Introduction
In this article we will discuss a uniform thermal expansion test case performed in ANSYS and compare it to the analytical solution (hand calculation).
Geometry, Mesh and Material
The geometry is a flat plate with dimensions of 150 mm X 150 mm X 10 mm with a 75 mm diameter thru hole at its center.
The figure below shows the mesh generated on the body. The material chosen is Aluminum with 2.1E-5 /C coefficient of thermal expansion.
Boundary Condition and Load
We want the plate to expand about its midpoint (center of the hole). The easiest way to do this is to create a remote displacement scoped to the plate surface as shown. Th point at the center of the plate is essentially fixed in all DOF and each node on the plate surface is scoped to it. This allows all the nodes on the surface to translate “about” the center.
The environment temperature (initial temperature) was set to 20C and a temperature of 520C was applied, giving a delta T of 500C.
Results
The Figure below shows the total deformation of the plate. The deformation is symmetric along the center line of the plate.
Figure 5 shows an animation of the expansion at X10 Scale. The wireframe represents the original un-deformed position of the plate.
Finally, the X and Y direction deformations are shown below side by side.
We can see (from Figure 4) that the hole diameter increases by 2*(0.39375) = 0.7875 mm and the plate sides elongate ( by 2*(0.7875) = 1.575 mm
Results Verification
we will now perform the hand calculation and compare it to the FEA results.
We know that all dimensions of the plate should increase. For a dimensions, X
Delta X = (CTE)*(Delta T)*(X)
Delta Side = (2.1E-5)*(500)*(150) = 1.575 mm
Delta Diameter = (2.1E-5)*(500)*(75) = 0.7875 mm
We can see that the analytical and numerical results match exactly.
I hope this simple tutorial was of use. Feel free to leave a comment with any questions.
Important Point
It is important to note that we have performed the simulation of an idealized scenario of uniform expansion about plate center. In real world, the plate would be constrained a certain way (for example bolted at certain locations) which would affect the way it would deform under thermal load.