[sarrazs]

Hello
I'm doing transient simulations of a 3D bubble column on CFX using Euler-Euler approach. For the boundary condition, I add an air freeboard region on top the liquid phase and I set correctly the hydrostatic pressure. It works great in the serial calculation but It doesn't even start in the parallel calculation. I always get this error :
+--------------------------------------------------------------------+
| ERROR #004100018 has occurred in subroutine FINMES. |
| Message: |
| Fatal overflow in linear solver. |
+--------------------------------------------------------------------+
map size mismatch; abort
: File exists

I know that adding the air freeboard region is the cause of the error and I saw in the cfx guide that I can ignore it and it works for serial calculation but how can I make it work for parallel calculation and can anyone explain why it doesn't work??

[ghorrocks]

The parallel solver in CFX is very robust and rarely gives any different results to the serial solver (except faster). I think you have found one of the rare exceptions.

There is a brief discussion in the CFX documentation about convergence issues with parallel runs.

A key issue is if a partition boundary lines up with a discontinuity, such as a free surface, shock wave or other region of extremely high gradients. The default partitioner is very efficient but does not take into account these regions it should avoid. So if you try a different partitioner and make sure that partition boundaries are not close to high gradient areas that may help convergence.

[sarrazs]

Originally Posted by ghorrocks

The parallel solver in CFX is very robust and rarely gives any different results to the serial solver (except faster). I think you have found one of the rare exceptions.

There is a brief discussion in the CFX documentation about convergence issues with parallel runs.

A key issue is if a partition boundary lines up with a discontinuity, such as a free surface, shock wave or other region of extremely high gradients. The default partitioner is very efficient but does not take into account these regions it should avoid. So if you try a different partitioner and make sure that partition boundaries are not close to high gradient areas that may help convergence.

Thank you ghorrocks this is really helpful.

[JuPa]

Originally Posted by sarrazs

Thank you ghorrocks this is really helpful.

A quick test would be to reduce the number of partitions by half or quarter.

[sarrazs]

Originally Posted by JuPa

A quick test would be to reduce the number of partitions by half or quarter.

Thank you Jupa. I reduced it from 48 to 6. And I'm waiting for the results.

[ghorrocks]

I would use the recursive bisection partitioner, or if your domain is long and thin maybe the specified direction bisection one.

[sarrazs]

Originally Posted by ghorrocks

I would use the recursive bisection partitioner, or if your domain is long and thin maybe the specified direction bisection one.

My domain is 0.15x0.15x0.45 m
I'm not an expert in this I just write a submission file where I define the number of nodes and the number of cores ("processors") per node that I need. And the computer does the partition.
It didn't work for 6 cores but it worked for 5.
Thank you for your advice.

[ghorrocks]

You can always look at the partitions it defines in the post processor. The variable is "Real Partition Number". Then you can see where the boundaries are occurring.