|
[Sponsors] |
How to make the phase disappear by modifying the source |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
|
June 27, 2018, 04:14 |
How to make the phase disappear by modifying the source
|
#1 |
Member
zhubohong
Join Date: Apr 2018
Posts: 37
Rep Power: 8 |
Hello, everyone
I want to predict the fluaction of free surface, which is affected by bubble flow process, as shown in figure. I simulated three phases flow, top gas, injected gas and liquid steel. The top gas and liquid steel were treated as the continue phase dealed with the Free Surface Model, and injected gas was treated as the dispersed phase dealed with the Particel Model. However, in the real process, the top gas is actually the injected gas. But in my model, I divided it into two phases, because I want to reflect the free surface flow and bubble column simultaneously. In addtion, the gas will be pumped out of the reactor in the real process. But I can't simulate this process. So, I want to make the injected gas phase disappear when it meets the top gas phase (when the volume fraction of top gas is equal to 0.95 at the interface). I think it can be achieved by modify the source item in CFX. But I don't kown how to do. I need you guys give me some advices. Thanks! |
|
June 27, 2018, 06:07 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,728
Rep Power: 143 |
What is the physical size of the bubbles? What is the physical size of the vessel? How many bubbles are there (is it isolated bubbles, lots of bubbles or a foam of bubbles)?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
June 27, 2018, 06:19 |
|
#3 | |
Member
zhubohong
Join Date: Apr 2018
Posts: 37
Rep Power: 8 |
Quote:
volume fraction of gas bubble >10% |
||
June 27, 2018, 07:50 |
|
#4 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,728
Rep Power: 143 |
In that case:
It would be just possible to do this as a free surface model, if you have access to a large computing resources. Then you can do a direct model of all the physics. You also don't need to split the bubble phase from the continuous top gas phase, it can be all one gas phase. But this will be a seriously big simulation and you should only attempt it if you are experienced CFD operator with a lot of computer resources available. If your resources are smaller then look at Eularian or Lagrangian particle tracking. It is not clear to me at the moment whether Eularian or Lagrangian would be the better approach at this stage. I suspect they both could do it, in which case you should probably use the Eularian model as it is easier to use. Also I don't think you need to remove the bubble phase from the simulation when it reaches the top of the steel. It might be OK to allow the gas bubble phase to exist in the gas continuous phase - I suspect this will not cause any problems. But you better check this before you start using it.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
June 27, 2018, 13:27 |
|
#5 | |
Member
zhubohong
Join Date: Apr 2018
Posts: 37
Rep Power: 8 |
Quote:
I think my choice is right. I must divide the gas into two phases, because I should accuratly predict the bubble behavior. It means all of interphase forces must be considered. So only using the Free surface model can not meet my requirement. In addition, if I use the Lagrangain approach in my model, it will be meet the same problem. The bubble can not float out of the reactor. Of course, I can set the density of top gas with a larger value, but it doesn't match the reality. So, I think the better way is that making the injected gas disappear by modifying the source item. However, I just have this thought, I don't know how to do. I didn't found the related CFX tutorials. |
||
June 27, 2018, 18:36 |
|
#6 | |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,728
Rep Power: 143 |
Quote:
If you want the bubbles to disappear when they get to the continuous gas phase you can have a source term which is multiplied by the volume fraction of the continuous gas phase. Then it will automatically apply in the continuous gas phase region only. Also - Don't forget you can do this model by Eularian bubble model or a Lagrangian bubble model. The Eularian is likely to be easier, so I would use that one unless you can suggest a reason it will not work.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
||
June 28, 2018, 01:05 |
|
#7 | |
Member
zhubohong
Join Date: Apr 2018
Posts: 37
Rep Power: 8 |
Quote:
In addtion, if I use two phases to simulate, the outlet boundary is very hard to make sure. The overflow problem is coming. So, I should build a very large model. I used half a month to bluid the present model using PARTICEL+FREE SURFACE model. In the present model, I set a large value of the top gas density for letting injected gas flow out. But, the problem is obviously that, the larger density could restrict the fluaction of free surface. So, I think my final target about my model is to conquer the above problem. For the Lagrangian approach, actually, I have already used this method to simulate. I set the top gas density with a large value and let them flow out. Though the predicted results can be accepted, I still doubt whether this method is the right. This is because the high speed of injection gas and large volume fraction. So, another aim of my present work is to compare this two approaches, and discuss which approach may be more suitable for this chemical reactor. This is why I always emphasize I want to use the Eularian model at this time. Very very thanks for your reply!! |
||
June 28, 2018, 01:17 |
|
#8 | ||
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,728
Rep Power: 143 |
Quote:
Quote:
Did you see my last comment on your original question about making the bubble phase disappear at the gas continuous phase? I said "If you want the bubbles to disappear when they get to the continuous gas phase you can have a source term which is multiplied by the volume fraction of the continuous gas phase. Then it will automatically apply in the continuous gas phase region only."
