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

CFX-Solver

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 26, 2012, 09:46
Default
  #21
Member
 
Peter Galimutti
Join Date: May 2012
Posts: 37
Rep Power: 6
p.galimutti is on a distinguished road
i got this error few days ago! then I used a different computer and it worked, besides problem setup, it seems to me that it might be because of some missing files or memory problems. the other computer is a server and it just worked fine. try re-installing ansys or increase your system resources.
in the solver manager increase the memory allocation from default 1.0 to 2.0
p.galimutti is offline   Reply With Quote

Old   June 26, 2012, 10:17
Default
  #22
Senior Member
 
Join Date: Jul 2011
Location: Berlin, Germany
Posts: 150
Rep Power: 6
monkey1 is on a distinguished road
For me it still sounds like wrong BC settings or maybe even domain initialisations. The fact that cfx is running and trying to place a wall on the inlet to prevent flow from flowing OUT does not sound like files missing or insufficient memory but simply physically wring boundary conditions.

shanxuewenjdx maybe you could specify how you defined the BC's (inlet/outlet etc.)??? and the domain initialisations? Just wondering if you maybe have defined a higher pressure on the opening side than on the inlet side wich would cause a "reverse" flow...presuming that your gears are able to rotate and are not static.
monkey1 is offline   Reply With Quote

Old   June 26, 2012, 11:00
Default
  #23
Member
 
Luis Filipe Fabiani
Join Date: Apr 2009
Posts: 43
Rep Power: 9
lffabiani is on a distinguished road
Stefan, maybe this thread helps: Error message CFX Solver

Glenn was suggesting that maybe the solver has diverged (or did some division by 0) which caused the solver to crash.

Have you done a sensitivity check on the mesh? How many elements does it have? What is the Courant number for your simulation?

Best regards
lffabiani is offline   Reply With Quote

Old   June 27, 2012, 07:51
Default
  #24
Member
 
Join Date: Dec 2009
Posts: 38
Rep Power: 8
cfdgremlin is on a distinguished road
Are you running in parallel? I have seen this behaviour occcasionally from parallel runs of the CFX-Solver, in that the real problem is disguised, and associated messages are not output.

If you can run it in serial, and there is a problem with the setup, then the solver should write some messages which are more useful than just 'error code 255'.

CG
cfdgremlin is offline   Reply With Quote

Old   June 27, 2012, 22:34
Default
  #25
Member
 
Stefan
Join Date: May 2012
Posts: 48
Rep Power: 6
shanxuewenjdx is on a distinguished road
Quote:
Originally Posted by cfdgremlin View Post
Are you running in parallel? I have seen this behaviour occcasionally from parallel runs of the CFX-Solver, in that the real problem is disguised, and associated messages are not output.

If you can run it in serial, and there is a problem with the setup, then the solver should write some messages which are more useful than just 'error code 255'.

CG
many thanks!
I run it in serial. But if it was something with my setup,is it related to my inlet(I set it 0MPa) or outlet(20MPa)? After reading the CFX-help file ,it is recommended that inlet:0MPa,outlet:2.667kg/s according to the real situation.But it still can't be right
shanxuewenjdx is offline   Reply With Quote

Old   July 1, 2012, 21:19
Default
  #26
Member
 
Stefan
Join Date: May 2012
Posts: 48
Rep Power: 6
shanxuewenjdx is on a distinguished road
Hi,guys. I forgot the mesh statitics in CFX-SOLVER when the solver failed to solve the simulation. So is it for sure that the failure is caused by coarse mesh?
Attached Images
File Type: jpg 未命名.jpg (78.0 KB, 11 views)
shanxuewenjdx is offline   Reply With Quote

Old   July 1, 2012, 21:28
Default
  #27
Member
 
Stefan
Join Date: May 2012
Posts: 48
Rep Power: 6
shanxuewenjdx is on a distinguished road
the picture I copied from CFX-solver
Attached Images
File Type: jpg 未命名2.jpg (51.5 KB, 6 views)
File Type: jpg 未命名1.jpg (50.2 KB, 6 views)
File Type: jpg 未命名3.jpg (61.9 KB, 5 views)
File Type: jpg 未命名4.jpg (67.1 KB, 5 views)
File Type: jpg 未命名5.jpg (66.9 KB, 5 views)
shanxuewenjdx is offline   Reply With Quote

Old   July 1, 2012, 21:30
Default
  #28
Member
 
Stefan
Join Date: May 2012
Posts: 48
Rep Power: 6
shanxuewenjdx is on a distinguished road
And some other pictures
Attached Images
File Type: jpg 未命名6.jpg (74.6 KB, 6 views)
File Type: jpg 未命名.jpg (78.0 KB, 4 views)
shanxuewenjdx is offline   Reply With Quote

Old   July 2, 2012, 08:36
Default
  #29
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,274
Rep Power: 96
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
The average density of your fluid is 9e-7. Are you sure this is correct?
ghorrocks is offline   Reply With Quote

Old   July 2, 2012, 09:04
Default
  #30
Member
 
Stefan
Join Date: May 2012
Posts: 48
Rep Power: 6
shanxuewenjdx is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
The average density of your fluid is 9e-7. Are you sure this is correct?
I chose water as fluid material.anything wrong?
shanxuewenjdx is offline   Reply With Quote

Old   July 2, 2012, 12:17
Default
  #31
Member
 
Luis Filipe Fabiani
Join Date: Apr 2009
Posts: 43
Rep Power: 9
lffabiani is on a distinguished road
Well, given that water has a density of about 1.000 kg/m3 at room temperature and it is incompresible, 9e-7 sure means something is wrong.

