CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Is it possible high courant number by using cfx?

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

Like Tree1Likes
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 13, 2021, 22:19
Default Is it possible high courant number by using cfx?
  #1
New Member
 
Jin Seok Lee
Join Date: Aug 2021
Posts: 10
Rep Power: 2
jins9158 is on a distinguished road
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
jins9158 is offline   Reply With Quote

Old   September 14, 2021, 10:23
Default
  #2
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,064
Rep Power: 20
evcelica is on a distinguished road
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.
evcelica is offline   Reply With Quote

Old   September 14, 2021, 20:13
Default
  #3
New Member
 
Jin Seok Lee
Join Date: Aug 2021
Posts: 10
Rep Power: 2
jins9158 is on a distinguished road
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
jins9158 is offline   Reply With Quote

Old   September 15, 2021, 02:42
Default
  #4
Senior Member
 
Martin_Sz's Avatar
 
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 214
Rep Power: 10
Martin_Sz is on a distinguished road
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/
Martin_Sz is offline   Reply With Quote

Old   September 15, 2021, 04:00
Default Thank you for replying my question
  #5
New Member
 
Jin Seok Lee
Join Date: Aug 2021
Posts: 10
Rep Power: 2
jins9158 is on a distinguished road
Quote:
Originally Posted by Martin_Sz View Post
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.
jins9158 is offline   Reply With Quote

Old   September 15, 2021, 07:41
Default
  #6
Senior Member
 
Join Date: Jun 2009
Posts: 1,454
Rep Power: 27
Opaque will become famous soon enough
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.
Opaque is offline   Reply With Quote

Old   September 15, 2021, 20:50
Default Thank you for your concern
  #7
New Member
 
Jin Seok Lee
Join Date: Aug 2021
Posts: 10
Rep Power: 2
jins9158 is on a distinguished road
Quote:
Originally Posted by Opaque View Post
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?


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
jins9158 is offline   Reply With Quote

Old   September 15, 2021, 22:03
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,837
Rep Power: 132
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   September 16, 2021, 00:33
Default Thank you for replying my question
  #9
New Member
 
Jin Seok Lee
Join Date: Aug 2021
Posts: 10
Rep Power: 2
jins9158 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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.

I understand your talk

It is good for me

Thank you
jins9158 is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[General] Extracting ParaView Data into Python Arrays Jeffzda ParaView 19 June 11, 2020 15:54
Foam::error::PrintStack almir OpenFOAM Running, Solving & CFD 90 October 3, 2019 07:01
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


All times are GMT -4. The time now is 21:49.