[CFDJonas]

Hello,

I want to model a (very simple) tube. Homogenous, perfectly cylindrical, etc. For that I reduced the geometry to an 2D-rectangle, and made it axisymmetric. A picture of (a part of the mesh) is attached.

I want the flow to go from left to right. The conditions inside the tube are laminar (by considering the Reynolds number), therefore I chose the laminar viscous model.

Now to the interesting part: I want to model a heat source. In reality this should resemble a tube with oil heating it, therefore I calculated the needed heat transmittance coefficient (k in W/m^2 s) from the oil to the outer wall, and then the thermal conduction through the steel. This is fine as well (the oil is assumed to be isothermal).
In Fluent I chose "Convective" as a thermal boundary condition, entered the thermal transmittance coefficient and the (isothermal) oil temperature in there.

To ensure fully developed flow at the inlet of the tube, I enter a velocity profile at the inlet for the momentum boundary condition (which was beforehand simulated using the inlet conditions).

The simulation works fine, as long as I'm not using a temperature-dependent density correlation. As soon as I'm doing that, the continuity goes away and I even get backflow at the outflow BC.

Now to the question:

• Is is still okay to "assume" laminar flow, although I introduce a "radial" heat source?
• 'im not sure about the inlet thermal boundary condition. I assume T = const. Therefore I have no radial profile set. Maybe this is the problem; how would I come to a proper boundary condition for that? I'm open for any suggestions... even simulating more of the inlet region.
• I already tried a lot of variation in meshing (very fine uniform grid, very fine cells with inflation layers, even the whole thing as 3D was tried). I think the problem is not within the meshing... It's more about the boundary conditions not really acting together (but tell me if I'm wrong).
• Although a turbulence model "fixes" this problem I don't think that's the way to go. It seem's like it is just blurring the solution and making it converge that way... Am I right about that feel?

I really feel a little dumb as this seems like a pretty simple task... However it is really bugging me. Thanks to everyone helping!!!

CFDJonas

[CFDKareem]

Check your spatial discretization for pressure. If the density is variable, i.e. temperature dependent, you'll want to use PRESTO of Body Force Weighted. Try both and see if it stabilizes your solution.

If the density is changing a lot it may change your flow from laminar to turbulent. Calculate your reynolds number at your minimum density (assuming fluid is at maximum temp) and see if it is turbulent.

Try PRESTO and Body force weighted and let me know how it goes. If you're still struggling let me know and we can go from there.

[CFDJonas]

Thank you for your answer!

I have tried both, PRESTO! and Body Force Weighted for the Pressure Discretization scheme. Sadly, with no success. The solution is the same.
I get a convergence with reverse flow in like half the surface of the outlet. (And a contiunity at ~10^-1). This leads to a "channel" of flow near the wall in complete opposite direction, back to the inlet.

You have said

If the density is changing a lot it may change your flow from laminar to turbulent.

How can this be explained? I already have the fear that this can be the case, but I can not explain it to me.

I have calculated the Reynoldsnumber throughout the whole temperature range I'm considering. It lies between 1600 and 1000. So for me it seems pretty laminar...

I have to add that the pressure level is quite high (fluid is in supercritical state).

Thank you for your help!

[CFDKareem]

Originally Posted by CFDJonas

Thank you for your answer!

I have tried both, PRESTO! and Body Force Weighted for the Pressure Discretization scheme. Sadly, with no success.

This is good. Glad you tried those both, so it looks like this is not the problem.

Originally Posted by CFDJonas

How can this be explained? I already have the fear that this can be the case, but I can not explain it to me.

The Reynolds number is dependent on the kinematic viscosity, where Kinematic viscosity = dynamic viscosity/fluid density and Reynolds number = (Fluid velocity x Internal pipe diameter) / Kinematic viscosity. As the density changes your reynolds number will change. As you've already tried, you can change the density to the maximum or minimum value and see how your reynolds number will change. If the density change is dramatic enough it could take your working fluid from laminar to turbulent, over ~4000 for pipe flow. From your calculations it looks like laminar should be okay.

Some follow-up questions...
1) How are you defining the variable density material property? i.e. Ideal Gas, incompressible ideal gas, etc.?
2) Are any other material properties temperature dependent (viscosity)?
3) If this data is not sensitive, can you provide me the boundary conditions for your set-up so I can set it up myself? I would need...
-Working Fluid
-Domain geometry (pipe diameter, length)
-Material properties
-Temperature of the oil and heat transfer coefficient on the walls
-Inlet and outlet conditions

I can set this up pretty quickly and try and trouble shoot myself.

[CFDJonas]

Some follow-up questions...
1) How are you defining the variable density material property? i.e. Ideal Gas, incompressible ideal gas, etc.?

The fluid in supercritical state. Later in the simulation process I also want to add reactions. I use empirical correlations from literature for the density temperature dependence.

2) Are any other material properties temperature dependent (viscosity)?
Yes, the other properties are all set temperature dependent as well. All by using UDFs and the individual correlation.

To get ahead of the questions: I have of course checked the temperature ranges and equations by plotting them. Also the implementation in the UDFs gives the expected values.

3) If this data is not sensitive, can you provide me the boundary conditions for your set-up so I can set it up myself? I would need...
-Working Fluid
-Domain geometry (pipe diameter, length)
-Material properties
-Temperature of the oil and heat transfer coefficient on the walls
-Inlet and outlet conditions

Fluid is a supercritical fluid, with properties stated above.
Domain Geometry has a high L/D ratio, the diameter is just a few mm. Length about 1 to 2 meters.
Material properties are as stated above.
Temperature of the oil is in the range of 180 to 220 degree Celsius.
Calculated heat transfer coefficient is in the region of 1000 to 4000 W/m^2 K.
Inlet is a mass-flow-inlet, for outlet I chose outflow (also tried with pressure-outlet before).
I recently updated the mesh to have a entry-length to generate a fully developed flow, before the heating at the wall is activated, and a "exit"-length, after the heating to give the fluid some time before hitting the outlet BC. The wall is therefore now divided in 3 "sections" (adiabatic - convective - adiabatic).

Again, thank you so much for your help! If this information is too vague, perhaps we could also have a short call. Then I could better explain the situation and/or tell you more details.

[zimao]

Maybe you could try to increase the heat load gradually from zero, after the solution is converged.

[CFDJonas]

Hello zimao,

I had that idea as well. Low temperature deltas were fine, but as the delta is getting bigger, the "divergence" also got bigger.

But I have good news: I think I solved the problem:

The stupid thing was, that I had gravity enabled. This means I had the Boussinesq buoyancy approximation enabled, which in turn assumes constant density... with "big" density gradients due to a temperature-dependence this seems to break the laminar model. Or at least the continuity.
With turned-off gravity I get a converging heat transfer problem.

Thank you CFDKareem again for your help. With your troubleshooting I came to the point, where I had to look at.