ME 455/555 Intro to Finite Element Analysis Fall 2011 Abaqus/CAE Axisymmetric tutorial

Abaqus/CAE Axisymmetric Tutorial (Version 6.11)

Problem Description
A round bar with varying diameter has a total load of 1000 N applied to its top face. The bottom of the bar is completely
fixed. Determine stress and displacement values in the bar resulting from the load.

©2011 Hormoz Zareh & Jenna Bell 1 Portland State University, Mechanical Engineering
ME 455/555 Intro to Finite Element Analysis Fall 2011 Abaqus/CAE Axisymmetric tutorial

Analysis Steps
1. Start Abaqus and choose to create a new model database
2. In the model tree double click on the “Parts” node (or right click on “parts”
and select Create)

3. In the Create Part dialog box (shown above) name the part and select
a. Axisymmetric
b. Deformable
c. Shell
d. Approximate size = 0.2
4. Create the geometry shown below (not
discussed here). *Note axisymmetric
parts must be drawn about the marked
axis of rotation.

©2011 Hormoz Zareh & Jenna Bell 2 Portland State University, Mechanical Engineering
ME 455/555 Intro to Finite Element Analysis Fall 2011 Abaqus/CAE Axisymmetric tutorial

5. Double click on the “Materials” node in the model tree

a. Name the new material and give it a

description
b. Click on the “Mechanical”
tabÎElasticityÎElastic
c. Define Young’s Modulus and the Poisson’s
Ratio (use SI units)
i. WARNING: There are no predefined
system of units within Abaqus, so the
user is responsible for ensuring that
the correct values are specified

6. Double click on the “Sections” node in the model tree

a. Name the section “AxisymmetricProperties” and select
“Solid” for the category and “Homogeneous” for the type
b. Select the material created above (Steel)

©2011 Hormoz Zareh & Jenna Bell 3 Portland State University, Mechanical Engineering
ME 455/555 Intro to Finite Element Analysis Fall 2011 Abaqus/CAE Axisymmetric tutorial

7. Expand the “Parts” node in the model tree and double click on “Section Assignments”
a. Select the surface geometry in the viewport
b. Select the section created above (Axisymmetric_Properties)

8. Expand the “Assembly” node in the model tree and then double click on “Instances”
a. Select “Dependent” for the instance type

9. In the model tree, under the expanded “Assembly” node, double click on “Sets”

©2011 Hormoz Zareh & Jenna Bell 4 Portland State University, Mechanical Engineering
ME 455/555 Intro to Finite Element Analysis Fall 2011 Abaqus/CAE Axisymmetric tutorial

a. Name the set “Fixed”

b. Select the lower edge of the surface in the viewport

c. Create another set named “Symmetry”

d. Select the left edge of the surface in the viewport

10. In the model tree, under the expanded “Assembly” node, double click on “Surfaces”
a. Name the surface “PressureLoad”
b. Select the top edge of the surface in the viewport

©2011 Hormoz Zareh & Jenna Bell 5 Portland State University, Mechanical Engineering
ME 455/555 Intro to Finite Element Analysis Fall 2011 Abaqus/CAE Axisymmetric tutorial

11. Double click on the “Steps” node in the model tree

a. Name the step, set the procedure to “General”, and select “Static, General”
b. Give the step a description

12. Expand the Field Output Requests node in the model tree, and then double click on F-Output-1 (F-Output-1 was
automatically generated when creating the step)
a. Uncheck the variables “Strains” and “Contact”

13. Expand the History Output Requests node in the model tree, and then right click on H-Output-1 (H-Output-1 was
automatically generated when creating the step) and select Delete

©2011 Hormoz Zareh & Jenna Bell 6 Portland State University, Mechanical Engineering
ME 455/555 Intro to Finite Element Analysis Fall 2011 Abaqus/CAE Axisymmetric tutorial

