# Solve the Navier stokes equations

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

 March 8, 2016, 05:51 Solve the Navier stokes equations #1 New Member   Rime Join Date: Jun 2015 Posts: 28 Rep Power: 3 Hi! How to solve unsteady N-S equations without using projection method (solve the coupled equation)? Thank you

 March 8, 2016, 07:47 #2 Senior Member   Michael Prinkey Join Date: Mar 2009 Location: Pittsburgh PA Posts: 276 Rep Power: 15 You can use fully coupled methods that linearize the mass and momentum components together and put those entries into a single sparse matrix and solve that repeatedly. Construction of particularly the mass conservation and pressure terms needs to be handled carefully--either staggered mesh or Rhie-Chow. That linearized system may need to be iterated a few times to converge. This leads to a very large sparse badly conditioned linear system and it generally takes a lot more work to solve than the individual fields in segregated methods. This is because the pressure equation for mass conservation is VERY hard to solve while the momentum equations are fairly easy--so the full system ends up stagnating because of the twitchy pressure behavior. It can be very useful for some problems with complicated physics, but for single-phase incompressible flow, this is generally NOT recommended especially for transient flows. You can also try to use Newton-Krylov methods with some underlying preconditioner (say an NS projection method!) to converge to the full-nonlinear system solution at each timestep. This may be recommended for some difficult problems or for very large timesteps, but again, probably not for transient incompressible NS. Projection methods are popular because they are fast and accurate enough, especially if the timestep must be small for accuracy reasons (as in LES/DNS).. And by "projection methods" here, I mean general fractional-step non-iterative methods. Note that all SIMPLE/PISO-type schemes for incompressible flow involve a projection step of sorts that solves for a pressure(-like) variable and uses it to make the mass flux (aka velocity) field conservative. The projection process of rendering the mass flux field conservative iteration-by-iteration or timestep-by-timestep is a central portion of almost every primative-variable incompressible CFD solver that I am aware of.

 March 8, 2016, 09:35 #3 Senior Member   Jonas T. Holdeman, Jr. Join Date: Mar 2009 Location: Knoxville, Tennessee Posts: 108 Rep Power: 10 If you want to try something really different that doesn't involve projection-based mixed methods, look at several FEM codes on the cfd wiki using a "pressureless" method. cfd-online.com/Wiki/Source_code_archive_-_educational

 March 8, 2016, 09:59 #4 Senior Member   Filippo Maria Denaro Join Date: Jul 2010 Posts: 2,518 Rep Power: 31 If you want to have some idea of the general coupled problem that can be then decomposed in fractional steps, I suggest https://www.researchgate.net/profile...3fd6000000.pdf http://faculty.nps.edu/fxgirald/Home...t_JCP_2002.pdf Rime likes this.

 March 11, 2016, 05:29 #5 New Member   Rime Join Date: Jun 2015 Posts: 28 Rep Power: 3 thank you for the interesting answers and documents. I have a question, what's the problem that i can have if I use for spatial discretization "collocation in the same node" (velocity and pressure)?

 March 11, 2016, 07:05 #6 Senior Member   Michael Prinkey Join Date: Mar 2009 Location: Pittsburgh PA Posts: 276 Rep Power: 15 The problem is generally called "pressure-velocity coupling" or "even-odd decoupling." This is a problem where the pressure and velocity fields can decouple on collated grids and exhibit cell-to-cell oscillations. On 2D Cartesian grids, this results in a checkerboard-type oscillations. It occurs because the central differencing approximation of the pressure gradient is approximated as (p[i+1] - p[i-1])/ (2*dx). The p[i] value does not enter the computation and so the odd-values of i and the even values i can (and do) drift apart, often catastrophically. The solution to this is either staggered mesh, whereby the pressure terms across a momentum cell can be computed as (p[east] - p[west])/dx where east and west of the pressures on the faces of the momentum cell. Or, by using Rhie-Chow to interpolate the discrete momentum relation (not including the pressure term) from the two neighboring cells to their shared face and evaluating the face velocity/massflux using that momentum interpolation and the pressure gradient term as (p[1] - p[0])/dn where 0 and 1 are the cells on the positive and negative side of the face and dn is the distance between the centroids of those two cells. Rime likes this.

 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 Alex1418 OpenFOAM Programming & Development 0 December 14, 2014 18:24 Mh.R Main CFD Forum 0 October 18, 2011 06:06 vinayender Main CFD Forum 2 December 1, 2009 01:12 J.J. Main CFD Forum 2 June 29, 2000 09:31 Marco Ellero Main CFD Forum 5 May 5, 1999 21:07

All times are GMT -4. The time now is 01:05.