What are the Inlet conditions?? In CFD-Post plot some variables (temperature, velocities, etc) to check if the problem is on a specific area of your domain.
lffabiani is offline   Reply With Quote

Old   July 2, 2012, 18:57
Default
  #32
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,274
Rep Power: 96
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I suspect that you are using 0 reference pressure and almost zero inlet/outlet pressure, leading to very low density fluid as the pressure is just about absolute zero. The reference pressure needs to be set at a suitable level for the simulation - if this thing is close to atmospheric pressure then use 1 [atm] for the reference pressure.
ghorrocks is offline   Reply With Quote

Old   July 2, 2012, 22:42
Default
  #33
Member
 
Stefan
Join Date: May 2012
Posts: 48
Rep Power: 6
shanxuewenjdx is on a distinguished road
Follows are my further information in my cfx-pre
Attached Images
File Type: jpg 未命名1.jpg (60.7 KB, 4 views)
File Type: jpg 未命名2.jpg (76.4 KB, 4 views)
File Type: jpg 未命名3.jpg (30.2 KB, 4 views)
File Type: jpg 未命名4.jpg (50.5 KB, 4 views)
File Type: jpg 未命名5.jpg (51.5 KB, 4 views)
shanxuewenjdx is offline   Reply With Quote

Old   July 2, 2012, 22:43
Default
  #34
Member
 
Stefan
Join Date: May 2012
Posts: 48
Rep Power: 6
shanxuewenjdx is on a distinguished road
And these pictures.
Attached Images
File Type: jpg 未命名6.jpg (50.9 KB, 2 views)
File Type: jpg 未命名7.jpg (24.2 KB, 2 views)
File Type: jpg 未命名8.jpg (35.6 KB, 2 views)
File Type: jpg 未命名9.jpg (35.0 KB, 2 views)
shanxuewenjdx is offline   Reply With Quote

Old   July 2, 2012, 22:50
Default
  #35
Member
 
Stefan
Join Date: May 2012
Posts: 48
Rep Power: 6
shanxuewenjdx is on a distinguished road
Quote:
Originally Posted by lffabiani View Post
Well, given that water has a density of about 1.000 kg/m3 at room temperature and it is incompresible, 9e-7 sure means something is wrong.

What are the Inlet conditions?? In CFD-Post plot some variables (temperature, velocities, etc) to check if the problem is on a specific area of your domain.
Thanks a lot. For more information, u can see more pictures above.the Inlet:2.37m/s.
As to the density of fluid,is the pre-setting I have finished is wrong or the cfx-solver itself?
shanxuewenjdx is offline   Reply With Quote

Old   July 2, 2012, 22:51
Default
  #36
Member
 
Stefan
Join Date: May 2012
Posts: 48
Rep Power: 6
shanxuewenjdx is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
I suspect that you are using 0 reference pressure and almost zero inlet/outlet pressure, leading to very low density fluid as the pressure is just about absolute zero. The reference pressure needs to be set at a suitable level for the simulation - if this thing is close to atmospheric pressure then use 1 [atm] for the reference pressure.
So kind you are. u can check further information from the above pictures.
shanxuewenjdx is offline   Reply With Quote

Old   July 3, 2012, 14:28
Default
  #37
Member
 
Luis Filipe Fabiani
Join Date: Apr 2009
Posts: 43
Rep Power: 9
lffabiani is on a distinguished road
Correct me if I am wrong, but it does not seem that the gears are turning. How can there be a flow if the gears are not turning?
lffabiani is offline   Reply With Quote

Old   July 3, 2012, 19:09
Default
  #38
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,274
Rep Power: 96
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I see your inlet and outlet are both 20MPa, and your reference pressure is 1atm. In that case you should use a reference pressure of 20.1MPa and an inlet and outlet pressure of 0 Pa.
ghorrocks is offline   Reply With Quote

Old   July 3, 2012, 23:49
Default
  #39
Member
 
Stefan
Join Date: May 2012
Posts: 48
Rep Power: 6
shanxuewenjdx is on a distinguished road
Quote:
Originally Posted by lffabiani View Post
Correct me if I am wrong, but it does not seem that the gears are turning. How can there be a flow if the gears are not turning?
The gear1 and gear2 are turning around their geometric centers respectively. the angular velocity both are 2000r/min,u can check that.
shanxuewenjdx is offline   Reply With Quote

Old   July 3, 2012, 23:53
Default
  #40
Member
 
Stefan
Join Date: May 2012
Posts: 48
Rep Power: 6
shanxuewenjdx is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
I see your inlet and outlet are both 20MPa, and your reference pressure is 1atm. In that case you should use a reference pressure of 20.1MPa and an inlet and outlet pressure of 0 Pa.
Thanks. there are 3 boundaries: inlet,outlet,inletsmall(you can check the first picture attached under the thread).the inlet:2.37m/s;outlet(opening) 20MPa;inletsmall(close to the outlet;set as opening )20MPa.The inletsmall I have modified ,not as OUTLET type
shanxuewenjdx is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Error message CFX Solver Fatnes CFX 25 July 3, 2015 10:32
CFX SOLVER error !!! mehrdadeng CFX 3 November 23, 2009 17:42
mach number and CFX 11.0 solver turbinesv CFX 5 January 5, 2009 06:43
CFX Solver to run 10 files sequentially Raj CFX 8 October 29, 2008 23:20
problem in CFX solver about isolated volumes Yuan CFX 2 August 16, 2004 22:54


All times are GMT -4. The time now is 10:19.