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

Scaled Euler-Lagrange Simulation

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   February 25, 2020, 02:44
Default Scaled Euler-Lagrange Simulation
  #1
New Member
 
Terry Jeffords
Join Date: Feb 2020
Posts: 3
Rep Power: 2
Lionheart is on a distinguished road
Hey simulation comissioners,



I am trying to simulate a particle flow out of a pressure vessel using the Euler-Lagrange method. To optimise the calculation time I am trying to scale the Navier Stokes equations, which should result in a system of dimensionless equations.

To consider the momentum loss of the continuous phase (air) due to the high particle mass load of circa 1 kg particles / 1 kg air, I am using the fully coupled model. This adds an additional source term in the momentum equation of air. In the CFX solver theory guide (see chapter 6.2) is written, that the new source can be expressed by: dS=-F_D dt

Where F_D is the drag force defnined by: F_D=-0.5 c_D rho_f A_f |u_s| u_s
When you multiply this source with the particle number rate (necessary after the theory guide) it has the entity [kg m/s]. But in fact it should be [kg /m s] to fit with the other terms in the NS-equation. So it has to be volume specific. But I got no clue how to solve this problem.



Did anybody before tryed to simulate a particle flow dimensionless?



I am pleased if you could help me.



Best regards Terry Jeffords
Lionheart is offline   Reply With Quote

Old   February 25, 2020, 17:45
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,473
Rep Power: 128
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
Why are you adding this source term? The fully coupled particle model already has it included. Why do you want to include it twice?

With particle loads as high as you describe the Lagrangian particle model does not sound suitable. Wouldn't a Eularian particle model be more appropriate?

Finally, CFX is a dimensional solver, so most people run it normal unit systems like m/s/kg. You can non-dimensionalise it, for simple single phase flows that is simple enough but it starts getting complex when you have complex models like a multiphase model to non-dimensionalise. Why non-dimensionalise your simulation? Were you getting problems when you ran it as a dimensional solver?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 26, 2020, 02:55
Default
  #3
New Member
 
Terry Jeffords
Join Date: Feb 2020
Posts: 3
Rep Power: 2
Lionheart is on a distinguished road
Hello Glenn,



this source term is added to the Navier Stokes equations if you want to capture the momentum loss of the continuous phase due to the high particle mass load. Otherwise it would not be physically correct. And I do not want to add this source term twice I just want to add a coefficient to it to make the whole equation dimensionless.



Well the problem is, that even though the mass fraction is high, the volume fraction is low with circa 1E-4 m particle / m air. So mass fraction is important for the momentum coupling and the volume fraction is important for the decision of Euler-Euler oder Euler-Lagrange. And I am not sure if Euler Euler works with such low volume fractions. What do you think?



Well I am getting no problems when running it dimensional, but some guys in literature down in their rabbid holes said the accuracy raises and computational effort decreases if you numerically solve something dimensionless. But so far the only thing I see is that the human effort raises ^^



Thank you very much so far
Lionheart is offline   Reply With Quote

Old   February 26, 2020, 04:48
Default
  #4
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,226
Rep Power: 20
Gert-Jan will become famous soon enough
With this small amount of volume fraction, I would opt for Lagrangian. However, the choice for Lagrange or Euler also depends on the question that you want to answer when doing CFD. What do you want to get out of it? E.g., if you have a size distribution, and want to know where goes what, then Lagrangian is easier to customize and to get the relevant data out of the simulation.
Gert-Jan is offline   Reply With Quote

Old   February 26, 2020, 06:15
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,473
Rep Power: 128
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
So you are trying to non-dimensionalise the built-in particle to fluid coupling force? Is that correct? Yes, this is going to be challenging. I would do a literature search to see how other researchers have non-dimensionalised multiphase flows. It is not trivial to do this, and there are likely to be several ways you can do it. I am not familiar with them, but I have studied works which non-dimensionalised thermal convection and that was complex enough (let alone trying to convince a dimensional solver to act in a non-dimensional way).

The mass fraction of particle is high but the volume fraction is low - OK. There are other factors in deciding Langrangian or Eularian. Lagrangian gives the precise track of a sample of particles, Eularian has many more models available to it (particle collison, wall lubrication, fluidised bed and many more - Lagrangian models don't have these options). Lagrangian models are only applicable to low particle volume fractions, but Eularian models can handle volume fractions from 0 to much higher.

Quote:
But so far the only thing I see is that the human effort raises
Yes, I was thinking exactly the same thing. Non-dimensionalisation can reduce round off errors and that can improve convergence and give more accurate and faster simulations. But if you are not getting significant round off errors in the first place then the gain will be negligible. A naive implementation of a dimensional solver can easily result in big round off errors, but CFX is a highly developed, well verified and optimised solver. It has many methods used to keep round off errors under control.

In other words, unless you know you are getting round off errors the non-dimensionalisation you propose is unlikely to help in CFX. If you are writing your own code then non-dimensionalisation is one of the easiest ways to keep round off errors down - I suspect that is what the papers you are reading have in mind.
Lionheart 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

Reply

Tags
dimensionless, drag coefficient, euler-lagrange, particle, scaled

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
Control simulation to apply different fields with chtMultiRegionFoam jmdf OpenFOAM Running, Solving & CFD 0 February 29, 2016 08:05
Segmentation fault during gust simulation Oshin SU2 3 February 16, 2016 12:03
Euler Lagrange Convergence Tips snpradeep CFX 2 May 6, 2013 08:15
EULER simulation Alexandre FLUENT 4 November 24, 2005 15:01
3-D Contaminant Dispersal Simulation Apple L S Chan Main CFD Forum 1 December 23, 1998 11:06


All times are GMT -4. The time now is 14:25.