[luk1]

Hello everybody,

I am about to run RANS simulations in a Backward facing step domain and I am using ANSYS CFX.
There is a heating plate at the bottom wall right behind the step. As a result, strong turbulence and heat transport occur in the same region. Of course, I expect a steady-state solution.
The isothermal simulation works well and the momentum field converges quickly. Since the problems occur as soon as heat enters the system, the energy equation seems to be responsible for the issues.

The complexity of the settings in CFX is reduced to the required minimum:
• heat flux BC for the heated wall; adiabatic BC for the other walls
• „thermal energy“ equation for the heat transer
• SST model
• no buoyancy

Reaching 200 time steps, the velocity field is solved properly and according to physics.
The conservation criteria (0.01) is met for all equations while the residual criteria (max. 1E-5) is met for all but the energy equation where drops to the order of magnitude 1E-1 after around 150 iterations and remains at this level--> see picture

The temperature field has kind of an instability right at the edge of the step close to the confining side walls which shows up fort he first time after around 150 time steps. It leads to a blow up of the temperature resulting in an unphysical range from 0 to 700K (instead of 300 to 310K) in this region. --> see picture (position: 0.1 mm from the wall in an 80mm wide channel)

An interesting observation is that the fluctuating rise and decrease of the temperature has a periodic behaviour --> see picture

The first assumption would be that the mesh is too coarse and not smooth enough for the small temperatur gradients in this particular region. So far, I have put a lot of work into the refinement of the mesh: every important requirement for a mesh seems to be met. Besides from that, I had the same issues when using a well-tried mesh which already delivered proper results for LES simulations.

What might be the reason for this behaviour? What could I do to „stabilize“ the simulation?
I also have access to FLUENT, in case this software offers more possibilities to take influence.
Thanks for helping!

[Opaque]

Have you tried decreasing your timestep a bit? say 1/2 of the current value.

The diagnostics shown indicates your timestep is just a bit aggressive, see work units for mass and momentum/turbulence

[luk1]

I could fix it in the end by using the advanced control option "Temperature damping" where I set a value 0.2. It helped avoiding the blow up of the temperature in this particular region. I also checked that the problem was fixed and not only postponed to higher iteration numbers.

In order to fix the problem with the work units for mass and momentum I set back the conservative lengthscale option for all equations. Before, aggressive was set here.