[cfd seeker]

Hello everybody,

i want to model the multiphase flow inside a hydraulic tank filled with oil let say 80% oil and 20% air. Initial pressure and temperature inside the tank are 1 bar and 20 deg C. If the temperature of liquid inside the tank increases to 120 deg C because of some external heat source, how will this effect the pressure in the tank. I am attaching a figure which represents this problem.

Tank_Simulation.jpg

1. what models and phenomenon do i need to consider in this problem?

2. oil will be modelled as continuous phase and air as dispersed fluid? is it correct?

3. how the iteration between the phases will be modelled?

4. what will be the important phenomenon while considering interaction between the phases? turbulence? heat transfer? vaporization? is it correct or any other phenomenon?

i looked for cfx tutorials but didn't find any tutorials in which Multiphase flow just because of heat transfer is modelled.

I am doing Multiphase simulations of such kind for the first time, so i really need modelling advice for this problem.

Thankyou in advance.

Regards

[ghorrocks]

This question is just a few lines of calculations from an undergraduate thermodynamics course. You don't need CFD for this.

But ignoring that, and answering your question anyway:
1) Model the air as ideal gas or some other realistic EOS, then you will get the pressure rise from temperature. Assuming the oil does not change density much you can model that as incompressible.
2) No, this looks like a free surface application. They are both continuous. Have a look in the CFX tutorials for how to set up free surface simulations. The free surface flow over a bump is the one to look at.
3) Do the tutorials and find out.
4) I don't know, you tell me. It could be any of them depending on what is happening.

[cfd seeker]

Originally Posted by ghorrocks

This question is just a few lines of calculations from an undergraduate thermodynamics course. You don't need CFD for this.

Yes i know this problem can be solved analytically and it belongs to undergraduate course Ofcourse i have solved it analytically by using two different methods. Some calculations broke at high volume fraction of oil and some calculations do-not match with eachother (two methods) again at high volume fraction of oil. Therefore i need to verify the analytical results with CFD especially at higher volume fraction of oil.


Thanks for your reply. I will look at the tutorial for free surface flow.

Turbulence, heat transfer and vaporization are the phenomenon which i think will be important as far as iteractions between the 2 phases are concerned. Boiling will not occur as the temperatures do-not reach the boiling range of oil.

Kindly comment if you think some other phenomenon needs to be considered for such a simulation?

Regards

[ghorrocks]

I don't know what you are modelling so cannot say what is important.

Your initial post suggests nothing is moving. So why do you think turbulence is important? And for heat transfer and vaporisation - are you interested in the transient behaviour or just the final equilibrium result? Because they are not important for the final equilibrium result.

[cfd seeker]

Originally Posted by ghorrocks

Your initial post suggests nothing is moving. So why do you think turbulence is important?

because the liquid level would rise in the tank because of thermal expansion, isn't the turbulence become relevant then?

And for heat transfer and vaporisation - are you interested in the transient behaviour or just the final equilibrium result? Because they are not important for the final equilibrium result

both of them. But isn't it necessary to model both of them even if i just want to see the final equilibrium state because without resolving the transients of the problem how one can acheive the equilibrium? Please correct me if wrong and why?

[ghorrocks]

Your initial post suggests the volumes are stationary and insulated. This means the equilibrium state is no flow and no heat transfer. This immensely simplifies things as you can ignore flow and heat transfer and just look at the volumes and fluid states. You would not bother to do this with CFD, it is a hand calculation (as per my first post).

If you are interested in the transient then you need to consider heat transfer and possibly fluid flow. But as I do not know what you are modelling or why you are modelling it I cannot say what is important.

[cfd seeker]

Originally Posted by ghorrocks

Your initial post suggests the volumes are stationary and insulated. This means the equilibrium state is no flow and no heat transfer. This immensely simplifies things as you can ignore flow and heat transfer and just look at the volumes and fluid states. You would not bother to do this with CFD, it is a hand calculation (as per my first post).

If you are interested in the transient then you need to consider heat transfer and possibly fluid flow. But as I do not know what you are modelling or why you are modelling it I cannot say what is important.

May be i didn't explain well. The system is not insulated and heat can enter or leave the system. The medium inside the tank gets heated because of heat transfer from some external source and i want to see how the liquid moves inside the tank because of heat transfer. How the pressure would increase and it's final equilibrium value?

As i mentioned already that the Tank is part of a Hydraulic system, so the pressure rise in the Tank (because of temperature rise) can create some significant forces on other parts of the hydraulic system(next to Tank) and needs to be some how compensated. So it is important to know the pressure rise in the tank.

