[Manu Poolakkal]

Originally Posted by Centurion2011

I see all kind of mistakes on these forums when dealing with convergence, so I will give brief review of methods...

At convergence, the following should be satisfied:

• All discrete conservation equations (momentum, energy, etc.) are obeyed in all cells to a specified tolerance OR the solution no longer changes with subsequent iterations.
• Overall mass, momentum, energy, and scalar balances are achieved.
• Monitoring convergence using residual history:
• Generally, a decrease in residuals by three orders of magnitude indicates at least qualitative convergence. At this point, the major flow features should be established.
• Scaled energy residual should decrease to 10-6 (for the pressure-based solver).
• Scaled species residual may need to decrease to 10-5 to achieve species balance.
• Monitoring quantitative convergence:
• Monitor other relevant key variables/physical quantities for a confirmation.
• Ensure that overall mass/heat/species conservation is satisfied.

In addition to residuals, you can also monitor lift, drag and moment coefficients.

Relevant variables or functions (e.g. surface integrals) at a boundary or any defined surface.

In addition to monitoring residual and variable histories, you should also check for overall heat and mass balances.

The net flux imbalance (shown in the GUI as Net Results) should be less than 1% of the smallest flux through the domain boundary

If solution monitors indicate that the solution is converged, but the solution is still changing or has a large mass/heat imbalance, this clearly indicates the solution is not yet converged.

In this case, you need to:

• Reduce values of Convergence Criterion or disable Check Convergence in the Residual Monitors panel.
• Continue iterations until the solution converges.

Selecting None under Convergence Criterion disables convergence checking for all equations.

Numerical instabilities can arise with an ill-posed problem, poor-quality mesh and/or inappropriate solver settings.

• Exhibited as increasing (diverging) or “stuck” residuals.
• Diverging residuals imply increasing imbalance in conservation equations.
• Unconverged results are very misleading!

Troubleshooting

• Ensure that the problem is well-posed.
• Compute an initial solution using a first-order discretization scheme.
• For the pressure-based solver, decrease underrelaxation factors for equations having convergence problems.
• For the density-based solver, reduce the Courant number.
• Remesh or refine cells which have large aspect ratio or large skewness.
• Remember that you cannot improve cell skewness by using mesh adaption!

Under-relaxation factor, α, is included to stabilize the iterative process for the pressure-based solver

• Use default under-relaxation factors to start a calculation.

Decreasing under-relaxation for momentum often aids convergence.
Default settings are suitable for a wide range of problems, you can reduce the values when necessary.
Appropriate settings are best learned from experience!

For the density-based solver, under-relaxation factors for equations outside the coupled set are modified as in the pressure-based solver.

A transient term is included in the density-based solver even for steady state problems.
The Courant number defines the time step size.
For density-based explicit solver:

• Stability constraints impose a maximum limit on the Courant number.
• Cannot be greater than 2(default value is 1).

Reduce the Courant number when having difficulty converging.
For density-based implicit solver:

• The Courant number is not limited by stability constraints.
• Default value is 5.

Convergence can be accelerated by:

• Supplying better initial conditions
• Starting from a previous solution (using file/interpolation when necessary)
• Gradually increasing under-relaxation factors or Courant number
• Excessively high values can lead to solution instability convergence problems
• You should always save case and data files before continuing iterations
• Controlling MultiGrid solver settings (not generally recommended)
• Default settings provide a robust Multigrid setup and typically do not need to be changed.

A converged solution is not necessarily a correct one!

• Always inspect and evaluate the solution by using available data, physical principles and so on.
• Use the second-order upwind discretization scheme for final results.
• Ensure that solution is grid-independent:
• Use adaption to modify the grid or create additional meshes for the grid-independence study

If flow features do not seem reasonable:

• Reconsider physical models and boundary conditions
• Examine mesh quality and possibly remesh the problem
• Reconsider the choice of the boundaries’ location (or the domain): inadequate choice of domain (especially the outlet boundary) can significantly impact solution accuracy

Numerical errors are associated with calculation of cell gradients and cell face interpolations.

