Stiffness of Tapered Beam

Transcription

1 Problem: A bar in tension has a conical shape of length L. The task is to find the stiffness of the tapered section. Compare the stiffness given by ANSYS to the theoretical stiffness given by: EA1 ( r2 r1 ) k = 1+ L r1 and compute a percent error between the computed and theoretical stiffness. Let r 1 be both.25 in or.5 in. Let r 2 be both.5 in or 2 in. Let L be both 2 in or 5 in. Perform the stiffness calculation for every combination of the above factors (8 runs in all). Joseph Shigley and Charles Mischke. Mechanical Engineering Design 5th ed. New York: McGraw Hill, May 2002.

2 Overview Anticipated time to complete this tutorial: 1.5 hours Tutorial Overview This tutorial is divided into five parts: 1) Tutorial Basics 2) Problem Planning 3) 4) Solution 5) Hand Calculations Audience This tutorial assumes an intermediate knowledge of ANSYS 8.0; therefore, it goes into moderate detail to explain each step. A problem planning section has been added to help set up the problem. More advanced ANSYS 8.0 users should be able to complete this tutorial fairly quickly. Prerequisites 1) ANSYS 8.0 in house Structural Tutorial 2) Completion of three or more Basic Machine Design Tutorials Objectives 1)Write ANSYS model with command lines in a log file 2)Use the log file to solve the problem for each run 3)Use the log file to compute the desired results for each run Outcomes 1) Learn how to set up the problem before starting Ansys 2) Increase familiarity with the graphical user interface (GUI) 3) Learn how to create and mesh more complex geometries 4) Increase familiarity with post processing tools 2

3 In this tutorial: Instructions appear on the left. Stiffness of Tapered Beam Visual aids corresponding to the text appear on the right. Tutorial Basics All commands on the toolbars are labeled. However, only operations applicable to the tutorial are explained. The instructions should be used as follows: Bold > Example: Italics MB1 MB2 MB3 Text in bold are buttons, options, or selections that the user needs to click on > Preprocessor > Element Type > Add/Edit/DeleteFile would mean to follow the options as shown to the right to get you to the Element Types window Text in italics are hints and notes Click on the left mouse button Click on the middle mouse button Click on the right mouse button Some basic ANSYS functions are: To rotate the models use Ctrl and MB3. To zoom use Ctrl and MB2 and move the mouse up and down. To translate the models use Ctrl and MB1. 3

4 Problem Planning The repetitious nature of this problem suggests the use of a log file. The variable parameters include r 1, r 2, and L. You will input these as scalar parameters. Although the applied force and Young's Modulus will not vary from run to run, you will include them as scalar parameters because you will use them in scalar calculations. For example, the theoretical value of k for a tapered beam can be entered as a scalar parameter in the following way: K_theoretical = ( *E*r1*r1/L)*(1+(r2-r1)/r1) The tapered section under investigation will be created from 2 circular cross sections with radii r 2 and r 1 at the left and right ends respectively. A third, tapered section, will then be defined by using the first two cross sections as its ends. To find k in ANSYS you will use the relation K_act = F/x This means that you will apply a force in the positive x direction at the right end of the beam and then measure the resulting displacement at the right end of the beam. Again, you will use a scalar calculation to have ANSYS solve for the value of K_act. You will also have ANSYS perform a scalar calculation for the percent error between K_theoretical and K_actual. The formula for percent error is given by Percent_Error = 100*(K_theoretical - K_act)/K_theoretical This lesson will lead you through the steps of writing a log file. Instructions on each command (pulled from the ANSYS help file) appear in the right column. Commands that you should write to your log file will appear as 8 pt. Arial text in the left column. The information contained in this tutorial will be valuable to you as you do other analysis in ANSYS. Please pay careful attention to the instructions in the right column and do not gloss over the information given for each command. 4

5 1) Start a new notepad file. Give it an appropriate file name and save it to the desired directory. 2) The first command of the log file will be an instruction to tell ANSYS to clear whatever database it is working on and start a new one. The syntax used to perform this operation is shown to the right in bold text. The options for the clear (i.e. START or NOSTART are also shown with their definitions. Type the following command line as the first line in your notepad file: /CLEAR, Read Clears the database. Read File read option: START -- Reread start80.ans file (default). NOSTART -- Do not reread start80.ans file. /CLEAR, START 3) Next, you are going to enter a command to change the file name of your project. /FILNAME,Stiffness of Tapered Beam,1 /FILNAME, Fname, Key Changes the Jobname for the analysis. Fname Name (32 characters maximum) to be used as the Jobname. Defaults to the initial Jobname as specified on the ANSYS execution command, or to File if none specified. Key Specify whether to use the existing log and error files or start new files. 0, OFF -- Use existing log and error files. 1, ON -- Start new log and error files (old files are closed but not deleted). 4) Next, you are going to enter a command to give the project a title. /TITLE,TAPERED BEAM /TITLE, Title Defines a main title. Title Input up to 72 alphanumeric characters. Parameter substitution may be forced within the title by enclosing the parameter name or parametric expression within percent (%) signs. 5

