Floating point error in Saturne

Just a quick note on the error you get in your first post.

I see that you are using a k-epsilon model for turbulence. Be sure that your flow is indeed turbulent (i.e. Reynolds number high enough), and also that your mesh is a high-Reynolds-number mesh because k-epsilon is a high-Reynolds model that uses wall functions to model the near-wall turbulence. If not, you can set the variable IDEUCH to 2 (go to advanced option in k-epsilon within the GUI, then tick the scalable wall-functions box) ; but the preferred way is to have a high-Reynolds mesh.

You're welcome

And feel free to contribute to Code_Saturne whenever you want ! Hopefully, there will be a decent forum and website soon enough.

Two-phase Eulerian-Lagrangian approach is used to simulate convected particles. It is related to particle tracking, not to two-phase flows like a water/steam mixing. Sorry <br /><br />Post edited by: David Monfort, at: 2008/05/16 21:51

Hi David,
You were talking about a &quot;High-Reynolds-Mesh&quot;. What exactly are the properties of such a mesh? I get the same error-messages as Claus did (floating point exception). But very suprising to me is that I have this problem although I use the scalable wall function.
Thanks
Martin

Hi Martin,

In CFD, when one talks about a &quot;High-Reynolds&quot; or &quot;Low-Reynolds&quot; mesh, one refers to the dimensionless wall distance (see e.g. y+ definition at CFD-online ).

Some turbulence models have originally been developed for high-Reynolds meshes (standard k-epsilon model, ...) and have to be used with wall-functions, while others should be use with low-Reynolds meshes, i.e. where y+ equals more or less to 1 (v2-f model, Large-Eddy Simulation, ...). This is a rather crude separation because one can use wall functions with Large-Eddy Simulation, or scalable wall function to remain in the validity domain of the model.

Make sure that your time-step is small enough for your study: look for the Courant max in the listing and check that it doesn't become higher that 1 to 10 (depending on your turbulence model). If it does decrease your time-step accordingly.

As for the floating point exception error you get, it is probably not related to your mesh. It is a general exception caught by the code when it encounters an error while doing arithmetic stuff (e.g. a division by zero, a float too large or too small, ...).

You may have a more precise idea of the error if you have a look at the end of the listing file, or at the erreur files. This can also arise if your calculation diverges, if so you can check in the listing the maximum value the velocities and/or pressure. If it keeps increasing or if you get NaN (it means &quot;Not a Number&quot;), then it will mean that your calculation has diverged.

If you are still stuck with your problem, please attach your listing (or part of) and your Fortran users (and xml file if you use the interface) so that I can have a look at it.

David<br /><br />Post edited by: David Monfort, at: 2008/07/29 22:02