CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLOW-3D (http://www.cfd-online.com/Forums/flow-3d/)
-   -   problem with the model of turbulence. (http://www.cfd-online.com/Forums/flow-3d/127063-problem-model-turbulence.html)

ounifiras December 2, 2013 16:20

problem with the model of turbulence.
 
dear JBurnham

When i run a simulation of a flow over labyrinth weir with the model of laminar ; the simulation converge and it give good results ; but for the same model when i use the turbulence model K-e with a Turbulent mixing length as 7% of the flow depth ho over the spillway the model does not converge and the simulation stop before the finish time and this post APPEAR: time-step <dtmin. I think the problem is related to the model of turbulence.

JBurnham December 3, 2013 13:12

DT is the time step size. DTMIN is the minimum time step size, which you can set. There are many possible reasons why the time step is too small. Check your mesh resolution, boundary conditions, initial conditions, and fluid parameters. If the simulation is very long, then set DTMIN = 1E-6 or 1E-7. You shouldn't use DTMIN that is smaller, it will never finish running.

ounifiras December 3, 2013 16:31

dear JBurnham
when i have use minimum step Time as 1e-40 . the simulation stop at 8 second an this message appear
''end of calculation at t= 8.001E+00 cycle = 7189
excessive pressure iteration failures''

JBurnham December 3, 2013 16:41

Ounifras - if the model is terminating because of bad pressures, then you have to revisit the model setup. Check the following:

1) mesh: a single cell aspect ratio should be <= 3:1, two neighboring cells should vary in length by <= 1.25:1, multi-blocks should have the same cell sizes or cell sizes that are 2x each other, and multi-block boundaries and grid lines should match gridlines in the neighboring blocks. Cells should be small enough to eliminate 'sliver cells', which happen when a small part of a cell is open to flow: velocities in that sliver get very high, and this causes problems for the solver.

2) boundary conditions: are they realistic? are they correct? do they match initial conditions? will there be splashing at the start of the simulation?

3) initial conditions: are they realistic? are they correct? do they match boundary conditions? will there be splashing at the start of the simulation?

4) geometry: have you checked and fixed your .stl files in another program like netfabb Studio? is all geometry adequately resolved at all places by at least two or three cells? are there sliver cells that need to be eliminated?

5) fluid and physics parameters: are all units correct and consistent? Do you understand the meaning of the input variables you've added?

6) if all of the above are true, start turning off physics models until only gravity and turbulence are left. Try running the model in 2-D. Once you've solved the problem, go back to 3-D.

This is a general guide. Unfortunately I don't have time to look at your case. If you have the option, I'd consider asking whoever sold you the software to provide training: it seems that some basic concepts of CFD are new to you. Good luck!

ounifiras December 3, 2013 17:05

thank you greatly Mr Jeff Burnham


All times are GMT -4. The time now is 23:06.