Lathe Cutter Workshop 2A Stress Analysis. Workshop Supplement January 20, 2001 Inventory #001442 W2-2 2A. Stress Analysis Lathe Cutter Description Solve.

Slides:

Advertisements

Similar presentations

ANSYS Model of a Cylindrical Fused Silica Fibre

Advertisements

Results Viewer Workshop 13D Postprocessing. Workshop Supplement November 1, 2002 Inventory # W D. Postprocessing Results Viewer Description.

Building Frame Workshop 4 Beam Modeling. Workshop Supplement October 30, 2001 Inventory # W Beam Modeling Building Frame Determine the deflections.

WS11-1 VND101, Workshop 11 MSC.visualNastran 4D Exercise Workbook Bracket.

3-D Bracket Workshop 10A Loading and Solution. Workshop Supplement February 7, 2006 Inventory # W A. Loading and Solution 3-D Bracket Description.

Module 5 Beam Modeling.

Swaybar-Shaft Assembly Workshop 8 Bonded Contact.

Bolt Torque Workshop 3 Surface Effect Elements. Workshop Supplement October 30, 2001 Inventory # W Surface Effect Elements Bolt Torque Description.

Finite Element Method FEM Dr. Mohammed Al-Hazmi ANSYS Basics Lecture 4.

Thermal Analysis Module 6. Training Manual January 30, 2001 Inventory # Thermal Analysis In this chapter, we will briefly describe the procedure.

Module 7 Modal Analysis.

Verifying Pressures Workshop 9 Macro Basics. Workshop Supplement October 30, 2001 Inventory # W Macro Basics Verifying Pressures Create a.

9.0 New Features Large Deformation Analysis of thin plate assembly spotwelded together Workshop 2 Spotwelds.

ANSYS Fundamentals This document contains no technical data subject to the EAR or the ITAR.

Large Deflection Arched Beam Workshop 7 Nonlinear Analysis.

University of Puerto Rico at Mayagüez Department of Mechanical Engineering Introduction to NX 6.0 Tutorial 1 Modified by (2011): Dr. Vijay K. Goyal and.

Problem 2: Thermal Solidification of a Casting University of Puerto Rico at Mayagüez Department of Mechanical Engineering Modified by (2008): Dr. Vijay.

Workshop :Bicycle Frame Design Modified by (2009): Dr. Vijay K. Goyal Associate Professor, Department of Mechanical Engineering University of Puerto Rico.

University of Puerto Rico at Mayagüez Department of Mechanical Engineering Introduction to NX 6.0 Tutorial 4 Modified by (2011): Dr. Vijay K. Goyal and.

Workshop: Bicycle Frame Design Modified by (2009): Neysa A. Fuentes Department of Mechanical Engineering University of Puerto Rico, Mayagüez Jelisa Torres.

Workshop 7: Thermal Steady State Analysis of a Composite Slab University of Puerto Rico at Mayagüez Department of Mechanical Engineering Modified by (2008):

Axisymmetric Wheel Workshop 1 Array Parameters. Workshop Supplement October 30, 2001 Inventory # W Array Parameters Axisymmetric Wheel Determine.

Features: 1. 2D structural analysis (plane stress) 2. Static analysis 3. Quarter symmetric 4. SI units 5. Only the yoke is modeled 6. Material properties.

Problem 1: Structural Analysis of Signs Post University of Puerto Rico at Mayagüez Department of Mechanical Engineering Modified by (2008): Dr. Vijay K.

Workshop 6: Thermal Analysis of a Plate with a Hole University of Puerto Rico at Mayagüez Department of Mechanical Engineering Modified by (2008): Dr.

1) Structural Symmetry 2) Bookshelf Problem Jake Blanchard Fall 2009.

9.0 New Features Metal Shaft with Rubber Boot Workshop 7 Load Steps in Workbench.

Collapse of Frame Workshop Thirteen REFERENCE: Training Manual Geometric Instability (9-74)

DYNAMICS for ANSYS 5.7 Workshop Supplement. January 30, 2001 Inventory # WS-2 Table of Contents Introductory Workshop Galloping Gertie W-4.

Submodeling Module 6. Training Manual January 30, 2001 Inventory # Submodeling Submodeling is a finite element technique used to get more.

Short Topics Chapter 14. Training Manual October 30, 2001 Inventory # In this chapter, we will present some general tips and “tricks” on how.

Implicit-to-Explicit Sequential Solution

REFERENCE: Training Manual Obtaining the Solution (3-28) Fishing Rod (part 2) Workshop Three Results File Options.

Explicit-to-Implicit Sequential Solution

Investigation of the Thermal Stresses in a Steel Plate.

