Learning Forum

[fyoussef]

Hello,

I'm simulating fluid flow within a gearbox using Fluent. I have set up a Volume of Fluid (VOF) model comprising two phases: oil and air. The interface tension is constant at 0.027 N/m. I’m accounting for body forces in an implicit model and considering wall adhesion with a sharp/dispersed configuration. Additionally, I've defined rotating walls and included a heat source in the system.

Using the SST $k\text{-}\omega$ turbulence model, the flow converges well, with a y+y^+y+ value under 5. I've also specified the oil viscosity as a function of temperature using an expression and assumed the air density to be that of an ideal, incompressible fluid. However, I’m not observing any significant convective heat transfer to the oil.

When I change the density from constant to temperature-dependent or assume the oil is an incompressible ideal fluid, the results seem counterintuitive. I don't understand how this adjustment affects the thermal conductivity of the oil, which I’ve set as constant.

Could you please offer any tips on improving the convective heat transfer to the oil in this simulation?

Best regards,

[Rob]

Where is the heat coming from? 

As oil is a liquid using incompressible ideal gas will not work well, and will reduce the density somewhat - that will have an effect on the temperature! 

[fyoussef]

I have defined a surface as a Heat Flux Bc 

 

[Rob]

Hmm, so same heat flux into the liquid and gas phases? That may give you an interesting temperature profile: look at how the heat is added using that boundary condition. 

[fyoussef]

In my fluid domain simulation, I noticed an interesting phenomenon: when simulating with a single phase, the convection behaves very well. However, once I switch to the Volume of Fluid (VOF) model, the results become unreasonable.

The surfaces I defined as heat sources are represented as follows: red indicates oil, while blue represents air.

 

[Rob]

In what way are the results unreasonable? If you set the same flux for wet & dry parts of the surface is that reasonable? 

[fyoussef]

When I switch to the Volume of Fluid (VOF) model, convection disappears entirely... this is my Problem... 
For my study, I assume that fluxes are generated due to friction between the gear teeth, resulting in rotationally symmetric flow. Therefore, simplifying the model to a cylindrical shape with defined fluxes in both phases seems reasonable to me. Could you please clarify why this approach might not be suitable?

[Rob]

In Fluent a heat flux bc forces that amount of heat through the surface uniformly. If the heat transfer is limited on the fluid side temperature is increased until sufficient energy is passed over: that can result in a fairly high dT in some cases. 

As I can't see any results it's difficult to comment. 

[fyoussef]

As you can see in the lower region, there’s almost no temperature gradient—ΔT here is less than 0.5°C, which is for a steady State simulation negligible. While the cylinder’s temperature is around 60°C, the fluid temperature remains at its initial level of about 27°C. 

 

[Rob]

Is there anyway for heat to leave the solid without going to the fluid? How long has this run (if transient)? 

[fyoussef]

There is no heat transfer from the solid, as I have already checked. If there were any way for heat to leave the solid, it should also occur when I run the same simulation with a single phase—unless I’m misunderstanding something. This is a steady-state simulation, running for over 2400 iterations.

[Rob]

What's the heat flux over the wall & wall:shadow pair solid to fluid zone? 

[fyoussef]

Each cylindrical heat source provides  circa 39,5 W. so the lower one 210156 W/m^2 and the middel one about 48954 W/m^2

[fyoussef]

I had to decouple the wall and wall:shadow boundaries. My goal was to keep the wall:shadow boundary as a coupled interface and set the wall as a heat source. However, this approach did not work as expected. When I attempted to set one boundary to a heat flux, the other would automatically change as well, limiting me to choose either temperature or heat flux for both, but not the coupled setting.

I’m not sure why Fluent enforces this behavior, preventing me from independently configuring the boundary conditions on wall and wall:shadow.

[Rob]

If you decoupled the two walls there is no heat transfer between the two. You can add heat to a solid, or there's a wall heat generation rate (you must give the wall a thickness in the thermal bc part of the panel).