CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   solver error (http://www.cfd-online.com/Forums/cfx/133591-solver-error.html)

Jared1986 April 17, 2014 05:16

solver error
 
1 Attachment(s)
Hello to everyone,
I have error message in solver and I don't what does it mean. Does anybody have experience with this kind off error please?

Attachment 30228

mvoss April 17, 2014 08:42

"not enough space"
malloc = memory allocation

Jared1986 April 17, 2014 08:59

Yes I thought that could be small space, but I had allocated 80% of my memory space for solver running, so I don't know, why I could see this message :-(

mvoss April 17, 2014 09:01

Try to set the memory alloc factor like 1.1. in the solver-settings. Sometimes it helps the solver to get it started.

Jared1986 April 17, 2014 09:44

I try to set different catalogue size and real size, but If I change entire allocation factor from 1.0 to 1.1. it increase allocated memmory for each components (real, integer ....) so I think that increase requirement on memory size a lot. I have 37 mil cells case and 80 GB of RAM and I have still troubles with right setting of real stack memmory

Abou ali April 17, 2014 13:50

Quote:

Originally Posted by Jared1986 (Post 486741)
. I have 37 mil cells case and 80 GB of RAM and I have still troubles with right setting of real stack memmory

May be the problem is in the hard disc space!!!!!!

Opaque April 17, 2014 16:32

The message you are getting is coming when reading the partitioning file for a parallel run. There is not enough memory available in the system to allocate the space required to read such dataset.

You can use the memory factors (s < 1.0x) to reduce the memory used by the simulation (not the file reader) until the simulation will not be able to run either.

ANSYS CFX solver requires ~ 1GB per 1M hex cells, and about 2GB per 1M cells for a hybrid mesh. Memory for other libraries such as the file reader (or MeTiS partitioner) is not included in such estimate. For parallel runs, you may have to add some overhead per partition ~20%, i.e. 1.2x to the previous estimate.

Have you tried to increase the number of partitions, and consequently reduce the memory required per partition. If increasing the number of partitions does not workaround the problem, you may need to contact ANSYS support directly.

Hope the above helps,

PS. I wonder what your model looks like that require at least 113 domains plus 2578 (perhaps more) CAD surfaces on a single domain.

ghorrocks April 17, 2014 22:02

That huge number of surfaces is going to cause problems. If they can be merged into a smaller number that will help a lot. If you need them all then you are going to have to face lots of memory problems as that is an unusually large number of surfaces.


All times are GMT -4. The time now is 23:04.