|
[Sponsors] |
October 26, 2014, 21:13 |
Real Stack Memory ERROR
|
#1 |
Senior Member
Ashkan Javadzadegan
Join Date: Sep 2010
Posts: 255
Rep Power: 16 |
Dear All,
I am stuck with the following error: _________________________________ *** INSUFFICIENT MEMORY ALLOCATED *** | | | | ACTION REQUIRED : Increase the real stack memory size. | | | | Details : | | Requested space : 201528 words | | Current allocated space : 191808656 words | | Current used space : 191757021 words | | Current free space : 51635 words | | Number of free areas : 1 | +--------------------------------------------------------------------+ Details of error:- ---------------- Error detected by routine MAKDAT CDANAM = IELG251 CDTYPE = REAL ISIZE = 201528 CRESLT = FULL _________________________________ I've gone through all previous threads on this error and tried to increase the memory up to 8x, but still get the same error. This cfx set-up used to work with no error; however, after activating transient statistics and defining few new variables, the above error showed up. Here is a summary of newly defined variable: New Variables: ABSPGX: abs(Pressure.Gradient X) ABSPGY: abs(Pressure.Gradient Y) ABSPGZ: abs(Pressure.Gradient Y) PG: sqrt(((Pressure.Gradient X)^2)+((Pressure.Gradient Y)^2)+((Pressure.Gradient Z)^2)) In "Transient Statistics" tab, I defined few cases to find the time-average of above variables over whole flow cycle as well as between specific times. Would be too pleased if any body can help me. Thanks AshtonJ |
|
October 27, 2014, 04:53 |
|
#2 |
Senior Member
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 361
Rep Power: 14 |
You've probably got some obsurdly long file names for your .def file. In execution control, under solver increase the solver memory allocation factor to 2.
Failing that just reduce your file names. |
|
October 27, 2014, 05:45 |
|
#3 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,700
Rep Power: 143 |
Why do you think file names has something to do with it? It is the real stack which has run out of space and that has no link to the file name to my knowledge.
I have a hunch there may be a problem (ie a bug) in CFX with using Pressure.Gradient X/Y/Z and transient statistics. Can you try doing transient statistics on just Pressure? Try a work around by defining a variable like PGX = Pressure.Gradient X, then define a transient statistic of abs(PGX). By the way: you have an error in your ABSPGZ function - you are using the Y gradient, not Z. |
|
October 27, 2014, 07:01 |
|
#4 |
Senior Member
Ashkan Javadzadegan
Join Date: Sep 2010
Posts: 255
Rep Power: 16 |
Thanks Glenn and RicochetJ.
I figured it out, the problem was because of choosing the full list of transient statistics. I changed it to Arithmetic Average and it works now. |
|
October 28, 2014, 06:41 |
|
#5 |
Senior Member
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 361
Rep Power: 14 |
||
October 29, 2014, 05:14 |
|
#6 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,700
Rep Power: 143 |
Weird. But it should have been the string stack which ran out of room, isn't it?
|
|
October 30, 2014, 11:16 |
|
#7 | |
Senior Member
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 361
Rep Power: 14 |
Quote:
Error out of sight is error out of mind! |
||
November 11, 2014, 20:47 |
|
#8 |
Senior Member
Ashkan Javadzadegan
Join Date: Sep 2010
Posts: 255
Rep Power: 16 |
I've found out what causes "INSUFFICIENT MEMORY ALLOCATED" error and wanted to share it here:
This error might occur 1- if you define a lot of additional variables 2- if you want to save all transient statistics I've had this problem for the last month and tried different ways to get rid of that error such as 1- Increasing the memory allocation factor up to 10x for “Partitioner”, “Solver” and “Interpolator” 2- Reducing the mesh from 1300,000 elements to 500, 000 elements None of them worked However, I fixed that problem by increasing the memory allocation factor within the CFX and also by ticking "Use Large Problem Partitioner" option and surprisingly the error is gone! |
|
September 23, 2015, 08:15 |
|
#9 | |
New Member
Join Date: Jul 2015
Location: Germany
Posts: 6
Rep Power: 10 |
Quote:
For everyone: Try to changed the allocation factor in CFX-Pre instead of the CFX-Solver Manager! This worked fine for me. |
||
November 8, 2018, 10:57 |
|
#10 | |
New Member
Join Date: Nov 2018
Posts: 4
Rep Power: 7 |
Quote:
Can anyone tell me where to find the allocation factor settings in CFX-Pre? Thanks |
||
November 8, 2018, 11:02 |
|
#11 | |
New Member
Join Date: Nov 2018
Posts: 4
Rep Power: 7 |
Quote:
Thanks |
||
November 8, 2018, 13:30 |
|
#12 |
Senior Member
Join Date: Jun 2009
Posts: 1,803
Rep Power: 32 |
cfx5solve -help
will provide you with the different options. For the ones that worked (assuming solver step failure) try cfx5solve -large -s 2 -def .... What is not clear from the original post is which component wrote the error? That is, what is the interpolator step, the partitioner step or the solver step. Each one of them have separate settings in the command line as well as in the user interface (CFX-Pre, or CFX-SolverManager) |
|
November 9, 2018, 04:30 |
|
#13 | |
New Member
Join Date: Nov 2018
Posts: 4
Rep Power: 7 |
Quote:
Thanks |
||
November 9, 2018, 05:28 |
|
#14 | |
Senior Member
Lance
Join Date: Mar 2009
Posts: 669
Rep Power: 22 |
Quote:
Right click Simulation control/insert/execution control/solver tab. But, you can also change it in the command line (see Opaque's suggestion on finding the syntax) |
||
November 9, 2018, 06:14 |
|
#15 |
New Member
Join Date: Nov 2018
Posts: 4
Rep Power: 7 |
Thanks a lot, the hint helped very much.
|
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[OpenFOAM] an error in Calculator's equation | immortality | ParaView | 12 | June 29, 2021 00:10 |
Compile calcMassFlowC | aurore | OpenFOAM Programming & Development | 13 | March 23, 2018 07:43 |
Mesquite - Adaptive mesh refinement / coarsening? | philippose | OpenFOAM Running, Solving & CFD | 94 | January 27, 2016 09:40 |
ParaView for OF-1.6-ext | Chrisi1984 | OpenFOAM Installation | 0 | December 31, 2010 06:42 |
UDF: DEFINE_CG_MOTION for vertical jump motion of an electrode! | alban | Fluent UDF and Scheme Programming | 2 | June 8, 2010 18:54 |