CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > FLUENT

Naca 0012 (compressible and inviscid) flow convergence problem

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

Like Tree7Likes
  • 1 Post By bipulsaha
  • 6 Post By Centurion2011

LinkBack Thread Tools Search this Thread Display Modes
Old   June 17, 2011, 07:43
Default Naca 0012 (compressible and inviscid) flow convergence problem
New Member
Bipul Saha
Join Date: Jun 2011
Posts: 1
Rep Power: 0
bipulsaha is on a distinguished road
I am currently modelling Flow around a 2D airfoil using Fluent 6.3.I have created 3 mesh geometries(coarse,medium,fine) in gambit and i am modelling it for 3 cases subsonic ,transonic and supersonic.I have gone through the fluent tutorials and have read a lot on the web on how to perform such simulations.But the problem is although i am getting almost accurate coefficient of lift,drag and pressure but my results are not converging.

I am using a density based solver and the flow is compressible and inviscid.Material is ideal gas and the cfl number i am using is .1.

Can someone please help me out.It will be a great help.
sherlock likes this.
bipulsaha is offline   Reply With Quote

Old   July 6, 2011, 07:51
Centurion2011's Avatar
Join Date: Jul 2011
Posts: 78
Blog Entries: 1
Rep Power: 19
Centurion2011 will become famous soon enough
about convergence in Fluent...

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 alsomonitor 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!

  • 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, reducethe Courant number.
  • Remesh or refine cells which have large aspect ratio or large skewness.
  • Remember that you cannot improvecell 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 thetime 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 whenhaving difficulty converging.
For density-based implicit solver:
  • The Courant number is not limitedby 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.


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...
Reggio, ebrahim27, nasser and 3 others like this.
Centurion2011 is offline   Reply With Quote


fluent, naca 0012

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
Incompressible and compressible flow. Confused student. Main CFD Forum 27 March 18, 2017 12:25
Solving Inviscid Compressible Flow mecbe2002 OpenFOAM 3 March 5, 2010 12:47
Compressible inviscid 1d spherical symmetry flow jinwon Main CFD Forum 0 July 12, 2007 13:13
Can 'shock waves' occur in viscous fluid flows? diaw Main CFD Forum 104 February 16, 2006 05:44
Inviscid Drag at subsonic, subcritical Mach # Axel Rohde Main CFD Forum 1 November 19, 2001 12:19

All times are GMT -4. The time now is 05:23.