FEALAB

 2. STRUCTURAL ANALYSIS ON THE TAPERED BAR

AIM: Determine the displacement and stress distribution in the Tapered bar due to application

of 10 kN of tensile force. The bar is made of steel (E = 210 x 109 Pa, Poisson ratio = 0.3).

Software Used: ANSYS Mechanical APDL

Procedure:

Step 1: Launch ANSYS

# Main Menu > Preferences > Structural and h-method

Step 2: Define Element Type

# Main Menu > Preprocessor > Element Type > Add/Edit/Delete - ADD

# Select Link and 3D finit stn 180 - OK

# element type - 1

Step 3: Define Element Cross Sectional Area (Section Properties)

# Main Menu > Preprocessor > Sections > Link > Add

# Add link section with id - 1  -OK

# cross sectional area (SECDATA): 0.000433

#Preprocessor > Sections > Link > Add

# Add link section with id - 2  -OK

# cross sectional area (SECDATA); 0.000299

#Preprocessor > Sections > Link > Add

# Add link section with id - 3  -OK

# cross sectional area (SECDATA): 0.000166

# Utility menu > List > Properties > Section Properties

Step 4: Define the Material Behavior

# Preprocessor > Material Props > Material Models, the Define Material Model

# Structural > Linear > Isotropic

# (E = 210 x 109 Pa, Poisson ratio = 0.3) - OK

Step 5: Define Nodes and Elements

# Preprocessor > Modeling > Create > Nodes > In Active CS

# x-coordinate for node 1 (i.e. 0) - Apply

   x-coordinate for node 2 (i.e. 0.2) - Apply

   x-coordinate for node 3 (i.e. 0.4) - Apply

   x-coordinate for the final node, node 4 (i.e. 0.6) - OK

#Preprocessor > Modeling > Create > Elements > Auto Numbered > Thru Nodes

# click on node 1 and then node 2. -  Apply

   click on node 2 and then node 3 - Apply

   click on node 3 and then node 4 - OK

# Preprocessor > Modeling > Move/ Modify > Elements > Modify Attrib

# Pick element number 2 - OK

# STLOC Attribute to change - Section Num SEC

# New Attribute Number - 2  -OK

# Preprocessor > Modeling > Move/ Modify > Elements > Modify Attrib

# Pick element number 3 - OK

# STLOC Attribute to change - Section Num SEC

# New Attribute Number - 3  -OK

# Utility Menu (top of the window)

# List > Elements > Nodes & Attributes

Step 6: Define Boundary Conditions

# Preprocessor > Loads > Define Loads > Apply > Structural > Displacement > On Nodes

# Select Pick All

# Select both UY and UZ

# displacement value - 0

# Preprocessor > Loads > Define Loads > Apply > Structural > Displacement > On Nodes

# Click on Node 1 - OK

# select UX ,UY and UZ

# displacement value - 0  - OK

Step 7: Define Loads

# Preprocessor > Loads > Define Loads > Apply > Structural > Force/ Moment > On Nodes

# Pick node 4 - OK

# direction of force - FX

# Force/ Moment value - 10000  -OK

Step 8: Solve the Problem

# Main Menu > Solution > Analysis Type > New Analysis

# Static - OK

# Solution > Solve > Current LS - OK

Step 9: Examine the Results

# Main Menu > General Postproc > List Results > Nodal Solution > DOF solution > Displacement Vector Sum - OK

# Results Viewer and select displacement vector sum and contour - close

# General Postproc > Element Table > Define Table > Add

# add the "1" after "LS,”  -  OK  - Close

# General Postproc > Plot Elem Table   and pick "AXIALSTR"  -  OK

Results: The nodal displacement and nodal stress values are shown in below table: