Re: [Xansys] [APDL][MEMORY] Ansys fails to allocate memory
32 GB of ram isn't much these days, but here are some suggestions:
You mentioned running 4 cores and 8 threads. Do you have hypterthreading turned on? If so, turn it off.
Are you using the launcher or command line? You should use the default memory management instead of setting the custom settings. In the launcher on the Customization/preferences tab, uncheck the box that says, "Use custom memory settings". When using the command line option, I see you have -m=24000 -db=20000 You are allocating 20000mb for database space, but allowing only 4000mb for solution scratch space. Remove both these options and let the program figure out what it needs within the available memory.
Use the default BCSOPTION and DSPOPTIONS. The default is to do partial in core and partial out of core based on available memory. You could be overconstraining the solver.
Joseph T Metrisin
Structures Lead
Florida Turbine Technologies, Inc
1701 Military Tr. Suite 110
Jupiter, FL 33458 U.S.A.
+1 (561)427-6346 Office
(561)427-6191 Fax
JMetrisin@fttinc.com
Visit our website: www.fttinc.com
FTT's public email encryption keys are stored on the FTT Verified Directory at http://keys.fttinc.com
Confidentiality Note:
The information contained in this transmission and any attachments are proprietary and may be privileged, intended only for the use of the individual or entity named above. If the reader of this message is not the intended recipient, you are hereby notified that any dissemination, distribution or copying of this communication is strictly prohibited. If you received this communication in error, please delete the message and immediately notify the sender via the contact information listed above.
-----Original Message-----
From: Germán Martínez [mailto:g.martinez-ayuso.841238@swansea.ac.uk]
Sent: Friday, August 11, 2017 7:20 AM
To: XANSYS Mailing List Temporary Home xansys-temp@xansystest.info
Subject: [FTT_SPAM] - [Xansys] [APDL][MEMORY] Ansys fails to allocate memory
Dear all,
I'm trying to run a big simulation in a Windows 10 machine (32GB of Ram, Xeon e3-1246 (4 cores, 8 threads), 24000 Virtual memory, Ansys installed in SSD, working folder in HHD). It's a composite wing beam
(shell281) with base excitation (large mass method) and with foam (naca, solid45) and a piezoelectric patch over (solid226). The piezoelectric patch is bonded to the shell elements using contact elements (conta174 and targe170) and it as a resistor (circu94) connected to the top and bottom layer of the patch. Most of the elements (76000 over 84203) are solid45.
Following the ansys contact technology guide, I setup the bonding like:
*get,max_elem_type_,ETYP, 0, num,max
target_elem_type_=max_elem_type_+1
ET,%target_elem_type_%,TARGE170
KEYOPT,target_elem_type_,5,5
*get,max_elem_type_,ETYP, 0, num,max
conta_elem_type_=max_elem_type_+1
ET,%conta_elem_type_%,CONTA174
! To define a shell-solid assembly using the internal MPC approach, you must set the following key options
! on the contact elements:
! KEYOPT(2) = 2 MPC-based approach
KEYOPT,conta_elem_type_,2,2
! KEYOPT(12) = 5 or 6 Bonded always or bonded initial
KEYOPT,conta_elem_type_,12,5
! KEYOPT(4) = 1 or 2 Nodal detection for CONTA171,
CONTA172, CONTA173, CONTA174 [1]
! KEYOPT(4) = 0 or 1 Contact normal direction for CONTA175
! KEYOPT,conta_elem_type_,4,1
!!!The following key options are ignored: KEYOPT(8), KEYOPT(10), KEYOPT(1) > 0.
! KEYOPT,conta_elem_type_,5,0 !Better use default.
! KEYOPT,conta_elem_type_,8,0 !Better use default.
! KEYOPT,conta_elem_type_,10,0 !Better use default.
! KEYOPT,conta_elem_type_,7,0
! Auto constraint type detection (default). Based on the underlying element type,
! this option automatically identifies the appropriate constraint type and internally sets KEYOPT(5)
! to the appropriate value: KEYOPT(5) = 1 for a solid-solid assembly; KEYOPT(5) = 2 for a shell-shell
! assembly; KEYOPT(5) = 3 for a shell-solid assembly
!
KEYOPT,conta_elem_type_,5,3
!! KEYOPT(9)
! Effect of initial penetration or gap:
! 0 -- Include both initial geometrical penetration or gap and offset
KEYOPT,conta_elem_type_,9,0
! KEYOPT(11)
! Shell thickness effect:
! 0 -- Exclude
! 1 -- Include
KEYOPT,conta_elem_type_,11,1
I detailed the contact because I think it could be helpful to understand the model.
