[khoopes]

I am having some trouble on a steady state simulation where I am coupling CFX with ANSYS, I keep getting really high temperatures on the CFX side, right before the simulation explodes after 30 or so iterations (2 or 3 exchanged with ANSYS). Right now I am trying to duplicate what I already have done within CFX as a CHT model but using ANSYS as an external solver for the heat transfer. This is so I can then move to a full 2 way FSI with a moving mesh later. So far these are the things that I have tried.

1. I checked all the material properties and units systems and made sure they were consistent. They were fine.
2. I checked the mesh and insured that it had a similar size on the fluid and solid sides.
3. I checked the boundary conditions and ran the fluid simulation on its own to make sure that it was working fine.
4. I made sure that the ANSYS starting temperature and the CFX starting temperature are the same so that initially there is not a huge heat flux.
4. I slowed the data transfer down by changing the under relaxation factor. This had the effect of solving for 1200 or so iterations (many ANSYS exchanges) which was showing some real promise, and then the simulation exploded as before with very high temperatures.

I am kinda at a loss as to what to try next. Any ideas?

[Thomas MADELEINE]

Hi,

The HTC (Heat Transfer Coefficient) is defined by the Heat flux divided by the temperature gap between the fluid and the wall. You can find more information in the CFX help.

Without tbulk parameter (in the expert parameter), CFX take the fluid temperature at the nearest cell of the wall. So it is highly mesh dependent and if the temperature of your fluid is close to the temperature of your wall in that area, the value of HTC can explode (divided by zero).

With tbulk parameter, CFX divides the Heat flux by the temperature gap between the wall and the temperature fixed in tbulk. So you can have a virtual temperature that will assure you will not get a "divide by zero error" on your HTC.

For a 1-way simulation, you can export your HTC in ANSYS Mechanical and use it with the fixed temperature of the tbulk.
I personally set the simulation like :
1 CFX simulation with fixed temperature of the wall and the tbulk parameter
2 ANSYS Mechanical with the HTC and fixed Temperature of the fluid (from the tbulk)

For a 2-Way simulation, I recommend to not export the HTC but rather the Heat Flux directly. For example, if you are running a simulation in CFX with a solid domain and a fluid domain, create a solid/fluid interface and set the heat flux equilibrium.

If it doesn't help, ANSYS made a webinar on 2Way simulation a couple of wekks ago (9th December). You can try to get the video to see if it can help.

Hope that will help your simulation.

Regards,
Thomas