CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Solver Overflow (http://www.cfd-online.com/Forums/cfx/105850-solver-overflow.html)

ziyasaydam August 10, 2012 13:21

Solver Overflow
 
Dear All,

I was simulating a multiphase case of a boat free to heave and pitch with the homogenous multiphase model. When I use the results with the homogenous model as initial conditions for the non-homogenous model case, the simulation ends with the linear solver overflow error. The problem shows itself in the monitors as a sudden decrease in the residuals (continuity and momentum terms). Also, while postprocessing, I have noticed substantial increase in velocity in a single cell along the boundary layer of the hull.

So far, I have tried variations in time step, different turbulence models, different meshes and varying some parameters in the turbulence modelling. I am not intending to try lower degree discretization or coarser meshes. The model has no interfaces in it and I'm using k-e as turbulence model. There is a sink term along the hull to prevent air entrapment (removing the term does not help).

I read through the older threads and seen that this is a common error and there is an faq about the subject. But in this case, it seemed to me as a local problem rather than a general tendency of divergence in the flow field. Has anyone came across to something similar or has an idea about what's going on?

ghorrocks August 12, 2012 08:05

Sounds strange. But I would be looking at your mesh quality in that area as a first guess.

Felggv August 13, 2012 10:25

Try the same simulation with a coarser mesh to see what happens...

ziyasaydam August 13, 2012 13:00

Ok, but may I ask what sort of benefit would we get if the solver does not fail on a coarser mesh?

Felggv August 13, 2012 14:31

If it works, then maybe the problem is with the mesh itself.

You see, if you have the same conditions with different meshes, one works, the other doesn't... so you have an initial guess of where the problem might be.

Have you noticed if the iterations go further with different timesteps? Maybe an adaptive condition?

EDIT: Another thing you should try is to modify the solver Memory Allocator Factor... try increasing it to something like 4 or whatever suits you. You could do this by editing the advanced controls at the beginning of your run settings.

ziyasaydam August 14, 2012 06:06

The iterations may go further if the time step is reduced. I could go up to a maximum of around 250. With a higher time-step it takes only a few iterations to diverge...
What sort of benefit would I get from increasing the solver memory allocation factor?

bratzinger August 14, 2012 09:06

http://www1.ansys.com/customer/conte...20/ans_per.pdf

Felggv August 14, 2012 09:31

Maybe it's running out of memory or something like that, happened with me here once.

ziyasaydam August 14, 2012 10:06

I found the exact same document after your post and surprisingly it works!!!
Although there is sufficient memory available (32 GB), it has to be manually allocated to the solver even on a 64 bit system and double precision case to prevent integer overflows. Thank you so much Felggv for the recommendation.

Maybe this is worth adding to the FAQ on solver overflow...

ghorrocks August 14, 2012 19:16

Quote:

Maybe this is worth adding to the FAQ on solver overflow...
Please do.

Felggv August 15, 2012 09:51

I'm struggling to run a simulation using a 4cm element size... I've been running it with the 4 cores of a i5 processor, it's the best I have here.

Monitoring it, I've seen it working at 100% CPU and almost 4GB RAM.

If I don't set these conditions it overflows.


All times are GMT -4. The time now is 14:24.