.
In the Material Models Available window, double-click on the following options: Structural, Linear, Elastic, Isotropic. A dialog box appears.
Type the text EXX in the EX field (for Young's modulus), and .3 for PRXY.
Click on . This sets Young's modulus to the parameter specified above. Material Model Number 1 appears in the Material Models Defined window on the left.
Select menu path to remove the Define Material Model Behavior dialog box.
Select menu path . The Polygon by Side Length dialog box appears.
Enter 6 for number of sides.
Enter W_FLAT for length of each side.
Click on OK. A hexagon appears in the Graphics window.
Select menu path . The Create Keypoints in Active Coordinate System dialog box appears.
Enter 7 for keypoint number. Type a 0 in each of the X, Y, Z location fields.
Click on Apply.
Enter 8 for keypoint number.
Enter 0,0,-L_SHANK for the X, Y, Z location, and click on Apply.
Enter 9 for keypoint number.
Enter 0,L_HANDLE,-L_SHANK for the X, Y, Z location, and click on OK.
Select menu path . The Window Options dialog box appears.
In the Location of triad drop down menu, select "At top left."
Click on OK.
Select menu path . The Pan-Zoom-Rotate dialog box appears.
Click on "Iso" to generate an isometric view and click on Close.
Select menu path . The Angle of Rotation dialog box appears.
Enter 90 for angle in degrees.
In the Axis of rotation drop down menu, select "Global Cartes X."
Click on OK.
Select menu path . The Plot Numbering Controls dialog box appears.
Click the Keypoint numbers radio button to turn keypoint numbering on.
Click the Line numbers radio button to turn line numbering on.
Click on OK.
Select menu path . The Create Straight Line picking menu appears.
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 () to zoom in.)
Click once on keypoints 7 and 8 to create a line between keypoints 7 and 8.
Click once on keypoints 8 and 9 to create a line between keypoints 8 and 9.
Click on OK.
Select menu path . The Line Fillet picking menu appears.
Click once on lines 8 and 9.
Click on OK in the picking menu. The Line Fillet dialog box appears.
Enter BENDRAD for Fillet radius and click on OK.
Click on SAVE_DB on the Toolbar.
In this step, you cut the hex section into two quadrilaterals. This step is required to satisfy mapped meshing.
Select menu path . The Plot Numbering Controls dialog box appears.
Click the Keypoint numbers radio button to Off.
Click on OK.
Select menu path .
Select menu path . The Divide Area by Line picking menu appears.
Click once on the shaded area, and click on OK.
Select menu path .
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 () to zoom in.)
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.
Select menu path . The Create Component dialog box appears.
Enter BOTAREA for component name.
In the Component is made of drop down menu, select "Areas."
Click on OK.
Select menu path . The Element Size on Picked Lines picking menu appears.
Enter 1,2,6 in the picker, then press ENTER.
Click on OK in the picking menu. The Element Sizes on Picked Lines dialog box appears.
Enter NO_D_HEX for number of element divisions and click on OK.
In this step, set the element type to PLANE182, all quadrilaterals for the area mesh.
Select menu path . The Element Attributes dialog box appears.
In the Element type number drop down menu, select “2 PLANE182” and click on OK.
Select menu path . The Mesher Options dialog box appears.
In the Mesher Type field, click on the Mapped radio button and then click on OK. The Set Element Shape dialog box appears.
Click on OK to accept the default of Quad for 2-D shape key.
Click on SAVE_DB on the Toolbar.
In this step, generate the area mesh you will later drag.
Select menu path . The Mesh Areas picking box appears.
Click on Pick All.
Select menu path .
Select menu path . The Element Attributes dialog box appears.
In the Element type number drop down menu, select “1 SOLID185” and click on OK.
Select menu path . The Global Element Sizes dialog box appears.
Enter L_ELEM for element edge length and click on OK.
Select menu path .
Click the Line numbers radio button to on if it is not already selected.
Click on OK.
Select menu path .
