CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

samll elem. diverge!?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 15, 1999, 08:28
Default samll elem. diverge!?
  #1
Astrid Barros
Guest
 
Posts: n/a
I have been reducing the size of the elements in 2D models (ex.: flow arround a cilinder), and when the elements get too small, the veloc. becomes too high and the results diverge. I am using FEM for spatial discretization. I reduced the time step, but it doesn't seem to make any difference, how much should it be diminished? Should the BC be changed (smaller incident velocs.?)
  Reply With Quote

Old   August 15, 1999, 08:30
Default Re: small elem. diverge!?
  #2
Astrid Barros
Guest
 
Posts: n/a
I have been reducing the size of the elements in 2D models (ex.: flow arround a cilinder), and when the elements get too small, the veloc. becomes too high and the results diverge. I am using FEM for spatial discretization. I reduced the time step, but it doesn't seem to make any difference, how much should it be diminished? Should the BC be changed (smaller incident velocs.?)
  Reply With Quote

Old   August 15, 1999, 13:04
Default Re: samll elem. diverge!?
  #3
John C. Chien
Guest
 
Posts: n/a
(1). Well, a pretty bad problem for FEM and FEM people. Sorry to say that! (2).There are several things you can do, because you are only running 2-D problems. (3). Run a case of flow over a cylinder at Reynolds number=10. Refine the mesh and see whether it still diverges. (4). Run a case of flow over a flat plate at the same low Reynolds number, and check out the result. (5). If you are still having the same problem, run a case of flow through space with nothing in it. In this case, you can place two moving walls on the top and the bottom, moving at the free stream velocity. (6). If the low Reynolds number cases work fine, you can move up the Reynolds number step-by-step, say 100,200, 400, 1000,10000 ...etc. (7). Assuming that it is already in the turbulent flow regime, you have to look into the turbulence modeling side, which is not easy to fix. I don't know whether you are using a turbulence model or not. ( if you are using a commercial code, it is a good idea, I think, not to mention the particular name of the code.)
  Reply With Quote

Old   August 15, 1999, 23:00
Default Re: samll elem. diverge!?
  #4
Duane Baker
Guest
 
Posts: n/a
Hi,

like any analysis, we need some good inputs to come-up with some suggestions.

1. What do you mean by small, how small, small in both dimensions, how many elements, skew, etc.

2. what type of FEM discretization? Q1/Q2 on tets, triangles, etc, what type of time advance,

3. What type of linear solver?

4. Is it turbulent or not? John already assumed that it is...I on the other hand do not make assumptions without basis???

5. Is it a good code....have you read the theory?

6. are you running single or double precision???

lots of work for you first!

Just a guess but it sounds like a round-off problem due to skew/aspect/neighboring element expansion or maybe not!!!

good luck............................Duane
  Reply With Quote

Old   August 16, 1999, 03:54
Default Re: samll elem. diverge!?
  #5
Dr. Hrvoje Jasak
Guest
 
Posts: n/a
For meshes which combine very large cells with very small ones, it sometimes helps (at least in FVM codes) to use the volume (area in 2-D) weighted residuals. This forces the solver to "converge" all the cells to the same level of accuracy; otherwise large cells carry a disproportionally large proportion of the residual. This, of course works only if you can actually modify the code.
  Reply With Quote

Old   August 16, 1999, 07:24
Default Re: samll elem. diverge!?
  #6
Astrid Barros
Guest
 
Posts: n/a
Hi, I observed digergence in two cases:

1) Moving cilinder: as the cilinder oscilated in the flow, if the domain where the mesh would be adapted is small, the elements would become very small on one side and then the speeds would go very big. If I simply make this domain bigger, it will all go ok.

2) Flow over a fixed cilinder: I was having good results for the cilinder up to Re = 4000 without turbulence modeling, and above that I am using LES. I am still analysing the results, but the force on the body was slightly high, for example at Re = 200, and then I changed my mesh from 1800 to 4300 nodes, making there size near the body go from 0.1 to 0.02 close to the body (they looked a litle stretched, they are tets.), and then these elems. close to the body also gave too big speeds after some steps.

I am using tet. elems, Q1/Q1 (linear), time advace Euler or Adams-Bashforth/Moulton, ready packages for linear solver, the code is mine (Ph.D. studies), with double pecision, I really have a difference in size of elements as I move away from the body, but not so big.

And Mr. Jasak, I didn't understand very well how I can use the reiduals, and I would like to implement that in my code, could you give me a tip? Thanking you all, Sincerelly yours, Astrid
  Reply With Quote

Old   August 16, 1999, 09:09
Default Re: samll elem. diverge!?
  #7
John C. Chien
Guest
 
Posts: n/a
(1). I am not sure that the methods you mentioned are finite element methods. My intuition says those are conventional finite difference methods. I am not working in the finite element method area, so I could be wrong. (2). If you suspect the problem is near the wall, you can try to put a few layers of uniform triangular cells on the cylinder wall. Based on what I have seen, this is how other people do for the mesh around the cylinder. (3). Then away from the cylinder you can merge it with a somewhat regular mesh aligned with the flow direction instead of around the cylinder. (4). Maybe the irregular mesh is giving you the problem. Are you solving compressible or incompressible flow equations? (5). So, try a more uniform mesh first to isolate the problem. ( I can't help you in terms of the finite element methods.)
  Reply With Quote

Old   August 17, 1999, 06:18
Default Re: samll elem. diverge!?
  #8
Dr. Hrvoje Jasak
Guest
 
Posts: n/a
Consider the matrix coefficient assembly for a mesh with cells of variable size. All the coefficients (we'll take the central coefficient a_P as an example) are extensive variables, i.e. at some stage during the matrix assembly they have been multiplied by the cell volume. In order to solve the system, we use iterative solvers, with the stopping criterion based on the sum of residuals. Therefore: 1) the larger the cell, the more residual it carries, as the residual is "volume-weighted", 2) the solver "concentrates" on removing the residual from "large" cells and not everywhere. As a consequence (of loose tolerances or extreme cell volume distribution), small cells may not be "solved" at all. Cure: when the matrix is assembled, divide through all the rows with the appropriate cell volume. Now all cells are equally important from the solver's point of "view".
  Reply With Quote

Old   August 17, 1999, 22:32
Default Re: samll elem. diverge!?
  #9
Astrid Barros
Guest
 
Posts: n/a
Dear Sirs Thank you very much for the help, I am going to try dividing the matrices by the volume of the elements (if I understood well, I will divide all matrices, [M], [k], [D], [C], etc...) and if I have good results I will inform you. Thanking you again, Sincerely yours, Astrid Barros
  Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Solution converged, and then diverge again. jrg FLUENT 2 April 1, 2013 23:10
calculation diverge after continue to run zhajingjing OpenFOAM 0 April 28, 2010 04:35
LES & NITA diverge problem wtyeh FLUENT 0 May 21, 2009 21:02
simple alghorithm diverge Mahdi Main CFD Forum 0 July 23, 2008 19:04
SOLUTIONS DIVERGE IN FLUENT Rif Main CFD Forum 3 February 4, 2008 11:39


All times are GMT -4. The time now is 20:55.