[ghorrocks]

Can you explain why the undergraduate style hand calculations are not suitable (even for the transient case) and why you need CFD?

[cfd seeker]

Originally Posted by ghorrocks

Can you explain why the undergraduate style hand calculations are not suitable (even for the transient case) and why you need CFD?

I explained already in the previous posts but i will try to summarize again. It has already been done with analytical methods using two different approaches. At higher volume fraction of oil the analytical calculations from two approaches are not matching with eachother. So i want to verify the analytical results using CFD.

I know this is not the trivial approach but in this case i have to do this.

[ghorrocks]

What you are proposing is a seriously difficult CFD simulation. It is going to take many days of work to get this right for an experienced CFD practitioner, months for a beginner. There is so much judgement and validation required to get this working that you can't possibly use this as a method to work out which of your analytical approaches is correct.

Wouldn't a more viable way forward be to check the assumptions inherent in your analytical approaches and see which approach is correct? Checking analytical calculations with CFD is backwards. You check CFD with analytical calculations, not the other way around.

[cfd seeker]

Originally Posted by ghorrocks

What you are proposing is a seriously difficult CFD simulation. It is going to take many days of work to get this right for an experienced CFD practitioner, months for a beginner. There is so much judgement and validation required to get this working that you can't possibly use this as a method to work out which of your analytical approaches is correct.

At the moment it is not very necessary to do this with CFD. Also we have got time for it, so that's why i want to give it a try. So can you recommend how to approach the problem. I did tutorial for Free surface flows but it is not similar to my case. Do i need to model it using Free surface flow and homogenous model and how vaporization will be modelled?

Wouldn't a more viable way forward be to check the assumptions inherent in your analytical approaches and see which approach is correct? Checking analytical calculations with CFD is backwards. You check CFD with analytical calculations, not the other way around

Yes as i already said that its not a trivial approach but in this case is needed.

[ghorrocks]

OK, answering your questions:

I think from what you have said you have a coherent oil/air interface, with no bubbles, droplets or particles about. In this case you should be using the free surface model. You need to choose appropriate material models, it sounds like an incompressible fluid is fine for the oil but the gas needs a compressible model. This model will handle the pressure rise from expansion of the gas.

If you want to include vaporisation of the oil then things get much more complex. I think you said this is below the boiling point of the oil, and I don't think any built in model in CFX handles vaporisation below the boiling point too well (but check this, I could be wrong). So if you do your own model you will need to make the gas a multicomponent mixture, and set source terms at the interface to vaporise oil. Determining the rate of vaporisation and applying the heat load and then removing that amount of oil from the liquid and adding it to the gas phase is the tricky bit. It will be challenging developing this, good luck!

[cfd seeker]

Originally Posted by ghorrocks

OK, answering your questions:

I think from what you have said you have a coherent oil/air interface, with no bubbles, droplets or particles about. In this case you should be using the free surface model. You need to choose appropriate material models, it sounds like an incompressible fluid is fine for the oil but the gas needs a compressible model. This model will handle the pressure rise from expansion of the gas.

But the thermal expansion of the oil will not be significant than the expansion of the oil? I saw a paper in which someone modelled the rise in liquid level of Tank due to thermal expansion in Fluent.

If you want to include vaporisation of the oil then things get much more complex. I think you said this is below the boiling point of the oil, and I don't think any built in model in CFX handles vaporisation below the boiling point too well (but check this, I could be wrong). So if you do your own model you will need to make the gas a multicomponent mixture, and set source terms at the interface to vaporise oil. Determining the rate of vaporisation and applying the heat load and then removing that amount of oil from the liquid and adding it to the gas phase is the tricky bit. It will be challenging developing this, good luck!

But what about the evaporation model which is there in CFX to model the evaporation of Fuel Spray? Or is it completely different thing?

please tolerate my questions even if they seem to be silly as I said I am new in this topic and want to learn Thankyou!!

[ghorrocks]

But the thermal expansion of the oil will not be significant than the expansion of the oil? I saw a paper in which someone modelled the rise in liquid level of Tank due to thermal expansion in Fluent.

In most applications thermal expansion of an incompressible liquid is insignificant. As you have not told us what you are modelling and why you are modelling it I have had to make guesses about what you are doing, and sometimes those guesses will be wrong.

But what about the evaporation model which is there in CFX to model the evaporation of Fuel Spray? Or is it completely different thing?

Rather than answering that question I think it will be very instructive if you look in the documentation and work that out for yourself.

