# Is it possible high courant number by using cfx?

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

 September 13, 2021, 22:19 Is it possible high courant number by using cfx? #1 New Member   Jin Seok Lee Join Date: Aug 2021 Posts: 10 Rep Power: 2 I am going to simulate flow analysis about humidity diffusion this analysis purpose is indoor comport analysis with reference to humidity. Fluid domain is apartment I made mixture gas which is composed of N2, O2, CO2, H2O, Ar (Ideal Gas) Fluid model is Thermal energy Inlet: 200CMH Outlet1: -200CMH Outlet2: -60CMH Opening: 0pa * Inlet, Outlet1 is Ventilation system * Outlet2 is Bathroom ventilator * Opening is window applying porous model Anlaysis type: Transient Total time: 3600[s] Time step: 0.2[s] Mesh node number: 600,000 node When I simulated this analysis, I knew CFL(Courant) number is high (CFL RMS number: 920 I searched variety of materials and I saw high CFL Number is not bad if I use implicit solver. Is it correct? I am not sure. Also I had a problem because simulation time will be very long if I reduce timestep to reduce CFL number So I want to fix time step(0.2s) if simulation analysis is not bad. Please give me some advice thank you

 September 14, 2021, 10:23 #2 Senior Member   Erik Join Date: Feb 2011 Location: Earth (Land portion) Posts: 1,061 Rep Power: 20 I would have just had two components in my fluid mixture: Dry Air, and Water Vapor. Forget mixing N2, O2, and Ar, They are already mixed homogeneously and act as a single fluid. I would use adaptive time stepping, and let the solver find an appropriate timestep. You can finesse this a bit after you see how it performs. -Erik If this proves to take too long, you could consider modeling the water vapor as a passive scalar, and freezing the fluids equations using expert parameters. You will of course have to start with converged steady state conditions first, then start the transient simulation with frozen fluid solver. (Set Expert Parameters solve fluids and solve turbulence to "f") Of course this is making simplifications, but if the buoyancy does not have much effect, and you don't have large transient vortices, the result could be close to the full transient analysis in a fraction of the computing time.

 September 14, 2021, 20:13 #3 New Member   Jin Seok Lee Join Date: Aug 2021 Posts: 10 Rep Power: 2 Thank you for replying my question your opinion is good for me However, I need to simulate 0s ~ 3600s time because time variation is to be important. So, I couldn't simulate steady state. I am going to simulate transient analysis and courant number(CFL) is high about 920 I used implicit solver. Could you give me advice about high courant number by using implicit solver? I just want to review to spread H2O gas. It is not important about "quantitative value" So I expect courant number is not important in case of my analysis

 September 15, 2021, 02:42 #4 Senior Member     Marcin Join Date: May 2014 Location: Poland, Swiebodzin Posts: 212 Rep Power: 10 If u Can manulaly change Courant Number in Simulation (like in FLuent ) U can do sensivity analysis to see a dependence of courant value on residuals __________________ Quick Tips and Tricks, Tutorials FLuent/ CFX (CFD) https://howtooansys.blogspot.com/

September 15, 2021, 04:00
Thank you for replying my question
#5
New Member

Jin Seok Lee
Join Date: Aug 2021
Posts: 10
Rep Power: 2
Quote:
 Originally Posted by Martin_Sz If u Can manulaly change Courant Number in Simulation (like in FLuent ) U can do sensivity analysis to see a dependence of courant value on residuals
Thank you for replying my question

Now, I have used 'CFX'

I think the convergence is good because

First. RMS residual U,V,W, P, H-energy, Mass fraction's value is lower 10^-4

Second. Monitoring points are constant

Third. Imbalance is close 0 value

So, I think I didn't need to test about courant number if courant number high is not matter.

 September 15, 2021, 07:41 #6 Senior Member   Join Date: Jun 2009 Posts: 1,441 Rep Power: 27 You seem to be fixated on the Courant Number, while your goal should be in obtaining an accurate and efficient simulation. If the initial results with an arbitrary time step (effectively arbitrary Courant Number if the mesh is fixed), go ahead and reduce/increase the timestep and see if your results improve or remain the same. Once you obtain a set of results that satisfy your needs, you have completed your goals. An implicit solver gives you the benefit of using a larger Courant number than an explicit solver; however, once your simulation is robust (converges) only accuracy matters, correct? I am not certain you will use the Courant number as part of your final comfort design, will you? __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

September 15, 2021, 20:50
#7
New Member

Jin Seok Lee
Join Date: Aug 2021
Posts: 10
Rep Power: 2
Quote:
 Originally Posted by Opaque You seem to be fixated on the Courant Number, while your goal should be in obtaining an accurate and efficient simulation. If the initial results with an arbitrary time step (effectively arbitrary Courant Number if the mesh is fixed), go ahead and reduce/increase the timestep and see if your results improve or remain the same. Once you obtain a set of results that satisfy your needs, you have completed your goals. An implicit solver gives you the benefit of using a larger Courant number than an explicit solver; however, once your simulation is robust (converges) only accuracy matters, correct? I am not certain you will use the Courant number as part of your final comfort design, will you?

But, I couldn't understand your talk

1. your opinion: however, once your simulation is robust (converges) only accuracy matters, correct?

>>> you means that the courant number is not important to verify simulation convergence?

2. your opinion: I am not certain you will use the Courant number as part of your final comfort design, will you?[/QUOTE]

>>> I don't understand

 September 15, 2021, 22:03 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 16,820 Rep Power: 132 Opaque is saying that you should not be so focussed on Courant number. The important thing is that you have a timestep which accurately resolves the transients in your simulation. As CFX is an implicit solver, it does not have a strict Courant number stability limit (like explicit solvers do). Courant number is just a way of determining the time step size, and in CFX a better approach is to find a time step size which is accurate in your case. The accurate time step size varies on many issues, including mesh quality, what multiphase effects are occurring and many others - and none of these issues are addressed by Courant Number. So Courant Number is not a very useful way of defining time step size in CFX, you might as well define the time step size directly. Opaque likes this. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

September 16, 2021, 00:33
Thank you for replying my question
#9
New Member

Jin Seok Lee
Join Date: Aug 2021
Posts: 10
Rep Power: 2
Quote:
 Originally Posted by ghorrocks Opaque is saying that you should not be so focussed on Courant number. The important thing is that you have a timestep which accurately resolves the transients in your simulation. As CFX is an implicit solver, it does not have a strict Courant number stability limit (like explicit solvers do). Courant number is just a way of determining the time step size, and in CFX a better approach is to find a time step size which is accurate in your case. The accurate time step size varies on many issues, including mesh quality, what multiphase effects are occurring and many others - and none of these issues are addressed by Courant Number. So Courant Number is not a very useful way of defining time step size in CFX, you might as well define the time step size directly.
Thank you very much.

It is good for me

Thank you