6 5) Type the command to enter the preprocessor. /PREP7 Enters the model creation preprocessor. /PREP7 6) Define the beam element for the model. You are going to use a Beam189 element for this model. ET,1,BEAM189 ET, ITYPE, Ename, KOP1, KOP2, KOP3, KOP4, KOP5, KOP6, INOPR Defines a local element type from the element library. ITYPE Arbitrary local element type number. Defaults to 1 + current maximum. Ename Element name (or number) as given in the element library in Chapter 4 of the ANSYS Elements Reference. The name consists of a category prefix and a unique number, such as BEAM3. The category prefix of the name (BEAM for the example) may be omitted but is displayed upon output for clarity. If Ename = 0, the element is defined as a null element. KOP1, KOP2, KOP3, KOP4, KOP5, KOP6 KEYOPT values (1 through 6) for this element, as described in the ANSYS Elements Reference. INOPR If 1, suppress all element solution printout for this element type. 7) Now you are going to set scalar parameters that you will call during other parts of the command sequence. Any scalar parameter is defined using the *SET command. *SET,F,1000 *SET,E,30E6 *SET,R1,.25 *SET,R2,.5 *SET,L,2 *SET,K_THEORETICAL,( *E*R1*R1/L)*(1+(R2-R1)/R1) *SET, Par, VALUE Assigns values to user-named parameters. Par An alphanumeric name used to identify this parameter. Par may be up to 32 characters, beginning with a letter and containing only letters, numbers, and underscores VALUE Numerical value or alphanumeric character string (up to 8 characters enclosed in single quotes) to be assigned to this parameter. 6

7 8) You will now write commands that define the material properties. MPTEMP,1,0 MPTEMP, STLOC, T1, T2, T3, T4, T5, T6 Defines a temperature table for material properties. STLOC Starting location in table for entering temperatures. T1, T2, T3, T4, T5, T6 Temperatures assigned to six locations starting with STLOC. MPDATA, Lab, MAT, STLOC, C1, C2, C3, C4, C5, C6 Defines property data to be associated with the temperature table. Lab Valid property label. (note only the applicable property labels are shown below). EX -- Elastic moduli (also EY, EZ). PRXY -- Major Poisson's ratios (also PRYZ, PRXZ). MPDATA,EX,1,0,E MPDATA,PRXY,1,0,.3 STLOC Starting location in table for generating data. Note that E is used in the definition of Young s modulus above. Earlier you defined E as a scalar parameter (30e6). 7

8 9) You will now define the cross sections of the end of the beam; you will name them A1 and A2. A1 will have radius r1 (already defined as a scalar parameter) and A2 will have radius r2. SECTYPE,1, BEAM, CSOLID, A1, 0 SECOFFSET, CENT SECDATA,R1,18,3,0,0,0,0,0,0,0 SECTYPE,2, BEAM, CSOLID, A2, 0 SECOFFSET, CENT SECDATA,R2,18,3,0,0,0,0,0,0,0 10) You will now define the tapered cross section using a similar command. The left end of the tapered section will be have cross section A2 (also defined as section 2 above). The right end of the tapered section will have cross section A1 (defined as section 1 above). The location of the left end of the beam will be X,Y,Z = 0,0,0 and the location of the right end of the beam will be X,Y,Z = L,0,0 where L was already defined as a scalar parameter. SECTYPE,3,TAPER,, SECDATA, 2,0,0,0, SECDATA, 1,L,0,0, SECTYPE, SECID, Type, Subtype, Name, REFINEKEY Associates section type information with a section ID number. SECID Section identification number. Type BEAM -- Defines a beam section. See subtypes below. TAPER -- Defines a tapered beam section. The sections at the end points must be topologically identical. Subtype When Type = BEAM, the possible beam sections that can be defined for Subtype are: RECT Rectangle QUAD Quadrilateral CSOLID Circular solid CTUBE Circular tube CHAN Channel I I-shaped section Z Z-shaped section L L-shaped section T T-shaped section HATS Hat-shaped section HREC Hollow rectangle or box ASEC Arbitrary section -- integrated cross-section inertia properties supplied by user MESH User-defined mesh -- see the SECREAD command for more information about this data Name An 8-character name for the section. SECOFFSET, Location, OFFSET1, OFFSET2, CG-Y, CG-Z, SH-Y, SH-Z Defines the section offset for cross sections. Location CENT -- Beam node will be offset to centroid (default). SECDATA See ANSYS help for information regarding the arguments for this function. Different arguments exist for each section type (i.e. beam or tapered) 8

