CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

reactingEulerFoam: ThermalPhaseChangePhaseSystem does not converge.

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 1 Post By arianam
  • 1 Post By erlend_grotle

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 29, 2016, 18:41
Default reactingEulerFoam: ThermalPhaseChangePhaseSystem does not converge.
  #1
New Member
 
mohsen ari.
Join Date: Apr 2013
Posts: 12
Rep Power: 8
arianam is on a distinguished road
I tried to model boiling with reactingEulerFoam and it worked as the first step.
more details:
The geometry is a simple closed block full of liquid water near saturation temperature. The block temperture on bottom surface is higher than Tsat.
The phase type is ThermalPhaseChangePhaseSystem for water in two phases of liquid and gas.

As the second step, I devided the block to half liquid and half gas by setfields. The species is still water.
By applying the same BCs, the solution does not converge. The temperature and pressures diverges very quickly to small values.
I looked more carefully in the code and I understood this might be due to Tf and interfacial mass transfer or phase change calculation.

So basically, I am trapped between using one of these two: InterfaceCompositionPhaseChangePhaseSystem that is for interfacial phase change and ThermalPhaseChangePhaseSystem that I need it for wall boiling phase change.

I know that this code is a new code, and few people have gone through it, but any help is appreciated!
Kummi likes this.
arianam is offline   Reply With Quote

Old   May 31, 2016, 11:46
Default
  #2
New Member
 
Simone Colucci
Join Date: Mar 2016
Location: Pisa (Italy)
Posts: 23
Rep Power: 5
S.Colucci is on a distinguished road
Quote:
Originally Posted by arianam View Post
I tried to model boiling with reactingEulerFoam and it worked as the first step.
more details:
The geometry is a simple closed block full of liquid water near saturation temperature. The block temperture on bottom surface is higher than Tsat.
The phase type is ThermalPhaseChangePhaseSystem for water in two phases of liquid and gas.

As the second step, I devided the block to half liquid and half gas by setfields. The species is still water.
By applying the same BCs, the solution does not converge. The temperature and pressures diverges very quickly to small values.
I looked more carefully in the code and I understood this might be due to Tf and interfacial mass transfer or phase change calculation.

So basically, I am trapped between using one of these two: InterfaceCompositionPhaseChangePhaseSystem that is for interfacial phase change and ThermalPhaseChangePhaseSystem that I need it for wall boiling phase change.

I know that this code is a new code, and few people have gone through it, but any help is appreciated!
Hi,
I did the same successfully! When you have this kind of problem I think it depends on the phase change rate that is too high because the water at initial conditions is too much oversaturated. If you need, I can send you the input file of my simulation.

Best Regards

Simone
S.Colucci is offline   Reply With Quote

Old   June 6, 2016, 12:42
Default
  #3
New Member
 
mohsen ari.
Join Date: Apr 2013
Posts: 12
Rep Power: 8
arianam is on a distinguished road
Quote:
Originally Posted by S.Colucci View Post
Hi,
I did the same successfully! When you have this kind of problem I think it depends on the phase change rate that is too high because the water at initial conditions is too much oversaturated. If you need, I can send you the input file of my simulation.

Best Regards

Simone

Thanks for your response Simone!
Actually, I pushed forward the problem. I do still think that convergence is a big issue for this case and solver. However, I could control it.
Now, The problem that I face is the diffusion of liquid and gas at the interface. So the interface fades with time which is not physical.
The pipe is closed with half liquid and half gas.The cylindrical patch is divided into two(in longitudinal direction) so that two different temperature is applied to these half cylinders.
Do you have any idea where the problem is?
Attached Images
File Type: jpg Screenshot from 2016-06-06 11:32:59.jpg (36.1 KB, 118 views)
arianam is offline   Reply With Quote

Old   July 14, 2016, 08:00
Default Interfacial phase change
  #4
New Member
 
Erlend Grotle
Join Date: Jul 2016
Posts: 12
Rep Power: 5
erlend_grotle is on a distinguished road
Hi,

Im searching for tutorial cases in which the problems you mention are relevant. I think InterfacialCompositionPhaseChange is the one I need, to solve direct-contact phase change in separated flow.

Which tutorial should I go to? Or even better- can you hand over the case you show with the tank?


