IV. Axisymmetric Analysis

Here axisymmetric analysis of a structure is introduced.

1.      DesignModeler

2.      Click Project tab > Advanced Geometry Defaults > select 2D for Analysis Type

3.      First, in a sketcher, sketch a line by [Draw > Line and Arc by Tangent] and use [Modify > Fillet] to round the lower right corner.

4.      Then, Offset > ctrl + select all lines > RMB > End Selection / Place Offset > move the cursor outward and click it to place the offset. RMB > End (end the offset). Draw lines at both ends to close the section. Also, place dimensions as:

Axisymmetric: Assumes that a 3-D model and its loading can be generated by revolving a 2-D section 360o about the y-axis. The axis of symmetry must coincide with the global y-axis. The geometry has to lie on the positive x-axis of the x-y plane. The y direction is axial, the x direction is radial, and the z direction is in the circumferential (hoop) direction. The hoop displacement is zero. Hoop strains and stresses are usually very significant. Example uses are pressure vessels, straight pipes, and shafts. Axisymmetric behavior cannot be used in a shape simulation.

5.      Concept > Surfaces from Sketches > select the sketch in Tree Outline > Apply > Generate.

6.      Project tab > New Simulation > Stress Branch – Ductile Materials.

7.      Click the surface body under Model > Geometry in the Tree Outline (see below) and then in the Details View, click Definition > Behavior > select Axisymmetric.

8.      Accept the material as is > Insert Supports > Structural > Given Displacement > (change the cursor selection mode) RMB > Cursor Mode > Edges > ctrl + select two end edges along the vertical axisymmetric axis > Apply > specify zero only for x-component.

9.      Structural > Pressure > ctrl + select all inner edges > Apply > enter 30 psi for Magnitude.

10.  Solve. The solution issues warning for under-constrained model. This is ok.

11.  Click Solution / Equivalent Stress in Tree Outline.

12.  Edges > Show Undeformed Wireframe

13.  See the total deformation with the mesh and the Safety Factor under Stress Tool. Note that the safety factor shows dangerous design.

IV. Axisymmetric Analysis in 3D

Here 3D axisymmetric analysis of a structure is introduced.

1.      DesignModeler

2.      Sketch the section as below and Generate.

3.      Modeling > select the sketch > Revolve > pick the vertical axis for rotation axis > Apply > keep 30 for Angle > select Yes for As Thin/Surface? And enter 0.125 for both Inward and Outward Thickness > Generate.

4.      New Plane > select Rotate about Y for Transform 1 > enter -30 for Value 1 > select Yes for Export Coordinate System > Generate. The model appears as the second figure above.

5.      Click Project tab > New Simulation

6.      Stress Branch – Ductile Materials

7.      Insert Supports > Structural > Given Displacement > ctrl + select all edge lines on one side > Apply > select the plane name that contains local coordinate system > enter zero only for z-component > hit CR

8.      Repeat this for the other edge with global coordinate system.

9.      Repeat this for both vertical tips at the center and enter zeros for x- and z-components > hit CR.

10.  Structural > Pressure > ctrl + select all inner surfaces > Apply > enter 30 for Magnitude > hit CR.

11.  Solve. Warning message appears for attached weak spring for solution. This is ok.

12.   The results appear as:

From the result for Safety Factor, it is noted that the design must be changed. Especially, the max stress occurs at the center of bottom lid that is flat. The stress distribution on the spherical top lid is minimal in contrast.