[wsh]

Dear users of CFD Online forum,
I am in progress of setting up transient thermal and I am having some doubts.

Please take a look:

This is my model of oil pan. It contains two domains: oil pan and layer of pcm around pan - both fluid. I have defined wall boundary conditions, called engine and ambient, no problem with that. I am not sure about "border" boundary condition - beetwen oil pan zone and pcm zone. I have red in Fluent help, that "coupled wall interface" boundary conditions couldn't work with heat transfer problems (5.4.1.3. Fluent 16 help), so I want to change type of bc to "interface", but this option is not available.

Could heat transfer simulation works with wall bc beetwen those two fluid domains? I think it's should be some kind of wall, made of same material as oil pan (steel), but on the other hand it must no stop heat transfer.

Please help me!

[LuckyTran]

Are you sure you are reading the manual correctly? Are you sure you cannot do a coupled wall? Heat transfer is permitted on a coupled wall, actually that is the only way to do a conjugate heat transfer problem.

Is the material in your pcm and oil pan different? You cannot use an interface across cell zones with different materials.

[wsh]

Hi LuckyTran,
Actually, you've made a good point, because chapter 5.4.1.3 is about non-comformal mesh and my mesh is well connected (I was using HyperMesh).

I was not sure when to use interface bc. I have two cell zones with different materials of course, both fluid.

Steady analisys worked fine and result seems to be okey, but my purpose is to check how long it will take to whole of pcm material to solidify so I want to run transient sim. It was a failure - see picture. No matter how big time step is and how many time steps I use, that simulation seems to be stopped and nothing changes. I have tried several mesh-sizes, viscosity models (since oil is temp-dependent material set as piecewise-linear) and hybrid or standard initialization. Boundary condition is convection both at "ambient" and "engine".

Before, I was making transient sim of pcm layer ONLY and it worked fine.

Any ideas?

steady:



transient:

[LuckyTran]

It sounds like you are trying to model the phase change?
Have you enabled the multi-phase options?

[wsh]

Yes, the main aim of simulations is to observe how pcm layer is solidifying.

I did not, actually I don't know nothing at all about multi-phase model. In my previous sim, which I have modelled only pcm layer there was only one fluid material and I have forgot about that... In every simulation where two different fluid materials occurs we have to use multi-phase options? In my simulation there is no flow, only heat exchange.

I better read fluent help for multi-phase.

EDIT: Well, actually, flow could happen because of density change over temperature decrease, could it matter?

[LuckyTran]

It's not because you have two different materials.

You simply need to enable the solidification option. Without enabling these multi-phase options, you are stuck with single-phase simulations, purely solid, purely liquid, or purely gas.

[wsh]

Of course I have enabled "Solidification & Melting" model and I have read both theory guide and modelling parts of solid/melting in Fluent help. But in Fluent 16 there are "Multiphase" and "Solidification & Melting" models as different options at models tab.

My previous sim of pcm layer only works without enabling "Multiphase" model, with only "Energy" and "Solidification & Melting" models on. I've made animation of pcm material solidyfing over time, pcm was changing from fluid to solid clearly.

[wsh]

I have quickly made another model which contains 3 cell zones: 2 fluids (oil and pcm layer) and 1 solid for oil pan itself. When exporting mesh grom HyperWorks to Fluent hp does even made special connectors of interface for solid-fluid boundary.

The results are the same - after x iterations and time steps heat is not transfered from walls, like physics had failed...

[LuckyTran]

Check the thermal boundary condition in your wall|shadow-wall pair and make sure it is coupled. I think the default is adiabatic.

[wsh]

It is coupled.

I thought, that every wall with heat flux more then zero is non-adiabatic. Anyway, I can't change heat flux values when using coupled thermal conditions. I have tried running sim with "heat flux" and "temperature" boundary conditions and manipulating wall thickness also, no results - energy residual still flat

[LuckyTran]

Can you describe your initial conditions and boundary conditions? Are you even running the transient simulation properly? I clearly see a temperature gradient so there is some communication and the coupled boundary is working.

[wsh]

I think the problem is i am not running transient simulation properly Because steady simulation seems working fine.

So i describe conditions in first model (with two cell zones only):
*horizontal "engine" wall on top is set as convection; heat transfer coef = 2; free steam temp = 303; wall thickness, heat gen rate and contact resistancy =0; (too lazy for units) (further I want to set Profiles to simulate engine cooling, just like in my pcm-layer only simulation)
*second wall "ambient", all around pcm layer (and two short, horizontal lines on top, on tle left and right side of "engine" wall bc);heat transfer coef = 10; free steam temp = 255; wall thickness, heat gen rate and contact resistancy =0
*"border" and "border-shadow" wall; coupled; heat gen rate and contact resistancy =0; wall thickness =0,003

standard ini: 313 K for now but I have tested with hybrid init too. Later on I consider using UDF to set other init temp at both cell zones

I have tested time steps from 0,1s to 60s and mesh from 5mm to 2mm

[LuckyTran]

What is the time-constant for your problem (in the lumped capacitance sense)? Is your simulation time comparable to this time-scale?

