[zhubohong]

Hello,
I want to simulate the three phases flow in a reactor, two continue phases, and one dispersed phase. I tried to use the FREE SURFACE MODEL to deal with the flow between the two continue phases, and use the PARTICEL MODEL to deal with bubble colume between the continue phase and dispersed phase.
But, the simulation process always has a fatal error as shown below:
ERROR #001100279 has occurred in subroutine MESG_RETRIEVE.
Message:Stopped in routine ASS_MSF_BFORCE
Does anybody konw this error? ASS_MSF_BFORCE, thanks for your help!

[Gert-Jan]

The error messages do not make sense. You should provide the last part of the output file with the text above this error.

But to my best knowlegde it is not possible to perform Lagrangian particle tracking in combination with 2 phase Eulerian-Eulerian model. So, probably that is the problem.

Also if you have 2 mixed fluids, then the free surface model is inappropriate. This is only useful for flat free surfaces.

Are the two continuous phases miscible like water and ethanol, or inmiscible like water and oil?

[zhubohong]

Originally Posted by Gert-Jan

The error messages do not make sense. You should provide the last part of the output file with the text above this error.

But to my best knowlegde it is not possible to perform Lagrangian particle tracking in combination with 2 phase Eulerian-Eulerian model. So, probably that is the problem.

Also if you have 2 mixed fluids, then the free surface model is inappropriate. This is only useful for flat free surfaces.

Are the two continuous phases miscible like water and ethanol, or inmiscible like water and oil?

Thanks for your advices. My model can be described as the oil-gas-water flow in a tank. The height of tank is 1 m, 0.6 for water, and 0.4 for oil. The gas is injected from the bottom nozzle. Actually, I have known how to use DPM+VOF model to simulate it. But this time, I want to use E-E approach. I always get that error. I dont know what it mean, and how to solve it.

[Gert-Jan]

The error messages do not make sense. You should provide the last part of the output file with the text above this error. Or the complete output file.

[zhubohong]

Originally Posted by Gert-Jan

The error messages do not make sense. You should provide the last part of the output file with the text above this error. Or the complete output file.

Parallel run: Received message from slave
Slave partition : 11
Slave routine : ErrAction
Master location : Message Handler
Message label :001100279
Message follows below

ERROR #001100279 has occurred in subroutine ErrAction.
Message:
Stopped in routine ASS_MSF_BFORCE
ERROR #001100279 has occurred in subroutine MESG_RETRIEVE.
Message:
Stopping the run due to error(s) reported above
An error has occurred in cfx5 solve:

The ANSYS CFX solver exited with return code 1. No results file
has been created.

End of solution stage.

Sorry, I dont know how to show the completed out file, thanks for your attention!

[Gert-Jan]

Still not enough info. The real error is given above these lines.

The output file is just a simple text file on your computer. It has the extensions .out
Not too complicated....
Alternatively, open the run in the solver manager and copy the complete text in the text-window to a text-file and share that file.

[zhubohong]

Originally Posted by Gert-Jan

Still not enough info. The real error is given above these lines.

The output file is just a simple text file on your computer. It has the extensions .out
Not too complicated....
Alternatively, open the run in the solver manager and copy the complete text in the text-window to a text-file and share that file.

This is out file. Too much thanks for you

[Gert-Jan]

You are very far away from a succesful simulation.
Do you have someone around with some experience? Like a supervisor?

1) You mentioned:
"The height of tank is 1 m, 0.6 for water, and 0.4 for oil."
But if I look at your output file, the first thing I noticed is:

+--------------------------------------------------------------------+
| Average Scale Information |
+--------------------------------------------------------------------+

Domain Name : Default Domain
Global Length = 6.9745E+02
Minimum Extent = 7.9191E+02
Maximum Extent = 8.1200E+02

I think you have to downscale by a factor 1000. You don't have to remesh, you can downscale in Pre.

2) Like most beginners, you turn on all physics that are relevant and then keep fingers crossed and hope CFX understands. But that is a asking for troubles.

Therefore: start as simple as possible. Delete all obsolete physics. Try to get that running first and then increase complexity by adding physics step by step. So remove:
- Surface tension. This make everything far too complicated. you don't need it anyway on this scale (only in geometries of mm scale).
- Lift coefficients
- ENHANCED TURBULENCE PRODUCTION MODEL
- maybe start with 1 continuous phase. You can also add the second one at a later stage

3) run auto timescale.