Select menu path . The Sweep Areas along Lines picking box appears.
Click on Pick All. A second picking box appears.
Click once on lines 8, 10, and 9 (in that order).
Click on OK. The 3-D model appears in the Graphics window.
Select menu path .
Click on SAVE_DB on the Toolbar.
Select menu path . The Select Component or Assembly dialog appears.
Click on OK to accept the default of select BOTAREA component.
Select menu path . The Clear Areas picking menu appears.
Click on Pick All.
Select menu path .
Select menu path .
Select menu path . The Select Component or Assembly dialog appears.
Click on OK to accept the default of select BOTAREA component.
Select menu path . The Select Entities dialog box appears.
In the top drop down menu, select "Lines."
In the second drop down menu, select "Exterior."
Click on Apply.
In the top drop down menu, select "Nodes."
In the second drop down menu, select "Attached to."
Click on the "Lines, all" radio button to select it.
Click on OK.
Select menu path . The Apply U,ROT on Nodes picking menu appears.
Click on Pick All. The Apply U,ROT on Nodes dialog box appears.
In the scroll list for DOFs to be constrained, click on "ALL DOF."
Click on OK.
Select menu path .
In the top drop down menu, select "Lines."
Click on the "Sele All" button, then click on Cancel.
Select menu path . The Symbols dialog box appears.
Click on the "All Applied BCs" radio button for Boundary condition symbol.
In the Surface Load Symbols drop down menu, select "Pressures."
In the “Show pres and convect as” drop down menu, select "Arrows."
Click on OK.
In this step, apply pressure on the handle to represent 100 N finger force.
Select menu path . The Select Entities dialog appears.
In the top drop down menu, select "Areas."
In the second drop down menu, select "By Location."
Click on the "Y coordinates" radio button to select it.
Enter BENDRAD,L_HANDLE for Min, Max, and click on Apply.
Click on "X coordinates" to select it.
Click on Reselect.
Enter W_FLAT/2,W_FLAT for Min, Max, and click on Apply.
In the top drop down menu, select "Nodes."
In the second drop down menu, select "Attached to."
Click on the "Areas, all" radio button to select it.
Click on the "From Full" radio button to select it.
Click on Apply.
In the second drop down menu, select "By Location."
Click on the "Y coordinates" radio button to select it.
Click on the "Reselect" radio button.
Enter L_HANDLE+TOL,L_HANDLE-(3.0*L_ELEM)-TOL for Min, Max.
Click on OK.
Select menu path . The Get Scalar Data dialog box appears.
In the scroll box on the left, scroll to "Model Data" and select it.
In the scroll box on the right, scroll to "For selected set" and select it.
Click on OK. The Get Data for Selected Entity Set dialog box appears.
Enter "minyval" for the name of the parameter to be defined.
In the scroll box on the left, click once on "Current node set" to select it.
In the scroll box on the right, click once on "Min Y coordinate" to select it.
Click on Apply.
Click on OK again to select the default settings. The Get Data for Selected Entity Set dialog box appears.
Enter "maxyval" for the name of the parameter to be defined.
In the scroll box on the left, click once on "Current node set" to select it.
In the scroll box on the right, click once on "Max Y coordinate" to select it.
Click on OK.
Select menu path . The Scalar Parameters dialog box appears.
Type the text PTORQ=100/(W_HEX*(MAXYVAL-MINYVAL)) in the Selection text box and click on Accept.
Click on Close.
Select menu path . The Apply PRES on Nodes picking menu appears.
Click on Pick All. The Apply PRES on Nodes dialog box appears.
Enter PTORQ for Load PRES value and click on OK.
Select menu path .
Select menu path .
Click on SAVE_DB on the Toolbar.
Select menu path . The Write Load Step File dialog appears.
Enter 1 for load step file number n.
Click on OK.
In this step, you define the downward pressure on top of the handle, representing 20N (4.5 lb) of force.
Select menu path . The Scalar Parameters dialog box appears.