Ways to contain the numerical errors:

• Use higher-order discretization schemes (second-order upwind, MUSCL)
• Attempt to align grid with the flow to minimize the “false diffusion”
• Refine the mesh
• Sufficient mesh density is necessary to resolve salient features of flow
• Interpolation errors decrease with decreasing cell size
• Minimize variations in cell size in non-uniform meshes
• Truncation error is minimized in a uniform mesh
• FLUENT provides capability to adapt mesh based on cell size variation
• Minimize cell skewness and aspect ratio
• In general, avoid aspect ratios higher than 5:1 (but higher ratios are allowed in boundary layers)
• Optimal quad/hex cells have bounded angles of 90 degrees
• Optimal tri/tet cells are equilateral

A grid-independent solution exists when the solution does not change when the mesh is refined.
Below is a systematic procedure for obtaining a grid-independent solution:

• Generate a new, finer mesh.
• Return to the meshing application and manually adjust the mesh.
• OR Use the solution-based adaption capability in FLUENT.
• VERY IMPORTANT: Save the case and data files first.
• Create adaption register(s) and adapt the mesh. Data from the original mesh is interpolated onto the finer mesh. FLUENT offers dynamic mesh adaption which automatically changes the mesh according to user-defined criteria.
• Continue calculations until convergence.
• Compare the results obtained on the different meshes.
• Repeat the procedure if necessary.

To use a different mesh on a single problem, use the TUI commands file/write-bc and file/read-bc to facilitate the setup of a new problem.
Better initialization can be obtained via interpolation from existing case/data by using solution data interpolation
A web-based training module is available to train users in replication of case setup and solution data interpolation.

Summary:

Solution procedure for both the pressure-based and density-based solvers is identical.

• Calculate until you get a converged solution
• Obtain a second-order solution (recommended)
• Refine the mesh and recalculate until a grid-independent solution is obtained.

All solvers provide tools for judging and improving convergence and ensuring stability.

All solvers provide tools for checking and improving accuracy.

Solution accuracy will depend on the appropriateness of the physical models that you choose and the boundary conditions that you specify.

sorry for lengthy post... sometimes people are lazy when theory is involved...

for convergence, is it necessary to display "solution converged!" or something like that in fluent?
my simulation is for a double pipe counter flow heat exchanger (3d). even after 10000 iteration fluent is not displaying anything like "solution converged !" but the results seem to be not changing. what should i do? how can i check whether the solution is converged or not?

[kaeran]

Hi Centurion 2011,

I got a big problem in convergence criterion for my simulation through Ansys Fluent.
I have almost tried all steps that you have suggested in your post about convergence. Let me expalin my problem first.

Inorder to run a transient simulation, initial converged inputs are essential. So, I ran a steady state pressure based simulation.
Convection and conduction processes takes place in quenching. So,obviously energy and turbulent models were switched on.
I used pressure based coupled solver with pseudo transient method to speed up the convergence.
The discretization schemes were (default),
Pressure- Standard
Momentum- second order upwind
Energy- second order upwind

I have tried Higher order term relaxation with default (0.75) relaxation factor and also 0.25 (in another simulation). The simulation ran for 5000 iterations with pseudo time step of 1e-05.

The result was not so convincing i.e., the solution was not converged.
At the end of the simulation, my conservative terms (residuals)were of the order
continuity e-03
momentum e-05 in x direction
e-04 in y direction
e-05 in z-direction respectively
energy e-17
mass imbalance e+02

These residuals keeps on oscillating and I couldn't standardise the solution.I have also cross-checked the mesh. It has decent orthogonal quality and skewness.

Minimum orthogonal quality is 0.20
Max. Skewness is 0.85
Max aspect ration is 45

but, these values are accepted as the geometry of the CAD model is relatively complex.

And my question here is , should I try for more iterations or should I further reduce relaxation terms?

If there are any other suggestions, it is always welcome.
And please correct me, if the steps that I mentioned here are inappropriate.


I also expect inputs from everyone.

[Centurion2011]

sorry, wasn't around for quite some time, didnt see questions

[kaeran]

got my problem solved long back

[imran99]

Originally Posted by Centurion2011

I see all kind of mistakes on these forums when dealing with convergence, so I will give brief review of methods...

