|
[Sponsors] |
![]() |
![]() |
#1 |
New Member
Join Date: Nov 2017
Posts: 27
Rep Power: 8 ![]() |
Hi,
My solver is failing with return code 1, but without any error message. Exact same project that worked a few days ago doesn't work now. Tried duplicating and running a simulation that worked fine before, but still same problem. Does anyone know what the problem could be? Thanks! |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
If it gave you an error code it gave you an error message. The error code is not much use in CFX as there is no table of what those codes mean (in fact I don't know why they bother giving error codes....). You need the error text and the context which it occurred in to work it out.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#3 |
New Member
Join Date: Nov 2017
Posts: 27
Rep Power: 8 ![]() |
This is all the information I'm getting:
|
|
![]() |
![]() |
![]() |
![]() |
#4 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
Context is important. Please attach the entire output file.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#5 |
New Member
Join Date: Nov 2017
Posts: 27
Rep Power: 8 ![]() |
Output file is attached below:
|
|
![]() |
![]() |
![]() |
![]() |
#6 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
Now I can see the CCL is read correctly, the partitioner completes successfully and the run fails as it starts the solver.
I suggest you: * Run this single processor and see if it runs * If it does run single processor then check your parallel setup * If it does not run check you have adequate memory and disk space available
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#7 | |
New Member
Join Date: Nov 2017
Posts: 27
Rep Power: 8 ![]() |
Quote:
I tried running on single processor and this time the solver started, but crashed on the first iteration. This time I got a warning message saying insufficient memory allocated. So I guess we found the source of the problem (although strange since the exact same setup worked before and with 58 GB RAM available). After that I tried with "Large problem" checked and still single processor. Now it seems to work, but takes forever to iterate. Also tried allocating more memory and with parallel setup, but with no luck. I will try to decrease the number of elements in my mesh to make the problem smaller, but it is a problem that requires a very large fluid domain and also a very fine mesh around areas of special interest so this will likely decrease the accuracy of my simulations. Once again thank you for your help! |
||
![]() |
![]() |
![]() |
![]() |
#8 |
Senior Member
M
Join Date: Dec 2017
Posts: 692
Rep Power: 12 ![]() |
In execution control, there should be a solver -> solver memory -> memory allocation factor. Try to increase it like 1.2, 1.4, 1.6 until it works.
|
|
![]() |
![]() |
![]() |
![]() |
#9 |
New Member
Join Date: Nov 2017
Posts: 27
Rep Power: 8 ![]() |
||
![]() |
![]() |
![]() |
![]() |
#10 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
If the error is now about the integer stack size, this is because at the start of a run CFX estimates the memory it will use and allocates that space. If the estimate is very wrong it fills the space it will crash with a stack size error. Note that this can occur on quite small simulations as it is does not mean you have filled the physical memory - just the estimate CFX made at the start of the run.
So first try to increase the stack to 2 or maybe 3 times the original guess. There is no point going beyond 2 or 3 as if this does not work it means something is fundamentally wrong with your simulation and it is gobbling up all the space you allocate. This can be caused by excessively complex GGI interfaces, CCL which is too long, excessively complex CEL, too many boundary conditions and many other causes (but all to do with something being excessively complex)
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Fluent Adjoint Solver? | ex10148 | FLUENT | 16 | September 28, 2018 08:11 |
thobois class engineTopoChangerMesh error | Peter_600 | OpenFOAM | 4 | August 2, 2014 09:52 |
Divergence problem | Smaras | FLUENT | 13 | February 21, 2013 05:03 |
3d vof | Smaras | FLUENT | 2 | February 19, 2013 06:58 |
why the solver reject it? Anyone with experience? | bearcat | CFX | 6 | April 28, 2008 14:08 |