9 11) You will now define keypoints used in the model. K,1,0,0,0, K,2,L,0,0, K, NPT, X, Y, Z Defines a keypoint. NPT Reference number for keypoint. If zero, the lowest available number is assigned [NUMSTR]. X, Y, Z Keypoint location in the active coordinate system. 12) You will now create a line between keypoint 1 and 2. L,1,2 L, P1, P2, NDIV, SPACE, XV1, YV1, ZV1, XV2, YV2, ZV2 Defines a line between two keypoints. P1 Keypoint at the beginning of line. If P1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). P2 Keypoint at the end of line. 13) You will now define the element line attributes for the created line. LATT,1,,1,,,,3 LATT, MAT, REAL, TYPE, --, KB, KE, SECNUM Associates element attributes with the selected, unmeshed lines. MAT, REAL, TYPE Material number, real constant set number, and type number to be associated with selected, unmeshed lines. KB, KE Beginning and ending orientation keypoints to be associated with selected, unmeshed lines. SECNUM Section identifier to be associated with selected, unmeshed lines. 9

10 14) Define the element size for the line. LESIZE,ALL,L/25,,,,1,,,1, LESIZE, NL1, SIZE, ANGSIZ, NDIV, SPACE, KFORC, LAYER1, LAYER2, KYNDIV Specifies the divisions and spacing ratio on unmeshed lines. NL1 Number of the line to be modified. If ALL, modify all selected lines [LSEL]. SIZE If NDIV is blank, SIZE is the division (element edge) length. The number of divisions is automatically calculated from the line length (rounded upward to next integer. 15) Mesh the line. LMESH,1 LMESH, NL1, NL2, NINC Generates nodes and line elements along lines. NL1, NL2, NINC Mesh lines from NL1 to NL2 (defaults to NL1) in steps of NINC (defaults to 1). 16) Turn on the 3D display of the elements. /ESHAPE,1,0 /ESHAPE, SCALE, KEY Displays elements with shapes determined from the real constants or section definition. SCALE Scaling factor: 0 -- Use simple display of line and area elements (default) Use real constants or section definition to form a solid shape display of elements. KEY Current shell thickness key: 0 -- Use current thickness in the displaced solid shape display of shell elements (valid for SHELL181, SHELL208, and SHELL209). Default Use initial thickness in the displaced solid shape display of shell elements. 10

11 17) Enter a command to replot the element shape. /REPLOT 18) Exit the preprocessor. FINISH 19) Enter the solver. /SOLU Enters the solution processor. /SOL 20) Constrain the left end of the beam in all DOF. DK,1,,,,0,ALL,,,,,, DK, KPOI, Lab, VALUE, VALUE2, KEXPND, Lab2, Lab3, Lab4, Lab5, Lab6 Defines DOF constraints at keypoints. KPOI Keypoint at which constraint is to be specified. Lab Valid degree of freedom label. VALUE Degree of freedom value or table name reference for tabular boundary conditions. VALUE2 Second degree of freedom value (if any).. KEXPND Expansion key: 0 -- Constraint applies only to the node at this keypoint Flags this keypoint for constraint expansion. Lab2, Lab3, Lab4, Lab5, Lab6 Additional degree of freedom labels. The same values are applied to the keypoints for these labels. 11

12 21) Apply the force, F, to keypoint 2 in the positive x direction. FK,2,FX,F FK, KPOI, Lab, VALUE, VALUE2 Defines force loads at keypoints. KPOI Keypoint at which force is to be specified. Lab Valid force label. Structural labels: FX, FY, or FZ (forces) VALUE Force value or table name reference for specifying tabular boundary conditions. 22) Create a command to solve the model. SOLVE 23) Exit the solver. FINISH 23) Enter the post processor. /POST1 24) Plot nodal solution for the x component of stress. AVPRIN,0, PLNSOL, S,X, 0,1.0 /POST1 Enters the database results postprocessor. AVPRIN, PLNSOL See ANSYS help for information regarding the arguments for this function (too long to list here). 25) Create three more scalar parameters that calculate K_act, X_Disp, and Percent_Error. *SET,K_ACT,F/UX(2) *SET,X_DISP,UX(2) *SET,PERCENT_ERROR,100*(K_THEORETICAL- K_ACT)/K_THEORETICAL 26) Exit the post processor. FINISH 27) Save the log file. 12

13 Solution 28) Copy the contents of the log file into the command line in ANSYS and press enter. Press enter to close the appropriate dialog boxes and proceed with the solution. 29) When the solution is finished select > Parameters > Scalar Parameters The Scalar Parameters window will open. You can read the values of k_theoretical, k_act, and Percent_Error. Make a table and record the answers. 30) Run all combinations of r1, r2, and L described in the problem statement. Make a table and record the answers. Simply change the parameters (r1, r2, and L) in the log file and re-run the solution. 13

14 K_Theoretical is given by the following equation for a tapered beam Hand Calculations k = EA1 ( r2 r1 ) 1+ L r1 14