Truss Bracket. Problem:

Transcription

1 Problem: The truss structure shown above is mounted on the sides of buildings during construction for use as scaffolding for workers. A design team has created a new bracket design (shown below) to use with the truss structure and want to know if the new bracket design is safe. The material for the bracket and the connecting pin is steel with a yield strength of 35 kpsi. The loads on the pin are know to be 14,825 lb in the minus X direction and 4856 lb in the Y direction. Determine if the new bracket design is safe using yielding as the failure criteria. Y X

2 Overview Anticipated time to complete this tutorial: 1 hour Tutorial Overview This tutorial is divided into four parts: 1) Tutorial Basics 2) Preprocessing 3) Solution 4) Post Processing Audience This tutorial assumes familiarity of ANSYS 8.0; therefore, it does not go into step by step detail. Prerequisites 1) ANSYS 8.0 in house Structural Tutorial 2) Completion of all Basic Machine Design Tutorials 3) Completion of the 3D Knuckle Pin Joint Tutorial Objectives 1) Create a solid model representation of the bracket 2) Create contact elements to model the interaction between the pin and the bracket 3) Determine if the bracket is a safe design for the given loads. Outcomes 1) Explore possibilities with the graphical user interface (GUI) 2) Learn how to create and mesh a complex geometries 3) Increase efficiency in problem set up and solving speed 2

3 In this tutorial: Instructions appear on the left. 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 A log file approach would be an excellent choice for solving this problem. The instructions given in this tutorial follow this approach. You will begin by creating log file commands to define the material properties, the geometry, and the mesh. You will then paste those commands into the ANSYS command line and build the model up to that point. Then you will use the contact wizard in the GUI to define contact surfaces between the pin and the hole. You will open the session editor and copy the commands that ANSYS used while creating the contacts and paste it into your log file. You will finish the tutorial by writing solution and post processing log file commands. The end result will be a log file useful for solving the entire problem. As you work through this tutorial, some new ANSYS features will be explained and the command lines for the log file will be given to you. Other log file commands you have used in other tutorials and will not be given to you. The 3D Knuckle Pin Joint uses many of the commands that you will need to solve this problem as well. It is recommended that you complete the 3D Knuckle Pin Joint tutorial before beginning this one. Drawings of the truss bracket are given below and on the next page. All dimensions are given in inches. 4

5 Problem Planning 5

6 1) Make the first two lines of the log file instructions for ANSYS to clear whatever database it is working on and start a new one. FINISH /CLEAR,NOSTART 2) Add commands to add a file name and title. /FILNAME, /TITLE, Test for Failure 3) One thing nice about a log file is that you can create prompts to allow the user to enter information. This is done through the *ASK command. Information on how to use the *ASK command is found in ANSYS help. For this problem the user will be prompted for the X and Y loads applied to the pin. Add the two lines of command as shown. The user inputted values will be stored in UFX, and UFY respectively. *ASK,UFX,'ENTER THE VALUE OF FX (LB),0 *ASK,UFY,'ENTER THE VALUE OF FY (LB),0 *ASK, Par, Query, DVAL Prompts the user to input a parameter value. Par An alphanumeric name used to identify the scalar parameter. Query Text string to be displayed on the next line as the query (32 characters maximum). Characters having special meaning (such as $!,) should not be included. DVAL Default value assigned to the parameter if the user issues a blank response. 4) Type the command to enter the preprocessor. /PREP7 5) Define the beam element for the model. You are going to use a solid95 element for this model. ET,1,SOLID95 6

