|
[Sponsors] |
April 12, 2023, 23:10 |
ERROR #001100279 - (malloc) Not enough space
|
#1 |
Member
Join Date: May 2022
Posts: 61
Rep Power: 4 |
hi everyone, can someone point to how do i fix this error? solver is giving me this after a few hours running. already tried running as "double precision", "large problem", and putting memory allocation factor of 2 on partitioner, solver and interpolator settings. never had this happen before so im kind of lost. got space on hard drive as well - although it says malloc, so memory issue -, and tried running on other machine.
thanks in advance Code:
+--------------------------------------------------------------------+ | Writing transient file 185_full.trn | | Name : Transient Results 1 | | Type : Standard | | Option : Timestep Interval | +--------------------------------------------------------------------+ +--------------------------------------------------------------------+ | ERROR #001100279 has occurred in subroutine ErrAction. | | Message: | | insert_index: (malloc failed) syserr:: Not enough space | | | | | | | | | | | +--------------------------------------------------------------------+ +--------------------------------------------------------------------+ | ERROR #001100279 has occurred in subroutine ErrAction. | | Message: | | iocnt: can't insert index without sorting | | | | | | | | | | | +--------------------------------------------------------------------+ +--------------------------------------------------------------------+ | ERROR #001100279 has occurred in subroutine ErrAction. | | Message: | | WriteLong: insert index failed: what=G/FLOWS/MOM_FL1 where=ZN1/FS- | | 23416 | | | | | | | | | +--------------------------------------------------------------------+ +--------------------------------------------------------------------+ | ERROR #001100279 has occurred in subroutine ErrAction. | | Message: | | iif_create_empty: error allocating new index: malloc of 2560256 b- | | ytes failed | | | | | | | | | +--------------------------------------------------------------------+ +--------------------------------------------------------------------+ | ERROR #001100279 has occurred in subroutine ErrAction. | | Message: | | iocnt: open the primary file failed | | | | | | | | | | | +--------------------------------------------------------------------+ +--------------------------------------------------------------------+ | ERROR #001100279 has occurred in subroutine ErrAction. | | Message: | | OpenFile: open primary file failed | | | | | | | | | | | +--------------------------------------------------------------------+ +--------------------------------------------------------------------+ | An error has occurred in cfx5solve: | | | | The ANSYS CFX solver exited with return code 1. No results file | | has been created. | +--------------------------------------------------------------------+ End of solution stage. |
|
April 13, 2023, 18:35 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,741
Rep Power: 143 |
I think the malloc error comes about when it has run out of system memory (RAM). Are you sure you have enough RAM for what you are trying to do?
Also consider running over multiple systems in multiprocessor mode, or over more nodes if you are already doing this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
April 13, 2023, 18:55 |
|
#3 | |
Member
Join Date: May 2022
Posts: 61
Rep Power: 4 |
Quote:
i tried increasing the OS pagefile and it still happened. its been running under intel mpi local, 4 cores (student version limitation). trying now as serial to see if it works. |
||
April 13, 2023, 19:15 |
|
#4 |
Senior Member
Join Date: Jun 2009
Posts: 1,820
Rep Power: 32 |
Very interesting error.
May I ask which release version you are using? Which OS, Windows or Linux? Your model seems to have a lot of CAD parts, FS23416 is FaceSet 23411 in domain/zone 1.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
April 13, 2023, 19:20 |
|
#5 |
Member
Join Date: May 2022
Posts: 61
Rep Power: 4 |
win10. i usually run cfx on a centos - after building it up on my windows - cluster but for some reason, its giving me an error when i try to import this one.
|
|
April 14, 2023, 11:17 |
|
#6 |
Member
Join Date: May 2022
Posts: 61
Rep Power: 4 |
tried doubling ram to 32gb, same error. going crazy here.
|
|
April 14, 2023, 15:50 |
|
#7 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,836
Rep Power: 27 |
Maybe share the complete output file (upload in the "Go advanced"-menu? This might give us more insight.
|
|
April 15, 2023, 18:30 |
|
#8 |
Member
Join Date: May 2022
Posts: 61
Rep Power: 4 |
hi, here is the output.txt from my last run. thanks
edit: sorry, it says "output.txt: Your file of 427.5 KB bytes exceeds the forum's limit of 195.3 KB for this filetype." |
|
April 15, 2023, 18:31 |
|
#9 | |
Member
Join Date: May 2022
Posts: 61
Rep Power: 4 |
Quote:
https://we.tl/t-tQpV8f4hDt thanks! |
||
April 15, 2023, 22:37 |
|
#10 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,741
Rep Power: 143 |
I do not download stuff from unknown sites.
