# Solver Equations

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

 August 8, 2003, 11:54 Solver Equations #1 Carola Guest   Posts: n/a Hi Guys!, I would like to Know how CFX-5.5.1 solve their hydrodynamics equations. I've been reading something about "Cuopled Solver" but I donīt get it!!. Take Care, Carola

 August 10, 2003, 18:42 Re: Solver Equations #3 Glenn Horrocks Guest   Posts: n/a Hi Robin, Thanks for the excellent summary of the nuts and bolts. Can I ask a few additional questions? 1) Are multiple domains solved simultaneously, or is each domain solved individually with inter-domain links which get updated each iteration? 2) The U,V,W,P equations are coupled together. When the simulation includes temperature, turbulence, additional variables etc, are those equations solved together with the UVWP equations, or are they solved seperately (ie additional variables are uncoupled)? Regards, Glenn

 August 11, 2003, 10:38 Re: Solver Equations #4 Robin Guest   Posts: n/a Hi Glenn, 1) Multiple domains are solved simultanously. General Grid Interfaces (GGI) are fully coupled and active. At a GGI, conservative fluxes are mapped across overlapping sub-faces, as opposed to simply interpolating nodal values. A GGI interface is therefore fully conservative (conservation is not an option, or afterthought). 2) The mass and momentum equations are strongly coupled, therefor U-mom, V-mom, W-mom, and P-Mass are always solved fully coupled. The energy equation (T for Thermal Energy or H for Total Energy) is not as strongly coupled and is therefore solved segregated from the others. Turbulence is dominated by source terms, and also would not benefit from coupling, and additional variables are also solved segregated. In theory, you could couple everything, but performance gains are only to be had where the inter-equation coupling is stong, such as it is with U, V, W, P and reactions. Regards, Robin

 August 11, 2003, 14:06 Re: Solver Equations #5 Carola Guest   Posts: n/a Hi Robin, Thank you so much!!!!!!. I donīt want to be annoying but I have another question to you: Could you please explain me how cfx-5.5.1 solve the equations of "Eddy dissipation Model" (combustion)?. Iīve been searching about combustion models but I just found two or three basic equations which are not enough to my boss. Besides, I'm designing a combustion chamber so I want to know what is the best combustion model in CFX-5.5.1 (advantages, disadvantages). Thanks in advance! Carola

 August 11, 2003, 16:58 Re: Solver Equations #6 Robin Guest   Posts: n/a Hi Carola, Unfortunately I am not very knowledgable in this area. Although I am sure there are other on the forum who are, a detailed discussion of the EDM model is probably more than most are prepared to commit to on a forum. If you interested in the details of it's implementation in CFX-5 and the existing documentation is insufficient, I suggest contacting Technical Support. As for the model itself, best to look it up in the literature. Regards, Robin

 August 11, 2003, 17:38 One more question to Robin #7 Paul Guest   Posts: n/a Hi, Robin I am still not 100 percent sure what is going on in multiple domains. if they are solved simultanously, how the inlet conditions pass through these domains and how flow variables are passed on the domain interfaces? is it possible that the the current domain is solved one iteration or time step lagged behind the previous domain?

 August 11, 2003, 22:29 Re: One more question to Robin #8 Robin Guest   Posts: n/a Hi Paul, I see what you are getting at. You have a set of linear equations, so how can you solve them all at once? When we say "solved simultaneously" we mean that there is one set of linearized equations solved simultaneously at 1 timestep. Since the coefficients are non-linear, the equations must be updated after each timestep. Consider the flux of U momentum through a face. The flux is equal to the mass flow times the U velocity component. Since mass flow is equal to the U velocity times density you get: flux = U * rho * U You can only solve for one of those U's at a time, so the existing solution is used to get the mass flow (mass flow would be the coefficient in this case) and we solve for U. Now that you have the new value of U, you can update the mass flow and solve again. This update is done from one timestep to the next. At an interface, the coefficients are calculated based on the existing solution on either side of the interface, rather than interpolating values onto nodes and assebling the equations from those. Does this clarify it a bit? If not, I suggest taking a course on CFD or reading a decent textbook before I end up typing one up on CFD-Online Best regards, Robin

 August 11, 2003, 22:37 Re: One more question to Robin #9 Paul Guest   Posts: n/a I got it. Thanks. Robin

 August 12, 2003, 08:27 Help me Robin #10 Carola Guest   Posts: n/a One more time Robin!, I got a couple of questions to you: 1)What do you mean when you say:"... An error correction is solved on each of the coarser grids and passed back up to the finer grids to improve the solution..", I understood like with every iteration the error is reduced until it reach the tolerance value..., Iīm wrong?.Where this error correction come from?. 2)What is the diference between time step and iteration?. Sorry if I made a lot of stupid questions but I finally found someone who can explain to me this kind of things in a very simple way ! Take Care, Carola

 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 Peter_600 OpenFOAM 4 August 2, 2014 09:52 makaveli_lcf OpenFOAM Running, Solving & CFD 3 September 11, 2013 12:44 ozzythewise OpenFOAM Running, Solving & CFD 3 February 8, 2011 16:28 suitup OpenFOAM Running, Solving & CFD 0 January 20, 2010 08:45 ztdep Main CFD Forum 2 March 21, 2006 02:58

All times are GMT -4. The time now is 00:26.