7 6) Add the commands to define the material properties. The MP command to add a material model has been used in other tutorials. Additional properties that can be added for a material will now be shown. For this model we will add the density and define data points to map the stress-strain curve for the material. All of the commands needed are briefly explained to the right. See ANSYS help for additional information. MP, Lab, MAT, C0, C1, C2, C3, C4 Defines a linear material property as a constant or a function of temperature. 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). For this model a custom stress strain curve will be added. This curve dictates that the material will start to yield at stresses of 35 kpsi. Once you understand how these commands are used, add the following to your log file. MP,EX,1,30e6 MP,PRXY,1,0.3 MP,DENS,1,0.283/386 TB,MISO,1,1,6, TBTEMP,0 TBPT,,.0015,45000 TBPT,,.0133,47000 TBPT,,.0266,54000 TBPT,,.05,62000 TBPT,,.1,70000 TBPT,,.15,73000 After you have entered the commands above you can run your log file up to this point and then view a plot of the materials stress-strain curve by going to > Preprocessor > Material Props > Material Models > Material Model Number 1 > Multilinear Isotropic >Then click on the graph button TB, Lab, MAT, NTEMP, NPTS, TBOPT Lab Valid property label. (note only the applicable property label is shown below). MISO -- Multilinear isotropic hardening using von Mises or Hill plasticity MAT Material reference number NTEMP The number of temperatures for which data will be provided NPTS Number of data points to be specified for a given temperature. TBTEMP, TEMP, KMOD TEMP Temperature value (defaults to 0.0 if KMOD is blank). TBPT, Oper, X, Y Oper - Leave blank for this case X value of the point (strain, or H, or closure value). Y The corresponding Y value of the point (stress, or B, or pressure value). 7

8 7) Create the geometry for the bracket and the pin. There are several ways to do this. The challenge of this tutorial will be to build the geometry in an efficient and accurate manner. The geometry can be built using commands that have been demonstrated in other tutorials. The following commands may be helpful: SET - define scalar parameters BLOCK - create solid blocks CYL4 - create cylinders VSBV - subtract volumes VGLUE - glue volumes together For example, you could first build the two plates using the BLOCK command. Second, you could build a solid cylinder and use the VSBV command to subtract it from the plate to create the hole. Then create another cylinder in the same place the size of the pin. Finally, use the VGLUE command to glue the appropriate geometry parts together. (Don t glue the pin and the plate together.) Note: In order to know the appropriate volume numbers to use in this command, you may have to run your log file up to this point, plot the volumes, and turn on the volume numbers. 8

9 8) Set the mesh size for different parts of the model. Use the LESIZE and AESIZE commands to set the number of divisions or element size for the lines and areas indicated. Note: In order to know the appropriate line and area numbers to use in these commands, you may have to run your log file up to this point, plot the line and areas, and turn on the line and area numbers. The numbers below refer to the number of divisions for the lines indicated and the element size for the areas indicated. These are the mesh sizes used in the creation of the tutorial. Feel free to mesh the model in a different manner; however, note that too coarse of mesh will not give the correct result and too dense of a mesh will significantly increase the time the computer needs to solve the model. Area, 0.1 (outer surface of head of pin) Examples: LESIZE,60,,,15,,,,,1 AESIZE,17,0.1, Line, 10 Line, 7 Line, 3 Line, 15 Line, 15 Line, 15 Line, 15 Line, 10 9

10 9) Mesh the model using the volume sweep command. VSWEEP,ALL 10) Add constraints to the bracket and the pin. This can be accomplished using the ASEL,NSLA, and D commands. ASEL - select areas NSLA - select nodes associated with selected areas D - constrain degrees of freedom Constrain the back of the truss in all degrees of freedom and constrain the pin so that it cannot slide out of the bracket. Example code: Back of Truss ASEL,S,AREA,,6 NSLA,S D,ALL,UX,0 D,ALL,UY,0 D,ALL,UZ,0 Pin ASEL,S,AREA,,17 NSLA,S D,ALL,UZ,0 Note: The area numbers given in the code may not be the same as the ones in your model. Verify that you have entered the right area number in your code. 10