Edit the output file to get it under the file size limit. If there are lots of iterations then chop out the iterations where nothing much happens.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
April 15, 2023, 22:40 |
|
#11 |
Member
Join Date: May 2022
Posts: 61
Rep Power: 4 |
hey Glenn! I removed some stuff from the middle of the .txt and attached it
thanks! |
|
April 15, 2023, 23:00 |
|
#12 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,741
Rep Power: 143 |
You are writing a results file every time step, and each results file contains the mesh and full particle track information. This is going to generate a lot of increasingly large transient results files.
Some suggestions: * Do you really need to save a results file every time step? * Do you need to include the particle track data every time step? * Do you need to include the mesh every time step? * Do you need to include all the variables every time step? (eg fluxes and all the other stuff which is rarely used) If you can remove any of these things from the transient results file, or just save them less frequently it will probably make a big difference. Other points: * This simulation is using 5GB on a 32GB machine. It should run OK. * The mesh is quite small (197k nodes) * Simulation is transient, laminar, particle tracking. Nothing too unusual here.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
April 15, 2023, 23:14 |
|
#13 | ||
Member
Join Date: May 2022
Posts: 61
Rep Power: 4 |
hey! thanks for the answer!
I'm pretty certain I could live with the final (last time step) result for the moment. where in PRE should i change this? Quote:
this is news to me. i didnt know the mesh is included. what would be the use of that, in results? (not being ironic, really asking because maybe i use it and didnt even know) Quote:
thanks!!!!!! |
|||
April 15, 2023, 23:20 |
|
#14 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,741
Rep Power: 143 |
You can select the transient results file options in CXFX-Pre, in the output tab (transient results file options).
Everything is pretty obvious, except including the mesh has some implications: * If you include the mesh then all transient results files are complete and can be loaded stand-alone, or used for initial conditions for other runs. * If you do not include the mesh you save the space of the mesh in each file (which if the mesh is stationary makes a lot of sense), but it means you cannot use the no-mesh transient results for initial conditions, and you can only read the data from the time step if you later do write a results file including the mesh. This happens by default at the end of a run. But if your run crashes before you get to the end (like your run is doing now) then all your transient results files are unreadable as there is no mesh information. There is also a lot of options on the particle tracks - how many to include, how much resolution to write, what variables to include and so on. Between the transient results file options and the particle track results file options you will need to reduce the amount of stuff you are saving to avoid this malloc error.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
April 16, 2023, 21:43 |
|
#15 | |
Member
Join Date: May 2022
Posts: 61
Rep Power: 4 |
Quote:
still didnt run results to find out if ill miss anything, but ill post here as soon as i do. now that it ran, would you guess the reason why it wont survive under “standard”? thanks again, leo |
||
April 16, 2023, 21:53 |
|
#16 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,741
Rep Power: 143 |
The file size of standard is much larger. So it has filled your hard drive up, or the particle tracks are taking up so much space that it runs out of memory working it all out.
If you want to work out exactly why it is failing you are going to have to try a few options (eg is it the particle tracks? or the general results file?) and check things like memory useage and disk space during a run. Also, don't forget that as you appear to be a student you probably have a disk space limit. Maybe the CFX temporary files got big enough they hit your disk space limit? All of these things are unique to your setup, so you are going to have to check them out. We cannot tell you what the problem is.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
April 16, 2023, 22:08 |
|
#17 | |
Member
Join Date: May 2022
Posts: 61
Rep Power: 4 |
Quote:
best, leo Last edited by lgtmelo; April 16, 2023 at 22:08. Reason: typo |
||
April 16, 2023, 23:25 |
|
#18 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,741
Rep Power: 143 |
CFX has no space limit. It has been scaled to billions of nodes and thousands of partitions. The student version does have a node and partition limit but if it hits those it should give an error clearly saying it has hit that limit.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Error: Out of scheme heap space | SSG_NJ | FLUENT | 2 | July 24, 2021 06:31 |
Run OpenFoam in 2 nodes of a cluster | WhiteW | OpenFOAM Running, Solving & CFD | 16 | December 20, 2016 00:51 |
[Commercial meshers] ST_Malloc: out of memory.malloc_storage: unable to malloc Velocity SA, | cfdproject | OpenFOAM Meshing & Mesh Conversion | 0 | April 14, 2009 15:45 |
How to model the NR eqns in a domain with empty space | Vasilis | Main CFD Forum | 1 | April 14, 2009 04:35 |
Fatal error error writing to tmp No space left on device | maka | OpenFOAM Installation | 2 | April 3, 2006 08:48 |