**1. Introduction**

For those of you who are choosing a cylinder for the body of the ROV, this note
gives some tips about carrying out FEA for the analysis of a cylinder.

**2. FEA Model Details**

It was assumed that the cylinder was:

- Made from aluminium
- Outside diameter of 250 mm
- Overall length (between restraints) of 1.005 m
- Thickness of all surfaces: 5 mm
- External pressure was 1 MPa.

**3a. Using Solid Works and COSMOSWorks**

The following is probably the easiest way to do the analysis assuming there are no ends in the cylinder, but that it is constrained from buckling by reinforcements (restraints) at 1 m intervals. A 90 degree arc of the cylinder will be modelled, as by using appropriate constraints (roller / sliding on the straight edges) this allows first mode buckling to be simulated. Only half the length is modelled (0.5m) and with one end un-constrained and the other end fixed, this provides the equivalent to 1 m length, but simplifies model set up.

- 1. In Solid Works, start a New, Part. Start Sketch, Click on Front Plane.
- 2. Using Cetre, Start Arc and Finish Arc draw 90 degrees of arc. Repeat with and Arc of larger radius. Exaggerate the differences between the arcs for ease of drawing.
- 3. Using Line connect the ends of the inner and outer arcs together.
- 4. Using Dimension, measure radius of inner arc and separation between inner and outer arcs.
- 5. Change the dimensions in (4) double click on them and enter 120mm and 5 mm respectively.
- 6. End Sketch
- 7. Click on Extrude Base and enter depth of 500 mm and click OK.
- 8. From the COSMOSWorks menu click on Study, type in a name and then select Static for the stress anaylysis and Buckling for the buckling analysis.
- 9. Apply material (AL 3003 is probably 'nearest most likely').
- 10. Apply restraints to one end face and the two straight side faces.
- 11. Apply a pressure load to the external cylindrical surface of the cylinder of 1000000N/m
^{2} - 12. Mesh the component.
- 13. Run the Job.
- 14. Look at the results, Check that the plots of the deformed shape and displacement is reasonable. Look at the Stress plot for the stress analysis and Displacement for the buckling analysiss.
- 15. By right clicking on the 'Stress' in the left hand column, then click on Define, the stresses plotted can be changed.
- 16. Using Results Tools, Probe, stresses at specific points can be displayed in a table and plotted.

**3b. Results of the Static Analysis**

These results are away from the constrained end.

The three principal stresses on the outer curved surface away from the ends were:

- Sigma 1: 0
- Sigma 2: -1 MPa
- Sigma 3: -24.5 MPa
- von Mises stress on inner surface was 25.5 MPa and 24 MPa on the outer surface.

The theoretical hoop stress, sigma = pressure x radius/thickness = -25 MPa.

**3c. Results of the Buckling Analysis**

The buckling factor was 4.519, indicating that the theoretical external pressure to cause
buckling was 4.5MPa. Under an external pressure of 4.5 MPa the maximum von Mises stress
would be just under 115 MPa, which is below the yield strength of most aluminium alloys.

**4a. Using Pro/E and Mechanica Structure**

Here it is assummed that a cylinder with flat ends is being modelled:

- 1. Do the modelling of the complete cylinder in Pro/E, it is assumed that the circular section is in the X-Y plane with the Z axis coincident with the cylinder axis (one surface of one of the end faces should be at Z=0).
- 2. To simplify placing constraints, cut away three quarters of the cylinder, leaving the quarter in the +ve X +Y quadrant.
- 3. Construct a point at X=0, Y=0, Z=0, on one surface of one of the ends.
- 4. Transfer the model to Mechanica Structure.
- 5. Specify the material.
- 6. Apply the pressure to the curved outer surface and to the outer surfaces of the two ends.
- 7. Apply the constraints - symmetry along the faces that lie in the X-Z plane and in the Y-Z plane and fix the constructed point on the X=0, Y=0, Z=0 to have zero translation in the Z direction.
- 8. Set up and carry out a Static Analysis.
- 9. Note the values of the three principal stresses.
- 10. Set up and carry out a Buckling analysis.
- 11. Note the Buckling Factor.

Autogem produced 1316 elements

**4b. Results of the Static Analysis**

The three principal stresses on the outer curved surface away from the ends were:

- Sigma 1: -1MPa
- Sigma 2: -12.75 MPa
- Sigma 3: -24.5 MPa
- von Mises stress: 20.36 MPa

The theoretical hoop stress, sigma = pressure x radius/thickness = -25 MPa.

**4c. Results of the Buckling Analysis**

The constraints applied allow the expected first buckling mode for a cylinder,
but it should be noted that achieving in practice the theoretical results depends upon high
geometric accuracy of the manufactured item, even very minor variation from the
stated dimensions can cause large reductions in the buckling loads.

The buckling load factor, mode 1, was 3.4 from the Mechanica analysis.
This means that buckling would occur at an external pressure of 3.4 MPa.
This would give a von Mises stress of
69MPa, which is well below the yield strength of any aluminium alloy.

**5. Differences in Results**

It should be noted that what seem like minor differences between these two
approaches has given quite different results. The reason for this is:

The Cosmos model had no closed ends and no axial load and zero axial stress, whereas the Mechanica model had closed ends, with pressure applied to them and consequently an axial stress equal to half the radial stress.

You should note that although these differences are significant, even very minor changes or errors in loads and especially in restraints can make very big differences to results.

The mode 1 deformed shape from COSMOSWorks is shown below:

The mode 1 deformed shape from Mechanica is shown below:

The calculation below uses the approximate formula from Roark for a short cylinder length L with the ends held circular but not otherwise constrained:

This gives the failure pressure as 2.46 MPa, somewhat lower than the 3.4 MPa and 4.5 MPa computed by the FEA, above.

Return to Module Introduction

David J Grieve, 12th September 2006, (previously 26th February 2003).