CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

Strange temperature behaviour with interFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 11, 2012, 16:51
Question Strange temperature behaviour with interFoam
  #1
Member
 
Tayo
Join Date: Aug 2012
Location: FL
Posts: 94
Rep Power: 5
tayo is on a distinguished road
Hello all,

I added energy equation to interFoam following example in this trend

It compiles, runs and converges fine but I keep getting strange results with the temperature. I simulated rising bubble at high pressure. The problem is that after few time steps, the bubble temperature acts like a heat source such that the bubble temperature rises (+30k) above the saturated temp even when the surrounding liquid is also set at saturated condition. It's like perpectual motion machine of the 1st order (no heat source yet bubble temperature keeps increasing, even when I initialize the bubble temp to same as the surrounding). The bubble should atleast stay at around the same temperature as the surrounding liquid for now, right?

Temperature BC used are same as bubble, i.e. inlet, wall and internal field are at saturated temp; no phase change and no wall heating for now. My solver seems fine, similar what was used in the trend. 0.5 was used for maxCo and maxAlphaCo. Please how do I get the bubble temperature to behave right? Every advice is welcomed please. Thanks
tayo is offline   Reply With Quote

Old   December 12, 2012, 05:14
Default
  #2
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 240
Rep Power: 9
olivierG is on a distinguished road
hello,

I faced this issue some time ago with this solver (interFoam + T).
To solve this issue, i have added a limiter to T (min and max), and also use a lower time step + more corrector for the Pimple loop.
This effect (heated bubble) should disappear after some time step, and the limiter on T will not be used, but help for the first iterations.

regards,
olivier
olivierG is offline   Reply With Quote

Old   December 12, 2012, 13:53
Default
  #3
Member
 
Tayo
Join Date: Aug 2012
Location: FL
Posts: 94
Rep Power: 5
tayo is on a distinguished road
It has been resolved. Thanks Oliver. I actually noticed that setting the maxCo and maxAlphaCo to around 0.1 provided better results, yet it did not really resolve the issue. The true problem was with convective term. The way it was computed in the trend is not quite correct. What I did was to divide through my rhoCp and solve the energy eqn in the form below.

ddt(T) + div(phi,T) == laplacian(kappa/rhoCp,T)

From this, I think the best way to compute the convective term might be to simply multiply the flux with rhoCp i.e.
rhoPhiCp = phi*rho1*cp1*alpha1 + (scalar(1) - alpha1)*rho2*cp2*phi

thus, solving energy eqn as in the trend would be
ddt(rhoCp,T) + div(rhoPhiCp,T) == laplacian(kappa,T)

Note that I computed my kappa using simple VOF relation:
kappa = k1*alpha1 + k2*(scalar(1) - alpha1)


Now, I have another question:
What's the effect of including pressure in the equation? i.e.
ddt(rhoCp,T) + div(rhoPhiCp,T) + div(phi,p_rgh) == laplacian(kappa,T)
Every comment is welcomed.

Last edited by tayo; December 12, 2012 at 14:53.
tayo is offline   Reply With Quote

Old   July 11, 2014, 06:07
Default
  #4
Member
 
sajad
Join Date: Aug 2013
Posts: 64
Rep Power: 4
seju is on a distinguished road
dear foamer,
I know this post write for many time ago,but I face to this problem right now, I wanna simulation rising bubble with temp, following this boundary conditions:
upper wall 312k
and else is zeroGradient and my box have 298k.
after few iteration bubble temp be 400k.
can you help me plz?
how can I solve this problem?
seju is offline   Reply With Quote

Old   July 11, 2014, 06:16
Default
  #5
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 240
Rep Power: 9
olivierG is on a distinguished road
Hello,

You can now use compressibleInterFoam (from OF 2.2. and 2.3).

regards,
olivier
olivierG is offline   Reply With Quote

Old   July 11, 2014, 06:39
Default
  #6
Member
 
sajad
Join Date: Aug 2013
Posts: 64
Rep Power: 4
seju is on a distinguished road
Quote:
Originally Posted by olivierG View Post
Hello,

You can now use compressibleInterFoam (from OF 2.2. and 2.3).

regards,
olivier
dear olivier
in my case bubble is incompressible. how can used this solver? don't you know about my problem? why bubble temp increase?
best regard
Sajad
seju is offline   Reply With Quote

Old   July 11, 2014, 06:51
Default
  #7
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 240
Rep Power: 9
olivierG is on a distinguished road
hello,

Well if the temperature of the bubble will change, then your case is not incompressible, unless you consider small temperature variation.

And even with incompressible gaz (thus small temperature effect), you can use compressibleInterFoam solver.

regards,
olivier
olivierG is offline   Reply With Quote

Old   July 11, 2014, 07:04
Default
  #8
Member
 
sajad
Join Date: Aug 2013
Posts: 64
Rep Power: 4
seju is on a distinguished road
Quote:
Originally Posted by olivierG View Post
hello,

Well if the temperature of the bubble will change, then your case is not incompressible, unless you consider small temperature variation.

And even with incompressible gaz (thus small temperature effect), you can use compressibleInterFoam solver.

regards,
olivier
dear olivier
thanks for reply again, I wanna simulation bubble next to a wall, wall have 312k and box have 298k, after spend time, I must saw change bubble temp change but this change is between 298 to 312. but I saw this temp=400k, for this simulation can I use compressibleInterFoam?
thanks
seju is offline   Reply With Quote

Old   July 11, 2014, 07:20
Default
  #9
Member
 
Tayo
Join Date: Aug 2012
Location: FL
Posts: 94
Rep Power: 5
tayo is on a distinguished road
Hi Seju, double check how you're implementing the convection term in your energy equation. Seems you might have problem with your flux.
tayo is offline   Reply With Quote

Old   July 11, 2014, 07:28
Default
  #10
Member
 
sajad
Join Date: Aug 2013
Posts: 64
Rep Power: 4
seju is on a distinguished road
Quote:
Originally Posted by tayo View Post
Hi Seju, double check how you're implementing the convection term in your energy equation. Seems you might have problem with your flux.
dear Tayo
this is my energy equation:
fvScalarMatrix TEqn
(
fvm::ddt(rhoCp, T)
+ fvm::div(rhoPhiCpf, T)
- fvm::laplacian(kappaf, T)
);

TEqn.solve();
I simulation same you simulation this and I use
HTML Code:
[B]Diverging result for Temperature field in interFoam [/B]
I dont know why this is wrong. I valid this code for single phase but in two phase I have strange temp.
seju is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
strange curvature with interFoam (comparison with Brackbill work) duongquaphim OpenFOAM Running, Solving & CFD 23 July 25, 2013 01:03
kOmegaSST omega residuals strange behaviour zordiack OpenFOAM Running, Solving & CFD 0 August 8, 2012 16:23
buoyantBoussinesqSimpleFoam strange behaviour Mojtaba.a OpenFOAM Running, Solving & CFD 1 August 7, 2012 07:08
Adding temperature field to InterFoam yapalparvi OpenFOAM Running, Solving & CFD 8 October 14, 2009 20:18
Strange multicomponent source behaviour Zitron CFX 4 July 12, 2007 15:32


All times are GMT -4. The time now is 11:33.