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

Convergence problem

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

Like Tree2Likes
  • 2 Post By Centurion2011

Reply
 
LinkBack Thread Tools Display Modes
Old   September 3, 2013, 10:32
Default Convergence problem
  #1
Member
 
Ali Mohamadi
Join Date: Aug 2012
Posts: 32
Rep Power: 4
Alimohamadi_nasr is on a distinguished road
I have worked on a geometry (3D) that has one inlet (velocity Inlet) and three out let (pressure outlet) which the shape is similar to (+), inlet channel (upside) is converging and three others are diverging. The Reynolds number in critical point is about 700 and flow is incompressible. I have solved it with coarse mesh by using first and second order of discretization.

By making the mesh finer, I only could solve it in first order with very good convergence criteria (density is below 10^-12); however, I could not solve it in second order. Residual jumped and after descending in some iteration it goes straight forward. I must mention that I made the mesh fine with constant coefficient (1.7) in all directions to preserve aspect ratio and skewness constant (I think my problem is sensitive to aspect ratio).

I used the solution of first order as initial condition of second order. I solved it with segregated and coupled algorithm, steady and unsteady with decreasing time step up to (10^-7), also I decreased under relation factors or currant number to lowest possible number. In all these cases residual fall and then go again straight forward with a little fluctuation.

There is only one point that the height of my channel is uniform in all parts and it equals to 0.2 mm, when I wanted to solve it in 2D form the flow became completely unstable and sometimes it diverged; however, after changing to 3D I could converged it in some cases but when I increase the mesh from 3 cells to higher number (5,6, ) I have convergence problem.

I use fluent 14; do you have any suggestion for me?
Is it possible that changing fluent to CFX could be useful for me?
Alimohamadi_nasr is offline   Reply With Quote

Old   September 4, 2013, 05:28
Cool
  #2
Member
 
Centurion2011's Avatar
 
Join Date: Jul 2011
Posts: 69
Blog Entries: 1
Rep Power: 9
Centurion2011 will become famous soon enough
chek this first
__________________
I'M NOT A GYNECOLOGIST BUT I'LL TAKE A LOOK.
Centurion2011 is offline   Reply With Quote

Old   September 4, 2013, 05:35
Default
  #3
Member
 
Ali Mohamadi
Join Date: Aug 2012
Posts: 32
Rep Power: 4
Alimohamadi_nasr is on a distinguished road
Thank you very much, I had read your post before, It was good review for me.
I think my problem is about mesh; however, its difficult to find proper mesh for this problem.
Alimohamadi_nasr is offline   Reply With Quote

Old   September 4, 2013, 05:37
Default
  #4
Member
 
Centurion2011's Avatar
 
Join Date: Jul 2011
Posts: 69
Blog Entries: 1
Rep Power: 9
Centurion2011 will become famous soon enough
What is your geometry? I could not understand it from your first post. Can you give us a screenshot (upload it first to some free server for pictures)? What mesh did you use?
__________________
I'M NOT A GYNECOLOGIST BUT I'LL TAKE A LOOK.
Centurion2011 is offline   Reply With Quote

Old   September 4, 2013, 05:47
Default
  #5
Member
 
Ali Mohamadi
Join Date: Aug 2012
Posts: 32
Rep Power: 4
Alimohamadi_nasr is on a distinguished road
I use triangular mesh in all domain.
Attached Images
File Type: jpg 1.jpg (71.8 KB, 28 views)
Alimohamadi_nasr is offline   Reply With Quote

Old   September 4, 2013, 05:50
Default
  #6
Member
 
Centurion2011's Avatar
 
Join Date: Jul 2011
Posts: 69
Blog Entries: 1
Rep Power: 9
Centurion2011 will become famous soon enough
perhaps solution of first order is good enough. My problems also sometimes (with Mach number above 1) have difficulties converging with second order methods. Maybe your mesh is too fine. Try coarsening it a bit
__________________
I'M NOT A GYNECOLOGIST BUT I'LL TAKE A LOOK.
Centurion2011 is offline   Reply With Quote

Old   September 4, 2013, 06:07
Default
  #7
Member
 
Centurion2011's Avatar
 
Join Date: Jul 2011
Posts: 69
Blog Entries: 1
Rep Power: 9
Centurion2011 will become famous soon enough
The following guidelines can help you make sure your CFD simulation is a succes:

1. Examine the quality of the mesh.
There are two basic things that you should do before you start a simulation:
Perform a mesh check to avoid problems due to incorrect mesh connectivity,
etc.
Look at maximum cell skewness (e.g., using the Compute button in the Contours
dialog box). As a rule of thumb, the skewness should be below 0.98.
If there are mesh problems, you may have to re-mesh the problem.

