[ghorrocks]

No surprises the simulation is not working. As stated in the beginning this is a very difficult simulation.

Some comments:
* You have defined time steps of 0.001[s]. Is this a guess, or from a sensitivity study? If it is a guess then it is almost certainly wrong. Once you have the basic simulation working you need to do a sensitivity analysis.
* Likewise for your convergence tolerance. You need to check this with a sensitivity analysis.
* You have defined a 1000W heat flux on the outer surface (I presume it is the outer surface, you have not shown what your geometry is). So the thing will heat up forever. This will mean you probably go outside your ranges for your defined properties very quickly.
* Don't use second order time stepping while you are doing basic debugging. Do debugging with first order and switch to second order when everything is working.

But the big issue with your simulation is you are trying to get too much working at once. You should do a first simulation with incompressible air and oil with constant properties working and get the free surface model functioning. Once that is working then make air an ideal gas (still with constant properties). And once that is working then add your variable properties.

If you do everything at once you have no idea where to look to fix the problem. So add the complexity one bit at a time.

[cfd seeker]

* You have defined time steps of 0.001[s]. Is this a guess, or from a sensitivity study? If it is a guess then it is almost certainly wrong. Once you have the basic simulation working you need to do a sensitivity analysis.

yes this is just the starting guess. Ok i will first do the sensitivity analysis for timestep size.

* Likewise for your convergence tolerance. You need to check this with a sensitivity analysis.

You mean make it more tighter?

* You have defined a 1000W heat flux on the outer surface (I presume it is the outer surface, you have not shown what your geometry is). So the thing will heat up forever. This will mean you probably go outside your ranges for your defined properties very quickly.

yes this was also just a starting guess and yes it is defined on the outer wall. But i didn't know that this gonna heat up the walls forever. As the heat flux or heat transfer coefficient is not known, the only info available is that the fluids inside tank heat up to 120 °C. Now i made a 1mm thickness around the tank walls and doing CHT (defined temperature on the outer wall and used the Fluid-Solid interface) to heatup the fluids(oil+air) inside the tank by defining the temperature of 160 °C on the outer walls of solid domain.

But the big issue with your simulation is you are trying to get too much working at once. You should do a first simulation with incompressible air and oil with constant properties working and get the free surface model functioning. Once that is working then make air an ideal gas (still with constant properties). And once that is working then add your variable properties.

Ok currently in the new model with CHT i have used Air as incompresible fluid at 25 °C and also for Oil i am using constant properties.

I will do the sensitivity analysis of timestep on this model first.

Geometry is a simple 2D rectangle with 10cm*15cm as shown in the attached picture. Now in the new simulation where i am doing CHT analysis, i have added a wall of 1mm around this recatangle.

2D_geometry.jpg

[cfd seeker]

i did the simulation by modelling the 1mm thickness for CHT simulation with constant properties but again with 0.001 s tim step (sensitivity analysis to follow). The convergence is good except for the energy imbalance in Solid Domain as shown in attached figure.

But when i looked at the Oil temperature in CFD Post, it seems that there is very little or not heat flow across the CHT interface, as shown by the contours of oil temperature in the attached figure. It seems the oil and air are heated by being heated up. I don't know if this is due to the low heat intensity or because of some problem in the interface setup. Can you comment on this?

case ccl is also attached as a .txt file.

[ghorrocks]

Why do you say the energy imbalance is bad? That is a very low imbalance, it is unlikely that is a problem.

When you add the outer shell you add thermal mass to the system. This means it will take extra time to heat up, and the heat from outside will take a while to conduct into the fluid. You probably just have to run it longer for the heat to conduct through more.

But before you do, have a careful think about the thermal boundary conditions so you match what is actually happening. Defining constant heat flux and a fixed outer temperature result in very different results. Also things like a convection condition may be relevant, and that is a different condition again. You need to choose the right condition so the thermal load is correctly applied over time.

[cfd seeker]

Originally Posted by ghorrocks

But before you do, have a careful think about the thermal boundary conditions so you match what is actually happening. Defining constant heat flux and a fixed outer temperature result in very different results. Also things like a convection condition may be relevant, and that is a different condition again. You need to choose the right condition so the thermal load is correctly applied over time.

