|
[Sponsors] |
Update of coefficients in linearized momentum equation |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
June 29, 2017, 14:43 |
Update of coefficients in linearized momentum equation
|
#1 |
Senior Member
cyln
Join Date: Jul 2016
Posts: 102
Rep Power: 10 |
Hello,
I have been reading the documentation for CFX, however, I am getting difficulty to understand the following: For a steady-state simulation, - What is the residual level that one converges the solution of the linearized equations before the coefficients are updated? - How many updates are realized to the coefficients before the resultant velocity field is used to drive the solution of the pressure field from the pressure equation? Cheers |
|
June 29, 2017, 18:38 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,819
Rep Power: 144 |
It is very rare to be concerned about the linear solver. Have a look in CFX-Pre in the expert parameters for the linear solver settings. But I repeat that this is not something most users need to adjust.
CFX is a coupled solver. It does not have separate momentum and pressure equations like many other solvers do. Each coefficient loop updates both the momentum and pressure simultaneously. |
|
June 30, 2017, 00:03 |
|
#3 |
Senior Member
cyln
Join Date: Jul 2016
Posts: 102
Rep Power: 10 |
Thanks Glenn, I cannot really see the relevant information there.
I mean I know that, during the solution, the pressure substituted into the momentum equation is indirectly taken in the continuity equation such that the resulting velocity must satisfy the continuity equation. This requires the calculations of pressure and velocity to be coupled. So, the method for coupling the equations in CFX is the SIMPLE scheme of Patankar, as modified by Rhie and Chow. The sequence of the operations in SIMPLE algorithm is given in Patankar's Numerical Heat Transfer and Fluid Flow, as follows: 1. Guess the pressure field p* 2. Solve the momentum equations to obtain u*, v*, w* 3. Solve the p' (pressure correction) equation 4. Calculate p by adding p' and p* 5. Calculate u, v, w from their starred values using the velocity-correction formulas 6. Solve the discretization eqn for other phi's (i.e. turbulence quantities) 7. Treat the corrected pressure p as a new guesses pressure p*, return to step 2 and repeat the whole procedure until a converged solution is obtained. This procedure is applied on discretized linearized governing equations. These equations contain coefficients which are basically non-linear. However, assumed constant in each iteration and updated in the next due to non-linear nature of coefficients. I am really confused about inner and outer loop iterations. How are these coefficients updated? I read in literature that, for transient simulations, (just an example) one inner loop iteration (also called coeff. loop) per outer loop iteration and multiple outer loop iterations per time step are used. What is really happening within these loops? CFX documentation does not sufficiently explain these. Also, to what level of residuals is the pressure equation solved before the resultant revised pressure field is used to repeat the solution of the momentum equations for a revised velocity field? I would be grateful if you could explain these to me. Thanks. |
|
June 30, 2017, 11:29 |
|
#4 |
Senior Member
Join Date: Jun 2009
Posts: 1,852
Rep Power: 33 |
Not sure where you got the information that the current/latest ANSYS CFX uses a SIMPLE algorithm as described by Patankar. It does NOT in any way or form.
It does use a Rhie-Chow approach for colocated variables (pressure, and velocity). It does build a discretized momentum equation, along with a continuity equation where Pressure is the solved variable. The 4 equations are solved in call to its linear solver, and the linear equations are converged to a certain tolerance (not specified by the user), once those linear equations are solved, the coeffcients are updates (outer loop) and the new linear system is solved. Iterate until the user specified converged residual value is achieved. |
|
June 30, 2017, 11:48 |
|
#5 |
Senior Member
cyln
Join Date: Jul 2016
Posts: 102
Rep Power: 10 |
I see this in some published papers. For ex, see ''Predictions of a Turbulent Separated Flow Using Commercial CFD Codes'', by Gianluca Laccarino, 2001. I have seen this in other papers as well.
If the SIMPLE algorithm is NOT used in any way or form, then people are really confused or not sure about the algorithm. Can you please explain the difference between SIMPLE and Rhie-CHow approach? Regards |
|
July 1, 2017, 06:59 |
|
#6 | |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,819
Rep Power: 144 |
CFX3 and CFX4 were SIMPLE based solvers. The paper you quote might have used these older versions of CFX. From about 2002 they developed CFX5 which morphed into the current V18 - and this only had the coupled solver from day one.
There has been no confusion on the CFX forum about this issue. The experienced members of this forum have always corrected people who are confused about this (and it happens quite a bit). Quote:
|
||
July 1, 2017, 11:45 |
|
#7 |
Senior Member
cyln
Join Date: Jul 2016
Posts: 102
Rep Power: 10 |
Ohh now I see it. Thanks for the explanation. It would be awesome if you could recommend a paper/book explaining Rhie-Chow approach. I would like to read in more detail.
Thanks |
|
July 2, 2017, 06:10 |
|
#8 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,819
Rep Power: 144 |
Most modern CFD textbooks will cover this, such as Anderson or Versteeg's textbook.
|
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
solving the momentum equation in UEqn. | callahance | OpenFOAM | 2 | October 18, 2012 09:38 |
error message | cuteapathy | CFX | 14 | March 20, 2012 06:45 |
Constant velocity of the material | Sas | CFX | 15 | July 13, 2010 08:56 |
Viscosity and the Energy Equation | Rich | Main CFD Forum | 0 | December 16, 2009 14:01 |
Momentum equation of Darcy's law | sambatra | OpenFOAM Running, Solving & CFD | 2 | April 17, 2009 03:27 |