CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   About Solver Overflow (

Felix November 2, 2006 10:26

About Solver Overflow
Hello everyone,

I know this question as been treated in many previous posts but I never found a clear answer. I am actually simulating flows in elbow draft tubes and often get the "LINEAR SOLVER OVERFLOW". As I understand it, it is really a mesh issue (in my case at least) as two different meshes behave differently.

I give you an example. One of my tetra mesh was running well but the Y+ value was too large so I refined the near-wall prism layer. The calculation crashed after about 15 iterations and the total pressure loss between the inlet and the outlet had reached 10^15 or so. I also had the same problem with Hexa meshes.

Does anyone have a valuable experience regarding this problem? I suspect large aspect ratios to be part of the answer but then how can we respect the requirements on Y+ (I'm using SST) ? Also, calculating in double precision didn't help.

I'm sure this post can be helpful to help many of us. Regards,


Felix November 2, 2006 10:31

Re: About Solver Overflow
Hello again,

I add some computational details to help you understand my case:

I run in steady-state mode (transient doesn't help) with the SST turbulence model. I have a Y+ < 2 in the part of interrest so aspect ratios can easily be over 1000 in this area. The inlet boundary condition is a velocity profile and the outlet of the domain is an opening.

Thanks again, have a nice day,


johnny November 2, 2006 11:49

Re: About Solver Overflow
You could refine the mesh parallel to the walls to improve aspect ratios. General mesh quality is also important. What are your minimum face angles?

Also, reducing the timestep can improve the stability of the code.

Felix November 2, 2006 13:33

Re: About Solver Overflow
Hello Johnny

Thanks for your advices. Depending of the mesh I use ( Hexa or Tetra) the minimum angle is always around 14-15 degrees and the quality is around 0.2. The timestep I use is already quite small, around 0.001 second.

Your idea of reducing the wall elements is excellent to reduce the aspect ratios but gives a very large number of elements. Too large, to be honest. Also, this has been impossible in Hexa since the refinement can not be done locally near the wall (only there) as far as I know.

Can Hexa meshes be used with the SST turbulence model? Is mesh refinement the real cause of this problem?



Andy November 3, 2006 04:55

Re: About Solver Overflow
Hey Felix,

what kind of software do you use for generating your mesh? I am asking because I have similar problems with a airfoil- like profile mounted on a blunt body (a kind of wing-root-situation). I have cut out the region of interest in my CAD-model and meshed it in ICEM with TETRA and added a Prism-Layer in order to get a Y+ < 2. The big issue is that ICEM is telling me that the element quality is alright (worst volume-element about 0.07) however the solver will still show large oscillations and crash after a few (ten or so) time steps.

I am supposing that the problem is the translation from ICEM to CFX. Maybe the small PRISM-elements are transformed in a way that they allow the flow to exit my domain through the solid wall.

I know that will not help you but maybe there are others that have faced the same problem and even others that know a solution... ?

Regards Andy

Felix November 3, 2006 09:50

Re: About Solver Overflow
Hi Andy,

I also use ICEM to mesh my geometry. I don't think that the translation is the problem, as you suggest it as these software are made to work together. Also a colleague told me that he had the same problem as we do only by refining his prism layer ( 5 thick layers refined into 21 layers).

I still don't have a clue...If you find something interesting just let me know!

Regards, Felix

fcabrales October 26, 2010 18:34

Hi !

I am getting exactly the same problem that you obtained. I import one of the meshes of my domain from ICEM to CFX and after some iterations the solver crashes with that "Overflow error". I would like to know if you were able to find any solution to this problem. I tried all possible timescales, turbulence models, meshes and so on, but I keep on getting this error.

I really appreciate your help.


Josh October 26, 2010 21:22

We need more info. What are your boundary conditions? What are you modelling?

michael_owen October 26, 2010 22:52

This is almost always a problem with the solver having a hard time getting started from a poor initial condition. Drop the timescale by 2 orders of magnitude, and when the residuals have peaked and are slowly but smoothly falling, start ramping the timescale back up slowly until you get to a reasonable timescale for the problem.

Also, is the problem compressible? Velocity specified inlets can be inappropriate for compressible flow. Read the documentation on inlet BCs for compressible flow.

I'm not sure if the flow is interior or exterior, but if it's the former, you may get this error when you are trying to shove more air through the device than it is capable of delivering.

Lazier, problems with very large ratios of any kind (nozzle flows to vacuum, CHT problems, problems with high aspect ratios in the inflation layer, free surface calculations, etc) should always be run in double precision. This will not avoid solver overflow, but it will avoid machine roundoff error.

fcabrales October 27, 2010 11:32

I am simulating a mixing tank with a rotative domain and a stationary one. The two domains are connected by interface through a GGI connection and I use the multiple frame of reference approach. Tha tank is fully closed and all the walls are no-slip.

Josh October 27, 2010 17:00

Michael's suggestion is correct: poor initial conditions are probably causing this. Alternatively, non-physical boundary conditions could also be the problem. You don't appear to be using any openings (inlets, outlets) so the first option is more likely the problem.

Have you tried solving the simulation with simpler numerical methods? For example, try using a lower-order advection scheme, lower-order turbulence model, lower-order turbulence numerics, etc. If this converges, gradually increase the order of accuracy.

All times are GMT -4. The time now is 05:26.