# Two fundamental questions about icoFoam while updating the velocities and pressure

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

 LinkBack Thread Tools Display Modes
 May 27, 2007, 01:02 (1) In typical CFD literature, #1 Member   roy fokker Join Date: Mar 2009 Posts: 44 Rep Power: 8 (1) In typical CFD literature, after the pressure correction equation is solved, the velocity is updated by adding the initial tentative velocity U* solved from the UEqn == -fvc::grad(p*), here p* is the initial pressure and the velocity correction U' from the pressure correction -rUA*fvc::grad(p'),i.e. U=U*+U'---------(a) However from icoFoam code, it seems that the velocity is updated using: U = rUA*UEqn.H()-rUA*fvc::grad(p')----------(b) the difference between (a) and (b) is rUA*grad(p*), which is the gradient of initial pressure gradient, is there any reference for this difference? (2) I didn't find the code for updating the pressure field which, in typical CFD literature, is p=p*+p', it seems that icoFoam is using the pressure correction value as the pressure value: p=p'? I wonder if I have made my question clear, am I misunderstanding some basic concepts? Thanks a lot!

 May 27, 2007, 04:00 This is pretty basic stuff - h #2 Senior Member   Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,758 Rep Power: 21 This is pretty basic stuff - have a look at my Thesis: - we solve for the pressure and not pressure correction - the derivation of the pressure laplacian is given in detail in the Thesis. Enjoy, Hrv __________________ Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk

 May 27, 2007, 04:43 Thanks, actually I already rea #3 Member   roy fokker Join Date: Mar 2009 Posts: 44 Rep Power: 8 Thanks, actually I already read your thesis section 3.8.1, and I know that the pressure laplacian correction is from Eqn 3.141, because I read the wiki page: http://openfoamwiki.net/index.php/IcoFoam it says: ... // take a Jacobi pass and update U. See Hrv Jasak's thesis eqn. 3.137 and Henrik Rusche's thesis, eqn. 2.43 // UEqn.H is the right-hand side of the UEqn minus the product of (the off-diagonal terms and U). // See Eqn. 7.37 of Ferziger and Peric. U = rUA*UEqn.H(); Ferziger's 7.37,7.39 is a pressure correction p' Do you mean that your equation 3.137, 3.141 is the pressure p and not p'? And therefore the PISO loop is different (or slightly different) from the procedure by Ferziger? I know this is quite fundamental, thanks for your reply.

 May 31, 2007, 09:40 Roy, You are right that the #4 Member   David P. Schmidt Join Date: Mar 2009 Posts: 70 Rep Power: 8 Roy, You are right that the icoFoam implementation differs slightly from Feriger and Peric. The reference to Eqn. 7.37 in the Wiki comments is also misleading (mea culpa). So the pressure Equation is Eqn. 7.35 from Ferziger and Peric; e.g. it is for the whole pressure, not just the correction to the estimated pressure field. If this explanation makes sense, and you think you could improve the Wiki text, feel free to correct it. David

 May 31, 2007, 15:58 Thanks, in fact I plan to make #5 Member   roy fokker Join Date: Mar 2009 Posts: 44 Rep Power: 8 Thanks, in fact I plan to make a step by step explanation of the icoFoam with PISO, the wiki page seems too simple an explanation for beginners. So far I still have some problem about one line: adjustPhi(phi, U, p);

 May 31, 2007, 16:41 Consider a case which has zero #6 Senior Member   Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,758 Rep Power: 21 Consider a case which has zero gradient boundary condition on the pressure all the way around, like a pipe wit zero gradient outlet. In such a case, the pressure equation will not guarantee global continuity. At the same time, if the mass flux in is not identical to mass flux out, the pressure equation (= continuity condition) will not have a solution. adjustPhi will look for cases where p has got no fixed boundary condition and adjust total outflow from the domain after the momentum predictor to match the total inflow. Standard practice, slightly unusual packing :-) Enjoy, Hrv mgg and franciscofelis like this. __________________ Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk

 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 Palani Velladurai Main CFD Forum 2 March 16, 2007 11:22 dbxmcf OpenFOAM Running, Solving & CFD 0 February 26, 2007 23:16 dbxmcf OpenFOAM Running, Solving & CFD 0 October 6, 2006 11:32 Jon Main CFD Forum 0 September 24, 2005 20:47 Jim Kim Main CFD Forum 1 March 25, 2005 11:30

All times are GMT -4. The time now is 10:13.

 Contact Us - CFD Online - Top