BR
Erlend
erlend_grotle is offline   Reply With Quote

Old   July 25, 2016, 17:47
Default
  #5
New Member
 
mohsen ari.
Join Date: Apr 2013
Posts: 12
Rep Power: 8
arianam is on a distinguished road
Hi Erlend,
I think the best tutorial for you would be :
tutorials/multiphase/reactingTwoPhaseEulerFoam/RAS/wallBoiling
It is a good starting point for your case that is not very far from what you try to model by OpenFOAM. it is based in ThermalPhaseChangeModel.
For wall phase change, you can use the wall functions implemented in most recent vesions of OpenFOAM.(alphatPhaseChange family wall functions).
Best,
Mohsen

Quote:
Originally Posted by erlend_grotle View Post
Hi,

Im searching for tutorial cases in which the problems you mention are relevant. I think InterfacialCompositionPhaseChange is the one I need, to solve direct-contact phase change in separated flow.

Which tutorial should I go to? Or even better- can you hand over the case you show with the tank?


BR
Erlend
arianam is offline   Reply With Quote

Old   July 26, 2016, 03:15
Default
  #6
New Member
 
Erlend Grotle
Join Date: Jul 2016
Posts: 12
Rep Power: 5
erlend_grotle is on a distinguished road
Hi arianam,
Thanks for your reply. I want to have interfacial phase change between liquid and gas, direct-contact. Do you think the model are relevant for this as well?
I will investigate and do the tutorial.

BR
Erlend
erlend_grotle is offline   Reply With Quote

Old   July 26, 2016, 12:56
Default
  #7
New Member
 
mohsen ari.
Join Date: Apr 2013
Posts: 12
Rep Power: 8
arianam is on a distinguished road
Yes. AFAK, this phase system model (ThermalPhaseChangePhaseSystem) takes in to account the two phase change mechanisms(volume and wall). idmdt field corresponds to interfacial phase change that is the same as volumic phase change. wdmdt is the wall phase change term obtained by wall function phase change term. The total phase change is the sum of two. However, you should know that the model doest not seem capable of modelling interfacial phase change in form of evaporation(diffusion of liquid phase in gas phase). For that, you need to change to InterfaceCompositionPhaseChangePhaseSystem.
Best,
Mohsen

Quote:
Originally Posted by erlend_grotle View Post
Hi arianam,
Thanks for your reply. I want to have interfacial phase change between liquid and gas, direct-contact. Do you think the model are relevant for this as well?
I will investigate and do the tutorial.

BR
Erlend
arianam is offline   Reply With Quote

Old   July 27, 2016, 08:02
Default
  #8
New Member
 
Erlend Grotle
Join Date: Jul 2016
Posts: 12
Rep Power: 5
erlend_grotle is on a distinguished road
Thank you arianam for this information.

BR
Erlend
erlend_grotle is offline   Reply With Quote

Old   July 29, 2016, 09:02
Default
  #9
New Member
 
Erlend Grotle
Join Date: Jul 2016
Posts: 12
Rep Power: 5
erlend_grotle is on a distinguished road
Dear Mohsen,

I have tried to change the tutorial "wallboiling" to a closed system with only walls. Then I use setFields to create a stratified initial case. I am excluding heat supply and try with slight temperature difference between liquid and gas. The results are strange.

I have not changed the Properties in any way. Is this related to unphysical starting conditions, or do I have to change the model properties? Im not sure if the stratified case can run with the existing model set-up.
Sorry for the lack of information, but if I understood you correctly you had looked into almost similar case.

Thanks,
Erlend
erlend_grotle is offline   Reply With Quote

Old   August 1, 2016, 12:04
Default
  #10
New Member
 
mohsen ari.
Join Date: Apr 2013
Posts: 12
Rep Power: 8
arianam is on a distinguished road
Hi,
How do you apply the difference between liq and gas temperatures? If you apply it by setFields, it is OK.
Surely, you will have the problem of convergence in stratified case, and need to work on that.
Did you cancel the boiling conditions or you want to keep them?
If it is possible, upload your case, so I might be able to help you in a more efficient way.
Best,
Mohsen
Quote:
Originally Posted by erlend_grotle View Post
Dear Mohsen,

I have tried to change the tutorial "wallboiling" to a closed system with only walls. Then I use setFields to create a stratified initial case. I am excluding heat supply and try with slight temperature difference between liquid and gas. The results are strange.

