CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM Bugs (
-   -   Cases with small length scale work fine on a single processor but fail in parallel (

adona058 February 25, 2009 16:44

Hopefully a quick question for
Hopefully a quick question for someone out there to answer.

I have a case with a cell lenght scale of ~0.00002 (not unreasonably small). When decomposed, solvers such as InterDyMFoam fail to get past the first pressure iteration (i.e. the solver goes through the maximum number of iterations).

Yet when run on a single processor, everything proceeds fine.

I currently have 10 decimals of precision set in the controlDict file...

Does anyone know if I need to make some other settings changes to make a small-scale case work in parallel?



mattijs March 6, 2009 06:02

What is the case? Refinement/u
What is the case? Refinement/unrefinement or moving mesh? There should be no dependency on scale (only once dimensions/timesteps approach 1e-15 or so). Do you write the mesh binary?

nikos_fb16 March 26, 2009 01:46

GAMG / floatTransfer 1?
Hi adam,

if you're using the GAMG solver probably the parameter "floatTransfer" in the global controlDict (etc/controlDict) is set to 1. You should set it to 0, this will help.

adona058 April 16, 2009 12:29

Still having problems... Test Case attached
2 Attachment(s)
Hi Mattijs, Nikolaos.

Sorry for the late response to your replies, for some reason my email notification from the forum hasent been working.

I tired doing modifications based on both of your comments, with no luck. Using ascii or binary write formats did not appear to have an impact. I also tried moving the pdRefProbe location to ensure it was within the first processor (which didnt have an effect). Modifying the term in the controlDict file (etc/controDict) also didn't affect the results.

The simulation runs in parallel for a number of iterations, but eventually fails.

I have attached a simple test case in the hopes of obtaining some help in solving this problem ( To minimize the size, I only included the blockmesh dictionary file and boundary file (you'll have to run blockMesh)

The test case is for a droplet in simple shear. Try running the case on a single processor, and on multiple processors (currently set up to decompose into 4).

I have also attached the output from my machine for both the single and parallel runs (

Please take a look and get back to me with any additional suggetions. This is a rather large problem for me, as I have some large grids (multi-million cell) that I need to run cases on, which would take an unreasonable amount of time on a single processor.

I know that the problem is not limited to the interDyMFoam solver, as I have another custom solver that experiences similar problems. It also uses the GAMG solver for the pressure field.

adona058 April 16, 2009 12:47

Still having problems... Additional Note
As an additional Note, there is no adaptive meshing in this case. I am using interDyMFoam as an example since I need it for other similar cases.

mattijs April 17, 2009 04:41

From your runParFoam.o56029 file:

Pstream initialized with:
floatTransfer : 1

If you look at the error traceback it is due to a sigfpe - usually a division by 0 or an overflow. A division by 0 would show up in the traceback as originating from '/' so it is an overflow. See also

All times are GMT -4. The time now is 09:55.