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

OpenFOAM wonbt solve the momentum U equation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 3, 2008, 18:53
Default I'm trying to run icoFoam on a
  #1
sek
Member
 
Sung-Eun Kim
Join Date: Mar 2009
Posts: 76
Rep Power: 8
sek is on a distinguished road
I'm trying to run icoFoam on a 2-D (1-cell thickness) mesh that was converted from a FLUENT case file. I ran checkMesh on the mesh and everything looked fine. The icoFoam keeps skipping the U (momentum equation) solving the pressure equation only. Has anyone had the same problem?
sek is offline   Reply With Quote

Old   March 4, 2008, 14:50
Default Sounds like the tolerance you
  #2
pbo
Member
 
Patrick Bourdin
Join Date: Mar 2009
Posts: 40
Rep Power: 8
pbo is on a distinguished road
Sounds like the tolerance you specified for U is already met by the solution you start from.
Tighten the tolerance on U, and icoFoam will start solving for the momentum equations.
pbo is offline   Reply With Quote

Old   March 4, 2008, 16:41
Default Thanks for your time. Even if
  #3
sek
Member
 
Sung-Eun Kim
Join Date: Mar 2009
Posts: 76
Rep Power: 8
sek is on a distinguished road
Thanks for your time. Even if it's the case, it should print out the residual info etc. I reduced the tolerance. Still, icoFoam doesn't solve the momentum equations.
sek is offline   Reply With Quote

Old   March 4, 2008, 17:15
Default I bet your front and back empt
  #4
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
I bet your front and back empty planes are bent. Run checkMesh from the dev version on it - you should get something like:

Checking geometry...
Boundary openness (8.47033e-18 -8.47033e-18 -4.51751e-17) OK.
This is a 2-D mesh
Domain bounding box: (0 0 0) (0.1 0.1 0.01)

(mine is a 2-D mesh).

Alternatively, replace the boundary condition on front and back from empty to symmetryPlane and see what happens. If it starts solving, your domain is bent (look at it sideways).

Please let me know,

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

Old   March 5, 2008, 09:38
Default Hrv, Thanks for your time o
  #5
sek
Member
 
Sung-Eun Kim
Join Date: Mar 2009
Posts: 76
Rep Power: 8
sek is on a distinguished road
Hrv,

Thanks for your time on this. Changing empty type to symmetryPlane, OF indeed solves U.

Whn I did checkmesh, the only difference from yours is that it says

...
This is a 3-D mesh.

My colleague got this mesh by extruding 2-D mesh in Gridgen.

I see no sign of trouble at all. I seem to recall that OF once complained about "no solving direction ... (-1 -1 -1)" For this case, checkMesh doesn't say anything that indicates potential for troubles. iIt "silently" skips the momentum equations without any error message or warning at all.
sek is offline   Reply With Quote

Old   March 6, 2008, 17:27
Default The problem turned out to be t
  #6
sek
Member
 
Sung-Eun Kim
Join Date: Mar 2009
Posts: 76
Rep Power: 8
sek is on a distinguished road
The problem turned out to be the extrusion process done in Gridgen. The extrusion somehow created a conical section of the cylinder surface and one of the boundary thereforem got curved! When the 1-cell thick mesh is generated correctly, the problem went away. And the solver starts solving the momentum equations. Some osrt of warning message would be useful.
sek 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
Momentum Equation Munir Ahmed Khan FLUENT 0 August 27, 2008 07:57
Has anyone tried a delta form of pressure equation pressurecorrection equation with OpenFOAM sek OpenFOAM Running, Solving & CFD 2 July 24, 2007 07:53
How to solve another continuum and momentum eqn? west_wing FLUENT 0 August 25, 2003 10:00
Momentum Equation Andrew CFX 1 July 25, 2003 15:38
momentum equation cfp CFX 0 July 8, 2002 04:48


All times are GMT -4. The time now is 11:10.