[zhubohong]

Haha, Actually, I am a freshman for CFD online, so I dont know how to show my question. for example, how to attach the geometry. At the begining, you asked me the details of my case. I dont know how to describe it. So, I used the similar case to represent to you (The height of tank is 1 m, 0.6 for water, and 0.4 for oil.). I think the simulation method between this similar case and my real case is same. I am not a fresheman for CFX. I know how to model the liquid-gas two phases flow using the Particel Model for many cases. But, this time, I want to simulate three phase flow, two gas phase, and one liquid phase. Just like, a glass with half part of water, and half part of air. And we inject the air from the bottom of glass. I mean that no matter what kind of materials or geometris or initization conditions we choose. The simulation method between these cases is same. If we just model the glass (full of water) with bottom air injection. It is very easy to use the PARTICEL MODEL with degassing condition. However, if we model this case(a glass with half part of water, and half part of air), how to deal with the added air(at above part of glass), treat it as continue phase? or dispersed phase? how to deal with the outlet condition at this time. Is it still use the dagessing consition, or use some other outlet condition for instead. Actually, I want to obtain the result, which can reflect both bubble column (injected gas) and the variety of free surface between the water and top air. So I used PARTICEL MODEL for gas-liquid (at the beginning, I just used the drag force, and didnt activate other non-drag force ), and FREE SURFACE FOR air-liquid. But I found if I used these two model together, there always had the same error as shown above.
Very thanks for your patient reply!

[zhubohong]

Originally Posted by Gert-Jan

You are very far away from a succesful simulation.
Do you have someone around with some experience? Like a supervisor?

1) You mentioned:
"The height of tank is 1 m, 0.6 for water, and 0.4 for oil."
But if I look at your output file, the first thing I noticed is:

+--------------------------------------------------------------------+
| Average Scale Information |
+--------------------------------------------------------------------+

Domain Name : Default Domain
Global Length = 6.9745E+02
Minimum Extent = 7.9191E+02
Maximum Extent = 8.1200E+02

I think you have to downscale by a factor 1000. You don't have to remesh, you can downscale in Pre.

2) Like most beginners, you turn on all physics that are relevant and then keep fingers crossed and hope CFX understands. But that is a asking for troubles.

Therefore: start as simple as possible. Delete all obsolete physics. Try to get that running first and then increase complexity by adding physics step by step. So remove:
- Surface tension. This make everything far too complicated. you don't need it anyway on this scale (only in geometries of mm scale).
- Lift coefficients
- ENHANCED TURBULENCE PRODUCTION MODEL
- maybe start with 1 continuous phase. You can also add the second one at a later stage

3) run auto timescale.

Haha, Actually, I am a freshman for CFD online, so I dont know how to show my question. for example, how to attach the geometry. At the begining, you asked me the details of my case. I dont know how to describe it. So, I used the similar case to represent to you (The height of tank is 1 m, 0.6 for water, and 0.4 for oil.). I think the simulation method between this similar case and my real case is same. I am not a fresheman for CFX. I know how to model the liquid-gas two phases flow using the Particel Model for many cases. But, this time, I want to simulate three phase flow, two gas phase, and one liquid phase. Just like, a glass with half part of water, and half part of air. And we inject the air from the bottom of glass. I mean that no matter what kind of materials or geometris or initization conditions we choose. The simulation method between these cases is same. If we just model the glass (full of water) with bottom air injection. It is very easy to use the PARTICEL MODEL with degassing condition. However, if we model this case(a glass with half part of water, and half part of air), how to deal with the added air(at above part of glass), treat it as continue phase? or dispersed phase? how to deal with the outlet condition at this time. Is it still use the dagessing consition, or use some other outlet condition for instead. Actually, I want to obtain the result, which can reflect both bubble column (injected gas) and the variety of free surface between the water and top air. So I used PARTICEL MODEL for gas-liquid (at the beginning, I just used the drag force, and didnt activate other non-drag force ), and FREE SURFACE FOR air-liquid. But I found if I used these two model together, there always had the same error as shown above.
Very thanks for your patient reply!

[Gert-Jan]

So, your vessel is approxmately 600 m in diameter. That is a huge application. Is it a lake (RH Dam simulation)?

If so,
- then switch off surface tension. You only need that for mm-applications.
- Regarding the modelling approach, it is important to know what question you are trying to answer. In other words: what is more important? The bubbles in the water? The waves on the surface? Mixing of the gasses? Gas concentration on the shore?
Bubbles and free surface are in general not a very good combination. Do I see it correctly that you are trying to get the best of both worlds?
- Did you consider ito treat it as a 2 phase simulation with a gas that constist of 2 components (Air & Ar).
- You have to set hydrostatic pressure as an initial guess. See reference Guide paragraph 10.3.1.

Regs, Gert-Jan

[zhubohong]

Originally Posted by Gert-Jan

So, your vessel is approxmately 600 m in diameter. That is a huge application. Is it a lake (RH Dam simulation)?

