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

Modelling condensing flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 30, 2006, 08:20
Default Modelling condensing flow
  #1
Ryan Sidin
Guest
 
Posts: n/a
I was wondering if CFX allows you to solve a user-defined advection-reaction type of equation for the liquid dispersion in condensing/evaporating flows. Does anyone know about this?

  Reply With Quote

Old   November 30, 2006, 10:55
Default Re: Modelling condensing flow
  #2
opaque
Guest
 
Posts: n/a
Dear Ryan,

Would you mind elaborating on the equation?

For example, you can create an ADDITIONAL VARIABLE (also known as a passive scalar). Then, you can select the type of physics transport you require: transient, advection and diffusion. They are listed as:

1 - Transport Equation = Transient + Advection + Diffusion + Sources

2 - Diffusive Transport = Transient + Diffusion + Sources

3 - Poission Equation = Diffusion + Sources.

Will this help?

Opaque
  Reply With Quote

Old   November 30, 2006, 12:38
Default Re: Modelling condensing flow
  #3
Ryan Sidin
Guest
 
Posts: n/a
Dear Opaque,

The variables I am trying to solve by means of the added equations are regrettably not passive scalars. Amongst others, they include the liquid mass fraction which links the liquid dispersion to the liquid/vapor mixture via the equation of state. Therefore you need to solve the extra transport equations (transient + advection + sources) for the extra variables simultaneously with the fluid dynamics equations for the mixture. In condensing flow theory, these extra equations are the so-called moment equations for the droplet size distribution. Viscous effects are neglected so that the fluid dynamics equations for the mixture reduce to the Euler equations for compressible flow.

So given the above: do you perhaps know if it is possible to plug such a model into CFX?

Best regards,

Ryan.
  Reply With Quote

Old   November 30, 2006, 12:51
Default Re: Modelling condensing flow
  #4
opaque
Guest
 
Posts: n/a
Dear Ryan,

In the upcoming ANSYS CFX 11.0, there is the Droplet condensation model. The documentations states that:

"The system of equations involves one continuous phase and any number of dispersed (condensed) phases. The condensed phases travel at the speed of the continuous phase.Any combination of condensed phases can exist in the solution so that for the continuous phase, mass conservation becomes:

..... Equation 251.

where the mass sources are summed over the condensed phases. The condensed phases can change size by condensation or evaporation. For a condensed phase, mass conservation is:

..... Equation 252.

where each dispersed phase has a corresponding number equation of the form:

..... Equation 253.

and is the nucleation model with units defined as the number of droplets generated per unit time per unit volume of vapor and is the nucleated droplet mass based on the critical radius . Note that the droplets are transported with the mixture velocity since no slip is assumed between the phases. The usual constraint applies for the volume fractions where:

... "

Is that what you are looking for? 11.0 does not have a DQMOM model?

Opaque

  Reply With Quote

Old   November 30, 2006, 17:24
Default Re: Modelling condensing flow
  #5
Ryan
Guest
 
Posts: n/a
Dear Opaque,

that indeed looks quite promising. If CFX 11.0 uses a moment method (either with QMOM, DQMOM, or some other type of closure) then this would be very useful to me. I am currently working as a PhD-student on a novel method to determine the droplet size distribution using the flow field solution obtained with a moment method. I have written my own fortran-code to solve the fluid dynamics equations simultaneously with either the population balance equation or the moment equations. This of course for a 1-dimensional flow in a Laval nozzle. CFX would provide a step up to 3D, more relevant test cases.

Could you perhaps show me the equations for the condensation model that will be implemented? I would very much like to see them. Do you also know if you can iplug in your own closure model?

Also, thanks for your swift and clear replies which I have been receiving thus far.

Best regards,

Ryan.

  Reply With Quote

Old   November 30, 2006, 17:53
Default Re: Modelling condensing flow
  #6
opaque
Guest
 
Posts: n/a
Dear Ryan,

Please contact your ANSYS CFX support representative, and request a copy of the solver theory documentation for the up coming 11.0 release. In particular the multiphase flow section about the Droplet Condensation Model.

You are most welcome,

Regards, Opaque

  Reply With Quote

Old   December 8, 2006, 17:48
Default Re: Modelling condensing flow
  #7
HekLer
Guest
 
Posts: n/a
It is possible to implement DQMOM in CFX using user fortran to calculate nucleation sources and the AV equations to track the moments.

There was a presentation given at the oil & gas conference in Brazil recently by someone from ESSS.

  Reply With Quote

Old   December 12, 2006, 06:43
Default Re: Modelling condensing flow
  #8
Ryan
Guest
 
Posts: n/a
This is quite an interesting remark. I can obtain the size distribution function by postprocessing the solution obtained with the moment method. What is not clear to me is that whether or not the MOM-method you plug in can be solved simultaneously with the fluid dynamics equations, and not in a post-processing stage. By the way, in the solver theory of CFX-11 (preview version), it is mentioned that the condensation model simply uses an equivalent monodisperse distribution (i.e. a mean radius) to determine the growth contribution in the method of moments.
  Reply With Quote

Old   December 14, 2006, 01:02
Default Re: Modelling condensing flow
  #9
HekLeR
Guest
 
Posts: n/a
The DQMOM moment equations can be solved simultaneously with the other equations and used as input into the particle diameter calculation (eg: mean diameter calc).

You are right. The droplet model in CFX 11 is monodisperse. Polydisperse DQMOM is coming for CFX 12.

  Reply With Quote

Reply

Thread Tools
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
Flow meter Design CD adapco Group Marketing CD-adapco 3 June 21, 2011 08:33
VOF modelling open channel river flow Matthew Roberts FLUENT 6 July 31, 2009 12:52
modelling blood flow in arteries with starcd sara CD-adapco 5 April 10, 2007 09:17
Modelling flow around a ship's hull using vof Manoj Kumar FLUENT 0 February 26, 2005 17:22
Basic Multiphase Flow Modelling krishna Main CFD Forum 2 August 27, 2004 08:40


All times are GMT -4. The time now is 00:34.