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

Convergence question with regards to discretization

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 15, 2010, 23:47
Default Convergence question with regards to discretization
  #1
New Member
 
Karan Anand
Join Date: Feb 2010
Posts: 23
Rep Power: 8
karananand is on a distinguished road
I have a model where the turbine blades are cooled internally. The discretization to NS equation was first performed with 1st order upwind for momentum, energy and viscous model chosen and standard for pressure. The gradient was calculated with Least squares Cell based. the solution converged with residual set to 1e-4 for all except 1e-6 for energy.

After the solution converged, to get more accurate results, I switched to Second order upwind for all except pressure which was left as standard with gradient calculated with Least squares Cell based. This time however the solution seems stagnant with continuity at 1e-2, turbulence at around 5e-4 and momentum around 2e-4 energy is at 1e-5. I started with the converged solution to begin with.

Why is it that the solution is not getting converged for second order upwind? Is there a way I can force the solution to converge for this discretization method?
karananand is offline   Reply With Quote

Old   July 16, 2010, 08:45
Default
  #2
Senior Member
 
karine
Join Date: Nov 2009
Posts: 158
Rep Power: 8
thecfduser is on a distinguished road
Hi
1-u are doing a DNS (laminar model in Fluent)?? if yes how much cells do u have, whar is ure Re
2-u are using steady solver?? if yes is the flow really steady???

I need to know ure answers so i can know what is the problem.
FOr convergence, it is not like this that u must do:
try to monitor variables in the flow -by exemple Vz in point P-. For a steady solver, u will get convergence when ure variables dont change anymore.
thecfduser is offline   Reply With Quote

Old   July 16, 2010, 12:10
Default
  #3
New Member
 
Karan Anand
Join Date: Feb 2010
Posts: 23
Rep Power: 8
karananand is on a distinguished road
Quote:
Originally Posted by thecfduser View Post
Hi
1-u are doing a DNS (laminar model in Fluent)?? if yes how much cells do u have, whar is ure Re
No I am not doing a DNS.
Turbulence model: k-w SST.
At inlet (which is the hub of the blade) the velocity is 1.2266 m/s.
Other operating conditions/Boundary conditions:
Operating pressure: 1.435 MPa
Air temp: 500 K
Airfoil temp: 300 K (instead of cooling, heating is applied as it is easy to converge due to change in viscosity of air, this is done to study the effect of heat transfer coefficient)
Outlet: OUTFLOW
Air properties:
Viscosity (): 2.6375 x 10-5 kg/ms
Thermal Conductivity: 0.040284 W/m-K
Specific heat: 1030.305 J/kg-K
Density of air: incompressible-ideal gas
(using ideal gas law, around the inlet, density is 10 kg/m3)

Quote:
Originally Posted by thecfduser View Post
2-u are using steady solver?? if yes is the flow really steady???
Implicit pressure based solver with Pressure-vel coupling set to SIMPLE
I need the solution for a steady state. The model has no significant curvature , nor high values of natural convection.

Grid is Hybrid with hex core and tetra around. Have a prism boundary layer at the airfoil surface.

Quote:
Originally Posted by thecfduser View Post
try to monitor variables in the flow -by exemple Vz in point P-. For a steady solver, u will get convergence when ure variables dont change anymore.
Is there a specific variable you are taking about and where should it be?

Is absolute pressure or velocity at outlet a good option?
should I also monitor local surface temperature or Nu number or heat transfer coefficient at point?

are these good enough variables to check for convergence?

Thanks for your help.
karananand is offline   Reply With Quote

Old   July 16, 2010, 13:02
Default
  #4
Senior Member
 
karine
Join Date: Nov 2009
Posts: 158
Rep Power: 8
thecfduser is on a distinguished road
can u send a photo of ure geometry? tell me also if u have highly deformed mesh.

for monitoring, i suggest that u monitor 2-3 variables, and make at least one of these in the interior domain.

In fact, it is possible that ure 'steady - state' include some coherent motion that persists. While using hgh order descretisatin scheme (and of course a better turbulence model, lessly diffusive) ure simulation can better reproduce those strctures.
So ure residuals and monitors will include a cyclic behavior and it will not conerge.