At convergence, the following should be satisfied:

• All discrete conservation equations (momentum, energy, etc.) are obeyed in all cells to a specified tolerance OR the solution no longer changes with subsequent iterations.
• Overall mass, momentum, energy, and scalar balances are achieved.
• Monitoring convergence using residual history:
• Generally, a decrease in residuals by three orders of magnitude indicates at least qualitative convergence. At this point, the major flow features should be established.
• Scaled energy residual should decrease to 10-6 (for the pressure-based solver).
• Scaled species residual may need to decrease to 10-5 to achieve species balance.
• Monitoring quantitative convergence:
• Monitor other relevant key variables/physical quantities for a confirmation.
• Ensure that overall mass/heat/species conservation is satisfied.

In addition to residuals, you can also monitor lift, drag and moment coefficients.

Relevant variables or functions (e.g. surface integrals) at a boundary or any defined surface.

In addition to monitoring residual and variable histories, you should also check for overall heat and mass balances.

The net flux imbalance (shown in the GUI as Net Results) should be less than 1% of the smallest flux through the domain boundary

If solution monitors indicate that the solution is converged, but the solution is still changing or has a large mass/heat imbalance, this clearly indicates the solution is not yet converged.

In this case, you need to:

• Reduce values of Convergence Criterion or disable Check Convergence in the Residual Monitors panel.
• Continue iterations until the solution converges.

Selecting None under Convergence Criterion disables convergence checking for all equations.

Numerical instabilities can arise with an ill-posed problem, poor-quality mesh and/or inappropriate solver settings.

• Exhibited as increasing (diverging) or “stuck” residuals.
• Diverging residuals imply increasing imbalance in conservation equations.
• Unconverged results are very misleading!

Troubleshooting

• Ensure that the problem is well-posed.
• Compute an initial solution using a first-order discretization scheme.
• For the pressure-based solver, decrease underrelaxation factors for equations having convergence problems.
• For the density-based solver, reduce the Courant number.
• Remesh or refine cells which have large aspect ratio or large skewness.
• Remember that you cannot improve cell skewness by using mesh adaption!

Under-relaxation factor, α, is included to stabilize the iterative process for the pressure-based solver

• Use default under-relaxation factors to start a calculation.

Decreasing under-relaxation for momentum often aids convergence.
Default settings are suitable for a wide range of problems, you can reduce the values when necessary.
Appropriate settings are best learned from experience!

For the density-based solver, under-relaxation factors for equations outside the coupled set are modified as in the pressure-based solver.

A transient term is included in the density-based solver even for steady state problems.
The Courant number defines the time step size.
For density-based explicit solver:

• Stability constraints impose a maximum limit on the Courant number.
• Cannot be greater than 2(default value is 1).

Reduce the Courant number when having difficulty converging.
For density-based implicit solver:

• The Courant number is not limited by stability constraints.
• Default value is 5.

Convergence can be accelerated by:

• Supplying better initial conditions
• Starting from a previous solution (using file/interpolation when necessary)
• Gradually increasing under-relaxation factors or Courant number
• Excessively high values can lead to solution instability convergence problems
• You should always save case and data files before continuing iterations
• Controlling MultiGrid solver settings (not generally recommended)
• Default settings provide a robust Multigrid setup and typically do not need to be changed.

A converged solution is not necessarily a correct one!

• Always inspect and evaluate the solution by using available data, physical principles and so on.
• Use the second-order upwind discretization scheme for final results.
• Ensure that solution is grid-independent:
• Use adaption to modify the grid or create additional meshes for the grid-independence study

If flow features do not seem reasonable:

• Reconsider physical models and boundary conditions
• Examine mesh quality and possibly remesh the problem
• Reconsider the choice of the boundaries’ location (or the domain): inadequate choice of domain (especially the outlet boundary) can significantly impact solution accuracy

Numerical errors are associated with calculation of cell gradients and cell face interpolations.