Type the text PDOWN=20/(W_FLAT*(MAXYVAL-MINYVAL)) in the Selection text box and click on Accept.
Click on Close.
Select menu path . The Select Entities dialog appears.
In the top drop down menu, select "Areas."
In the second drop down menu, select "By Location."
Click on the "Z coordinates" radio button to select it.
Click on the "From Full" radio button to select it.
Enter -(L_SHANK+(W_HEX/2)) for Min, Max.
Click on Apply.
In the top drop down menu, select "Nodes."
In the second drop down menu, select "Attached to."
Click on the Areas, all radio button to select it, and click on Apply.
In the second drop down menu, select "By Location."
Click on the "Y coordinates" radio button to select it.
Click on the "Reselect" radio button.
Enter L_HANDLE+TOL,L_HANDLE-(3.0*L_ELEM)-TOL for Min, Max.
Click on OK.
Select menu path . The Apply PRES on Nodes picking menu appears.
Click on Pick All. The Apply PRES on Nodes dialog box appears.
Enter PDOWN for Load PRES value and click on OK.
Select menu path .
Select menu path .
Select menu path . The Write Load Step File dialog box appears.
Enter 2 for Load step file number n, and click on OK.
Click on SAVE_DB on the Toolbar.
Select menu path . The Solve Load Step Files dialog box appears.
Enter 1 for Starting LS file number.
Enter 2 for Ending LS file number, and click on OK.
Click on the Close button after the Solution is done! window appears.
Select menu path .
Select menu path . The List Reaction Solution dialog box appears.
Click on OK to accept the default of All Items.
Review the information in the status window, and click on Close.
Select menu path . The Symbols dialog box appears.
Click on the "None" radio button for Boundary condition symbol, and click on OK.
Select menu path . The Edge Options dialog box appears.
In the Element outlines for non-contour/contour plots drop down menu, select "Edge Only/All."
Click on OK.
Select menu path . The Plot Deformed Shape dialog box appears.
Click on the "Def + undeformed" radio button and click on OK.
Select menu path . The Save Plot Controls dialog box appears.
Type "pldisp.gsa" in the Selection box, and click on OK.
Select menu path . The Angle of Rotation dialog box appears.
Enter 120 for Angle in degrees.
In the Relative/absolute drop down menu, select "Relative angle."
In the Axis of rotation drop down menu, select "Global Cartes Y."
Click on OK.
Select menu path . The Contour Nodal Solution Data dialog box appears.
In the scroll box on the left, click on "Stress." In the scroll box on the right, click on "Intensity SINT."
Click on OK.
Select menu path . The Save Plot Controls dialog box appears.
Type "plnsol.gsa" in the Selection box, and click on OK.
Select menu path .
Select menu path . The List Reaction Solution dialog box appears.
Click on OK to accept the default of All Items.
Review the information in the status window, and click on Close.
Select menu path .
Type "pldisp.gsa" in the Selection box, and click on OK.
Select menu path . The Plot Deformed Shape dialog box appears.
Click on the "Def + undeformed" radio button if it is not already selected and click on OK.
Select menu path .
Type "plnsol.gsa" in the Selection box, and click on OK.
Select menu path . The Contour Nodal Solution Data dialog box appears.
In the scroll box on the left, click on "Stress." In the scroll box on the right, scroll to "Intensity SINT" and select it.
Click on OK.
Select menu path . The Offset WP tool box appears.
Enter 0,0,-0.067 for X, Y, Z Offsets and click on OK.
Select menu path . The Hidden-Line Options dialog box appears.
In the drop down menu for Type of Plot, select "Capped hidden."
In the drop down menu for Cutting plane is, select "Working plane."
Click on OK.
Select menu path . The Pan-Zoom-Rotate tool box appears.
Click on "WP."
Drag the Rate slider bar to 10.
On the Pan-Zoom-Rotate dialog box, click on the large round dot several times to zoom in on the cross section.