CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Continuity eq convergence problem (http://www.cfd-online.com/Forums/fluent/47216-continuity-eq-convergence-problem.html)

 carno February 4, 2008 05:32

Continuity eq convergence problem

I am solving a CFD analysis of fuel injector (0.5mm nozzle). But I am facing the problem of convergence especially in continuity equation.

Mesh is tetra with prism layers at strategic locations. Actually there may be cavitation happening. I tried to activate that also. But same problem. Now I want to initialize the solution from converged w/o cavitation solution.

After that I did 100% hexa mesh. But the problem with convergence still persists.

What could be the reason?

 TL Balasubramanian February 4, 2008 05:45

Re: Continuity eq convergence problem

Is it getting diverged or slow convergenece? Are you using pressure based solver or density based solver? Are u solving energy equation also?

You can try changing the underrelaxation factors of solution/controls. sometimes if we start with close to exact solution, residuals does not decreases by high order, in that case convergence is decided not by value of residuals.

 carno February 4, 2008 06:13

Re: Continuity eq convergence problem

1. It is not slow convergence, but in fact it is divergence. +ve slope of the continuity eq line. 2. I tried reducing the URF, but in vain. 3. I am using pressure based solver and no energy eq solution. 4. I tried pr-pr BC combination and velocity inlet and pressure outlet BC combination. 5. There is one inlet and two outlets. 6. I am using double precision

Thanks

 jesse February 4, 2008 10:17

Re: Continuity eq convergence problem

there are many factors concerned with divergence, as far as mesh is concerned, for nozzle,not prism necessary,if you want, set up a boudary layer;

 Carlos February 8, 2008 05:04

Re: Continuity eq convergence problem

Sounds like you have checked all the right things here but the problem is almost certainly your mesh.

If you have a nozzle as fine as 0.5mm then you will have very large shear stresses in the flow leading to MASSIVE pressure gradients. If you resolve this region with a fine enough grid then the solution can gradually increase from cell to cell.

If you have too few cells in this critical region, as is probably the case, then the solver is forced to jump the flow variables too much from cell to cell. Applying a boundary layer grid is a good idea if you can get it to work as you want it.

Alternatively try a tet mesh with very fine cells where you expect the pressure/velocity gradients to be highest. Make sure you don't have any inverted elements also (grid->check-> make sure the smallest element volume isn't negative) and check the mesh quality.

You could have a few distorted cells elseware which are screwing everything up. Keep equiangle skew below 0.85. If you do relax the solution make sure you don't drop the URF's too much. Keep pressure at 0.15-0.2 and momentum at 0.3-0.5 to aid convergence.

First try using the standard k-epsilon model then look at other two equation models with the appropriate treatment for your Reynolds number. Then try RSM from one of these converged solutions.

Oh and make sure you do have a CONVERGED solution. To do this reduce the continuity convergence criterion in the residuals panel and drop it from 10^-3 to 10^-9. It will never reach 10^-9 for you problem but you need to let the solver iterate for at least 5000 iterations. Often, the residuals suddenly drop even when the solution looks converged. The only way to avoid convergence error is to apply the above step and wait until the gradient of the residuals is zero i.e. when the solution does not change and true convergence has been established - DO NOT TRUST THE DEFAULT CONVERGENCE LEVEL!!

Hope this helps and good luck,

Carlos.

 All times are GMT -4. The time now is 22:25.