If so,
- then switch off surface tension. You only need that for mm-applications.
- Regarding the modelling approach, it is important to know what question you are trying to answer. In other words: what is more important? The bubbles in the water? The waves on the surface? Mixing of the gasses? Gas concentration on the shore?
Bubbles and free surface are in general not a very good combination. Do I see it correctly that you are trying to get the best of both worlds?
- Did you consider ito treat it as a 2 phase simulation with a gas that constist of 2 components (Air & Ar).
- You have to set hydrostatic pressure as an initial guess. See reference Guide paragraph 10.3.1.

Regs, Gert-Jan

I am very surprised by your reply, especially the keyword "the RH dam simulation". Do you know the RH degasser? The one of the sencondary steelmaking process. Hi, friend, can you tell me your email, I really want to take a deep discussion with you.

[Gert-Jan]

Haha. I'm sorry my friend but I just copied this word from your text file.
I was trying to find out what you were doing and found the word 'Dam'. Combined with the dimensions I imagined you modelling a volcanic lake filled with CO2 like in Cameroon, or similar.

Sorry I don't know the application at all.

[zhubohong]

Originally Posted by Gert-Jan

Haha. I'm sorry my friend but I just copied this word from your text file.
I was trying to find out what you were doing and found the word 'Dam'. Combined with the dimensions I imagined you modelling a volcanic lake filled with CO2 like in Cameroon, or similar.

Sorry I don't know the application at all.

Hey, friend, actually, I am simulating the RH degasser reactor, a steelmaking process. as shown in the attached figure. It is a gas-lift reactor. The process can be described as: the RH degassing starts with lifting the ladle until immersing the snorkels in the molten steel. Then, the molten steel will be suctioned into the vacuum vessel through the snorkels as a result of reducing the pressure in vacuum vessel. Almost simultaneously, argon gas is injected into the up-snorkel, leading to the recirculation of
molten steel.
In my previous model, I treated the free surface of molten steel in the vacuum vessel as the degasing condition, which is considered as flat. Therefore, the previous model ignored the top vacuum part of vessel, and we can use the PARTICLE MODEL to simulate this process. However, in the real process, the free surface can not be flat, and it will has a certain fluctuation as a resulf of the turbulence flow.
So, at this time, I want to refresh my model to reflect the free surface fluctuation (of course, the gas-lift process still should be reflected). But, the question is how to treat the top vacuum part of vessel, how to define it? Actually, this process can be simulated using the VOF+DMP model, which treats the argon gas as the particle. But, DMP model has a obvious shortcoming, it can not be used in the case with high gas volume fraction. So, at this time, I want to simulate it using the E-E method.
Can you give me some constructive advices? Thank you!

[ghorrocks]

Thanks for explaining it - now we have some idea of what you are talking about.

An obvious response is to model this with steel and argon as continuous phases with a free surface model with homogeneous equations, and then add argon gas bubbles as a dispersed phase. If you have tried this has it worked successfully?

An alternate approach could be to use steel and argon as continuous phases with a free surface model, but this time with inhomogeneous equations. This will allow you to add argon as a small volume fraction at the bottom of the riser and it should rise and join the bulk of the argon above the steel surface when it emerges. The interphase drag law will need to be tuned to match the conditions you get for your argon bubbles.

I am not sure the inhomogeous approach is going to work in your case, but it is simpler to implement so could be worth considering.

[zhubohong]

Originally Posted by ghorrocks

Thanks for explaining it - now we have some idea of what you are talking about.

An obvious response is to model this with steel and argon as continuous phases with a free surface model with homogeneous equations, and then add argon gas bubbles as a dispersed phase. If you have tried this has it worked successfully?

An alternate approach could be to use steel and argon as continuous phases with a free surface model, but this time with inhomogeneous equations. This will allow you to add argon as a small volume fraction at the bottom of the riser and it should rise and join the bulk of the argon above the steel surface when it emerges. The interphase drag law will need to be tuned to match the conditions you get for your argon bubbles.

I am not sure the inhomogeous approach is going to work in your case, but it is simpler to implement so could be worth considering.

Thanks for your reply. Now I am simulating my model using the first method that you metioned. Unfortunately, it has not been successful. I am not sure that this method is reasonable.
The second method that you metioned is not appropriate, becasuse the non-drag force in my model plays a very important role, and we have already proven it in my previous model.
I always think that can I also treated the top gas as the dispersed phase. Therefore, the model have two kinds of dispersed phase and one continue phase. The question is how to define the outlet.

[ghorrocks]

Why hasn't your models using my first suggested method been successful?

What drag forces are present which makes the second suggestion unsuitable?

What is your question about the outlet? A quick look at this thread and it is not clear to me what your question is.