ME 4180 Fall 2015Name

ANSYS Lab 1

Given:

The following steel stepped shaft is to be analyzed using finite elements. Dimensions are in mm.

Required:

(a) Use ANSYS to construct three models of the component using BEAM188 elements. Make one model very coarse (9 elements each of length 50 mm), a second, finer model (18 elements each of length 25 mm), and a third model finer still (90 elements, each of length 5 mm). Do not attempt to model the fillets. (b) Prepare a table to compare the displacements and stresses using ANSYS with your hand calculations. For hand calculations of displacements, make a rough estimate by assuming that the shaft has a uniform cross-section of 40 mm diameter. For this rough estimate, you should use the beam tables and superposition. (c) Include plots of deformed shapes and stress contours for xx. Include convergence plots of the vertical displacements at the locations of the applied loads. Discuss your results thoroughly.

Soln:

Getting Started

  • Create folder in C:temp called myshaft
  • Start ANSYS using the interactive button
  • Set directory to the folder you set up in C:temp, give a jobname
  • Pick analysis type:
In ANSYS menu tree: Preferences/structural, h-method

Model Setup (Preprocessing)

Under Preprocessor/

  • Select element type:

/ Element type/ Add-Edit-Delete/ add button, beam 188(check options)

  • Input material properties:

/ Material properties/ Material Models/ Structural/ Linear/ Elastic/ Isotropic

E= 207GPa (enter as 207,000 MPa)

= 0.3 (try 0 even, it shouldn’t matter, but why?)

  • Create section profiles:

/ Sections/ Beam/ Common Sections/

  • Need 3 sections
  • Use apply button, be sure to change section number, diameter, and section profile.
  • Creating the geometry: (Lines require Keypoints, also place a Keypoint at the load location)

/ Modeling / Create/ Keypoints/ In Active CS

  • Type in coordinates for the endpoints of all lines (don’t supply a number and ANSYS will do it for you.)
  • Place an orientation Keypoint a long distance away from the model (number this something easy to remember like 9999)

/ Modeling / Create/ Lines/ Lines/ Straight line

  • Pick keypoints that makeup the lines.

(The zoom feature is under Plot Controls on the pull down menu)

Meshing the model:

/ Meshing/ Mesh Tool/

  • Element Attributes change pull down to lines and click set
  • Pick a line and assign the appropriate section number to it, also check the box for Orientation Keypoint
  • It will now ask for the Orientation Keypoint, type in its number, hit enter, and then click OK
  • Repeat as necessary (you can pick multiple lines that have the same attributes
  • Now mesh the model, by clicking the mesh button and picking the lines (notice that the lines turned blue, to see the elements sized appropriately take the next step, it is not necessary however)

Displaying size and shape of beam

/ In the PlotCtrls pull down menu

  • PlotCtrls/Style/Size and Shape/
  • Check the box labeled Display of Element.

Apply appropriate loads and boundary conditions:

/ Loads/ Define Loads/ Apply/ Structural/ Displacement/ On Keypoints

/ Loads/ Define Loads/ Apply/ Structural/ Force Moment/ On Keypoints (use N, not kN)

Solve the Model

Under Solution/

/ Solve/ Current LS

Examining the Results (Postprocessing)

Under General Postproc/

/Plot Results

/Query Results

Under PlotCtrls/Hard Copy/To File... (use .jpg or .png and give filename)

HW Reporting Guidelines

Raw Results

1. Figures of three different models showing element layout

2. Statement of boundary conditions

3. Contour plots of appropriate displacements and stresses (v, xx, xy)

4. Table of comparisons for displacement and stress (compare ANSYS FEA models to hand calculations using simple beam theory)

5. Converge plots using displacements at load points

Form and Style

1. Title Page

  • appropriate
  • brief, but complete

2. Abstract—brief condensation of the lab report

  • precise statement of the problem
  • description of methods/approach
  • major findings
  • conclusions
  • no external citations
  • no more than 200-250 words

3. Introduction

  • nature of the problem
  • purpose of investigation
  • scope of investigation
  • method of investigation

4. Technical Approach

  • overall plan of attack (further development of method of investigation)
  • necessary technical background
  • description of solution method(s)

5. Results and Discussion

  • description of results
  • trends among results
  • comparison to other solutions
  • appropriate tables and figures

6. Conclusions and Recommendations

  • main principles discovered in results
  • causal relations shown by results
  • generalizations shown by results
  • interpretations of results in light of previous studies
  • unresolved issues
  • points for further study

7. References

  • as necessary
  • enough detail to actually find

1