CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Convergence on skewed mesh (http://www.cfd-online.com/Forums/fluent/28432-convergence-skewed-mesh.html)

ales April 12, 2001 04:21

Convergence on skewed mesh
 
I am computing the task on mesh with highly skewed cells (in FLUENT 5.4). I am using second order discretizations schemes for all solved variables (turbulent flow). If I started with low relaxation factors (0.2-pressure, 0.4-momentum)the solution converged very slow and it will probable need a lot of iterations. When I want to speed up the convergence, I set the higher factors (0.3 - pressure, 0.5 - velocities). After twenty iterations of convergence the solution started to diverge and residuals steeply increased. The reason was the unrelistic variables just in the high skewed cells. For highly skewed meshes I found another pressure-velocity coupling PISO. I tried it, but without any efects. There is any good advice for solving problems on highly skewed meshes except the mesh improvement?

Anindya April 12, 2001 11:57

Re: Convergence on skewed mesh
 
Try to put higher relaxation factors for pressure and lower ones for velocities. This is because it is more difficult to converge pressure quantities than velocities. Try say 0.5-0.7 for pressure and 0.3 for velocities. See how your results converge now.

John C. Chien April 13, 2001 19:13

Re: Convergence on skewed mesh
 
(1). The mesh has to be consistent with the solutions. But with the current software approach, it is decoupled from the solution and is generated automatically for you. (2).So, the problem is with the approach built into the code. (3). The best way to use the current commercial code is to find out what meshes will be more acceptable to the code. So, it is easier to change the mesh first. (4). When the mesh is given automatically or arbitrarily, then even if one can get the converged solution, (which is unlikely), the solution will not be accurate because of the skewness of the mesh.(unless the code has special features to handle highly skewed cells) (5). The suggestion is always: change the mesh first. This will make it easier for the code in general. (it does not mean that you will get the converged solution automatically. it is still method, code, and problem dependent.)

Volker Pawlik April 17, 2001 07:17

Re: Convergence on skewed mesh
 
I noticed that only one cell with a skewness >= 0.98 as a part of a grid where all the others are <0.7 can cause a lot of difficulties with convergence.

So if there are only a few badly skewed cells, try to move nodes manually with tgrid. Very often the automatic smoothers keep bad cells over but a small node move helps the cells to reduce skewness below 0.9 or even 0.9. They are still not good to say it euphemisticly but fluent seems to be able to handle them without diverging.

What you should pay attention to is the cell volume after a node is moved. Sometimes it is not possible to see which node of a nearly flat cell must be moved to approve cell skewness AND to avoid negative volumes.

Volker

Scott W April 17, 2001 09:57

Re: Convergence on skewed mesh
 
If you can at all possibly avoid highly skewed cells, do it. Try this simple example: axisymmetric laminar flow down a pipe. Any solver should find a parabolic velocity profile after convergence. Now put just one highly skewed cell in the center of the pipe. Fluent currently will predict the flow will form two forks (as if the skewed cell was a solid obstacle), even when converged. If Fluent can't handle this simple flow, then it surely cannot handle complicated problems with highly skewed cells.

Volker Pawlik April 18, 2001 09:00

Re: Convergence on skewed mesh
 
Fortunately I cannot confirm your observations!

I created a 2d-mesh (Radius 40mm; Length 5000 mm: results from the inlet length for an inlet velocity of 0.176 m/s) with quad cells near the wall beginning with 6 mm and increasing in steps of 10%. The quads covered 50% of the radius. For the center zone (the other 50% of the radius) I generated triangles. In sum about 7 cells per Radius. Resulting in about 10000 cells in total.

The medium was air with fluent's standard properties. Resulting Re~=1000.

With the help of t-grid I distorted one cell near the axis to achieve a equi-vol-skewness of 0,98. (This seems to be suficient?) and another sharp one pointing in radial direction with a skewnes of 0.86.

I carried out the calculation till the Integral of the shear stresses on the pipe wall were constant (this corresponded with Residuals < 1E-4) and a litle bit longer (final residuals were lower than 1E-7).

The velocity profile at the exit (pressure-outlet) looked quite laminar..


All times are GMT -4. The time now is 21:10.