Convergence problem
 

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?

chek this first

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.

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 use triangular mesh in all domain.

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

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.

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.

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.

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?