I have not changed the Properties in any way. Is this related to unphysical starting conditions, or do I have to change the model properties? Im not sure if the stratified case can run with the existing model set-up.
Sorry for the lack of information, but if I understood you correctly you had looked into almost similar case.

Thanks,
Erlend
arianam is offline   Reply With Quote

Old   August 1, 2016, 12:55
Default
  #11
New Member
 
Erlend Grotle
Join Date: Jul 2016
Posts: 12
Rep Power: 5
erlend_grotle is on a distinguished road
Thanks for you help.
It is stable now. I added a heated wall in the bottom and slight temperature difference between liquid and gas. Only walls now, no empty patch.

Please find the attach case files, and any comment will be very much appreciated.

BR
Erlend
Attached Files
File Type: gz 04_wallboiling.tar.gz (63.9 KB, 31 views)
vince002 likes this.
erlend_grotle is offline   Reply With Quote

Old   August 1, 2016, 12:55
Default
  #12
New Member
 
Erlend Grotle
Join Date: Jul 2016
Posts: 12
Rep Power: 5
erlend_grotle is on a distinguished road
But there is nothing happening, so I guess there is something wrong with the set-up

BR
Erlend
erlend_grotle is offline   Reply With Quote

Old   August 1, 2016, 13:35
Default
  #13
New Member
 
mohsen ari.
Join Date: Apr 2013
Posts: 12
Rep Power: 8
arianam is on a distinguished road
There is not a fast magic way for using OpenFOAM. It need one to be consistent. I looked at your case, it is important to know that when you modify part of your case it need to consistent to the other parts. For example:
by checkingMesh:
Overall domain bounding box (0 0 0) (0.05 2 0.1)
But how come for settingField you use this?!:
regions
(
boxToCell
{
box (-100 -100 -100) (100 1 100);
fieldValues
(
volScalarFieldValue alpha.liquid 1
);
}

boxToCell
{
box (-100 1 -100) (100 100 100);
fieldValues
(
volScalarFieldValue alpha.gas 1

);
}

The other example, if you compare alpha.* files with k.* files in 0 folder after setting field, you will see that the size of internalFields are not the same. You might have changed the meshing, so you need to change other boundary conditions since this case initial condition for both internalFields and patchfields are not uniform. There is a matrix and array of numbers given for internal field and boundary field that is probably obtained from running the case with a simpler code without activating all of its features to find a stable initial condition.
So, what I suggest is that you go through all initial conditions, and set them uniformly since we do not have any idea which initial condition guess is better for you case.
Alway before running your case, check it out with paraFoam for t=0. As you can see, it gives you the error of the size of k field(it is the first field read) since it is not compatible to your mesh.
checkMesh gives you hint on the size of your matrixes.
Work on your case step by step. If there is nothing in that to change mesh, put it aside for the moment, and just concentrate on initial conditions.

I hope that you'll find this helpful.
Quote:
Originally Posted by erlend_grotle View Post
But there is nothing happening, so I guess there is something wrong with the set-up

BR
Erlend
arianam is offline   Reply With Quote

Old   August 1, 2016, 14:40
Default
  #14
New Member
 
Erlend Grotle
Join Date: Jul 2016
Posts: 12
Rep Power: 5
erlend_grotle is on a distinguished road
Thanks for your reply. I turned on to laminar for the moment, and that's why the k-files are not consistent with the rest.

BR
Erlend
erlend_grotle is offline   Reply With Quote

Old   February 8, 2017, 07:33
Default
  #15
New Member
 
Robin Scholtes
Join Date: Nov 2016
Posts: 6
Rep Power: 5
Prandtl_2 is on a distinguished road
Quote:
Originally Posted by arianam View Post
Thanks for your response Simone!
Actually, I pushed forward the problem. I do still think that convergence is a big issue for this case and solver. However, I could control it.
Now, The problem that I face is the diffusion of liquid and gas at the interface. So the interface fades with time which is not physical.
The pipe is closed with half liquid and half gas.The cylindrical patch is divided into two(in longitudinal direction) so that two different temperature is applied to these half cylinders.
Do you have any idea where the problem is?
Dear Mohsen,

I use the interCondensatingEvaporatingFoam solver from OpenFoam v1606+ and have a similar problem with the convergence at the interface between the liquid and gas phase.
Could you please describe how you controll it and how you solve your other problems? I hope I can transfer it to my case.

