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

Fluid Flow and Heat Transfer in a Mixing Elbow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 14, 2006, 14:59
Default Hello Foam users i am tryin
  #1
atzaru
Guest
 
Posts: n/a
Hello Foam users

i am trying to simulate Fluid Flow and Heat Transfer in a Mixing Elbow (a problem similar with the one in fluent tutorials).

the file can be downloaded here

MixingElbow.tar.bz2


hen i run the case i obtain always:


BICCG: Solving for Ux: solution singularity
BICCG: Solving for Uy: solution singularity
BICCG: Solving for h: solution singularity
ICCG: Solving for pd: solution singularity
time step continuity errors : sum local = nan, global = nan, cumulative = nan
rho max/min : 0 0
ExecutionTime = 0.34 s ClockTime = 0 s


Can anybody have a look on my file and give me a hint?
thanks
Atzaru
  Reply With Quote

Old   May 15, 2006, 11:52
Default Try checkMesh . MixingElbow
  #2
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,914
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Try

checkMesh . MixingElbow

Amongst other things it says

--> FOAM Serious Error :
From function primitiveMesh::checkClosedBoundary(const bool report) const
in file meshes/primitiveMesh/primitiveMeshCheck.C at line 91

And for 800 cells it says

High aspect ratio for cell 0: 1.59475e+197

IMHO you'll have a hard time to simulate anything on that mesh.
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   May 15, 2006, 12:00
Default One more remark: blockMesh com
  #3
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,914
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
One more remark: blockMesh complains about negative volumes (which is a strong indication for problems)

I think the problem is somewhere in your blockMeshDict
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   May 17, 2006, 08:07
Default Bernhard thanks a lot for your
  #4
atzaru
Guest
 
Posts: n/a
Bernhard thanks a lot for your sugestions. I corrected the geometry but it seems there is another problem

I attached again my case

MixingElbow.tar.gz

Here is what the openFoam reports when stops iterating after only 4 time steps:

Time = 4

BICCG: Solving for Ux, Initial residual = 0.331866, Final residual = 8.91692e-07, No Iterations 6
BICCG: Solving for Uy, Initial residual = 0.223996, Final residual = 8.35056e-06, No Iterations 6
BICCG: Solving for h, Initial residual = 0.274355, Final residual = 1.56448e-06, No Iterations 6


--> FOAM FATAL ERROR : Maximum number of iterations exceeded

From function specieThermo<thermo>::T(scalar f, scalar T0, scalar (specieThermo<thermo>::*F)(const scalar) const, scalar (specieThermo<thermo>::*dFdT)(const scalar) const) const
in file /home/dm2/henry/OpenFOAM/OpenFOAM-1.3/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 83.

FOAM aborting

Foam::error::printStack(Foam:stream&)
Foam::error::abort()
Foam::hThermo<foam::puremixture<foam::consttranspo rt<foam::speciethermo<foam::hconstthermo<foam::per fectgas> > > > >::calculate()
Foam::hThermo<foam::puremixture<foam::consttranspo rt<foam::speciethermo<foam::hconstthermo<foam::per fectgas> > > > >::correct()
buoyantSimpleFoam [0x805cf48]
__libc_start_main
__gxx_personality_v0

Anybody had a similar problem?

atzaru
  Reply With Quote

Old   May 17, 2006, 10:53
Default Hi Atzaru. Try what I alway
  #5
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,914
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Hi Atzaru.

Try what I always do: write out the solution at every timestep and look for strange pheomena. In your case that means: negative temperatures near the outlet at t=3 (which might cause problems for the perfect gas ...)

However. When I looked at the velocities at t=1 they were even stranger: velocities of up to 180 in the straight part that leads to the oulet, and they drop just before the bend. So I suspect there is still a problem with your blockMesh (but I'm not using that very often so I can't help you there, sorry)
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   May 17, 2006, 13:35
Default Thanks again Bernhard for your
  #6
atzaru
Guest
 
Posts: n/a
Thanks again Bernhard for your answer.

I suspect a bug in the solver because i have done a test using the same geometry and i just change the solver from buoyantSimpleFoam to the transient one buoyantFoam and it works ....the results looks as expected (so the geometry and mesh is good). I will try also to run my case in the OpenFoam version 1.2 and see if it runs or not.

In the buoyantSimpleFoam i keep receiving:






BICCG: Solving for Ux: solution singularity
BICCG: Solving for Uy: solution singularity
BICCG: Solving for h: solution singularity
ICCG: Solving for pd: solution singularity
time step continuity errors : sum local = nan, global = nan, cumulative = nan
rho max/min : nan nan
BICCG: Solving for epsilon: solution singularity
BICCG: Solving for k: solution singularity
ExecutionTime = 0.66 s ClockTime = 1 s

Can it be a bug in the solver or i am doing a stupid mistake?

Does anybody had similar experience with buoyantSimpleFoam ? Or does anybody have a similar working example and can email it to me?


MixingElbow_tr.tar.gz -transient case works

MixingElbow.tar.gz -steady state case does not run

Atzaru
  Reply With Quote

Old   May 17, 2006, 14:34
Default OK. I did two minor modificati
  #7
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,914
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
OK. I did two minor modifications (to the case from your 6:07am posting):

Change the IC for U from (0.2 0 0) to (0 0 0) and set g in the environmentalProperties to (0 0 0).

Now it runs and the result looks reasonable. But don't ask me why (maybe someone who knows more about the buoyant-solvers can tell you about the problem)
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   May 17, 2006, 17:47
Default Hi Bernhard You are right,
  #8
atzaru
Guest
 
Posts: n/a
Hi Bernhard

You are right, if i change the case to the particular one u have suggested it will run and the solution is believable. This is verys strange ...

I try also to switch from laminar to k-eps model and again the error appears.

Maybe Mr Hrvoje Jasak have some suggestions (or is a bug in the code?)?


Any suggestion will be appreciated
Atzaru
  Reply With Quote

Old   May 18, 2006, 08:33
Default Well: (I don't feel obliged
  #9
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Well:

(I don't feel obliged to answer all these questions because my time is very much in demand, so please go easy on calling out names. Also, it's been more than 10 years since I've meed a Mister) :-)

Of course, no bug in the code. I get:

Exec : buoyantSimpleFoam /home/hjasak/OpenFOAM/hjasak-1.3/run/support MixingElbow
Date : May 18 2006
Time : 08:33:59
Host : wooster
PID : 14907
Root : /home/hjasak/OpenFOAM/hjasak-1.3/run/support
Case : MixingElbow
Nprocs : 1
Create time

Create mesh for time = 0


Reading environmentalProperties
Reading thermophysical properties

Selecting thermodynamics package hThermo<puremixture<consttransport<speciethermo<hc onstthermo<perfectgas>>>>>
Floating exception


and that would be because your internal field for the temperature is set to zero!!!!.

Do yourself a favour and set the following in the .cshrc (or equivalent) - it will help you.

setenv FOAM_SIGFPE 1
setenv FOAM_SETNAN 1


Until next time,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   May 19, 2006, 02:06
Default Thank you for your kind answer
  #10
atzaru
Guest
 
Posts: n/a
Thank you for your kind answer. I will be more careful next time

Atzaru
  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
Mixing elbow case water heat transfer calculation buoyantFoam benyamin1 OpenFOAM Running, Solving & CFD 0 January 14, 2006 10:25
PHD posiiblets in heat transfer and fluid flow in yousef Main CFD Forum 0 July 29, 2005 16:07


All times are GMT -4. The time now is 06:04.