[Jared1986]

Hello to everybody,
I have troubles with setting of memory usage. I've found this error message

| ERROR #333100180 has occurred in subroutine Out_MemPar. |
| Message: |
| |
| The total number of words requested by partition 1 |
| for the Real stack is : 3345184000 |
| That exceeds the maximum of : 2147483648 |
| supported by the flow solver. Please reduce the memory usage. |
+--------------------------------------------------------------------+

Has anybody idea how to solve this issue?

I set this memory alocation for partitioner and solver.
PARTITIONER STEP CONTROL:
Multidomain Option = Independent Partitioning
Runtime Priority = Standard
EXECUTABLE SELECTION:
Use Large Problem Partitioner = Off
END
MEMORY CONTROL:
Catalogue Size Override = 1.5x
Integer Memory Override = 1.2x
Memory Allocation Factor = 1.0
Real Memory Override = 1.2x
END
PARTITIONING TYPE:
MeTiS Type = k-way
Option = MeTiS
Partition Size Rule = Automatic
Partition Weight Factors = 0.25000, 0.25000, 0.25000, 0.25000
END
END

SOLVER STEP CONTROL:
Runtime Priority = Standard
MEMORY CONTROL:
Catalogue Size Override = 1.05x
Integer Memory Override = 1.05x
Memory Allocation Factor = 1.0
Real Memory Override = 1.05x
END
PARALLEL ENVIRONMENT:
Number of Processes = 4
Start Method = Platform MPI Local Parallel
Parallel Host List = xwmlsomc0020*4
END
END

Thanks a lot

[chiragsvnit]

Please visit following links, it is similar to that. Perhaps, this will give you some idea about mesh density and solver capability and perform calculations for approximate required memory per node used by the CFX solver.
I had similar problem.

http://www.eureka.im/1775.html

http://www.cfd-online.com/Forums/cfx...erraction.html

http://www.cfd-online.com/Forums/cfx...erraction.html

[ghorrocks]

Your PC has run out of memory. Some possible way to fix it:

* If you are using a 32 version of CFX, try a 64 bit version (both OS and ANSYS CFX needs to be 64 bit)
* Use multi-processor operation to get the size of each partition down
* Corsen the mesh or use less physical models to decrease the size of the model.

[Antanas]

Originally Posted by ghorrocks

Your PC has run out of memory. Some possible way to fix it:

* If you are using a 32 version of CFX, try a 64 bit version (both OS and ANSYS CFX needs to be 64 bit)
* Use multi-processor operation to get the size of each partition down
* Corsen the mesh or use less physical models to decrease the size of the model.

Maybe he should try to increase memory allocation factor for real stack?

[ghorrocks]

The error message says that the requested real stack size exceeds the size allowable. You cannot define a larger real stack.

[Antanas]

Originally Posted by ghorrocks

The error message says that the requested real stack size exceeds the size allowable. You cannot define a larger real stack.

Yes. I guess you're right.

[Jared1986]

Good morning again, first I want to thank for your answers. I think that solution could by right setting of real stack memory for solver, I've tried to set some values of real stack, but without success. Is it possible to calculate number of words, which I could set for real stack memory? I am using 6 processors for calculation and I have 48 GB of RAM. I made mesh about 37M of elements and 24M of nodes. So I think that it could be possible to calculate it on my workstation. Does anybody have idea how set this real stack memory?

Thanks a lot

I obtain again this kind of error.

+--------------------------------------------------------------------+
| *** INSUFFICIENT MEMORY ALLOCATED *** |
| |
| ACTION REQUIRED : Increase the real stack memory size. |
| |
| Details : |
| Requested space : 23479892 words |
| Current allocated space : 883723584 words |
| Current used space : 385453263 words |
| Current free space : 498270321 words |
| Number of free areas : 636 |
+--------------------------------------------------------------------+


Details of error:-
----------------
Error detected by routine MAKDAT
CDANAM = CELRWRK CDTYPE = REAL ISIZE = 23479892
CRESLT = FULL

Current Directory : /FLOW/CEL1

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine MEMERR |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+

[Antanas]

Originally Posted by Jared1986

Does anybody have idea how set this real stack memory?

"Define Run" -> "Solver"-> "Solver Memory" -> "Detailed Memory Overrides"

[Jared1986]

Originally Posted by Antanas

"Define Run" -> "Solver"-> "Solver Memory" -> "Detailed Memory Overrides"

I did it 5 times maybe more. It is big issue to find right value for that. As I write before. Is it some formula how to calculate number of words, which is possible to set there or value for multiplying?

[ghorrocks]

If you need to increase this more than a small amount it means something is fundamentally wrong with your simulation. This can occur when you have complicated physics such as lots of particle tracks or GGI interfaces. More often than not there is an error in the setup of the complex physics and it runs out of stack space trying to sort it out.

Can you describe what you are modelling?

[Jared1986]

Originally Posted by ghorrocks

If you need to increase this more than a small amount it means something is fundamentally wrong with your simulation. This can occur when you have complicated physics such as lots of particle tracks or GGI interfaces. More often than not there is an error in the setup of the complex physics and it runs out of stack space trying to sort it out.

Can you describe what you are modelling?

I want to calculate thermal simulation for synchronous machine with salient pole. There are a lot of solid domains (heat source), where I had to set anisotropic conducitvity based on cylindrical components. I have rotating fluids. It was impossible to set symmetry because of rotation so I have few parts 360deg and almost 180 deg, where I used rot. per.. I have on each interface between fluids, where is different pitch angle, set frozen rotor (also between rotating and stationary fluid domains). I think that it is very complex case. I used SST turbulent model. Is it enough information?

[ghorrocks]

It says that you are likely to have a number of domains with complex meshes connected with complex GGI interfaces. When things are not quite right you can get the error message you show. So I would have a detailed look for weirdness in the meshes at the GGI interfaces and make sure they are as intended.

[Mazze[ITA]]

A workaround could be the switching to the Large Problem Partitioner (as it should be suggested during the Partitioning step). The problem is that it requires more memory than the standard partitioner, so you can incur into swapping...

 +--------------------------------------------------------------------+
 | ERROR #001100279 has occurred in subroutine ErrAction.             |
 | Message:                                                           |
 | The total number of words needed for the Integer stack exceeds th- |
 | e maximum supported by the standard partitioner: 2,147,483,647.    |
 | The run will continue with the stack size clipped to that value.   |
 | If the standard partitioner runs out of memory you will need to    |
 | run the large problem partitioner.                                 |
 |                                                                    |
 +--------------------------------------------------------------------+