2. Scale the mesh and check length units.
In ANSYS FLUENT, all physical dimensions are initially assumed to be in meters.
You should scale the mesh accordingly. Other quantities can also be scaled independently
of other units used. ANSYS FLUENT defaults to SI units.

3. Employ the appropriate physical models.

4. Set the energy under-relaxation factor between 0.95 and 1.
For problems with conjugate heat transfer, when the conductivity ratio is very high,
smaller values of the energy under-relaxation factor practically stall the convergence
rate.

5. Use node-based gradients with unstructured tetrahedral meshes.
The node-based averaging scheme is known to be more accurate than the default
cell-based scheme for unstructured meshes, most notably for triangular and tetrahedral
meshes.

6. Monitor convergence with residuals history.
Residual plots can show when the residual values have reached the specified tolerance.
After the simulation, note if your residuals have decreased by at least 3
orders of magnitude to at least 10−3. For the pressure-based solver, the scaled
energy residual must decrease to 10−6. Also, the scaled species residual may need
to decrease to 10−5 to achieve species balance.You can also monitor lift, drag, or moment forces as well as pertinent variables or functions (e.g., surface integrals) at a boundary or any defined surface.
7. Run the CFD simulation using second order discretization for better accuracy
rather than a faster solution.
A converged solution is not necessarily a correct one. You should use the secondorder
upwind discretization scheme for final results.

8. Monitor values of solution variables to make sure that any changes in the solution
variables from one iteration to the next are negligible.

9. Verify that property conservation is satisfied.
After the simulation, note if overall property conservation has been achieved. In
addition to monitoring residual and variable histories, you should also check for
overall heat and mass balances. At a minimum, the net imbalance should be less
than 1% of smallest flux through domain boundary.

10. Check for mesh dependence.
You should ensure that the solution is mesh-independent and use mesh adaption
to modify the mesh or create additional meshes for the mesh-independence study.

11. Check to see that the solution makes sense based on engineering judgment.
If flow features do not seem reasonable, you should reconsider your physical models
and boundary conditions. Reconsider the choice of the boundary locations (or the
domain). An inadequate choice of domain (especially the outlet boundary) can
significantly impact solution accuracy.
__________________
I'M NOT A GYNECOLOGIST BUT I'LL TAKE A LOOK.
Centurion2011 is offline   Reply With Quote

Old   September 4, 2013, 06:21
Default
  #8
Senior Member
 
duri
Join Date: May 2010
Posts: 130
Rep Power: 6
duri is on a distinguished road
It seems flow encounters very high adverse pressure gradient. It could be possible that separation in second order creates unsteadiness and possibly damped in first order solution. (picture of flow field would be helpful). Another possible reason could be incompatible boundary condition. Please post more details for better understanding of your issue.
duri is offline   Reply With Quote

Old   September 4, 2013, 09:46
Default
  #9
Member
 
Ali Mohamadi
Join Date: Aug 2012
Posts: 32
Rep Power: 4
Alimohamadi_nasr is on a distinguished road
Thank you very much dear "Centurion2011"
your information is very useful, in my case I study a lot about mesh. except skewness, aspect ratio is also very important. In the nozzle area, I used aspect ratio between 1 and 1.5 to solve it in first order discretization.
Alimohamadi_nasr is offline   Reply With Quote

Old   September 4, 2013, 10:18
Default
  #10
Member
 
Ali Mohamadi
Join Date: Aug 2012
Posts: 32
Rep Power: 4
Alimohamadi_nasr is on a distinguished road
Dear Duri

You are completely true, there is separation in existence in the right side and maybe in down part. I have attached the contours of pressure and velocity for both first and second order. I think I should make mesh more finer specially in right and down side. I used only rectangular cell, do you think combination with triangular is better or not?
do you have any suggestion for me?
Attached Images
File Type: jpg pressure-first order.jpg (85.0 KB, 15 views)
File Type: jpg velocity-first order.jpg (89.3 KB, 12 views)
File Type: jpg pressure-second order.jpg (81.2 KB, 13 views)
File Type: jpg velocity-second order.jpg (85.3 KB, 10 views)
Alimohamadi_nasr 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
convergence problem when use pisoFoam, LES for wind tunnel case Forrest_Lei OpenFOAM 3 July 19, 2011 06:00
convergence problem commonyue Main CFD Forum 1 December 1, 2009 03:54
Convergence of CFX field in FSI analysis nasdak CFX 2 June 29, 2009 01:17
3D Fluid Flow Convergence problem Emily FLUENT 2 March 21, 2007 23:18
Non Convergence of 3D Heat transfer cfd problem Balraj Main CFD Forum 3 December 9, 2004 00:24


All times are GMT -4. The time now is 11:54.