The problem is when I'm trying to solve, Ansys fails to allocate extra memory. See error below:
*** ERROR *** CP = 475.453
TIME= 11:52:04
There is not enough memory for the Sparse Matrix Solver to proceed.
This is likely due to the use of pivoting while factoring the matrix.
Please increase the virtual memory on your system and/or increase the
work space memory and rerun the solver. Alternatively, using the
DSPOPTION command to switch to a different memory mode and/or to
specify additional memory for the solver may also help. The memory
currently allocated for the Sparse Matrix Solver solver = 612 MB.
I have tried to setup the BCSOPTION and DSPOPTION to:
DSPOPTION,default,default,24000, , ,performance !
BCSOPTION,,FORCE,24000,,,performance !
Although I think the DSPOPTION is only valid for clusters or similar.
So far no results, the memory is not getting expanded.
I tried also to run the MAPDL using commands:
! GUI
"C:\Program Files\ANSYS
Inc\v181\ANSYS\bin\winx64\ansys181.exe" -g -m 24000 -db 20000 -np 4 -dir "E:\wing_test2" -j "wing_test2"
But no luck. I even tried to change the solver, as the message complains about sparse and pivoting (is there a way to disable pivoting?). I tried the JCG and it goes pretty fast solving but the results show there is no voltage through the thickness of the patch.
Also, if I disable the solid45 elements from the simulation, I can solve with sparse (it's only 8000 elements) and I got voltage in the resistor. But of course, I need to include those solid45 elements in the simulation.
So, finally, does anyone have an idea how to help Ansys to allocate memory? Sorry for the long email.
Thanks very much in advance. Kind regards,
German Martinez-Ayuso
College of Engineering,
Swansea University
Wales (United Kingdom)
--
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.
Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list
I second all of Joe's recommendations. Especially the custom memory settings. If you request 24GB initially, ANSYS tries to grow the memory in increments of 24GB, so if there is 32 on the system, then next request will be for 48 GB and it will fail.
Are you actually running on 4 cores? If so then the memory requested is PER CORE, not total.
Lastly, I would consider using SOLID185 instead of SOLID45's. I don't know for sure, it is possible that the memory management is not as robust for the old elements as it is for the new elements.
-Jim
James J. Kosloski
Director of Engineering Services
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762
www.caeai.com
P: 203.758.2914 | F: 203.758.2965 | E: kosloski@caeai.com
-----Original Message-----
From: Metrisin, Joe (FTTINC) [mailto:JMetrisin@fttinc.com]
Sent: Friday, August 11, 2017 8:34 AM
To: XANSYS Mailing List Temporary Home xansys-temp@xansystest.info
Subject: Re: [Xansys] [APDL][MEMORY] Ansys fails to allocate memory
32 GB of ram isn't much these days, but here are some suggestions:
You mentioned running 4 cores and 8 threads. Do you have hypterthreading turned on? If so, turn it off.
Are you using the launcher or command line? You should use the default memory management instead of setting the custom settings. In the launcher on the Customization/preferences tab, uncheck the box that says, "Use custom memory settings". When using the command line option, I see you have -m=24000 -db=20000 You are allocating 20000mb for database space, but allowing only 4000mb for solution scratch space. Remove both these options and let the program figure out what it needs within the available memory.
Use the default BCSOPTION and DSPOPTIONS. The default is to do partial in core and partial out of core based on available memory. You could be overconstraining the solver.
Joseph T Metrisin
Structures Lead
Florida Turbine Technologies, Inc
1701 Military Tr. Suite 110
Jupiter, FL 33458 U.S.A.
+1 (561)427-6346 Office
(561)427-6191 Fax
JMetrisin@fttinc.com
Visit our website: www.fttinc.com
FTT's public email encryption keys are stored on the FTT Verified Directory at http://keys.fttinc.com
Confidentiality Note:
The information contained in this transmission and any attachments are proprietary and may be privileged, intended only for the use of the individual or entity named above. If the reader of this message is not the intended recipient, you are hereby notified that any dissemination, distribution or copying of this communication is strictly prohibited. If you received this communication in error, please delete the message and immediately notify the sender via the contact information listed above.
-----Original Message-----
From: Germán Martínez [mailto:g.martinez-ayuso.841238@swansea.ac.uk]
Sent: Friday, August 11, 2017 7:20 AM
To: XANSYS Mailing List Temporary Home xansys-temp@xansystest.info
Subject: [FTT_SPAM] - [Xansys] [APDL][MEMORY] Ansys fails to allocate memory
Dear all,
I'm trying to run a big simulation in a Windows 10 machine (32GB of Ram, Xeon e3-1246 (4 cores, 8 threads), 24000 Virtual memory, Ansys installed in SSD, working folder in HHD). It's a composite wing beam
(shell281) with base excitation (large mass method) and with foam (naca, solid45) and a piezoelectric patch over (solid226). The piezoelectric patch is bonded to the shell elements using contact elements (conta174 and targe170) and it as a resistor (circu94) connected to the top and bottom layer of the patch. Most of the elements (76000 over 84203) are solid45.