14. Double click on the “BCs” node in the model tree

a. Name the boundary conditioned “Fixed” and select “Symmetry/Antisymmetry/Encastre” for the type

b. In the prompt area click on the Sets button

c. Select the set named “Fixed”

d. Select “ENCASTRE” for the boundary condition

e. Repeat the procedure for the symmetry restraint using the set
named “Symmetry”, select “XSYMM” for the boundary
condition

©2011 Hormoz Zareh & Jenna Bell 7 Portland State University, Mechanical Engineering
ME 455/555 Intro to Finite Element Analysis Fall 2011 Abaqus/CAE Axisymmetric tutorial

15. Double click on the “Loads” node in the model tree

a. Name the load “Pressure” and select “Pressure” as the type

b. Select surface named “Pressure”

c. For the magnitude enter the applied pressure in F/L2
∗ .

©2011 Hormoz Zareh & Jenna Bell 8 Portland State University, Mechanical Engineering
ME 455/555 Intro to Finite Element Analysis Fall 2011 Abaqus/CAE Axisymmetric tutorial

16. In the model tree double click on “Mesh” for the Bar part, and in the toolbox area click on the “Assign Element
Type” icon
a. Select “Standard” for element type
b. Select “Linear” for geometric order
c. Select “Axisymmetric Stress” for family
d. Note that the name of the element (CAX4R) and its description are given below the element controls

17. In the toolbox area click on the “Assign Mesh Controls” icon
a. Change the element shape to “Quad”
b. Change the Algorithm to “Medial axis” for a more structured mesh

©2011 Hormoz Zareh & Jenna Bell 9 Portland State University, Mechanical Engineering
ME 455/555 Intro to Finite Element Analysis Fall 2011 Abaqus/CAE Axisymmetric tutorial

18. In the toolbox area click on the “Seed Part” icon

a. Set the approximate global size to 0.0015

19. In the toolbox area click on the “Mesh Part” icon

20. In the model tree double click on the “Job” node

a. Name the job “Bar”
b. Give the job a description

©2011 Hormoz Zareh & Jenna Bell 10 Portland State University, Mechanical Engineering
ME 455/555 Intro to Finite Element Analysis Fall 2011 Abaqus/CAE Axisymmetric tutorial

21. In the model tree right click on the job just created (Bar) and select “Submit”
a. While Abaqus is solving the problem right click on the job submitted (Bar), and select “Monitor”

b. In the Monitor window check that there are no errors or warnings

i. If there are errors, investigate the cause(s) before resolving
ii. If there are warnings, determine if the warnings are relevant, some warnings can be safely
ignored

22. In the model tree right click on the submitted and successfully completed job (Bar), and select “Results”

23. In the menu bar click on ViewportÎViewport Annotations Options

a. Uncheck the “Show compass option”
b. The locations of viewport items can be specified on the corresponding tab in the Viewport Annotations
Options

©2011 Hormoz Zareh & Jenna Bell 11 Portland State University, Mechanical Engineering
ME 4555/555 Intro to Fin
nite Element Analyysis Fall 2011 Abaq
qus/CAE Axisymm
metric tutorial

2
24. Display th
he deformed contour
c of the (Von) Mises stress
a. Inn the toolbox area click on the “Plot Con
ntours on De formed Shappe” icon

©20111 Hormoz Zareh & Jenna Bell 12 Portland Statee University, Mech
hanical Engineering
ME 4555/555 Intro to Fin
nite Element Analyysis Fall 2011

2
25. To determ
mine the stresss values, fromm the menu bar b click Tool sÎQuery
a. Check the boxe es labeled “N
Nodes” and “SS, Mises”
b. Inn the viewporrt mouse overr the elementt of interest
c. Note that Abaq qus reports stress values from
f the integgration point
vaalues determined by proje ecting values from
f surrounnding integrat
i. The minimum and maximum
m strress values coontained in th
projeccted to the no
odes
d. Click on an element to store e it in the “Se
elected Probee Values” port

2
26. To change
e the output being
b displayed, in the me
enu tool bar cclick on Result
a. Se
elect “Spatial displacemennt at nodes”
i. Invariaant = Magnitu
ude

©20111 Hormoz Zareh & Jenna Bell 13