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

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

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. As you suggested, I used physical time step 100 sec but I got the same error again. I changed the physical time step by hit and trial to 1000 secs and it worked. whats the criteria to select the physical time step? satya

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.

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