Ways to contain the numerical errors:

• Use higher-order discretization schemes (second-order upwind, MUSCL)
• Attempt to align grid with the flow to minimize the “false diffusion”
• Refine the mesh
• Sufficient mesh density is necessary to resolve salient features of flow
• Interpolation errors decrease with decreasing cell size
• Minimize variations in cell size in non-uniform meshes
• Truncation error is minimized in a uniform mesh
• FLUENT provides capability to adapt mesh based on cell size variation
• Minimize cell skewness and aspect ratio
• In general, avoid aspect ratios higher than 5:1 (but higher ratios are allowed in boundary layers)
• Optimal quad/hex cells have bounded angles of 90 degrees
• Optimal tri/tet cells are equilateral

A grid-independent solution exists when the solution does not change when the mesh is refined.
Below is a systematic procedure for obtaining a grid-independent solution:

• Generate a new, finer mesh.
• Return to the meshing application and manually adjust the mesh.
• OR Use the solution-based adaption capability in FLUENT.
• VERY IMPORTANT: Save the case and data files first.
• Create adaption register(s) and adapt the mesh. Data from the original mesh is interpolated onto the finer mesh. FLUENT offers dynamic mesh adaption which automatically changes the mesh according to user-defined criteria.
• Continue calculations until convergence.
• Compare the results obtained on the different meshes.
• Repeat the procedure if necessary.

To use a different mesh on a single problem, use the TUI commands file/write-bc and file/read-bc to facilitate the setup of a new problem.
Better initialization can be obtained via interpolation from existing case/data by using solution data interpolation
A web-based training module is available to train users in replication of case setup and solution data interpolation.

Summary:

Solution procedure for both the pressure-based and density-based solvers is identical.

• Calculate until you get a converged solution
• Obtain a second-order solution (recommended)
• Refine the mesh and recalculate until a grid-independent solution is obtained.

All solvers provide tools for judging and improving convergence and ensuring stability.

All solvers provide tools for checking and improving accuracy.

Solution accuracy will depend on the appropriateness of the physical models that you choose and the boundary conditions that you specify.

sorry for lengthy post... sometimes people are lazy when theory is involved...

When using NITA in the fraction Step method. As CL And CD achived to their correct value and as time advances there is no changes in these values . but continuity residual varies between 0.1 to 0.001 . Is we can say solution converged or not . is solution correct or not??

[halouaneyacine]

Hello everyone,
I know that the pressure based solver is better for slow incompressible flow and the density-based solver is recommended for supersonic flow and shock waves simulation.
I'm wondering about the limitation of each solver?
when or where can I use them or cannot use them?

I prefer to give the reference of your answers and thank's a lot.
good luck.

[farzaneh.me2003]

Hi there
my case is about oil-WATER two phase flow. I couldn't achieve convergence because my continuity residuals are about 10^-2. what do you think about this problem? is this problem because of courant number(about 0.02) or momentum under relaxation(0.5) or multiphase flow coupled scheme that I used?

[Ema40]

Hello centurion2011.

I am simulating an open channel with some hydraulic structures inside it. Steady state, VOF for the free surface.

All the variables (xvelocity, y velocity, z velocity, k, epsilon, VOF of the secondary phase) converge with residual of 10^(-4), whereas the continuity equation residuals remain around 10^(-1), although the flow does not change any longer during iterations (10000 iterations!).

Do you know why?

Thank you

[asma hosseini]

Hello
I'm working a nano channel flow with electrophorse. I'm told get a plot of EOF velocity every 2000 iterations and when 2 plots had no changes, my solution is converged. I have calculated over 51000 iterations but plots change always. What should I do?

[imran99]

it will depend on type of problem steady/transient >you should run more than 150 non dimensional time. and see the pattern it will be of oscillatory nature. and reduce your time step size.

[Aohnia]

Originally Posted by Ema40

Hello centurion2011.

I am simulating an open channel with some hydraulic structures inside it. Steady state, VOF for the free surface.

All the variables (xvelocity, y velocity, z velocity, k, epsilon, VOF of the secondary phase) converge with residual of 10^(-4), whereas the continuity equation residuals remain around 10^(-1), although the flow does not change any longer during iterations (10000 iterations!).

Do you know why?