Tell me what do u get when u monitor variables, and u can do the same thing for ure simulation with 1st upwind, that maybe did not converge too
thecfduser is offline   Reply With Quote

Old   July 16, 2010, 13:16
Default
  #5
New Member
 
Karan Anand
Join Date: Feb 2010
Posts: 23
Rep Power: 8
karananand is on a distinguished road
As of now I am using quite a coarse mesh:
http://img85.imageshack.us/gal.php?g...meshstrctu.jpg

When i tried solving without monitoring variables except the default ones in fluent and put it to 10-4, the first order converged. (I didnt see the variables as such so ill plot them to check.) However, after I changed to 2nd order, I did not see any cyclic behavior (again for momentum, energy and cont). It was just that it was steady and converging towards the residuals.

Ill check using individual variables anyway. Also could the grid`s coarseness be one issue?
karananand is offline   Reply With Quote

Old   July 16, 2010, 13:33
Default
  #6
Senior Member
 
karine
Join Date: Nov 2009
Posts: 158
Rep Power: 8
thecfduser is on a distinguished road
Even if residuals drop under 10^-4, it is not sure that u converged. If residuals of continuty are >10^-2, it does not mean that u didnt converge.
Check the variables.
For the mesh, where there is coarse elements is it solid or fluid elements???
Anyway i dont think the mesh is a problem. Generally u have more chance to converge if the mesh is coarse (but with a bad solution...U must refine to verify that ure solution is independant of grid size). And ure mesh seems to be reasonnably good.

I advice u to use hexa in place of tetra elements (use non conformal grid)
thecfduser is offline   Reply With Quote

Old   July 16, 2010, 13:46
Default
  #7
Senior Member
 
Chris
Join Date: Jul 2009
Location: Ohio, USA
Posts: 169
Rep Power: 9
Chris D is on a distinguished road
I actually think that the mesh could be problem, particularly where the cell size seems to change very rapidly. I've seen bad grids that run with first order and blow up with second order in fluent. Maybe it's because first order is very dissipative and knocks out everything that could blow out the code. I'm not really sure, but that might have something to do with it.
Chris D is offline   Reply With Quote

Old   July 16, 2010, 14:44
Default
  #8
New Member
 
Karan Anand
Join Date: Feb 2010
Posts: 23
Rep Power: 8
karananand is on a distinguished road
Quote:
Originally Posted by thecfduser View Post
For the mesh, where there is coarse elements is it solid or fluid elements???
The entire domain is fluid. The outermost surface of the blade is the wall (surface mesh only-turbine blade inner surface) where I am checking the temperatures and other parameters

Quote:
I advice u to use hexa in place of tetra elements (use non conformal grid)
you mean hex in the entire domain or just the zone where I have hex-core?

Also in FLUENT, to have non conformal grid:
"If you create a single grid with multiple cell zones separated by a non-conformal boundary, you must be sure that each cell zone has a distinct face zone on the non-conformal boundary" -Fluent Manual:
http://cdlab2.fluid.tuwien.ac.at/LEH...ug/node175.htm

Accordingly, I will have to divide the entire zone where I have hex-core to separate zones for each little cylinder and then have non conformal grid.

Just to let you know. I am validating the results to published numerical work. The paper seems to have similar grid (conformal) but just had tet elements. I added hex-core to reduce the number of elements and seed things up.
karananand is offline   Reply With Quote

Old   July 16, 2010, 14:49
Default
  #9
New Member
 
Karan Anand
Join Date: Feb 2010
Posts: 23
Rep Power: 8
karananand is on a distinguished road
Quote:
Originally Posted by Chris D View Post
I actually think that the mesh could be problem, particularly where the cell size seems to change very rapidly. I've seen bad grids that run with first order and blow up with second order in fluent. Maybe it's because first order is very dissipative and knocks out everything that could blow out the code. I'm not really sure, but that might have something to do with it.
Ill try to reduce the rapidly changing cell sizes and re run the case.

Also had a question about monitoring variables inside the domain in fluent.
I have added surface monitors (monitoring abs pressure using mass avg, velocity using mass avg at outlet and heat transfer coeff at the required walls)

I did not get the volume monitoring option. Is the suggestion to pick a point in the domain and monitor that? or is it to monitor averaged values for the domain?
karananand 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
Problems with convergence with an easy system franzdrs Main CFD Forum 0 June 15, 2009 18:17
Question about convergence criteria? Thomas FLUENT 7 April 8, 2005 19:38
help! cyclone convergence question Lcw FLUENT 1 January 26, 2005 16:29
Discretisation / Convergence Question Johnny B FLUENT 1 November 15, 2003 15:27
Convergence Question Colin FLUENT 13 May 16, 2003 11:41


All times are GMT -4. The time now is 13:26.