CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLOW-3D

problem with the model of turbulence.

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 2, 2013, 16:20
Exclamation problem with the model of turbulence.
  #1
Member
 
ouni firas
Join Date: Oct 2013
Posts: 33
Rep Power: 3
ounifiras is on a distinguished road
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.
ounifiras is offline   Reply With Quote

Old   December 3, 2013, 13:12
Default
  #2
Senior Member
 
Jeff Burnham
Join Date: Apr 2010
Posts: 204
Rep Power: 8
JBurnham is on a distinguished road
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.
JBurnham is offline   Reply With Quote

Old   December 3, 2013, 16:31
Default
  #3
Member
 
ouni firas
Join Date: Oct 2013
Posts: 33
Rep Power: 3
ounifiras is on a distinguished road
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''
ounifiras is offline   Reply With Quote

Old   December 3, 2013, 16:41
Default
  #4
Senior Member
 
Jeff Burnham
Join Date: Apr 2010
Posts: 204
Rep Power: 8
JBurnham is on a distinguished road
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!
JBurnham is offline   Reply With Quote

Old   December 3, 2013, 17:05
Default
  #5
Member
 
ouni firas
Join Date: Oct 2013
Posts: 33
Rep Power: 3
ounifiras is on a distinguished road
thank you greatly Mr Jeff Burnham
ounifiras is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Implement an les turbulence model pante OpenFOAM Programming & Development 19 December 5, 2014 17:16
K - epsilon VS SST turbulence model Maicol Main CFD Forum 0 November 30, 2012 17:25
multiphaseInterFoam for RAS turbulence model chiven OpenFOAM Bugs 7 August 23, 2011 02:52
question about turbulence model selection and sensitivity karananand Main CFD Forum 1 February 26, 2010 05:41
Centrifugal Pump and Turbulence Model Michiel CFX 12 January 25, 2010 04:20


All times are GMT -4. The time now is 14:19.