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

Refiner Error 255

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 29, 2010, 02:05
Default Refiner Error 255
  #1
New Member
 
Alex
Join Date: Mar 2010
Location: Russia
Posts: 19
Rep Power: 7
a.m. is on a distinguished road
Send a message via ICQ to a.m.
Hello All,

I try to model CH4 combustion and I'd like to make mesh adaption in the reaction region. Hence, I set up CH4.Mass Fraction as adaption criteria in CFX12 Pre. Mesh Adaption was started every 10 iterations.
While solver was running, Refiner has started and terminated with the message:

"An error has occurred in cfx5solve:

The ANSYS CFX mesh refiner could not be started, or exited with return code 255:"

Before that one I've recived a windows send report message about refiner.

What does code 255 means?
When it usually appears?

Regards, A.m.
a.m. is offline   Reply With Quote

Old   March 31, 2010, 10:23
Default
  #2
New Member
 
zhao xin
Join Date: Feb 2010
Location: Goteborg
Posts: 28
Rep Power: 7
zxin is on a distinguished road
what i can tell you is, last time I encountered this error code is because of large aspect ratio which exceeded the limit.

Hope this would help..
zxin is offline   Reply With Quote

Old   April 1, 2010, 02:54
Default
  #3
New Member
 
Alex
Join Date: Mar 2010
Location: Russia
Posts: 19
Rep Power: 7
a.m. is on a distinguished road
Send a message via ICQ to a.m.
Thanks zxin,

I've solved this problem by mesh changing. First time I used ANSYS Meshing to generate mesh. I checked its quality in ICEM CFD and received following results: min = 0.013, max = 23.05, mean = 1.87 (aspect ratio).
Then I generated ICEM CFD mesh and checked it. I received following:
min = 0.25, max = 0.99, mean = 0.75 (aspect ratio). Also I decreased a numer of elements by a factor of 1.8 and removed prism layers (inflantion).
With the new mesh remesher works perfectly.

P.S.
old mesh

new mesh
a.m. is offline   Reply With Quote

Old   April 1, 2010, 03:51
Default
  #4
New Member
 
zhao xin
Join Date: Feb 2010
Location: Goteborg
Posts: 28
Rep Power: 7
zxin is on a distinguished road
That's great...
but sometimes, my mesh with aspect ratio close to 1000 generated by Ansys Mesh, works fine with CFX, CFX is quite stable solver, i think...
zxin is offline   Reply With Quote

Old   April 1, 2010, 06:32
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,954
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
But with no prism layers your boundary layer modelling will be hopeless. You clearly have a mesh quality problem, but you need to generate a high quality mesh with prism layers.
ghorrocks is offline   Reply With Quote

Old   April 1, 2010, 08:25
Default
  #6
New Member
 
Alex
Join Date: Mar 2010
Location: Russia
Posts: 19
Rep Power: 7
a.m. is on a distinguished road
Send a message via ICQ to a.m.
I' m modeling the CH4 combustion process, therefore finer stoichiometric region is more important for me then boundary layer.
a.m. is offline   Reply With Quote

Old   April 2, 2010, 06:07
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,954
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Isn't the heat transfer important? Won't that set the heat lost to the walls, and be a major contributor to combustion temperature? You will need a good prism layer mesh to resolve that.
ghorrocks is offline   Reply With Quote

Old   April 2, 2010, 08:04
Default
  #8
New Member
 
Alex
Join Date: Mar 2010
Location: Russia
Posts: 19
Rep Power: 7
a.m. is on a distinguished road
Send a message via ICQ to a.m.
Thanks ghorrocks,

Sure it is very important too and I'm working on it By the way, how many prism layers I need to resolve the wall heat transfer?
a.m. is offline   Reply With Quote

Old   April 3, 2010, 06:31
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,954
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
That's problem dependent. The discussion in the CFX documentation on near-wall modelling is a good starting point, but you then need to do a sensitivity study to find out what your specific case requires.
ghorrocks is offline   Reply With Quote

Old   April 4, 2010, 03:57
Default
  #10
New Member
 
Alex
Join Date: Mar 2010
Location: Russia
Posts: 19
Rep Power: 7
a.m. is on a distinguished road
Send a message via ICQ to a.m.
Thanks a lot!
a.m. is offline   Reply With Quote

Old   August 3, 2010, 20:38
Default Error Code 255
  #11
New Member
 
Maritime Systems Engineering
Join Date: Jul 2010
Posts: 13
Rep Power: 7
OffshoreStructuralEnginer is on a distinguished road
I do not know what Error code 255 means. Im not an expert at Ansys or CFD. But I do know that it has been solved, every single time, by deleting my mesh and remeshing with new settings. I am not saying you should do this. If you are truly desperate you may give it a try.
OffshoreStructuralEnginer is offline   Reply With Quote

Old   August 8, 2010, 04:22
Default Error 255
  #12
Senior Member
 
Ugly Kid Joe
Join Date: Aug 2010
Posts: 193
Rep Power: 7
vmlxb6 is on a distinguished road
What kind of meshing is advisable to solve the ERROR code 255 ???

I am using ICEM CFD to mesh my geometry. Am ugetting the following error
"The ANSYS CFX solver could not be started, or exited with return |
| code 255: . No results file has been created."

Now am using the following:

Mesh type on surface: All Tri
Mesh type in volume: Tetra/Mixed
surface Mesh method: Patch Independent
volume Mesh method: Robust (octree)

Thank you very much
vmlxb6 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



All times are GMT -4. The time now is 03:30.