# Modelling condensing flow

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

 November 30, 2006, 08:20 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?

 November 30, 2006, 10:55 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

 November 30, 2006, 12:38 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.

 November 30, 2006, 12:51 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

 November 30, 2006, 17:24 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.

 November 30, 2006, 17:53 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

 December 8, 2006, 17:48 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.

 December 12, 2006, 06:43 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.

 December 14, 2006, 01:02 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.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post CD adapco Group Marketing CD-adapco 3 June 21, 2011 08:33 Matthew Roberts FLUENT 6 July 31, 2009 12:52 sara CD-adapco 5 April 10, 2007 09:17 Manoj Kumar FLUENT 0 February 26, 2005 17:22 krishna Main CFD Forum 2 August 27, 2004 08:40

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