# Calculation of phi if velocity field is known

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 October 14, 2006, 17:14 Hello, I have a quick quest #1 Member   Ankur Gupta Join Date: Mar 2009 Posts: 38 Rep Power: 16 Hello, I have a quick question on the calculation of 'phi' - I am using a modified channelOodles solver. I have two mesh regions in my domain. I am solving for the flow in first mesh region. I want to solve for the transport of a scalar in my second mesh region, where I would like to have the same phi field as that of mesh 1. Is it okay to just copy the velocity field from region 1 to region 2 (for some reasons I can't copy the phi field directly) and calculate phi2 as follows: phi2 = (fvc::interpolate(U2) & mesh2.Sf()); Please comment on my approach !! Thanks! Regards, Ankur

 October 15, 2006, 01:47 Pretty bad. If you want to se #2 Senior Member   Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,896 Rep Power: 32 Pretty bad. If you want to see how bad it is, check the mass conservation on your second mesh. You have to do much better than this, otherwise you will have boundedness problems in the scalar transport. Hrv __________________ Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk

 October 15, 2006, 02:11 Hello Hrv, Could you please #3 Member   Ankur Gupta Join Date: Mar 2009 Posts: 38 Rep Power: 16 Hello Hrv, Could you please suggest me something (to copy velocity field from mesh 1 to mesh 2) with which I can get accurate answers while solving for scalar transport ?? Thanks! Regards, Ankur

 October 15, 2006, 02:32 Yes I can. In order to get co #4 Senior Member   Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,896 Rep Power: 32 Yes I can. In order to get conservative fluxes you will need to solve the pressure equation again on the new mesh - there is no other way of ensuring mass conservation. On balance, I would say you are (much) better off solving the scalar transport on the same mesh. However, if you have no choice, have a look at my Thesis and you will find the details. There, I was doing adaptive mesh refinement (in FOAM, of course!) and show how to interpolate the components and solve the pressure equation to get mass conservation. Enjoy, Hrv __________________ Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk

 October 15, 2006, 02:59 Hello Hrv, Thanks for the r #5 Member   Ankur Gupta Join Date: Mar 2009 Posts: 38 Rep Power: 16 Hello Hrv, Thanks for the reply. Here, I would like to mention something that I think I should have said before. Mesh 2 in my case is exactly twice of mesh 1 (Mesh 1 is a channel, mesh 2 is also a channel. Length of channel 2 is twice that of channel 1. Consider channel 2 to be of two parts - each part exactly equivalent to channel 1). My streamwise BC is periodic for channel 1, so basically I can just copy the velocity field of channel 1 to the two-parts of channel 2. So, if I am using the converged velocity field of channel 1 to get phi for channel 2, would I still have some mass conservation issues while solving scalar transport for mesh 2 ?? Regards, Ankur

 October 15, 2006, 03:46 You cannot copy the cell centr #6 Senior Member   Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,896 Rep Power: 32 You cannot copy the cell centre velocity and interpolate it because you will have a mass conservation error. If the two meshes match exactly, you could find face correspondence between the two meshes (they basically need to be identical) and map that. In all other cases, you need to solve the pressure equation. In any case, do whatever you think is good, calculate the flux divergence in each cell and compare it with the divergence of fluxes on the first mesh. That will tell you how wel you are doing - if the fluxes are not conservative, you will have trouble with scalar transport. Hrv __________________ Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk

 Thread Tools Search this Thread Search this Thread: Advanced Search 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 Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post qunwuhe@hotmail.com Main CFD Forum 4 October 14, 2007 07:38 williams FLUENT 2 June 1, 2007 12:34 JamesT Phoenics 5 May 31, 2007 04:44 Faiz Ahmed Main CFD Forum 0 March 5, 2006 10:11 gianluca FLUENT 0 November 29, 2004 10:10

All times are GMT -4. The time now is 18:20.

 Contact Us - CFD Online - Privacy Statement - Top