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

Doubt regarding Multiphase simulation

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 14, 2019, 06:34
Default Doubt regarding Multiphase simulation
  #1
Senior Member
 
Join Date: Mar 2013
Location: Germany
Posts: 324
Rep Power: 9
AS_Aero is on a distinguished road
Hi All

It might be a very basic question, but am not sure about this hence I want your suggestions.

Some people say for Multiphase simulation we need to have a CFL number less than 0.5 always. Is it true for all cases or is it something specific for some case ?
AS_Aero is offline   Reply With Quote

Old   January 14, 2019, 17:49
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,487
Rep Power: 118
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
No, not true at all. It is a very common misconception than CFL (or Courant number for incompressible flows) is a fundamental parameter for implicit CFD codes like CFX.

For a start, CFL requires a compressible fluid. CFL is undefined for incompressible fluids. So you cannot use CFL as a criteria for incompressible multiphase models (which is the most common type of multiphase model).

With compressible multiphase models, some multiphase models have simple multiphase characteristics and can handle much bigger timesteps than results from CFL=0.5. Some are very challenging and will require smaller time steps than CFL=0.5.

You determine the time step size for your simulation in CFX by a time step sensitivity study.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   January 15, 2019, 05:03
Default
  #3
Senior Member
 
Join Date: Mar 2013
Location: Germany
Posts: 324
Rep Power: 9
AS_Aero is on a distinguished road
So is it only for CFX or in general ? What about multiphase simulation of air bubbles in water channel using OpenFOAM ? There is it important to have CFL less than 0.5 since air bubbles are compressible ? (Sorry maybe I should ask this in OpenFOAM forum), but I thought you might be able to answer this as the physics is same.
AS_Aero is offline   Reply With Quote

Old   January 15, 2019, 08:11
Default
  #4
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Posts: 707
Rep Power: 11
Gert-Jan is on a distinguished road
There is Compressible and Compressible.

If you use compressible gas (ideal gas) to incorporate density differences as a result of hydrostatic pressure or varying temperature or composition, then consider this as Compressible version1. You can run this using Thermal energy in CFX. Your bubble size may change a little, depending on the static pressure and temperature, composition, etc. No need to limit yourself to CFL=0.5 in CFX.

If you have high velocities and significant gas volume fractions, then things become very complicated since the speed of sound of the mixture drops dramatically. This can result in choking flows with Mach around 1 and beyond. Then you also need to calculate compressible, but with Total Energy (in CFX). I call this Compressible version2. Required time steps will be low, CFL around 0.5.

I think this applies for both CFX and OpenFOAM when using a nice hex mesh. When applying an unstructered mesh, CFX tends to work fine, OpenFOAM is less foregiven and requires smaller steps. Then better use a poly mesh. However, this is based on my OpenFOAM experience some time ago. Possibly things have changed a lot. Better ask the OpenFOAM Forum.

Last edited by Gert-Jan; January 15, 2019 at 10:08.
Gert-Jan is offline   Reply With Quote

Old   January 15, 2019, 17:37
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,487
Rep Power: 118
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
CFX is an implicit solver. In fact most CFD codes are implicit solvers. There is no formal time step restriction on implicit solvers, you set the time step size based on discretisation accuracy and numerical stability considerations. So the way to set the time step size is by a time step size sensitivity study.

Explicit solvers have a hard limit of Courant number = 1 or CFL = 1, and usually they need a safety factor which brings it down to 0.5 to 0.75. This is from the numerical approach used and if you use CFL>1 it will immediately start to diverge. There are not many explicit solvers around, they tend to be mainly used for explosion and impact modelling (very fast transient events).

But a lot of people get the formal limit of explicit solvers confused and think it applies to implicit solvers as well.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks 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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Problem with 2-Way FSI Multiphase Simulation Juli Fluent Multiphase 4 March 21, 2017 09:27
2-Way FSI MultiPhase Simulation Juli ANSYS 0 March 17, 2017 05:52
Multiphase heat exchange simulation efer2109 STAR-CCM+ 1 September 15, 2016 14:22
Simulation multiphase airlift reactor with Eulerian multiphase model question???? dilok.kumyoo FLUENT 0 January 28, 2015 03:15
multiphase simulation... 2D flow through an elbow Tim CFX 10 April 3, 2008 19:13


All times are GMT -4. The time now is 09:35.