FEATool Multiphysics
v1.16.1
Finite Element Analysis Toolbox

This validation test case models temperature loading of a tapered hollow thick cylinder with a spherical bottom flange section. The solid object is assumed to be clamped vertically, but allowed to expand horizontally due to a linear temperature gradient. The stress in the zdirection at the bottom inner point is computed and compared to a reference value [1].
This model is available as an automated tutorial by selecting Model Examples and Tutorials... > Structural Mechanics > Temperature Loading of a Tapered Cylinder from the File menu, viewed as a video tutorial, or alternatively, follow the stepbystep instructions below.
Select the Linear Elasticity physics mode from the Select Physics dropdown menu.
The geometry consists of a thick cylindrical pipe section connected to a spherical bottom flange with a taper. As the geometry is axially symmetric, it is easiest to create by first using a 2D workplane to draft the crosssection, which then can be revolved into the three dimensional space.
Workplanes are defined by a point (local origin), normal (blue) and tangent vectors (yellow and red). The green circle shows a preview where the plane will be located in 3D space.
0 0 0
into the Workplane point edit field.0 1 0
into the Workplane normal vector edit field.Enter 1 0 0
into the Workplane tangent vector edit field.
Note that the local coordinate system will be mirrored in the yaxis. The outline sketch will therefore be drawn upside down so as to be in the positive halfplane of the 3D space.
First create a rectangle to cover the modeling region.
0.7071
into the x_{min} edit field.1.4
into the x_{max} edit field.1.79
into the y_{min} edit field.0
into the y_{max} edit field.Now create two circles, one with radius 1 and the other with 1.4.
1
into the radius edit field.1.4
into the radius edit field.Then make a polygon for the cylindrical connection.
Enter the following data into the Point coordinates table.
x  y  

1  0.7071  0.7 
2  1.2124  0.7 
3  1  1.39 
4  1  1.79 
5  0.7071  1.79 
The shape of the crosssection can be created by joining the polygon with the outer circle, subtracting the inner circle, and taking the intersection with the rectangle.
Select C2 and P1 in the geometry object Selection list box.
Press the & button.
The 2D outline sketch can now be revolved to a 3D solid (an outline preview of the revolution shape is shown in the 3D view). As this geometry is symmetric it is enough to model a quarter section and thereby also reducing the mesh size leading to faster simulations.
90
into the Revolution angle edit field.0 0 0
into the Revolution axis reference point edit field.Enter 0 1 0
into the Revolution axis vector edit field.
Select Close Workplane from the Options menu or press the close button in the Workplane window to go back to the main 3D modeling view.
The default grid may be too coarse to ensure an accurate solution. Decrease the grid size to 0.1 to generate a finer grid that better can resolve curved boundaries.
Press the Generate button to call the automatic grid generation algorithm.
0.3
for the Poisson's ratio and 210e9
for the Modulus of elasticity.Note that FEATool works with any unit system, and it is up to the user to use consistent units for geometry dimensions, material, equation, and boundary coefficients.
The temperature load is a linear expression in the radial direction sqrt(x^2+y^2)+z, but can also be coupled through the temperature from a heat transfer physics mode.
2.3e4
into the Thermal expansion coefficient edit field.sqrt(x^2+y^2)+z
into the Temperature edit field.As the quantities of interest here are stresses, it is appropriate to use a higher order discretization. This will result in more accurate evaluation of quantities involving derivatives of the solution variables such as stresses.
Select (P2/Q2) second order conforming from the FEM Discretization dropdown menu.
The two side boundaries are due to symmetry, and should therefore have their displacements constrained in the corresponding normal directions.
The solid should be clamped in the vertical direction, that is the zdisplacement at the top and bottom boundaries should be fixed.
Select the Fixed displacement, w radio button.
Open the postprocessing settings dialog box and select the zcomponent of the stress to visualize.
Press the Go to YZ View toolbar button.
The stress at the inner point (1, 0, 0) should be evaluated and compared to the reference value.
1
into the Evaluation coordinates in xdirection edit field.0
into the Evaluation coordinates in ydirection edit field.Enter 0
into the Evaluation coordinates in zdirection edit field.
The stress evaluated in the point compares well to the reference value of 105·10^{6} Pa.
The temperature loading of tapered cylinder structural mechanics model has now been completed and can be saved as a binary (.fea) model file, or exported as a programmable MATLAB mscript text file, or GUI script (.fes) file.
[1] NAFEMS publication TNSB, Rev. 3, The Standard NAFEMS Benchmarks, LE11 Solid Cylinder/Taper/Sphere  Temperature Loading Benchmark, 1990.