Actually the heat BC in not known exactly. The system should be able to withstand the maximum temperature of 120 °C, so in the theoretical calculations it was assumed that the fluids(air+oil) inside the tank instantly acheive the temperature of 120 °C from an initial temperature of 20 °C. So I am trying to acheive the uniform heating of fluids upto 120 °C by specifying the temperature higher than 120 °C on the walls. Any suggestions if i can do it in a better way?

[ghorrocks]

If you don't know the exact condition then you cannot put a boundary condition there and expect it to be accurate. If you guess a boundary condition (which is what you appear to be doing) then you have to appreciate that the thermal history of your model could be completely wrong.

You should look at what is doing the heating. Is there is temperature control circuit with a heating element which heats it to 120C then keeps it there? Or is 120C the equilibrium temperature it achieves in a balance between some heat source and heat lost to the environment (presumably as convection and radiation) Or is the surrounding environment 120C? You would model each of these scenarios differently.

Some options of what you could do include:
* specify everything to be 120C initially and use a specified temperature 120C outer boundary condition
* initial condition is 20C but outer boundary is 120C
* initial condition 20C, outer boundary is convection and/or radiation to 120C
* initial condition 20C, but then a heat source is applied which turns off when it gets to 120C and turns to a lower heating rate to only maintain the temperature

And there are more options if you think about it more. But which one you choose depends on what you are trying to model and whether it matters.

Also, you say "I am trying to acheive the uniform heating of fluids upto 120 °C by specifying the temperature higher than 120 °C on the walls." - how does applying a temperature higher than your target make it more uniform? Why are you applying a temperature higher than you say exists?

Finally - that comment states that uniform heating is required - this is a new concept in this discussion. Can you explain what you mean here?

[cfd seeker]

Originally Posted by ghorrocks

If you don't know the exact condition then you cannot put a boundary condition there and expect it to be accurate. If you guess a boundary condition (which is what you appear to be doing) then you have to appreciate that the thermal history of your model could be completely wrong.

You should look at what is doing the heating. Is there is temperature control circuit with a heating element which heats it to 120C then keeps it there? Or is 120C the equilibrium temperature it achieves in a balance between some heat source and heat lost to the environment (presumably as convection and radiation) Or is the surrounding environment 120C? You would model each of these scenarios differently.

Some options of what you could do include:
* specify everything to be 120C initially and use a specified temperature 120C outer boundary condition
* initial condition is 20C but outer boundary is 120C
* initial condition 20C, outer boundary is convection and/or radiation to 120C
* initial condition 20C, but then a heat source is applied which turns off when it gets to 120C and turns to a lower heating rate to only maintain the temperature

And there are more options if you think about it more. But which one you choose depends on what you are trying to model and whether it matters.

Also, you say "I am trying to acheive the uniform heating of fluids upto 120 °C by specifying the temperature higher than 120 °C on the walls." - how does applying a temperature higher than your target make it more uniform? Why are you applying a temperature higher than you say exists?

Finally - that comment states that uniform heating is required - this is a new concept in this discussion. Can you explain what you mean here?

As i told earlier that the only information available is that the product should be able to withstand the maximum temperature of 120 °C. So in the theoretical calculations it was assumed that the fluids inside the Tank instantly acheive 120 °C.

By uniform heating i mean that the whole mass of oil and air in the tank acheive the equilibrium temperature of 120 °C, starting from 20 °C. Just as an example, if there is a large reservoir and that outside temperature is 120 °C, then the whole mass of the reservoir does-not instantly acheive 120 °C. But in the theoretical calculations it was assumed like that.

So in the simulation, i want that the whole mass of fluids should acheive 120 °C at an equilibrium, in some time lets says 5 seconds.

[ghorrocks]

Then the simplest thing to do is to just impose 120C on the outer face. Then it will asymptotically approach 120C and not do any overshoot or anything (unless you have a heat source in this thing).

But whether it get to 120C in 5s is another matter. The thermal time constant is a function of the specific heat, mass, conductivity and other parameters so I cannot judge whether it will get to close to 120C within 5s.

[cfd seeker]

Originally Posted by ghorrocks

Then the simplest thing to do is to just impose 120C on the outer face. Then it will asymptotically approach 120C and not do any overshoot or anything (unless you have a heat source in this thing).