Thank you

Hi Ema40,

I'm having the same results for what it seems a similar problem to yours. Did you find out the reason why continuity equation residuals remain 10^(-1)?

Thanks in advance!

[mahipal parmar]

hi..i am trying to solve double pipe heat exchanger using inserts in CFD.
i used- double precision,
energy eq-on
model-turbulent(2 eq,stnd wall fun)

solution method:-SIMPLe(PRESSURE-VELOCITY BASED)-second order
my energy residules are not converges during solution.so ans is not converged.

boundary conditions:-
hot inlet:-mass flow rate-1.3 kg/s,inlet temp-413 k
hot outlet-pressure based
cold inlet:-mass flowrate-1.3, temp-298 k
cold outlet:-pressure base

any one have solution?plz guide me.
thanks in advance.

[Radwanma]

Hi All,

Could you confirm that the form of ct = Turbine_Torque / (0.5*density*pi*R^3*wind_speed^2) is correct to get coefficient of torque directly from fluent, please?
Thanks,

[Centurion2011]

You are all asking specific questions. This blog entry was written as a guideline only. Please post your questions on other subforums here

[luca007]

hello thank you for your help please im doing simulation in fluent for study the flow overe stepped spillways but the results its stay bed please i want to send you my projet to chek can you help me please ?

[G S Srivatsa]

Originally Posted by A CFD free user

Hi friend,
Obtaining a value of e-2 or even e-4 for residuals doesn't necessarily mean that your simulation is converged. However, a value of e-3 is acceptable for continuity, for other equations, it depends on your problem. For instance, in my recently work, a value of residual about e-8 is not enough to get convergence for a user_defined scalar! So, my suggestion is first, keep doing iteration until you don't observe any big change or oscillation in residuals. Secondly, in some cases, you need to monitor some effective parameters in your model beside the usual residuals monitoring. For example, depending on your work, you can monitor some surface or volume characteristics of flow. Only one more thing, in some cases you may not receive a very low residuals but the values will not change any more longer. In that case, your simulation is converged too. So, don't worry and be patient when you grip into a CFD problem.
Hope it helps.

Hello,

I am working on a flow simulation values over a blunt body with a spike, after running around 5000 iterations, the residuals(continuity, Energy, X-velocity and Y-velocity) are oscillating at E-3 and E-4 but the drag coefficient is constant, can I say my results have converged?

[luca007]

hello for I'm working for simulation for the flow over stepped spillways 10^-3
is enough ?
regards

[BlackHeartInertia]

I check mass imbalance and it was 1e-5 and I saved project. then it changes to 1e-3.. why? What should i do?

Sent from my SM-G570M using CFD Online Forum mobile app

[divergence]

Originally Posted by BlackHeartInertia

I check mass imbalance and it was 1e-5 and I saved project. then it changes to 1e-3.. why? What should i do?

Sent from my SM-G570M using CFD Online Forum mobile app

So you saved the case and the date and continued to iterate? Or did you read the saved files after closing the Fluent window? If it's the latter, then there's nothing weird about because those bumps come every time one reads an older case and continues the calculation. I have thought -not 100% sure about this- that the bumb in residuals is because the data is not saved in maximal size, i.e. in order to save disk space, Fluent chooses to neglect some decimals from cell values. After reading the case again, the program once again starts to use the defined amount of decimals, which causes a shock to the solution.

[BlackHeartInertia]

Originally Posted by divergence

So you saved the case and the date and continued to iterate? Or did you read the saved files after closing the Fluent window? If it's the latter, then there's nothing weird about because those bumps come every time one reads an older case and continues the calculation. I have thought -not 100% sure about this- that the bumb in residuals is because the data is not saved in maximal size, i.e. in order to save disk space, Fluent chooses to neglect some decimals from cell values. After reading the case again, the program once again starts to use the defined amount of decimals, which causes a shock to the solution.

It doesnt change after reading the case it change when i continue iterations. Now the mass imbalance is 1exp-7 but if I continue iterations maybe it can change to a different value like 0.001 (very different) so I dont know what it means or what to do. Should I continue iterations or stop there.

(In the case of residuals they are stable but dont decrease from arround 1 exp-2, and convergence monitors are stable)