11 11) Apply the forces to the ends of the pin. Use the ASEL, NSLA, commands to select the two areas that make up the ends of the pin. Divide the force equally among the nodes on ends of the pin. ASEL,S,AREA,,17 NSLA,S ASEL,A,AREA,,21 NSLA,A Note: The area numbers given in the code may not be the same as the ones in your model. Verify that you have entered the right area number in your code. Run your model up to this point. When you use the ASEL, and NSLA commands ANSYS will count how many nodes you have selected and display that number in the output window. Look in the output window to see how many nodes were selected. If you can t see that number copy and paste the above commands into the command prompt in the GUI and press enter. Check the output window again. Make sure that you have the right area numbers. Based on the mesh used in the tutorial, there were 204 nodes; 102 nodes on each side of the pin. Apply the force evenly over these selected nodes. Remember that UFX, and UFY are variables that contain the user inputted values for the FX and FY forces on the pin. F,ALL,FX,UFX/204 F,ALL,FY,UFY/204 12) Select all the nodes again. ALLSEL,ALL 11

12 13) You will now switch to the GUI and use the contact wizard to generate contact elements between the bracket and the pin. Once you have created the contacts, use the session editor to paste the command lines into your log file. The steps shown in the 3D Knuckle Pin Joint explain the process for creating the contacts. Use the following information as you create the contacts using the contact wizard. Use inner surface of the hole in the bracket as the target area. Target Surface = Areas Target Type = Flexible Use the outer surface of the hole (that makes contact with the bracket) as the contact surface Contact Surface = Areas Contact Element Type = Surface-to- Surface Unselect the option to include initial penetration. Select the option to create a symmetric pair. Enter a coefficient of friction of 0.2. Leave the other setting as the defaults. Once you have created the contact pair, open the session editor in the ANSYS main menu and copy all the commands used to create the contact pair. Paste them into your log file. 14) Add a command to reselect all the nodes. ALLSEL,ALL 12

13 15) When the contact pair was created, coincident nodes were created at the interface of the pin and the bracket. Some unneeded degrees of freedom in these nodes can be removed by defining coupled degrees of freedom between these coincident nodes (within a tolerance), which will decrease the solution time. Add the following command. CPINTF,ALL, ) Add commands to setup the solution and then solve the model. FINISH /SOL ANTYPE,0 NLGEOM,1 NSUBST,10,1000,1 AUTOTS,1 SOLVE FINISH FINISH Exits normally from a processor. /SOL Enters the solution processor. ANTYPE, Antype Specifies the analysis type and restart status. STATIC or 0 -- Perform a static analysis. Valid for all degrees of freedom NLGEOM, Key Includes large-deflection effects in a static or full transient analysis. ON -- 1 Large-deflection effects are to be included NSUBST, NSBSTP, NSBMX, NSBMN Specifies the number of substeps to be taken this load step NSBSTP Number of substeps to be used for this load step NSBMX Maximum number of substeps to be taken NSBMN Minimum number of substeps to be taken AUTOTS, Key Specifies whether to use automatic time stepping or load stepping ON -- 1 Use automatic time stepping SOLVE Starts a solution 13

14 17) Add commands to enter the post processor and to view the stresses. Review the command explanations to the right and then add the following code: /POST1 AVPRIN,0,, PLNSOL,S,EQV,0,1 /REPLOT /POST1 Enters the database results postprocessor. AVPRIN, KEY, EFFNU Specifies how principal and vector sums are to be calculated KEY Averaging key: 0 -- Average the component values from the elements at a common node PLNSOL, Item, Comp, KUND, Fact Displays results as continuous contours Item - S Component stress Comp - EQV Equivalent stress KUND - 0 Do not overlay undeformed structure display Fact - 1 (default) Scale factor for 2-D display for contact items. /REPLOT, Label Automatically reissues the last display command for convenience 18) Run your log file and view the results. When you run the log file you should get two user prompts asking for the FX and FY loads applied to the pin. Enter the following values in these prompts: For FX enter For FY enter 4856 Note depending on the speed of your computer it may take ten minutes or more for the solution to solve. 14

15 Post Processing 19) If everything was done correctly you should see a stress plot of the bracket and the pin similar to the one shown. Look at the stresses around the interface of the pin and the bracket. Under these loads the stress in the bracket exceeds the yield strength (35kpsi) and thus failure can occur. The bracket is not a safe design for the loads given. Try running the solution under different loads. 15