If you are proposing using this simulation as an introduction to multiphase modelling then I would suggest that a simpler multiphase simulation would be a much more appropriate starting point. Tutorial examples like free surface flow over a bump, particle laden flow around a butterfly valve and a few others are much more suitable starting points to learn multiphase flow. An excellent exercise would be to take a tutorial example and then do a validation and verification exercise on it to work out the mesh, time step and convergence parameters required to get it accurate. This would be a excellent starting point for learning multiphase flow.

[cfd seeker]

Originally Posted by ghorrocks

In most applications thermal expansion of an incompressible liquid is insignificant. As you have not told us what you are modelling and why you are modelling it I have had to make guesses about what you are doing, and sometimes those guesses will be wrong.

In Post #7 i specifically summarized and explained what i am doing and why i am doing this.

[ghorrocks]

I cannot answer your questions because your description is still too vague. The CFD simulation you propose is very complex and that means a lot of detail will be required to know what is going on:

* You say it is 80% hydraulic oil and 20% air. Does it start with the oil at the bottom m air at the top and a clear horizontal interface between the two? Is there any mist, bubbles or foam?
* Is the vessel closed or does it have some pressure controlling or changing device? Is the vessel rigid?
* How is it heated? Where is it heated? What is the heating power? What temperature is the heater?
* Is there any sources of flow or motion other than buoyancy?
* How big is the vessel? Does it have baffles or flow obstructions?

[cfd seeker]

* You say it is 80% hydraulic oil and 20% air. Does it start with the oil at the bottom m air at the top and a clear horizontal interface between the two? Is there any mist, bubbles or foam?

Yes it starts with oil at bottom and air at the top and there are no bubbles, mist or any other form of particles

* Is the vessel closed or does it have some pressure controlling or changing device? Is the vessel rigid?

Yes the vessel is closed with no pressure controlling device. It has just one outlet which will be assumed closed for this simulation. Tank is also rigid.

* How is it heated? Where is it heated? What is the heating power? What temperature is the heater?

Unfortunately the power of heating source is not known as the requirements are coming from the customers. The extreme condition is that the product should be able to withstand the temperature of 120 °C. That's why i assumed that if the oil is heated upto 120 C, what will happen.

* Is there any sources of flow or motion other than buoyancy?

Just the heat source in the form of temperature rise of oil as mentioned above.

* How big is the vessel? Does it have baffles or flow obstructions?

It is about 5 cm in diameter and 25 cm in length and no it does not have any baffles or obstructions.

Another question if can help. If i just want to simulate the thermal expansion of oil in the tank and corresponding pressure rise in the Tank, then i just need to model it as free surface flow with the temperature dependent properties of oil and buoyancy?

[ghorrocks]

OK, thanks for that. Also I assume that the oil does not boil before 120C, it remains liquid.

Based on that I would suggest a free surface simulation. This will handle the clear oil/air interface. It will also allow heat transfer from conduction and convection at the interface - but I would validate this if you want this to be accurate. You can define the air and oil material properties to have whatever physics you want, the free surface simulation can handle pretty much all the physical models. So you can have oil as variable density and variable properties no problems.

The buoyancy is handled automatically as you already have buoyancy from the free surface simulation and variable density.

So far so good, this is a straight forward simulation so far.

Things get much trickier when you consider mass transfer over the interface. I don't think CFX has a built in model for sub-boiling mass transfer, that is evaporation. Of course the partial pressure of hydraulic oil is going to be very, very low but you state this is important. For this bit of the model I would look at the built in mass transfer models for free surfaces. I suspect you will find they are not suitable and you need to develop your own model to handle this. This is not easy and would involve coupled source terms to handle mass transfer and heat transfer.

[cfd seeker]

Hello,

sorry for the v v late reply but i tried this simulation recently as i got busy with other simulations.

I did the simulation with air as Ideal gas and Oil with temperature dependent properties but the convergence does-not seems to be good. I did the simulation in 2D. As it is a closed tank, so at the walls i specified wall heat flux as a B.C. The attached pics show the convergence history. There is a large imbalance energy and mass equations of in oil as well as imbalance in energy equation of air as can be seen in the attched figure. I monitored the average domain pressure during the simulation (as i am intrested in this variable) and it keep on increasing during the simulation and doesnot seem to acheive an equilibrium.

I am also attching the .ccl file of the case, if you want to take a look at it.

mass_momentum.jpg energy.jpg turbulence.jpg pressure_rise.jpg imbalances.jpg

[cfd seeker]

Here the ccl file as .txt file

Tank_2D.txt