# courant number in vof

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

 November 3, 2013, 04:48 courant number in vof #1 New Member   ---reza Join Date: Nov 2013 Posts: 2 Rep Power: 0 hi all, i have a problem. when i use vof model, i must set courant number in this model. But this error is displayed. primitive error @ node 2: global courant number is greater than 250.0. the velocity field is probably diverging.please check the solution and reduce the time-step if necessary. Meanwhile time step=0.01,what can i do to solve this error?

November 8, 2013, 11:57
#2
Senior Member

Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 141
Rep Power: 6
Quote:
 Originally Posted by reza_gharib1369 hi all, i have a problem. when i use vof model, i must set courant number in this model. But this error is displayed. primitive error @ node 2: global courant number is greater than 250.0. the velocity field is probably diverging.please check the solution and reduce the time-step if necessary. Meanwhile time step=0.01,what can i do to solve this error?
You must select a smaller time step. For example I use time step=0.000001 in my problem

 December 26, 2013, 05:21 #3 New Member   ---reza Join Date: Nov 2013 Posts: 2 Rep Power: 0 thank you for your answer

 December 31, 2013, 19:43 #4 New Member   stefanus tobing Join Date: Oct 2013 Posts: 19 Rep Power: 5 hi, in my case, I want to fill the tub until it is full with water in 2D. if I use time step size low = 0,1; number of time step = 100; auto save every(time step) = 10 i need time until 60 s, until the tub is full but in interation (before the tub is full) i got error message in 2 s, . the tub is not full yet what things should i change? ps: error "Global courant number is greater than 250.00 The velocity field is probably diverging. Please check the solution and reduce the time-step if necessary." thanks alot, if you can help me, this now. Attachment 27667

 January 4, 2014, 04:53 #5 Senior Member   Jamal Foroozesh Join Date: Oct 2012 Location: Iran Posts: 141 Rep Power: 6 You must reduce time step,too. trust me mohammad hossein and stefenbink like this.

January 6, 2014, 16:06
#6
New Member

stefanus tobing
Join Date: Oct 2013
Posts: 19
Rep Power: 5
Quote:
 Originally Posted by jamalf64 You must reduce time step,too. trust me
thanks,, i have tried and it worked.
btw
is it can solve Divergence detected in AMG solver: pressure correction or x-momentum too? may calculation is end with divergence lately

January 7, 2014, 12:31
#7
Senior Member

Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 141
Rep Power: 6
Quote:
 Originally Posted by stefenbink thanks,, i have tried and it worked. btw is it can solve Divergence detected in AMG solver: pressure correction or x-momentum too? may calculation is end with divergence lately
Sorry, I dont know

 February 12, 2015, 05:43 #8 Member   enass Join Date: Feb 2015 Location: Alexandria-Egypt Posts: 30 Rep Power: 3 Mesh Requirements: Create uniform mesh. In regions where the mesh is refined, ensure that there is a gradual transition to the coarser mesh. Avoid sudden changes in cell size. The maximum skewness of the volume mesh should be less than 0.95 and maximum aspect ratio of tetrahedral cells should be less than 5. In compressible phase calculations, use of non-conformal interfaces can leads to solution instability and divergence. You should avoid non-conformal interfaces in the region of liquid-air interfaces. This is one limitation of VOF with compressible calculations. This limitation becomes magnified when you use MDM ( Explicit mesh update) with explicit VOF. Phase: Use compressible phase as primary phase. Viscous model: Check the Reynolds number and use Turbulence model if needed. Specified Operating density: Switch on the specified operating density and specify the density of lightest phase. Implicit body force: Turn on if dificulty in convergence. You should turn off when surface tension force is important and with small body forces. P-V Coupling: Use SIMPLEC/SIMPLE Spacial Discretization: Least Spquare Cell Based/ Green Gauss Cell Based URF: Use small values. Pressure-0.2, Momentum- 0.3, Turbulent kinetic energy- 0.5, Turbulent dissipation rate – 0.5. Use this command for better patching: (rpsetvar ‘patch/vof ? #t) If you face divergence at the beginning of the simulation, start the simulation with very small time step size, and increase after a few time steps if Global courant number is under control. The global courant number is printed in the Fluent console window ( with explicit VOF) at every time step. The Global courant number depends on the mesh size, velocity field, and the time step size used for the transport equations. If CFL exceeds 2 and keeps on increasing, that means your velocity field is increasing or/and the interface is moving through dense cells, and the time step size used is too high. You need to reduce the time step size to bring the Global courant number under control. For VOF calculations (using the Explicit scheme), FLUENT allows you to use variable time stepping in order to automatically change the time-step when an interface is moving through dense cells or if the interface velocity is high. If there are frequent velocity jumps in your problem, it is better to use the variable time stepping method to control the CFL under limit. The solution will be stable with the variable time stepping method. If you use the fixed time step, the CFL may exceed the value 2 whenever there is a velocity jump or when the interface is moving through dense cells, and your results will be time step size dependent. If you continue with the same time step size, the results will not be accurate, and this may even lead to divergence. It is better to use variable time stepping method for this type of problems and for compressible VOF calculations. Variable time stepping method: Here the input will be CFL. The global courant number is constant and the time step size varies with the velocity field. You should give appropriate value for Global courant number (CFL). Because, the time step size for transport equations are calculated from this CFL. You need to specify the Global courant number, minimum time step size, maximum time step size, minimum step change factor and maximum step change factor. Global courant number: The default value of the Global Courant number is 2, but smaller value may be required for more accurate solution and more stable numerical calculation. In some cases, you need to reduce this up to 0.5 for accurate results and . This is because the time step size (so, the CFL) should be small enough to get the accurate results. In some cases you may use CFL greater than 2 depending on the problem. Maximum Time step size: minimum grid size / maximum velocity in the domain Minimum Time step size: It should be greater than 1e-10. You cannot use time step size less than 1e-10. This is the limitation of VOF Explicit scheme. Minimum step change factor: The default value is 0.5. Maximum step change factor: The default value is 5. It is better to reduce this value to 1.5-2 to avoid the sudden increase in time step size. If the Explicit VOF with variable time stepping does not work, try the Implicit VOF scheme with Bounded Second Order Transient scheme. If still there is a divergence, check your mesh quality, boundary conditions and physics of the problem vga67, Ellie, stefenbink and 2 others like this.

 August 25, 2016, 04:52 #9 New Member   Thasneem Moosa Join Date: Mar 2016 Posts: 3 Rep Power: 2 Hello, In my analysis the fluid has to move against the gravity on heating in a Pulsating heat pipe(PHP) from the evaporator section in the bottom to the condenser in the top(of PHP).The movement of the fluid starts after a good 10s.But before it could reach 10s it shows courant no. error.Is it possible to give a larger step size say 10s initially and then reduce the time steps (Variable time stepping method) so as to get the lead?

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post fireman FLUENT 5 July 28, 2016 12:55 sharonyue OpenFOAM Running, Solving & CFD 13 January 2, 2013 23:40 xujjun CFX 9 June 9, 2009 07:59 kasim CFX 5 March 16, 2008 19:23 msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58

All times are GMT -4. The time now is 15:05.