## Mesh for heat transfer advise

## Mesh for heat transfer advise

(OP)

Hi, I am new of the forum and I posted the following post on "Mechanical Engineering - Heat transfer" but after that I found this section, dedicated to ANSYS that is more correct I think. So I moved the post here deleting the old one on the heat transfer section.

Currently I am involved on a calculation regarding the heat transfer on an expansion joint. Fundamentally an expansion joint is a corrugated pipe, very thin, to recover the expansion due to temperature of the other parts on the system. An idea of the geometry is attached.

I needed to recreate the correct boundary conditions, in term of temperatures, at the inlet of the expansion joint and for this reason I added a piece of pipe upstream with a small model of a burner ( here enter methane and air and a flame will developed: after that a transport of fluid is done by eddy dissipation and in 2 diameters the gas mix reach an homogenous temperature around 950°C ). This is just information: this part in not what I want discuss on the model. Outlet condition is easy: pressure outlet with 0 barg pressure.

As indicated in picture expansion joint has corrugation so I started my model with KW SST turbulence due to large amount of node used to model the upstream condition ( the burner... ). I kept YPlus between 30 and 300 to use the wall functions. Mesh has 15 layers inflation and convergence is good.

Now the problem: I tried a second run - very heavy - using a denser model to reach Yplus between 1 and 5. I do this just as a cross check. Results are COMPLETELY different: decreasing the size of the mesh I obtained a VERY less amount of heat exchanged! Please take care: I don’t speaking about heat transfer coefficient but about exchanged heat.

How explain this result and to which simulation trust?

It appears that internal routines of Fluent check the mesh and use wall function only if the mesh has not the correct yplus. Please consider this information with a grain of salt because I only heard it so I am not so confindent.

What to do in your opinion?

Thanks

Currently I am involved on a calculation regarding the heat transfer on an expansion joint. Fundamentally an expansion joint is a corrugated pipe, very thin, to recover the expansion due to temperature of the other parts on the system. An idea of the geometry is attached.

I needed to recreate the correct boundary conditions, in term of temperatures, at the inlet of the expansion joint and for this reason I added a piece of pipe upstream with a small model of a burner ( here enter methane and air and a flame will developed: after that a transport of fluid is done by eddy dissipation and in 2 diameters the gas mix reach an homogenous temperature around 950°C ). This is just information: this part in not what I want discuss on the model. Outlet condition is easy: pressure outlet with 0 barg pressure.

As indicated in picture expansion joint has corrugation so I started my model with KW SST turbulence due to large amount of node used to model the upstream condition ( the burner... ). I kept YPlus between 30 and 300 to use the wall functions. Mesh has 15 layers inflation and convergence is good.

Now the problem: I tried a second run - very heavy - using a denser model to reach Yplus between 1 and 5. I do this just as a cross check. Results are COMPLETELY different: decreasing the size of the mesh I obtained a VERY less amount of heat exchanged! Please take care: I don’t speaking about heat transfer coefficient but about exchanged heat.

How explain this result and to which simulation trust?

It appears that internal routines of Fluent check the mesh and use wall function only if the mesh has not the correct yplus. Please consider this information with a grain of salt because I only heard it so I am not so confindent.

What to do in your opinion?

Thanks

## RE: Mesh for heat transfer advise

This might help. Search - "wall functions and y+ requirements" or "What y+ should I use in my simulations?" on site : computationalfluiddynamics.com.au

## RE: Mesh for heat transfer advise

## RE: Mesh for heat transfer advise

I assume you use Ansys Fluent?

For heat transfer, 1) generally kw-SST is recommended, so you are good there. Further recommendations are 2) to have at least 10 cells inside the boundary layer. So you need to calculate the boundary layer thickness based on the Reynolds number. With kw-SST, if possible, 3) you should have y+ around 1 for the highest accuracy.

When you say "convergence is good", does it mean the converge of the temperature/heat transfer or do you mean the convergence of the residuals? Because the convergence of the latter does not necessarily mean your solution has converged.

Regarding Fluent checking the mesh and use wall functions if the y+ is not ok, this is true for the kw turbulence models (this is called the "Automatic Wall Treatment" in Fluent). When y+ becomes to large, Fluent will gradually use wall functions.

So to come back to your main question, without knowing much details about your solution/setup, I would say that you should trust your results from your fine mesh more than the one with 30<y+<300.

A note on heat transfer and heat transfer coefficient (HTC). You mention that you are comparing the heat transfer and not the HTC, which is the way to do the comparison. The HTC is mesh dependent unfortunately, unless you enter a temperature reference value (e.g. the temperature of the main flow) in the reference values section. Only then you can compare HTC correctly between different meshes. But your way of comparing results is the most sensible one.

Another tip maybe. It seems your geometry is axi-symmetric. To save computation time, you can you use an axi-symmetric 2D-model in Fluent, assuming your boundary conditions are axi-symmetric.

Good luck!

https://www.eng-tips.com/faqs.cfm?fid=376