Instead of convective conditions, try using specified wall temperatures and specify them to be your freestream temperatures. This will speed up the heat transfer and possibly help you notice changes.

Originally Posted by wsh

*"border" and "border-shadow" wall; coupled; heat gen rate and contact resistancy =0; wall thickness =0,003

This will result in 3mm thick aluminum layer separating the regions (and a small temperature drop across the wall). I think it is a small effect but I hope it's intentional.

[wsh]

After browsing Fluent 16 help I still do not know what you mean by "time-constant", "time-scale" Is it about how long it could take for simulation to get in steady state?

I have changed bc to temperatures but energy resideal remains flat. I have experimented with solution methods. I have run simulation with almost every spatial discretization options - no results. After changing transient formulation to Second Order Implicit residuals plots looks interesting:


but simulation still is going nowhere, here's a video: video of a 7 hours 52 minutes simulation (time step=60 sec, I have tried also 1 second time step for this case). Energy residual stays flat until ~18 time steps, and after goes crazy and simultaneously velocity and continuity residuals comes from outer space...

Time step of 1 secons is used on picture 2, but ts=60s behaves likewise.

Yes, that 3mm layer (should be steel eventually) should simulate oil pan steel walls. Engine wall should be 3mm thick, too.

Since I was making geo model in SolidWorks and mesh in HyperWorks I am considering making new geo and mesh models in design modeller and launching it via Ansys Workbench tonight.

Thanks for your previous help LuckyTran! I am still confused what am I doing wrong

[Rohtiwari]

Hello everyone,

I am solving heat transfer problem in a conjugate domain. I have made an interface between solid and fluid region, I have to add heat transfer coefficient value at the interface to consider contact resistance between the solid wall and fluid region but I am not able to find any option in FLUENT.

Please anyone can tell how to include contact resistance phenomena at the interface.

Thanks in advance

[LuckyTran]

Originally Posted by Rohtiwari

Hello everyone,

I am solving heat transfer problem in a conjugate domain. I have made an interface between solid and fluid region, I have to add heat transfer coefficient value at the interface to consider contact resistance between the solid wall and fluid region but I am not able to find any option in FLUENT.

Please anyone can tell how to include contact resistance phenomena at the interface.

Thanks in advance

In the thermal boundary conditions you can see something called a wall thickness (the default is 0). Also notice you can select a wall material (the default is aluminum). You need to set this thickness to the appropriate value to get the contact resistance. For contact resistance, which is purely 1D, you do not need to activate shell conduction. But I don't follow why there is a contact resistance between a fluid and solid? That is a solid-solid property.

[Rohtiwari]

Originally Posted by LuckyTran

In the thermal boundary conditions you can see something called a wall thickness (the default is 0). Also notice you can select a wall material (the default is aluminum). You need to set this thickness to the appropriate value to get the contact resistance. For contact resistance, which is purely 1D, you do not need to activate shell conduction. But I don't follow why there is a contact resistance between a fluid and solid? That is a solid-solid property.

Thanks for quick reply LuckyTran.

I have checked with this option. As per my knowledge, there should be sudden temperature drop at the interface between solid wall and fluid region and I am referring this temperature drop as contact resistance. However, after using your mentioned method, if I plot temperature profile across the interface there will be continuous decrement and no temperature drop phenomena observed.

Please correct if I am wrong in my theory.

[The_seeker]

Hi All
I am trying to simulate the conjugate cylindrical pin in a channel. I have gone through the tutorials and set up the case file, which I think is right. The bottom wall is heated and the coupled wall is used at solid-fluid interface. After running the simulation, I checked the heat flux contours on the walls. The flux on wall (air-side) is positive but on the wall-shadow (solid-side) it is negative. In the papers that I have gone through, the flux and temperature continuity is used at the coupled interface. The flux balance is :
ks dTs/dn = kf dTf/dn

For turbulent flows, the heat flux is calculated using the law of wall analogy as per the fluent guide. My doubts are as following:
1. I did not find the exact solution equation solved at the coupled boundary by FLUENT in the guide.
2. What is the sign convention used by FLUENT in solving heat flux at the boundary? What is the exact meaning on the wall and wall-shadow having different signs?

[vinerm]

The mathematical implementation of coupled boundary is essentially what you have given as equation - the flux conservation. Heat flux going out of fluid has to be equal to heat flux into the solid and vice-versa. Continuity of the temperature is not a necessary condition for coupled boundary but continuity of heat flux is and that is how coupled boundary is implemented; it just maintains same flux on both sides.

For the same reason, you get same values but with different signs for fluid and solid. Wall and Wall-Shadow are essentially two sides of the coupled wall; one belongs to fluid and the other to solid. Do note that wall may belong to solid while shadow may belong to fluid. It does not really matter. Heat lost by fluid is negative while gained is positive.