|
[Sponsors] |
April 17, 2014, 08:42 |
|
#2 |
Senior Member
Matthias Voß
Join Date: Mar 2009
Location: Berlin, Germany
Posts: 449
Rep Power: 20 |
"not enough space"
malloc = memory allocation |
|
April 17, 2014, 08:59 |
|
#3 |
New Member
Jarda Chlup
Join Date: Aug 2013
Posts: 21
Rep Power: 12 |
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 :-(
|
|
April 17, 2014, 09:01 |
|
#4 |
Senior Member
Matthias Voß
Join Date: Mar 2009
Location: Berlin, Germany
Posts: 449
Rep Power: 20 |
Try to set the memory alloc factor like 1.1. in the solver-settings. Sometimes it helps the solver to get it started.
|
|
April 17, 2014, 09:44 |
|
#5 |
New Member
Jarda Chlup
Join Date: Aug 2013
Posts: 21
Rep Power: 12 |
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
|
|
April 17, 2014, 13:50 |
|
#6 |
Member
Join Date: Nov 2009
Posts: 49
Rep Power: 16 |
||
April 17, 2014, 16:32 |
|
#7 |
Senior Member
Join Date: Jun 2009
Posts: 1,800
Rep Power: 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. Last edited by Opaque; April 17, 2014 at 18:14. |
|
April 17, 2014, 22:02 |
|
#8 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,696
Rep Power: 143 |
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.
|
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Building OpenFOAM1.7.0 from source | ata | OpenFOAM Installation | 46 | March 6, 2022 13:21 |
[blockMesh] blockMesh with double grading. | spwater | OpenFOAM Meshing & Mesh Conversion | 92 | January 12, 2019 09:00 |
checking the system setup and Qt version | vivek070176 | OpenFOAM Installation | 22 | June 1, 2010 12:34 |
[swak4Foam] groovyBC: problems compiling: "flex: not found" and "undefined reference to ..." | sega | OpenFOAM Community Contributions | 12 | February 17, 2010 09:30 |
Problem with compile the setParabolicInlet | ivanyao | OpenFOAM Running, Solving & CFD | 6 | September 5, 2008 20:50 |