CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Simulation doesn’t proceed

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 7, 2015, 03:22
Question Simulation doesn’t proceed
  #1
Senior Member
 
Anna Tian's Avatar
 
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 14
Anna Tian is on a distinguished road
I run CFX simulation by workbench. After I start to run the simulation, the simulation stuck at the message:

‘The MeTiS partitioning method allocates additional memory. Total memory usage will therefore exceed the values shown above.’

Then the simulation doesn’t proceed anymore.

I’m quite sure that I shall have enough memory (128 GB) available for that simulation (16 millions structured grids from ICEM, steady state SST).

The bad thing is: it doesn't give any error information. So that I have no clue what causes the problem and how to solve it.

I’m wondering what’s the reason of it? And how to solve this problem? Any hint?
__________________
Best regards,
Meimei
Anna Tian is offline   Reply With Quote

Old   July 7, 2015, 04:56
Default
  #2
Member
 
Jinwhan Ryuk
Join Date: Feb 2013
Location: South Korea
Posts: 91
Rep Power: 11
Whitebear is on a distinguished road
Do you have enough parallel licenses? Have you try to change memory allocation factor? 1.2x or 1.5x in solver option? Do you solve multiphase or multicomponent problem?
Whitebear is offline   Reply With Quote

Old   July 7, 2015, 05:41
Default
  #3
Senior Member
 
Anna Tian's Avatar
 
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 14
Anna Tian is on a distinguished road
Quote:
Originally Posted by Whitebear View Post
Do you have enough parallel licenses? Have you try to change memory allocation factor? 1.2x or 1.5x in solver option? Do you solve multiphase or multicomponent problem?
I have checked with another simulation that my machine has enough parallel licenses. I'm solving single phase problem with 2 domains defined (GGI as interface). Another simulation with 2 domains could run without problem.

I haven't tried memory allocation factor, because i never got a hint that tells memory is not enough.
__________________
Best regards,
Meimei
Anna Tian is offline   Reply With Quote

Old   July 7, 2015, 05:56
Default
  #4
Senior Member
 
Anna Tian's Avatar
 
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 14
Anna Tian is on a distinguished road
Quote:
Originally Posted by Whitebear View Post
Do you have enough parallel licenses? Have you try to change memory allocation factor? 1.2x or 1.5x in solver option? Do you solve multiphase or multicomponent problem?

Just tried memory allocation factor of 0.8 and 1.5. Not working
__________________
Best regards,
Meimei
Anna Tian is offline   Reply With Quote

Old   July 7, 2015, 06:00
Default
  #5
Member
 
Jinwhan Ryuk
Join Date: Feb 2013
Location: South Korea
Posts: 91
Rep Power: 11
Whitebear is on a distinguished road
Do you have many interger interfaces? What is the differences between the two problems?
Whitebear is offline   Reply With Quote

Old   July 7, 2015, 06:26
Default
  #6
Senior Member
 
Anna Tian's Avatar
 
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 14
Anna Tian is on a distinguished road
Quote:
Originally Posted by Whitebear View Post
Do you have many interger interfaces? What is the differences between the two problems?
There are two domains (named domain1, domain2) connected by a GGI interface. This is what I want to run. I run it, get problem specified above.

So I did the tests as below.

I run only domain1, no that problem.

I run only domain2, no that problem.

I create a simple domain3. Connect domain1 and domain3 by GGI. Working.
__________________
Best regards,
Meimei
Anna Tian is offline   Reply With Quote

Old   July 7, 2015, 06:27
Default
  #7
Senior Member
 
Anna Tian's Avatar
 
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 14
Anna Tian is on a distinguished road
Quote:
Originally Posted by Whitebear View Post
Do you have many interger interfaces? What is the differences between the two problems?
This is another problem i found out at the same time. It might be related to this one.

http://www.cfd-online.com/Forums/cfx...rted-icem.html
__________________
Best regards,
Meimei
Anna Tian is offline   Reply With Quote

Old   July 7, 2015, 06:48
Default
  #8
Senior Member
 
Anna Tian's Avatar
 
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 14
Anna Tian is on a distinguished road
Quote:
Originally Posted by Whitebear View Post
Do you have many interger interfaces? What is the differences between the two problems?
I figure out that the 'problematic' simulation could run actually. It is not stuck there as I said before. But it takes more than 5 hours to start. Too slow.

Never got this 'slow' problem before at the same workstation. So it shall not be caused by hardware.
__________________
Best regards,
Meimei
Anna Tian is offline   Reply With Quote

Old   July 7, 2015, 19:46
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,265
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Very complex configurations can take ages to start. For instance lots of GGIs or boundaries, lots of CEL, lots of additional variables.
ghorrocks is offline   Reply With Quote

Old   July 7, 2015, 22:18
Question
  #10
Senior Member
 
Anna Tian's Avatar
 
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 14
Anna Tian is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Very complex configurations can take ages to start. For instance lots of GGIs or boundaries, lots of CEL, lots of additional variables.
Is there a good way to reduce the too long starting time besides reducing these factors you mentioned?
__________________
Best regards,
Meimei
Anna Tian is offline   Reply With Quote

Old   July 7, 2015, 22:26
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,265
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
ANSYS has already worked hard to make simulations start as quickly as possible. There are no quick fixes to make it go faster, if there were they would already be in the software.

There must be something about your simulation which is causing the very long start time. If you want us to help you you will have to describe what you are doing.

For instance: How many nodes in your mesh? How many boundaries, GGIs and anything else you have set up?
ghorrocks is offline   Reply With Quote

Old   July 7, 2015, 23:17
Default
  #12
Senior Member
 
Anna Tian's Avatar
 
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 14
Anna Tian is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
ANSYS has already worked hard to make simulations start as quickly as possible. There are no quick fixes to make it go faster, if there were they would already be in the software.