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|||
June 28, 2018, 01:48 |
|
#9 | |
Member
zhubohong
Join Date: Apr 2018
Posts: 37
Rep Power: 8 |
Quote:
Another question: I am very make sure if I choose the interphase transfer with Particel Model, the predict results of bubble column is very nice. But if I change to use the Free surface model, it is suitable? As we know, the Free surface model makes the two phases have a stratification trend, it is suitable for bubble column? Sorry, because I have no any experience about modifying the source, I don't sensitive to your this comment:“If you want the bubbles to disappear when they get to the continuous gas phase you can have a source term which is multiplied by the volume fraction of the continuous gas phase. Then it will automatically apply in the continuous gas phase region only.” I will consider it later, seriouly! |
||
June 28, 2018, 02:04 |
|
#10 | |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,728
Rep Power: 143 |
Quote:
What don't you understand about my suggestion for a source term to make the bubbles disappear? If you make the source term which makes the gas bubble phase disappear multiply by the continuous gas volume fraction then it will be zero in the steel (so it does not apply) and full value in the continuous gas region (so it applies). This appears to answer your original question of how to make the bubble gas phase disappear in the continuous gas phase.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
||
June 29, 2018, 00:26 |
|
#11 | |
Member
zhubohong
Join Date: Apr 2018
Posts: 37
Rep Power: 8 |
Quote:
|
||
June 29, 2018, 03:34 |
|
#12 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,728
Rep Power: 143 |
The "Free surface flow over a bump" tutorial shows the use of a free surface model.
Other tutorials cover lagrangian models, eularian models, phase change, and so on. The CFX documentation has extensive details of the available models and on the ANSYS Customer website there is training material on multiphase models which goes into a lot of depth and is highly recommended. If you think the official tutorials are weak then I suspect you have not seen all the available material - it is extensive and thorough. I will not have time to write a step by step tutorial for you. If you don't understand what you are doing you should not be attempting a challenging multiphase simulation.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
July 4, 2018, 03:39 |
|
#13 | |
Member
zhubohong
Join Date: Apr 2018
Posts: 37
Rep Power: 8 |
Quote:
|
||
July 4, 2018, 07:54 |
|
#14 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,728
Rep Power: 143 |
The source term approach is not a phase change application. It will just magically disappear, there is no physics behind it.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
July 6, 2018, 02:48 |
|
#15 |
Member
zhubohong
Join Date: Apr 2018
Posts: 37
Rep Power: 8 |
||
July 6, 2018, 03:41 |
|
#16 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,728
Rep Power: 143 |
It is similar, I guess. In that case it assumes the boundary is the location of the free surface and allows the dispersed phase to cross it and leave the domain and does not allow the continuous phase to leave, it acts like a wall.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
July 6, 2018, 05:26 |
|
#17 | |
Member
zhubohong
Join Date: Apr 2018
Posts: 37
Rep Power: 8 |
Quote:
Is it possible to modify the property of injected gas? Just like, when the injected bubble meets the top gas phase, the density of it change to zero? If the density value of injected gas is equal to zero, is there the injected gas phase still in domain? Otherwise, I still need to find a way around modifying the source. |
||
July 6, 2018, 07:29 |
|
#18 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,728
Rep Power: 143 |
You can't make the density of a fluid go to zero. It will crash the solver.
I have already said three times in this thread how to make a source term to remove the gas bubble phase in the continuous gas phase region. You define a source term to set the volume fraction of the gas bubble phase to zero, and multiply the source term by the volume fraction of the continuous gas phase. If you don't understand my suggestion please tell me what you would like me to explain. If you continue to ignore my suggestions I will give up responding to you.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
July 12, 2018, 10:59 |
|
#19 | |
Member
zhubohong
Join Date: Apr 2018
Posts: 37
Rep Power: 8 |
Quote:
|
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[OpenFOAM.org] Patches to compile OpenFOAM 2.2 on Mac OS X | gschaider | OpenFOAM Installation | 136 | October 10, 2017 17:25 |
OpenFOAM without MPI | kokizzu | OpenFOAM Installation | 4 | May 26, 2014 09:17 |
Trouble compiling utilities using source-built OpenFOAM | Artur | OpenFOAM Programming & Development | 14 | October 29, 2013 10:59 |
"parabolicVelocity" in OpenFoam 2.1.0 ? | sawyer86 | OpenFOAM Running, Solving & CFD | 21 | February 7, 2012 11:44 |
UDFs for Scalar Eqn - Fluid/Solid HT | Greg Perkins | FLUENT | 0 | October 11, 2000 03:43 |