But don't you think that by this way only the fluid near to walls (or in case of CHT near the Fluid-Solid interface) will get heated and reach temperature of 120 °C as the heat conduction is very slow process.

[ghorrocks]

Why don't you just use a heat source term to cook the entire thing to any temperature you want in any amount of time you want? Then you don't need to worry about annoying things like what is physically possible

[cfd seeker]

Originally Posted by ghorrocks

Why don't you just use a heat source term to cook the entire thing to any temperature you want in any amount of time you want? Then you don't need to worry about annoying things like what is physically possible

yes i also thought about it today and derived the heats required for the temperature rise of 120 °C starting from 20 °C, using the equation

 
Q = m*Cp*dT
dT = Temperature difference
Watt = Q/s, lets say in 5 seconds
Heat Source = W/V
V= Volume of Tank

i think you are also talking about this?

[ghorrocks]

No, that is not what I meant. That equation will just give you how much heat you need to add to get it to the desired temperature. If you apply this heat on the outer wall it will still take lots of time to conduct in. So it will be a bit quicker than just imposing 120C on the outer walls, but whether it will be quick enough to get it to equilibrium in 5s? That depends on many things.

What I was talking about was to use a heat source term over the entire thing. Then you don't need conduction to transfer the heat, the heat is applied everywhere. You can get it to any temperature you like at any speed you like. Look in the documentation on source terms.

[cfd seeker]

Originally Posted by ghorrocks

No, that is not what I meant. That equation will just give you how much heat you need to add to get it to the desired temperature. If you apply this heat on the outer wall it will still take lots of time to conduct in. So it will be a bit quicker than just imposing 120C on the outer walls, but whether it will be quick enough to get it to equilibrium in 5s? That depends on many things.

No, i am not saying to apply the heated calculated thorugh this equation as a heat flux on the outer wall rather to use this heat as a source term applied in the domain.

What I was talking about was to use a heat source term over the entire thing. Then you don't need conduction to transfer the heat, the heat is applied everywhere. You can get it to any temperature you like at any speed you like. Look in the documentation on source terms.

Ok i will look in the CFX documentation, how they are suggesting

[ghorrocks]

What I was suggesting was a heat source term of the type

S = -C(T-T_target)

Where C is a large number. You might want to use a source term coefficient of -C to linearise it and assist convergence. If you set T_target to 120C then it will go to 120C in the first time step. Alternately you can ramp it in anyway you like.

Using this technique you can make the temperature anything you like as quickly as you like.

[cfd seeker]

Originally Posted by ghorrocks

What I was suggesting was a heat source term of the type

S = -C(T-T_target)

Where C is a large number. You might want to use a source term coefficient of -C to linearise it and assist convergence. If you set T_target to 120C then it will go to 120C in the first time step. Alternately you can ramp it in anyway you like.

Using this technique you can make the temperature anything you like as quickly as you like.

Ok thanks a lot, i will think about it. This will be specified by inserting a Subdomain and then under Sources tab, as shown by the attached figure?

heat_source.jpg

[ghorrocks]

Yes, that is where you apply it. You need to set the source term and a source coefficient.

[cfd seeker]

Thanks a lot.

The equation you suggested must have units of W/m^3, so the coefficient C must get the units of W/(m^3*K), any idea how i can calculate/estimate this coefficient for my case?

S = -C(T-T_target)

T would be initial temperature?

[ghorrocks]

C is just a large number. Try 1e6.

T is the local temperature.

[cfd seeker]

Ok thank you. I am trying this.

But if i have to define energy source with the help of expression then "C" with get multiplied by the term (T-Ttarget) and the resulting value will be used as a value for volumetric heat source, so the value of this parameter "C" seems to effect the simulation. Isn't it?

When you say its just a large number then it seems it doesn't matter what is the magnitude of this parameter or am i missing something?

Is this a correct way to define the energy source (with the help of CEL expression using S= -C*(T-Ttarget)) ?

[ghorrocks]

Yes, you are missing something

The term T-T(target) goes to zero as the solver gets the subdomain to approach the desired temperature. So yes, the C term generates a lot of heat initially when the temperature is way off but it goes to zero as it converges on T(target).