CFL Number in CFX RANS

AS_Aero · March 28, 2017, 10:59

Hi

I have a doubt regarding the CFL number in CFX. When you do a RANS computation in CFX and you are not able to give precisely a delta T or time step and which means I have given auto time scale factor of 1 and I am getting a CFL number maximum of 2000 also my simulation gets converged though. So should I really bother for RANS computation my CFL number which is really high though. If YES !! How can I change my deltaT in CFX for RANS ?
Thanks in advance !!

ghorrocks · March 28, 2017, 19:32

Quote:

When you do a RANS computation in CFX and you are not able to give precisely a delta T or time step

? This is wrong. Yes, you can specify the time step in CFX. In steady state simulations it is a pseudo-timestep.

If you are doing a steady state simulation then the CFL number based on the pseudo-time step is not important. In a steady state simulation all the transient features should converge to zero. CFX is an implicit solver anyway and is therefore not limited to a fixed CFL number.

AS_Aero · March 29, 2017, 01:48

Thanks for the explanation !! I was doing a Steady State RANs and then when I calculate the CFL Number in cFX in Post Process
the maximum val of CFL number is around 1000. So I was kind of puzzled. Doesnt it affect my results

ghorrocks · March 29, 2017, 05:21

CFL can be ignored for steady state simulations. It is only of relevance to transient simulations, and even then it is only of marginal use IMHO.

LUO DAN · April 1, 2019, 22:41

I have a question about CFL. Recently I am simulating a co2 two phase flow in a nozzle, it can run only with a very small timestep (choose auto timescale——timescale factor is 10^-6, the case can not run with a bigger timestep) , so it is hard to converge even it runs 60,000 steps.
I read a paper about co2 two phase flow named"AN INVESTIGATION OF REAL GAS EFFECTS IN SUPERCRITICAL CO2 CENTRIFUGAL COMPRESSORS", in which "The CFL number in the steady calculation was decreased below 1 when approaching the critical point, while the acoustic CFL number was kept close to unity" was mentioned. I checked the max-CFL in my CFX-post is 0.0001838, it is so small. When I simulated the steady case, I can not find the option to change the CFL in CFX-pre. I am so confused why my case is so hard to converge.
thank you

ghorrocks · April 1, 2019, 23:48

CFX does use a pseudo-time step for steady state simulations, but has no options for setting it by the CFL number. That is because in my experience it is of little use. The best way to set a steady state simulation time step is to start with a reasonable guess (auto time scale is OK for this) and then manually adjust it up or down using "Edit run in progress" depending on how the convergence is progressing.

CFX has options to use CFL based time stepping for transient simulations, but I do not recommend it for most applications. adaptive time stepping homing in on 3-5 coeff loops per iteration is much preferred, or a fixed time step set by a sensitivity analysis.

If you need to run with a tiny CFL it suggests that your simulation is very numerically unstable. You say this is a two phase CO2 model, so you are running some complex physics - numerical problems are to be expected here. But the simulation can be improved by improving mesh quality and using double precision numerics.

LUO DAN · April 2, 2019, 03:04

yes, I have used double precision in my case, and I tried different timesteps, only 10^-6 or even smaller timestep can make it. Thank you very much for explaining me about the CFL, I learned that.

March 28, 2017, 10:59	CFL Number in CFX RANS	#1
AS_Aero Senior Member Join Date: Mar 2013 Location: Germany Posts: 357 Rep Power: 14	Hi I have a doubt regarding the CFL number in CFX. When you do a RANS computation in CFX and you are not able to give precisely a delta T or time step and which means I have given auto time scale factor of 1 and I am getting a CFL number maximum of 2000 also my simulation gets converged though. So should I really bother for RANS computation my CFL number which is really high though. If YES !! How can I change my deltaT in CFX for RANS ? Thanks in advance !!

April 1, 2019, 23:48		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,816 Rep Power: 144	CFX does use a pseudo-time step for steady state simulations, but has no options for setting it by the CFL number. That is because in my experience it is of little use. The best way to set a steady state simulation time step is to start with a reasonable guess (auto time scale is OK for this) and then manually adjust it up or down using "Edit run in progress" depending on how the convergence is progressing. CFX has options to use CFL based time stepping for transient simulations, but I do not recommend it for most applications. adaptive time stepping homing in on 3-5 coeff loops per iteration is much preferred, or a fixed time step set by a sensitivity analysis. If you need to run with a tiny CFL it suggests that your simulation is very numerically unstable. You say this is a two phase CO2 model, so you are running some complex physics - numerical problems are to be expected here. But the simulation can be improved by improving mesh quality and using double precision numerics. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
decomposePar -allRegions	stru	OpenFOAM Pre-Processing	2	August 25, 2015 03:58
DecomposePar unequal number of shared faces	maka	OpenFOAM Pre-Processing	6	August 12, 2010 09:01
[blockMesh] BlockMeshmergePatchPairs	hjasak	OpenFOAM Meshing & Mesh Conversion	11	August 15, 2008 07:36
Unaligned accesses on IA64	andre	OpenFOAM	5	June 23, 2008 10:37
ICEM and CFX report different number of elements	Chris Basciano	CFX	0	July 20, 2007 17:24

March 29, 2017, 01:48		#3
AS_Aero Senior Member Join Date: Mar 2013 Location: Germany Posts: 357 Rep Power: 14	Thanks for the explanation !! I was doing a Steady State RANs and then when I calculate the CFL Number in cFX in Post Process the maximum val of CFL number is around 1000. So I was kind of puzzled. Doesnt it affect my results

March 29, 2017, 05:21		#4
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,816 Rep Power: 144	CFL can be ignored for steady state simulations. It is only of relevance to transient simulations, and even then it is only of marginal use IMHO.

April 1, 2019, 22:41		#5
LUO DAN New Member luo dan Join Date: Sep 2018 Posts: 27 Rep Power: 7	I have a question about CFL. Recently I am simulating a co2 two phase flow in a nozzle, it can run only with a very small timestep (choose auto timescale——timescale factor is 10^-6, the case can not run with a bigger timestep) , so it is hard to converge even it runs 60,000 steps. I read a paper about co2 two phase flow named"AN INVESTIGATION OF REAL GAS EFFECTS IN SUPERCRITICAL CO2 CENTRIFUGAL COMPRESSORS", in which "The CFL number in the steady calculation was decreased below 1 when approaching the critical point, while the acoustic CFL number was kept close to unity" was mentioned. I checked the max-CFL in my CFX-post is 0.0001838, it is so small. When I simulated the steady case, I can not find the option to change the CFL in CFX-pre. I am so confused why my case is so hard to converge. thank you

April 2, 2019, 03:04		#7
LUO DAN New Member luo dan Join Date: Sep 2018 Posts: 27 Rep Power: 7	yes, I have used double precision in my case, and I tried different timesteps, only 10^-6 or even smaller timestep can make it. Thank you very much for explaining me about the CFL, I learned that.