[amrrhm]

I have a simple simulation contains single phase and inlet and outlet and couple of pipes and a symmetry boundary condition. When I run it in serial, there is no error and it seems it is fine, but when I run it in parallel I get the following error during reading the surface.in (if I use embedding I will get the same during reading embedded.in):

ERROR: cell is too underesolved -- it is cut by more than 100 independent surfaces

any ideas what is this error and how to fix it.

Thanks

[alemoine]

Hi amrrhm,

Would you be able to explain your geometry and case setup in more detail? A picture of your geometry would be very helpful. In addition could you answer the following questions:

• What is the base grid size you are using and the corresponding geometry dimensions (click the "Geometry Information" button located on the left side of Studio)?
• When you ran the Diagnosis Tool with all of the default settings, did you find any issues?
• What version of CONVERGE are you using?

Thank you,

[amrrhm]

Hi alemoine,

Please find the top view and perspective view attached.

1. I have used several grid size from 1e-3 to 1e-5 and also various embedding scales and layers for the tubes part. The geometry dimensions are 0.34 x 0.052 x 0.1420. The diameter of tubes are about 2.3e-3.

2. There is no error in diagnostic tool.

3. I am using 2.3.11

Thanks for your help.

[alemoine]

Hi Amrrhm,

The error message you are seeing is a combination of the geometry and current restrictions in our domain decomposition algorithm.

The geometry you presented has 216 channels. When CONVERGE is preparing to decompose the domain for parallelization, it is finding that there are more than 100 pipes in a parallel block (please see Chapter 11 of the CONVERGE Theory Manual for more information on Parallel Processing). While the pipes themselves are all connected and associated with the same Boundary ID, the parallel blocks are unable to recognize them as being part of a continuous surface.

The restriction of having less than 100 surfaces in a parallel block will be removed from future versions of CONVERGE. In the mean time, here are some steps you can take to get your simulation to run:

• Set the parallel_scale to give the smallest possible block size (i.e. parallel_scale = -1). By making the parallel blocks smaller, there are less pipes that can be contained in a block.
• Coarsen the base grid. Your current base grid is set to 0.001 m. You can coarsen this to 0.002 m

Best Regards,