Best regards
Robin
Prandtl_2 is offline   Reply With Quote

Old   February 22, 2017, 09:58
Default
  #16
New Member
 
Robin Scholtes
Join Date: Nov 2016
Posts: 6
Rep Power: 5
Prandtl_2 is on a distinguished road
Hello,

Meanwhile I also use reactingEulerFoam.

My aim is to simulate the evaporation of water into air and I would follow the mass fraction of water vapour in air.

For my case I devided my domain into a liquid phase (water) at the bottom and gas phase (0.5 air/ 0.5 water vapour) on the top by setfields.
I used the interfaceCompositionModel "saturated" with the saturation model ArdenBuck.
But at the moment my simulation break up very fast and I have no increasing of the vapour mass fraction in the gas phase.

Could anyone please help me?

Best regards

Robin
Prandtl_2 is offline   Reply With Quote

Old   May 20, 2017, 14:34
Default
  #17
Senior Member
 
Join Date: Aug 2014
Location: Germany
Posts: 292
Rep Power: 9
BlnPhoenix is on a distinguished road
Quote:
Originally Posted by Prandtl_2 View Post
Hello,

Meanwhile I also use reactingEulerFoam.

My aim is to simulate the evaporation of water into air and I would follow the mass fraction of water vapour in air.

For my case I devided my domain into a liquid phase (water) at the bottom and gas phase (0.5 air/ 0.5 water vapour) on the top by setfields.
I used the interfaceCompositionModel "saturated" with the saturation model ArdenBuck.
But at the moment my simulation break up very fast and I have no increasing of the vapour mass fraction in the gas phase.

Could anyone please help me?

Best regards

Robin

Hi Robin,

have you managed to converge your case? I'm trying reactingTwoPhaseEulerFoam right now and tried to get it stable by increasing Pimple Iterations and lower convergence parameters.
BlnPhoenix is offline   Reply With Quote

Old   January 2, 2018, 15:16
Default
  #18
New Member
 
Hz Lin
Join Date: Jan 2018
Posts: 2
Rep Power: 0
linhz0hz is on a distinguished road
Hello,
I am also hitting similar problems.
I tried to modify the bubbleColumnEvaporating example for reactingTwoPhaseEulerFoam and I want to model boiling of water. I changed the bottom to be a wall, and then increased the temperature close to saturation. I changed to Antoine saturation model because I eventually need to model some other liquid, but ArdenBuck is only for water (as I understand).
I kept the 350 degree temperature, but still I am finding that the solver will diverge and get non-physical temperatures (negatives or over 1000K). I tried to get finner mesh and smaller time-step which mediated this problem, and the solver can run fine with 350deg initial temperature. But when I increase the temperature a bit that issue hits me again. I am not sure if I should just increase mesh size or there is something fundamentally wrong with my setting / BC.

I am an undergrad student just stated to learn CFD and OpenFOAM on my own, any help greatly appreciated.
linhz0hz is offline   Reply With Quote

Old   November 19, 2019, 18:16
Default Theory behind phase change
  #19
Member
 
Stanley John
Join Date: Sep 2018
Posts: 43
Rep Power: 3
sjohn2 is on a distinguished road
Does anyone have the theory behind the
thermalPhaseChangeTwoPhaseSystem ?

How does OpenFoam compute the mass trasnfer terms based on interpolation from the saturation values provided in .csv files?
sjohn2 is offline   Reply With Quote

Reply

Tags
reactingtwophaseeulerfoam

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
can't converge in FLUENT ok___ko FLUENT 1 April 30, 2013 03:47
Gmres fails to converge, but LU is fine sbabbi Main CFD Forum 1 April 11, 2013 09:54
HELP !In relaxtion factor converge is taken or not MANOJ KUMAR FLUENT 5 September 22, 2005 05:16
Converge problem for multiphase flow Jen FLUENT 2 September 8, 2005 09:47
Converge problem for multiphase flow Jen FLUENT 4 July 20, 2005 17:52


All times are GMT -4. The time now is 07:25.