REFERENCE: Training Manual Node-to-Surface Elements (8-16) Beam Tip Contact Workshop 12 Node-to-Surface Elements.

Structural Analysis Chapter 10. Training Manual October 30, 2001 Inventory # In this chapter, we will describe the specifics of a structural.

Importing Geometry Workshop 5. Workshop Supplement October 30, 2001 Inventory # W Importing Geometry Description Import the following CAD.

Axisymmetric Rotating Disk Workshop 3A Optimizing the Design.

Batch Mode: Plate with Hole at Center Workshop 13A Short Topics.

WS4-1 WORKSHOP 4 Stadium Truss NAS120, Workshop 4, November 2003.

Surface-to-Surface Simulation

Workshop 13 Bolt Pretension

Axisymmetric Rotating Disk Workshop 2A Parametric Modeling.

Workshop 1 Contact Stiffness

Springback Analysis Workshop 10. Workshop Supplement March 15, 2001 Inventory # WS10-2 Utility Menu > File > Read Input from … > stamp.inp > OK.

Rib Forging Workshop Nine REFERENCE: Training Manual Viscoplasticity (5-35)

Volumetric Locking Workshop Two REFERENCE: Training Manual Element Technology (2-64)

Buckling of Arch Workshop Twelve REFERENCE: Training Manual Geometric Instability (9-56)

Pillow Block Workshop 6 Solid Modeling: Top-Down.

Snap Fit Workshop Seventeen Introduction to Contact REFERENCE: Training Manual Introduction to Contact (7-69)

Workshop 2 Steel Bracket Modified by (2008): Dr. Vijay K. Goyal Associate Professor, Department of Mechanical Engineering University of Puerto Rico at.

Bending of a Pipe by a Punch Workshop 8. Workshop Supplement March 15, 2001 Inventory # WS8-2 Utility Menu > File > Read Input from … > pipe.inp.

WORKSHOP 15 PARASOLID MODELING NAS120, Workshop 15, November 2003 WS15-1.

NLISO Material Model Workshop Four REFERENCE: Training Manual Rate-Independent Plasticity (3-65)

Simulating a Deep Drawing Process Workshop 2. Workshop Supplement March 15, 2001 Inventory # WS2-2 Utility Menu > File > Read input from …> deep.inp.

COUPLED ANALYSES Chapter 7. Training Manual May 15, 2001 Inventory # Fluid-Structure Analysis “One Way” Analysis –Structural deformation effect.

Truss Structure Workshop Five Convergence Criteria REFERENCE: Training Manual Obtaining the Solution (3-51)

Crank Shaft Workshop 5 Submodeling. Workshop Supplement October 30, 2001 Inventory # W Submodeling Crank Shaft Description Perform a submodeling.

REFERENCE: Training Manual Friction (4-18) Planar Seal (part 2) Workshop 2 Contact with Friction Constant Friction Coefficient.

Stress Relaxation Workshop Six REFERENCE: Training Manual Implicit Creep (4-32)

ANSYS Basics Workshop 3A Introductory Workshop. Workshop Supplement October 30, 2001 Inventory # W3-2 3A. Introductory Workshop ANSYS Basics In.

ANSYS Basics Workshop 1 Introductory Workshop. Workshop Supplement January 30, 2001 Inventory # W1-2 Introductory Workshop ANSYS Basics In this.

Connecting Rod Workshop 7A Solid Modeling: Bottom-Up.

Chapter Overview In this exercise, a model of a cylindrical pipe is modeled as being crushed between rigid bodies. This model is created using 2D shell.

WORKSHOP 7 LINEAR CONTACT

WORKSHOP 2 SOLID-TO-SOLID CONTACT

NECKING OF A TEST SPECIMEN

Module 6 Submodeling.

Presentation transcript:

Lathe Cutter Workshop 2A Stress Analysis

Workshop Supplement January 20, 2001 Inventory # W2-2 2A. Stress Analysis Lathe Cutter Description Solve a 3-D stress analysis of the lathe cutter model below. Review the results in the general postprocessor by: 1) plotting the displacements 2) listing reaction forces 3) plotting the von Mises stress 4) animating the von Mises stress Resolve the solution using a different set of constraints and compare the stress results to the first solution.

