
[Sponsors] 
March 29, 2001, 14:34 
convergence for higher grid points

#1 
Guest
Posts: n/a

Hi Everybody,
I am solving 2d laminar incompressible flow through wavy duct. Corner points are given in a file GRID that is read by READCO(GRID) command in Q1 file. At Re=1500 for 10X25 cells, %error falls down to 1.0E1 for all variables(convergence ensured) after 400 sweeps. I have used SELREF=T and RESFAC=1e3. I have set relaxation factor 0.2 for P1, 2e4 for V1, 2e4 for W1. But for grid points increased to 50X50, the %error for V1, W1 and P1 don't fall below 1e+3 after 500 sweeps and for further sweeps the solution diverges. If i change the ralaxation factor for V1 and W1 to 2e6 after 400 sweeps, the %error for P1 comes down to 1e1 within few sweps but for V1 and W1 error became fixed to the value in the order of 1e+3. I understand that as the realaxtion factor for V1 and W1 is very low, so the changes are very slow . But my question is, can i take it as converged solution?? If not, what should i do to achieve convergence?? And also let me know the following related to convergence: (1) How does the relaxation factor depend on number of grid points?? (2) How can be the RESREF value estimated from the sources term printed in the result file?? (3) If the solution don't converge for higher grid points, what are the steps can be taken?? It seems to be pretty simple for the experts. Still I would appreciate insight view from them as it's related with the grid independent solution and hence the accuracy of the results. Thanking you, Sandip 

April 4, 2001, 03:57 
Re: convergence for higher grid points

#2 
Guest
Posts: n/a

In general terms, there are three main tools that are used to determine whether reasonable convergence has been achieved:
(a) source balance (b) residual behaviour (c) spot value behaviour. Good source balance (nett source printout in result file) should give a discrepancy between the positive and negative sums that is a small percentage of either; values of <1% should usually be achieved, and considerably lower figures are not uncommon  but a law of diminishing returns applies, with the cost in CPU time of the extra convergence being rather greater than that required to get to a reasonable level. Of course, not all variables can be expected to balance: the effect of solid obstructions enters the momentum equations through the pressure gradient, which is a builtin source rather than an externally imposed one it does not therefore appear in the source balance. Typically, mass (R1/R2) and energy will balance, as will most other scalars, but care is still needed: if the value of a scalar is given a fixed value anywhere, the source required to preserve that value is NOT included in the source printout. Source imbalance is a clear indication that convergence has not yet been achieved; source balance does not, though, necessarily indicate that convergence has been achieved  residual and spot value behaviour should also be considered. Residuals are the imbalances (or errors) in the equations for each solved variable, summed over the cells within the computational domain. These can either be absolute (SELREF=F) or relative (SELREF=T); in the latter case the imbalances are scaled with respect to a value that is intended to represent the flux of the variable throughout the domain. For maintained users, more detailed information can be foundin the FAQs of the support section of CHAM's website. Interpretation of residuals can be difficult and very subjective. What is certainly true is that residual values should typically go down by at least a factor of 100 from the value after the initial few sweeps (assuming that the calculation is starting from an arbitrary initial state). Eventually, the residuals are likely to level out, with small oscillations about a fairly constant value. This is usually an indication of convergence, but not always: too tight relaxation can sometimes suggest this sort of behaviour because variables are not able to change by much on each sweep, while too loose relaxation can prevent residuals falling further because the variable values are oscillating. Spot value behaviour is therefore useful in determining whether or not the levelled residuals can be trusted! If the spot values in a representative region of the flow have settled down to a moreorless constant value, it is reasonable to assume (if the residual behaviour looks promising)that convergence has been achieved; if the changes are still significant, convergence has not been achieved. Some care is still needed though: apparent settling down of spot values might be caused by tootight relaxation, resulting in a very slow drift that can be mistaken for real convergence. Most CFD practitioners rely on their judgement, based on the above guidelines and their own experience. For convergence, the absolute residuals should ideally be less than 1% of a reference flux for each variable. For convectiondominated flow, the falsetimestep relaxation can be estimated from L/(U*N), where U is the inlet velocity, N is the number of cells in the N direction, and L is the domain length in the N direction. This arranges that the falsetransient terms is comparable in magnitude to the convection terms. Mesh refinement can lead to convergence problems, and as noted in the previous paragraph, heavier relaxation is sometimes needed. Refining the mesh can also lead to illconditioned meshes in BFC problems, i.e. the mesh becomes too skewed for the solver. 

April 5, 2001, 01:07 
Re: convergence for higher grid points

#3 
Guest
Posts: n/a

(1). Convergence problem is the key issue in the iterative numerical solution procedure. (2). The procedure starts with an intial guess, and through the iteration, you hope that it will be changed into the final converged solution. (3). If you spend more time in solving algebraic or ordinary differential equation using various iterative methods, you will be able to get a better feeling about how an iterative method actually work. (4). A good example is: the zigsaw puzzle. Near the end, when there are only a few pieces left, you can easily complete the picture. This is not the case at the begining when you have many pieces with no one in place. So, the degree of difficulty is normally printed on the outside of the box in terms of the total number of pieces. (5). In mathematical terms, this is related to the degree of freedom. (6). In the finite volume approach, when the number of cells for a particular problem (or geometry) is small, the cell is coarse, and everything got smoothed out. You can easily see this when you have only one cell for your problem. When you zoom in and increase the number of cells, you will pick up more detailed features of the geometry and related problems. At this point, if you still use the coarse mesh approach, then you can easily mess up these needed features and create unexpected problems. (7). This is the reason why I have been saying that: (a). a CFD code is not CFD. (b). running a CFD code is not CFD. (8). To get the converged solution, you first need to know the solution so that you can zoom in and identify it. It will also guide you in creating a consistent mesh and distribution. And most important of all, provide a good and reasonable initial guess. (9). The ability to do so depends on your "experience" of the problem you are trying to solve.


April 15, 2009, 13:25 

#4 
New Member
Nguyen Ngoc Tu
Join Date: Apr 2009
Posts: 2
Rep Power: 0 
You can find this document they teach how to solve convergence trouble, how it relate to the grid, I already try, it is effective
Name is "TR010 Phoenics frequently asked Questions, a selection ( Version 2006) http://www.cham.co.uk/documentation/tr010.pdf 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
"grid points" or "grid interface"  ztdep  Main CFD Forum  1  June 6, 2007 15:00 
Grid convergence  samir  FLUENT  2  April 17, 2005 00:13 
Higher order discretization on staggered grid  Chandra Shekhar  Main CFD Forum  9  January 27, 2005 17:31 
Temperature at grid points..  Elana  FLUENT  1  July 21, 2002 16:53 
Findig grid points in BFC ?  Frank Rueckert  Main CFD Forum  0  September 16, 1999 10:26 