Workshop :Bicycle Frame Design Modified by (2009): Dr. Vijay K. Goyal Associate Professor, Department of Mechanical Engineering University of Puerto Rico at Mayagüez Thanks to Josymir Lopez Ferrer, enrolled in INME 4058 section 2008 University of Puerto Rico at Mayagüez Department of Mechanical Engineering

This is a simple static analysis of a frame of bicycle using a hollow aluminum tube. The schematic dimensions of the bicycle are shown in the figure 1. Initially, the flowing cross-sectional dimensions are used for all frames: Outer diameter φ = 25mm and Thickness t =2mm. Problem Description The material properties of aluminum are: Material PropertiesValues Young’s Modulus (E)70 Gpa Poisson’s Ration (ν)0.33 Density (ρ)2,580 kg/m3 Ultimate Tensile Strength(σU) 210 Mpa Elongation at Break10 %

Problem Description (cont.) Even if the bike is under the dynamic loads, only the static design criteria is considered here: due to vertical bending. Vertical bending test: When an adult rides the bike, the nominal load can be estimated by the vertically downward load of 600N at the seat position and a load of 200N at the pedal crank location. When a dynamic environment is simulated using the static analysis, the static loads are often multiplied by a certain “G-factor”. In this design project, use G = 2. Use ball-joint boundary condition for the front dropout (1) and sliding boundary condition for rear dropouts ( 5 and 6 ).

Starting ANSYS From your desktop: Click on: START > All Programs > ANSYS > ANSYS Product Launcher. Here we will set our Working Directory and the Graphics Manager

Select the Working Directory and type the name of work shop on Job Name. Working Directory Setup

Click the button: Customization/Preferences. On the item of Use custom memory settings type 128 on Total Workspace (MB): and type 64 on Database (MB): Then click the Run bottom. Graphics Setup * This setup applies to computers running under 512 MB of RAM

Go to customization preferences and choose custom memory settings and give values of 128 and 64 for the total workspace and database memory respectively. Click Run to start

This is ANSYS’s Graphical User Interface window. ANSYS GUI Overview

We’ll set preferences in order to filter quantities that relate to this discipline only. Click Preferences from ANSYS Main Menu. Select (check): “Structural ” & h-Method ” Step 1: Set Preferences

Pre Processing

Define element Types 1) Go to ANSYS Main Menu > Preprocessor > Element type > Add/Edit/Delete 2) In the display window named Element Type Click ADD In the new display window select pipe and Elast straight 16 3) Then click OK on Library of Element Types and CLOSE on the window of Element Types Step 2: Element Type ANSYS Main Menu

Step 2: Element Type  You should have one element type on the Element Types window

Step 3: Real constants This part is to enter the dimensions of the tube: Outer diameter φ = 25mm and Thickness t =2mm Go to ANSYS Main Menu > Real Constants > Add/Edit/Delete > Add > OK IMPORTAT!!! You have to use all the dimension on the same unit since ANSYS is a dimensionless Program. We will use all the dimensions on meters > Add the values φ =.025 and t =.002 > OK > The window of Real Constants (3) now said SET 1 > CLOSE (2 ) (1 ) (3 )

Now we are going to define the bicycle frame constant material properties. We are going to define the material’s behavior and then we’ll define Young’s Modulus (E), poison’s ratio ( ν), and density ( ρ ). GO to ANSYS Main Menu > Preprocessor > Material Properties > Material Models A new window ‘Define Material Model Behavior (1)’ will appear, on this window make a Double- click on Structural > Linear > Elastic > Isotropic > a new window will appear (2) > put the values of Young’s Modulus (E) = 7E10 and poison’s ratio ( ν) =0.33 > OK > CLOSE To enter the value of density = 2580 > Double-click on Density > enter the value > OK > CLOSE Step 4: Define Materials (1) (2) (3) (2 ) (3 )

We’ll start by creating keypoints –Keypoints: These are points, locations in 3D space. ANSYS Main Menu > Preprocessor > Modeling > Create > Keypoints > In active CS Enter 1 for Keypoint Number, enter 0, 0.325, 0 for X, Y, Z respectively. Click Apply Step 5: Build Geometry Keypoint s X (m) Y (m) Z (m)

Make the same for the next seven Keypoints (don’t forgot change the Keypoint Number), we have a total of eight Keypoints. After put the values of Keypoint 8, press OK, don’t press APPLY, if you press APPLY, press CANCEL. Enter 2 for Keypoint Number, enter 0, 0.400, for X,Y,Z respectively. Click Apply Enter 3 for Keypoint Number, enter 0.500, 0.400, 0 for X,Y,Z respectively. Click Apply Enter 4 for Keypoint Number, enter 0.400, 0, 0 for X,Y,Z respectively. Click Apply Enter 5 for Keypoint Number, enter 0.825, 0, for X,Y,Z respectively. Click Apply Enter 6 for Keypoint Number, enter 0.825, 0, for X,Y,Z respectively. Click Apply Enter 7 for Keypoint Number, enter 0.400, 0, for X,Y,Z respectively. Click Apply Enter 8 for Keypoint Number, enter 0.400, 0, for X,Y,Z respectively. Click OK Display Window after creating all eight Keypoints Choosing Isometric view on the right menu Step 4: Build Geometry

