[AxelWal]

Hi all,

Firstly, just a small background. I am an Mech. eng. /designer and I have been self learning ANSYS and Fluent aside my job in-order to develop new skills, so bear with me if I am missing some obvious knowledge required to solve my issue. I have been reading a lot of forum posts and watching different tutorials in order to try to understand what is causing my issue, without resolve.

My issue is related to a very simple 2D buoyancy driven flow caused by a cable heating up. More specifically a single 10mm OD cable in free air. I have real life data of said cable gathered with 4 different currents.

For the simulation I have simplified the cable to a two layer object (core and boundary) and calculated an internal volumetric heat generation of the cable based on the resistance of individual wires. I have already used the ANSYS mechanical workbench to confirm that my baseline model of the simplified cable should be correct, by applying a simple convection to air on the surface of the cable and comparing the resulting data to the experimental data I have gathered. The results between mechanical sim. and real life agree within 0.1 degrees (kelvin/celsius) on multiple different currents.

In FLUENT I am simulating with pressured based solver, Ideal-Gas-Law based natural convection, laminar flow (the flow is very slow, and I am anyways only interested in what happens on the immediate vicinity of the cable, turbulence further upstream does not interest me), SIMPLE pressure velocity coupling (as suggested by ANSYS for boyancy driven flows) and PRESTO! pressure spatial discredization (as recommend by ANSYS).

I have succesfully done a 2D natural convection simulation of the cable inside a small and a large closed box in Fluent (all walls forced to a constant temperature).

The area of small box is roughly 20cm2 and the area of the large box is roughly 0.8m2

The small box converges very well with Steady state simulation to 1e-5 residuals for continuity and velocities and 1e-10 for energy. However the temperature of the cable is affected by the air recirculating back to the vicinity of the cable before reaching ambient temperature. Therefore the simulation is not a proper representation of a cable in free air.

The trouble begins with the large box. The idea of using large box is to ensure surrounding air reaches ambient temperature before circulating back to the cable. The exact same input with a larger box is unable to converge in Steady state, and I have to do an Transient simulation with adaptive time stepping (to save simulation time) in order to reach convergence. The results do agree with real life data on the cable temperature. However running the simulation takes unnecessarily long (one hour as opposed to one minute with steady state).

The real issue is when I try to use the exact same input as the small or the large box has, but instead open one or multiple sides the box to represent a real life scenario where the cable is just hanging in free air, without anything surrounding it. If I open any side of the box by applying a pressure-inlet or -outlet boundary condition, the simulation is not able converge with steady or transient solver, and instead just oscillates from the very beginning. I tried checking the contrours of velocity, density and temperature with different open box boundary conditions applied during the calculation, and it looks like Fluent is trying to reproduce a picasso painting every time.

TLDR; I am able to do a simulation of a cable (and multiple cables) in a small closed box with natural convection air circulation, but struggling heavily trying to simulate the cable in free air.

If someone is able to understand my explanation and is willing to help a beginner, I would highly appreciate. If someone has some literature or tutorial I could look at regarding natural convection in free air in FLUENT, it would also be extremely helpful. Moreover is what I am trying to do even possible with FLUENT?

The reason I want to simulate the cable in complete free air, is to verify that the same method of simplifying the cable as I have done in Mechanical workbench is also correct in Fluent, and to find out the impact of different sizes of inflation layers etc. in order to verify that Fluent is spitting out correct results when compared to real life data, before proceeding to more complex simulations with closed volumes.

[MKuhn]

Hi Axel, the flow of a natural convection can be so randomly, that a steady state solution does not exist. Hear are some hints: The idea of the pressure boundaries should be the right way. I would recommend a pressure inlet on the bottom and a pressure outlet on the top, with a slightly lower pressure as at the inlet. Sometimes it helps to use a turbulence model, even the flow is laminar in global-scale. Also try to start with a lower heat load in your cable. Use Incompressible Ideal Gas Law instead of Ideal Gas Law. Leave the operating pressure by default of 101325 Pa.

[AxelWal]

Originally Posted by MKuhn

Hi Axel, the flow of a natural convection can be so randomly, that a steady state solution does not exist. Hear are some hints: The idea of the pressure boundaries should be the right way. I would recommend a pressure inlet on the bottom and a pressure outlet on the top, with a slightly lower pressure as at the inlet. Sometimes it helps to use a turbulence model, even the flow is laminar in global-scale. Also try to start with a lower heat load in your cable. Use Incompressible Ideal Gas Law instead of Ideal Gas Law. Leave the operating pressure by default of 101325 Pa.

Hi!

Thanks for your response, sorry for late reply, I managed to yesterday solve all of my convergence and correlation issues. The original post was a bit messy, but here is what I did:

1. Symmetry of the problem along the vertical axis, instead of trying to simulate the whole volume. This I think mainly solves the steady state issue for the boyancy problem. When observing the flow, I could see that it is indeed bouncing back and forth between the two sides of the volume.

2. I only "opened" the top of the simulated fluid volume, and I used an "pressure outlet" boundary condition with normal to boundary backflow direction with ambient temperature, this in combination with the symmetry along vertical axis allowed new air to flow down along the edges and circulate back up when the cable was heating the air.

3. Improved mesh, I improved the resolution and the inflation layer, this most likely helped with convergence a lot. I have now checked, and improving the mesh further has negligible impact on results.

4. Switched to double precision, this seems to help with erronous convergence in first iterations.

5. Added radiation equations, for a single cable in free case I simply used Rosseland. Radiation seemed to be my missing link to get the model to correlate with real life data.

Here are some pretty pictures if you are curious

https://imgur.com/a/qVesLlr