There must be something about your simulation which is causing the very long start time. If you want us to help you you will have to describe what you are doing.

For instance: How many nodes in your mesh? How many boundaries, GGIs and anything else you have set up?
17millions structured grids nodes. 15 boundaries. 30 expressions.
__________________
Best regards,
Meimei
Anna Tian is offline   Reply With Quote

Old   July 8, 2015, 00:16
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,265
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
17 million grids (elements?) is getting large, but should not take 5 hours to start unless you have run out of memory or some other problem.

I would do some basic fault finding. Take a simple simulation (like a tutorial example) and make it 17 million elements. Does it run quickly? Remesh your simulation with half the number of elements - does it start quickly?
ghorrocks is offline   Reply With Quote

Old   July 8, 2015, 00:23
Default
  #14
Senior Member
 
Anna Tian's Avatar
 
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 14
Anna Tian is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
17 million grids (elements?) is getting large, but should not take 5 hours to start unless you have run out of memory or some other problem.

I would do some basic fault finding. Take a simple simulation (like a tutorial example) and make it 17 million elements. Does it run quickly? Remesh your simulation with half the number of elements - does it start quickly?
Yes. I tried. It would be much faster if I coarsening grids.

By the way, once I have run the simulation and use its result file as initial solution of a new simulation. The simulation would start very fast without any problem.

So I guess maybe that's because the initial solution grids of the 'too slow' simulation do not correspond to the new simulation.

I asked the question below as well for this reason.

http://www.cfd-online.com/Forums/cfx...nning-cfx.html
__________________
Best regards,
Meimei
Anna Tian is offline   Reply With Quote

Old   July 8, 2015, 00:26
Default
  #15
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,265
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Quote:
Yes. I tried. It would be much faster if I coarsening grids.
No, you have missed the point. It is trying to work out whether it is simply the size of the simulation which is the problem or your problem specifically, regardless of the size.

Quote:
So I guess maybe that's because the initial solution grids of the 'too slow' simulation do not correspond to the new simulation.
If you are using an initial condition which requires interpolation this can be very slow, especially for large grids. That would explain the problem.
ghorrocks is offline   Reply With Quote

Old   July 8, 2015, 03:31
Question
  #16
Senior Member
 
Anna Tian's Avatar
 
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 14
Anna Tian is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
No, you have missed the point. It is trying to work out whether it is simply the size of the simulation which is the problem or your problem specifically, regardless of the size.


If you are using an initial condition which requires interpolation this can be very slow, especially for large grids. That would explain the problem.
Then how to avoid slow interpolation in workbench?
__________________
Best regards,
Meimei
Anna Tian is offline   Reply With Quote

Old   July 8, 2015, 04:06
Default
  #17
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,265
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Do not specify an initial condition results file. Leave it blank.
ghorrocks is offline   Reply With Quote

Old   July 8, 2015, 11:12
Default
  #18
Senior Member
 
Anna Tian's Avatar
 
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 14
Anna Tian is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Do not specify an initial condition results file. Leave it blank.
Yes. I the default setting of Workbench cfx pre is blank as shown in the figure attached.

But it actually uses one as I got the following lines in the output file.


INITIAL VALUES SPECIFICATION:
INITIAL VALUES CONTROL:
Use Mesh From = Solver Input File
Continue History From = Workbench Initial Values
END
INITIAL VALUES: Workbench Initial Values
Option = Results File
File Name = 20_fine_019.res
END
END
END


If I change the setting, i will get the error message as stated in the thread below.

http://www.cfd-online.com/Forums/cfx...nning-cfx.html
Attached Images
File Type: jpg 1.jpg (11.7 KB, 7 views)
__________________
Best regards,
Meimei
Anna Tian is offline   Reply With Quote

Old   July 8, 2015, 11:43
Default
  #19
Senior Member
 
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 511
Rep Power: 19
singer1812 is on a distinguished road
Lets go back to your original warning. Did you increase the amount of memory for the "partitioner" (not the run, there is a difference)?

I dont use Solver Manager to start my jobs but in command line it is:

-size-part <factor>

I have had to increase this with 2 domain GGI runs before as CFXs estimate is low.

The command -size will just increase the solver memory, but not alter the allocation for the partitioner.
singer1812 is offline   Reply With Quote

Old   July 9, 2015, 04:20
Default
  #20
Senior Member
 
Anna Tian's Avatar
 
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 14
Anna Tian is on a distinguished road
Quote:
Originally Posted by singer1812 View Post
Lets go back to your original warning. Did you increase the amount of memory for the "partitioner" (not the run, there is a difference)?

I dont use Solver Manager to start my jobs but in command line it is:

-size-part <factor>

I have had to increase this with 2 domain GGI runs before as CFXs estimate is low.

The command -size will just increase the solver memory, but not alter the allocation for the partitioner.
Yes. I once tried by increasing the allocation factor to 1.5. It still reacts slow if it use another simulation's result file as the initial solution.

According to the discussions above, there's no hint that the problem is caused by lack of memory up to what we see now.
__________________
Best regards,
Meimei
Anna Tian is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Waterbell Simulation o.b.m Fluent Multiphase 1 November 5, 2015 06:55
mass flow rate issue in supersonic nozzle simulation xkang FLUENT 0 July 31, 2014 17:06
Simulation of a complex wing in solidworks flow simulation niels1900 FloEFD, FloWorks & FloTHERM 6 April 20, 2011 11:44
GUI crash and simulation engine still running RPJones FLOW-3D 2 November 9, 2010 09:18
3-D Contaminant Dispersal Simulation Apple L S Chan Main CFD Forum 1 December 23, 1998 11:06


All times are GMT -4. The time now is 13:43.