
[Sponsors] 
September 3, 2013, 10:32 
Convergence problem

#1 
Member
Ali Mohamadi
Join Date: Aug 2012
Posts: 32
Rep Power: 4 
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? 

September 4, 2013, 05:35 

#3 
Member
Ali Mohamadi
Join Date: Aug 2012
Posts: 32
Rep Power: 4 
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. 

September 4, 2013, 05:37 

#4 
Member

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. 

September 4, 2013, 05:47 

#5 
Member
Ali Mohamadi
Join Date: Aug 2012
Posts: 32
Rep Power: 4 
I use triangular mesh in all domain.


September 4, 2013, 05:50 

#6 
Member

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. 

September 4, 2013, 06:07 

#7 
Member

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 remesh 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 underrelaxation factor between 0.95 and 1. For problems with conjugate heat transfer, when the conductivity ratio is very high, smaller values of the energy underrelaxation factor practically stall the convergence rate. 5. Use nodebased gradients with unstructured tetrahedral meshes. The nodebased averaging scheme is known to be more accurate than the default cellbased 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 pressurebased 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 meshindependent and use mesh adaption to modify the mesh or create additional meshes for the meshindependence 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. 

September 4, 2013, 06:21 

#8 
Senior Member
duri
Join Date: May 2010
Posts: 130
Rep Power: 6 
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.


September 4, 2013, 09:46 

#9 
Member
Ali Mohamadi
Join Date: Aug 2012
Posts: 32
Rep Power: 4 
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. 

September 4, 2013, 10:18 

#10 
Member
Ali Mohamadi
Join Date: Aug 2012
Posts: 32
Rep Power: 4 
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? 

Thread Tools  
Display Modes  


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 