Following the ansys contact technology guide, I setup the bonding like:
*get,max_elem_type_,ETYP, 0, num,max
target_elem_type_=max_elem_type_+1
ET,%target_elem_type_%,TARGE170
KEYOPT,target_elem_type_,5,5
*get,max_elem_type_,ETYP, 0, num,max
conta_elem_type_=max_elem_type_+1
ET,%conta_elem_type_%,CONTA174
! To define a shell-solid assembly using the internal MPC approach, you must set the following key options
! on the contact elements:
! KEYOPT(2) = 2 MPC-based approach
KEYOPT,conta_elem_type_,2,2
! KEYOPT(12) = 5 or 6 Bonded always or bonded initial
KEYOPT,conta_elem_type_,12,5
! KEYOPT(4) = 1 or 2 Nodal detection for CONTA171,
CONTA172, CONTA173, CONTA174 [1]
! KEYOPT(4) = 0 or 1 Contact normal direction for CONTA175
! KEYOPT,conta_elem_type_,4,1
!!!The following key options are ignored: KEYOPT(8), KEYOPT(10), KEYOPT(1) > 0.
! KEYOPT,conta_elem_type_,5,0 !Better use default.
! KEYOPT,conta_elem_type_,8,0 !Better use default.
! KEYOPT,conta_elem_type_,10,0 !Better use default.
! KEYOPT,conta_elem_type_,7,0
! Auto constraint type detection (default). Based on the underlying element type,
! this option automatically identifies the appropriate constraint type and internally sets KEYOPT(5)
! to the appropriate value: KEYOPT(5) = 1 for a solid-solid assembly; KEYOPT(5) = 2 for a shell-shell
! assembly; KEYOPT(5) = 3 for a shell-solid assembly
!
KEYOPT,conta_elem_type_,5,3
!! KEYOPT(9)
! Effect of initial penetration or gap:
! 0 -- Include both initial geometrical penetration or gap and offset
KEYOPT,conta_elem_type_,9,0
! KEYOPT(11)
! Shell thickness effect:
! 0 -- Exclude
! 1 -- Include
KEYOPT,conta_elem_type_,11,1
I detailed the contact because I think it could be helpful to understand the model.
The problem is when I'm trying to solve, Ansys fails to allocate extra memory. See error below:
*** ERROR *** CP = 475.453
TIME= 11:52:04
There is not enough memory for the Sparse Matrix Solver to proceed.
This is likely due to the use of pivoting while factoring the matrix.
Please increase the virtual memory on your system and/or increase the
work space memory and rerun the solver. Alternatively, using the
DSPOPTION command to switch to a different memory mode and/or to
specify additional memory for the solver may also help. The memory
currently allocated for the Sparse Matrix Solver solver = 612 MB.
I have tried to setup the BCSOPTION and DSPOPTION to:
DSPOPTION,default,default,24000, , ,performance !
BCSOPTION,,FORCE,24000,,,performance !
Although I think the DSPOPTION is only valid for clusters or similar.
So far no results, the memory is not getting expanded.
I tried also to run the MAPDL using commands:
! GUI
"C:\Program Files\ANSYS
Inc\v181\ANSYS\bin\winx64\ansys181.exe" -g -m 24000 -db 20000 -np 4 -dir "E:\wing_test2" -j "wing_test2"
But no luck. I even tried to change the solver, as the message complains about sparse and pivoting (is there a way to disable pivoting?). I tried the JCG and it goes pretty fast solving but the results show there is no voltage through the thickness of the patch.
Also, if I disable the solid45 elements from the simulation, I can solve with sparse (it's only 8000 elements) and I got voltage in the resistor. But of course, I need to include those solid45 elements in the simulation.
So, finally, does anyone have an idea how to help Ansys to allocate memory? Sorry for the long email.
Thanks very much in advance. Kind regards,
German Martinez-Ayuso
College of Engineering,
Swansea University
Wales (United Kingdom)
--
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.
Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list _______________________________________________
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.
Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list
This email and any attachments may contain privileged or confidential information of Computer Aided Engineering Associates. This e-mail is intended solely for the use of the individual or entity to which it is addressed. If you are not the intended recipient of this e-mail, you are hereby notified that any copying, distribution, dissemination or action taken in relation to the contents of this e-mail and any of its attachments is strictly prohibited and may be unlawful. If you have received this e-mail in error, please notify the sender immediately and permanently delete the original e-mail and destroy any copies or printouts of this e-mail as well as any attachments.