|
[Sponsors] |
![]() |
![]() |
#1 |
Guest
Posts: n/a
|
Hi, I am trying to model a concentric straight tube heat exchanger using CFX 5.4.1. Heat transfer is between hot water and cold water seperated by 2 mm tube wall.The length of heat exchanger is 2 m. Solver has stopped prematurely with the following error message.
----------------------------------------------------------- ERROR #004100018 has occurred in subroutine FINMES Message: fatal overflow in linear solver --------------------------------------------------------------- Can anybody tell me what might be the reason? Thanks, satya |
|
![]() |
![]() |
![]() |
#2 |
Guest
Posts: n/a
|
FINMES means 'Final message' which is a very helpful message!??
Can't say what might be the reason. Did it occur after one iteration? After 10? Did you get any upper or lower limits in temperature/enthalpy? What is your physical timestep? Reduction by a factor 10 to 100 might help. Good luck, Astrid |
|
![]() |
![]() |
![]() |
#3 |
Guest
Posts: n/a
|
Thanks Astrid, Solver stopped after 27 iterations when I used Auto time step. I thought "FINMES" means Fine mesh, so I was playing around with mesh size and its quality
![]() |
|
![]() |
![]() |
![]() |
#4 |
Guest
Posts: n/a
|
The general rule of thumb for getting steady state solutions to fluid flow problems is that physical timestep should be selected based on a characteristic length over velocity scale for your problem. Generally CFX-5 will work well with 1/5 -> 1/3 of the characteristic timescale when using the high resolution advection scheme, and probably higher if you are running first order.
If you have pure diffusion however (as in the case of a conducting solid) there is no need to hold back. You can use basically use an infinite timestep. Do this by setting the physical timestep for your solid domains to something like 1e20 seconds. You can do this using the definition file editor and setting "Solid Timescale Control = Physical Timscale" and "Solid Timscale = 1.0e20 [s]" in the CONVERGENCE CONTROL section of the solver command file. Neale. |
|
![]() |
![]() |
![]() |
#5 |
Guest
Posts: n/a
|
Hi, Do you have access to CFX5.5 as they have sorted out some possible errors that can lead to the FINMES error from occuring. in the past I have found that the error occured where there were large stagnant regions of low velocity in a model, or where the mesh resolution was insufficient, ie only 2 mesh cells between surfaces. Hope this helps Stuart
|
|
![]() |
![]() |
Thread Tools | Search this Thread |
Display Modes | |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Concentric Tube Heat Exchanger Analysis | Abhishek | CFX | 3 | November 8, 2011 06:45 |
Concentric Tube Heat exchanger (pipe in pipe) in 2D | ckliew | ANSYS | 0 | February 24, 2011 08:48 |
Concentric tube heat exchanger (Air-Water) | Young | CFX | 5 | October 7, 2008 00:17 |
Concentric tubes heat exchanger | FTM | CFX | 6 | April 10, 2006 19:14 |
Convective Heat Transfer - Heat Exchanger | Mark | CFX | 6 | November 15, 2004 16:55 |