CREATING THE LINES to make the bicycle frame Now we are going to create lines that will connect the keypoints, we can made this using two different procedures, using the ANSYS Main Menu or using codes. For this type of geometry is more appropriate use CODES. Using Main Menu: We’ll start by creating straight lines from keypoint 1 to 2. Main Menu > Preprocessor > Modeling > Create > Lines > Lines > Straight Lines –This feature creates a straight line between two points. For the first Line select keypoints 1 and 2 and for the second line select keypoints 2 and 3 and continue with the other lines. Click Apply and OK Step 4: Build Geometry

Using Main Menu:

Step 4: Build Geometry Using CODES: In the ANSYS Command Prompt L,1,2 “Lines, node, node” L,2,3 L,3,4 L,4,7 L,4,8 L,7,5 L,8,6 L,5,6 L,1,4 L,3,5 L,3,6 Geometry after the 11 lines

Here we’ll define the meshing for our bicycle frame. ANSYS Main Menu > Preprocessor > Meshing > Size control > ManualSize > Lines > All Lines In SIZE Element edge length Click OK Step 5: Create Mesh

Select all the 11 lines

Step 6: Define Loads To apply the constrains: Keypoint 1 - ball joint constrains UX, UY, UZ Preprocessor > Loads > Define loads > Apply > Structural > Displacements > On keypoints > select the keypoint 1 > Select UX,UY,UZ > OK

Step 6: Define Loads Keypoint 5 and 6 - sliding boundary condition for rear dropouts. Preprocessor > Loads > Define loads > Apply > Structural > Displacements > On keypoints > Select the keypoints 5 and 6 Final view after apply the constrains Select UY, UZ and ROTX, ROTY, ROTZ > OK

Vertical bending test: We have to apply to loads, one vertically downward load of 600N *2 = 1200N at the seat position and a load of 200N*2= 400N at the pedal crank location. Go to Loads > Define Load > Structural > Force/Moment > On Keypoints > select key point 3 > OK In Lab Direction Of Force/Mon > select FY In apply as > constant value In VALUE Force/moment value > enter the since is down force due the Adult > OK For the 400N load > ON keypoint > select keypoint 4 > OK > In Lab Direction Of Force/Mon > select FY > In apply as > constant value > In VALUE Force/moment value > enter the -400 Step 6: Apply Loads Insert the direction of the load Insert the Value of the load

Step 6: Apply Loads Final view after apply the constrains and the loads

Solution

To start the solution phase it is important to set the type of analysis. Analysis type We will perform a static analysis since we only want stresses and deflections. To select analysis type click: SolutionAnalysis TypeNew AnalysisStaticOk

Now we proceed to solve the problem. To do this click: Solve SolutionSolveCurrent LS Note: When the pop up windows appear click the OK button.

Post Processing

Step 8: Review Results

To see the Deformation General Postproc > Plot Results > Deformed Shape > on the new window > Def + underformed > OK

Step 8: Review Results

Deflections: Nodal Solution General Postproc > Plot Results > Contour plot > Nodal solution On the Display Window > select Nodal Solution > DOF Solution > Displacement vector sum On Undisplaced shape key > select Deformed shape (or your preference) > OK

Step 8: Review Results

Stresses - Von Misses General Postproc > Plot Results> Contour Plot > Nodal Solution On the display window > Stress > von Mises Stress > Ok !!

Von Misses Stresses

Cross Section For a cross section … Go to menu.. WorkPLane > Display working plane.. An additional 3 axes appears, that is your working plane Go to.. WorkPLane > Offset WP to > by nodes > select the node closer to the cross section that you wan > OK Selected node

Cross Section (1) Then go to… WorkPLane > Offset WP by Increments… And play with the movement of the working plane… Remember you want to cut the cross section with the planes X and Y. (2)PlotCtrls > Style > Hidden line Options.. (3)In the display window in [/TYPE] Type of plot.. Select SECTION > OK (4) Play with the view until obtain cross section

Cross Section

Bending moment Select Element Table > Define Table... to define the table (remember SMISC,6 and SMISC,12) ADD > by sequence num > SMISC and put, 6 > apply > put 12 and OK > close

Bending moment And, Plot Results > Line Elem Res... to plot the data from the Element Table > choose and OK

Bending moment