Workshop Supplement January 20, 2001 Inventory # W2-3 2A. Stress Analysis Lathe Cutter Loads and Material Properties for the first solution:

Workshop Supplement January 20, 2001 Inventory # W2-4 2A. Stress Analysis Lathe Cutter Loads and Material Properties for the second solution:

Workshop Supplement January 20, 2001 Inventory # W2-5 2A. Stress Analysis Lathe Cutter 1.Enter ANSYS in the working directory specified by your instructor using “cutter” as the jobname. 2.Set the GUI Preferences to Structural: –Main Menu > Preferences … Select “Structural”, then [OK]

Workshop Supplement January 20, 2001 Inventory # W2-6 2A. Stress Analysis Lathe Cutter 3.Import the “cutter.igs” IGES file using the “No defeaturing” option: –Utility Menu > File > Import > IGES … Select “No defeaturing”, then [OK] Select “cutter.igs’, then [OK] –Or issue: /AUX15 IOPTN,IGES,NODEFEAT IGESIN,cutter,igs,

Workshop Supplement January 20, 2001 Inventory # W2-7 2A. Stress Analysis Lathe Cutter 4.Scale the model by converting centimeters to inches: –Main Menu > Preprocessor > Operate > Scale > Volumes + [Pick All] –Enter 1/2.54 for RX, RY, and RZ –Set IMOVE to “Moved”, then [OK] –Or issue: VLSCAL, ALL,,, 1/2.54, 1/2.54, 1/2.54,, 0, 1 –Utility Menu > Plot > Volumes –Or issue: VPLOT

Workshop Supplement January 20, 2001 Inventory # W2-8 2A. Stress Analysis Lathe Cutter 5.Read input from “cutter-area.inp” to create a small area for applying pressure load at tip: –Utility Menu > File > Read Input from … Select “cutter-area.inp”, then [OK] –Or issue: /INPUT,cutter-area,inp

Workshop Supplement January 20, 2001 Inventory # W2-9 2A. Stress Analysis Lathe Cutter 6.Specify the element type: –Main Menu > Preprocessor > Element Type > Add/Edit/Delete … [Add...] –Select “Structural Solid” and “Tet 10node 92”, then [OK] [Close] –Or issue: ET,1,SOLID92

Workshop Supplement January 20, 2001 Inventory # W2-10 2A. Stress Analysis Lathe Cutter 7.Define elastic modulus for material 1 to be 10e6 (Aluminum): –Main Menu > Preprocessor > Material Props > Material Models … Structural -> Linear -> Elastic -> Isotropic Set EX = 10e6 (Young’s modulus in psi for Aluminum) Set PRXY =.32 [OK] Select Material > Exit –Or issue: MP,EX,1,10e6 MP,PRXY,1,.32

Workshop Supplement January 20, 2001 Inventory # W2-11 2A. Stress Analysis Lathe Cutter 8.Activate smartsize meshing and mesh the model with tetrahedral elements: –Main Menu > Preprocessor > MeshTool … Activate “Smart Size” Set Smart Size level to 4 [Mesh] [Pick All] [Close] –Or issue: SMRT,4 MSHAPE,1,3D MSHKEY,0 VMESH

Workshop Supplement January 20, 2001 Inventory # W2-12 2A. Stress Analysis Lathe Cutter 9.Apply area “symmetry” constraint to restrain attachment region: –Utility Menu > Plot > Areas –Main Menu > Solution > -Loads- Apply > -Structural- Displacement > -Symmetry B.C.- On Areas + Pick areas 18, 19, 25, and 26, then [OK] –Or issue: DA,18,SYMM DA,19,SYMM DA,25,SYMM DA,26,SYMM

Workshop Supplement January 20, 2001 Inventory # W2-13 2A. Stress Analysis Lathe Cutter 10.Apply pressure load at tip: –Main Menu > Solution > -Loads- Apply > -Structural- Pressure > On Areas + Pick area 1, then [OK] VALUE = [OK] –Or issue: SFA,1,1,PRES,10000

Workshop Supplement January 20, 2001 Inventory # W2-14 2A. Stress Analysis Lathe Cutter 11.Save the database and obtain the solution: –Click the “SAVE_DB” button in the Toolbar (or select: Utility Menu > File > Save as Jobname.db) –Main Menu > Solution > -Solve- Current LS Review the “/STATUS Command” window and then close it [OK] [Close] - to close the yellow message window after the solution is completed –Or issue: /SOLU SOLVE

Workshop Supplement January 20, 2001 Inventory # W2-15 2A. Stress Analysis Lathe Cutter 12.Review the results: 12a. Plot displacements: –Main Menu > General Postproc > Plot Results > -Contour Plot- Nodal Solu... Select “DOF solution” and “Translation USUM”, select “Def + undef edge”, then [OK] –Or issue: /POST1 PLNSOL,U,SUM,2,1

Workshop Supplement January 20, 2001 Inventory # W2-16 2A. Stress Analysis Lathe Cutter

