|
[Sponsors] |
Is it possible high courant number by using cfx? |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
September 13, 2021, 22:19 |
Is it possible high courant number by using cfx?
|
#1 |
Member
Jin Seok Lee
Join Date: Aug 2021
Posts: 52
Rep Power: 4 |
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: 1,167
Rep Power: 23 |
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 |
Member
Jin Seok Lee
Join Date: Aug 2021
Posts: 52
Rep Power: 4 |
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: 232
Rep Power: 12 |
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 | |
Member
Jin Seok Lee
Join Date: Aug 2021
Posts: 52
Rep Power: 4 |
Quote:
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: 1,804
Rep Power: 32 |
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 |
Thank you for your concern
|
#7 | |
Member
Jin Seok Lee
Join Date: Aug 2021
Posts: 52
Rep Power: 4 |
Quote:
Thank you for your concern 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: 17,703
Rep Power: 143 |
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.
__________________
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 | |
Member
Jin Seok Lee
Join Date: Aug 2021
Posts: 52
Rep Power: 4 |
Quote:
I understand your talk It is good for me Thank you |
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[General] Extracting ParaView Data into Python Arrays | Jeffzda | ParaView | 30 | November 6, 2023 21:00 |
Foam::error::PrintStack | almir | OpenFOAM Running, Solving & CFD | 91 | December 21, 2022 04:50 |
SimpleFoam & Theater | jipai | OpenFOAM Running, Solving & CFD | 3 | June 18, 2019 10:11 |
[mesh manipulation] Importing Multiple Meshes | thomasnwalshiii | OpenFOAM Meshing & Mesh Conversion | 18 | December 19, 2015 18:57 |
same geometry,structured and unstructured mesh,different behaviour. | sharonyue | OpenFOAM Running, Solving & CFD | 13 | January 2, 2013 22:40 |