Workshop Supplement January 20, 2001 Inventory # W2-17 2A. Stress Analysis Lathe Cutter 12b. List reaction forces: –Main Menu > General Postproc > List Results > Reaction Solu... Select “All items”, then [OK] –Or issue: PRRSOL

Workshop Supplement January 20, 2001 Inventory # W2-18 2A. Stress Analysis Lathe Cutter

Workshop Supplement January 20, 2001 Inventory # W2-19 2A. Stress Analysis Lathe Cutter 12c. Plot von Mises stress: –Main Menu > General Postproc > Plot Results > -Contour Plot- Nodal Solu... Select “Stress” and “von Mises SEQV”, then [OK] –Or issue: PLNSOL,S,EQV

Workshop Supplement January 20, 2001 Inventory # W2-20 2A. Stress Analysis Lathe Cutter 12d. Capture the image then minimize : –Utility Menu > Plot Cntrls > Capture Image –Minimize the window for later comparison

Workshop Supplement January 20, 2001 Inventory # W2-21 2A. Stress Analysis Lathe Cutter 12e. Animate the von Mises stress: –Utility Menu > PlotCtrls > Animate > Deformed Results... Select “Stress” and “von Mises SEQV”, then [OK] –Or issue: PLNSOL,S,EQV ANCNTR,10,0.5

Workshop Supplement January 20, 2001 Inventory # W2-22 2A. Stress Analysis Lathe Cutter

Workshop Supplement January 20, 2001 Inventory # W2-23 2A. Stress Analysis Lathe Cutter 13.Close the animation and delete the area symmetry constraints: [Close] –Utility Menu > Plot > Areas –Main Menu > Solution > -Loads- Delete > -Structural- Displacement > On Areas + Pick areas 18, 19, 25, and 26, then [OK] [OK] –Or issue: DADELE,18,ALL DADELE,19,ALL DADELE,25,ALL DADELE,26,ALL 14.Apply “ALL DOF” constraint to areas 18, 19, and 26: –Main Menu > Solution > -Loads- Apply > -Structural- Displacement > On Areas + Pick areas 18, 19, and 26, then [OK] Select “All DOF”, then [OK] –Or issue: DA,18,ALL DA,19,ALL DA,26,ALL

Workshop Supplement January 20, 2001 Inventory # W2-24 2A. Stress Analysis Lathe Cutter 15. Change the title: –Utility Menu > File > Change Title … Type in the title: Lathe Cutter - with ALL DOF constraint on areas at hole [OK] 16.Save the database and obtain the solution: –Pick the “SAVE_DB” button in the Toolbar (or select: Utility Menu > File > Save as Jobname.db) –Main Menu > Solution > -Solve- Current LS [OK] [Close] –Or issue: SAVE /SOLU SOLVE 17.Review the results: –Main Menu > General Postproc > Plot Results > -Contour Plot- Nodal Solu... Select “Stress” and “von Mises SEQV” [OK] –Or issue: PLNSOL,S,EQV

Workshop Supplement January 20, 2001 Inventory # W2-25 2A. Stress Analysis Lathe Cutter Open minimized plot from previous analysis to compare results

Workshop Supplement January 20, 2001 Inventory # W2-26 2A. Stress Analysis Lathe Cutter 17.Save and exit ANSYS: –Pick the “QUIT” button from the Toolbar (or select: Utility Menu > File > Exit...) Select “Save Everything” [OK] –Or issue: FINISH /EXIT,ALL

2-D Corner Bracket Tutorial Workshop 2B Stress Analysis

Workshop Supplement January 20, 2001 Inventory # W2-28 2B. Stress Analysis 2-D Corner Bracket Tutorial Description This workshop introduces you to ANSYS tutorials — solved, step-by-step examples that are available on-line in HTML format. The problem consists of a static analysis of a corner bracket modeled with 2-D plane stress elements.

Workshop Supplement January 20, 2001 Inventory # W2-29 2B. Stress Analysis 2-D Corner Bracket Tutorial 1.Enter ANSYS in the working directory specified by your instructor using “bracket” as the jobname. 2.Access the ANSYS on-line tutorials: –Utility Menu > Help > ANSYS Tutorials Open the “Structural Tutorial” folder Select the “Static Analysis of a Corner Bracket” folder Perform steps 1 through 26 –Or issue the following path in your browser’s “Go to:” window: Unix: \ansys57\docu\english\ansyshelp\Hlp_UI_Tutorials.html Intel-PC: D:/ansys57/docu/english/tuthelp.chm (Note, ask your instructor for the path name on your machine that points to the TUTORToc.htm file)