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

Solver can not produce result

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 15, 2013, 05:06
Default Solver can not produce result
  #1
New Member
 
Join Date: May 2013
Posts: 10
Rep Power: 4
dlugi91 is on a distinguished road
Hi All,
I am working on air flow over wing (subsonic and supersonic) and when I start solver, it worked few seconds and i see ,that message: "The solver failed with a non-zero exit code of: 2". After i can not edit setup because CFX-Pre have some error. When i try resolve this issue i saw that air does not flow through the connection of solids, which make up the model. But i don't know how connect this solids to air flow through them.

This is image of my model with marked faces in which i have problem.
dlugi91 is offline   Reply With Quote

Old   May 15, 2013, 06:31
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You either need to remesh to make the mesh regions join up or connect them with GGI interfaces.
ghorrocks is offline   Reply With Quote

Old   May 15, 2013, 15:54
Default
  #3
New Member
 
Join Date: May 2013
Posts: 10
Rep Power: 4
dlugi91 is on a distinguished road
I connect this regions with GGI interface and Solver start but in iteration 46 the same error show up. I don't know if I set properly this interface or it's diffferent issue. If i post details of this error from Ansys or output from Solver it will help in the aid?
dlugi91 is offline   Reply With Quote

Old   May 15, 2013, 18:24
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Please post your output file as an attachment, and some images of what you are seeing.
ghorrocks is offline   Reply With Quote

Old   May 17, 2013, 09:39
Default
  #5
New Member
 
Join Date: May 2013
Posts: 10
Rep Power: 4
dlugi91 is on a distinguished road
There is photo's, output file and error details:


Attached Files
File Type: zip error output.zip (12.0 KB, 4 views)
dlugi91 is offline   Reply With Quote

Old   May 17, 2013, 19:07
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Also what is the geometry? I have no idea what those blocks are. Some explanation would be useful.

You have had a divide by zero error. See this FAQ: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F
ghorrocks is offline   Reply With Quote

Old   May 19, 2013, 07:55
Default
  #7
New Member
 
Join Date: May 2013
Posts: 10
Rep Power: 4
dlugi91 is on a distinguished road
I want to simulate air flow over wing with subsonic and supersonic speed. I choose NACA 0009 profile to simple simulation. Midle block on geometry is space over a wing, left and right blocks are space in a front of wing and behind wing. My simulation is very similar to example in cfx tutorial (charper 10), so I modeled my geometry on this example. I mesh geometri and set boundaries like in this example and when I start solver for supersonic flow I see error, I wrote about early. So I make wrong geometry or mesh? Or I set wrong boundaries.
dlugi91 is offline   Reply With Quote

Old   May 19, 2013, 10:46
Default
  #8
New Member
 
Roland Su
Join Date: May 2013
Posts: 5
Rep Power: 4
Rolandy is on a distinguished road
Hi,
Your analysis relate to external flow field. In the case as you describe, if you surpress the solid the geometry or mesh is commenly no wrong. Notice your boundaries and interface setting.
Rolandy is offline   Reply With Quote

Old   May 19, 2013, 16:09
Default
  #9
New Member
 
Join Date: May 2013
Posts: 10
Rep Power: 4
dlugi91 is on a distinguished road
Settings of boundaries and interfaces are on output file in post #5.
dlugi91 is offline   Reply With Quote

Old   May 19, 2013, 19:33
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
To model this supersonic you will probably need local timescale factor (using about 5.0) to start the convergence along, and once that is going switch back to phyisical time scale. And the physical time scale will need to be very small.

And mesh quality will be important. If the mesh adjacent to the airfoil is not nice you will have problems with convergence.
ghorrocks is offline   Reply With Quote

Old   May 21, 2013, 01:59
Default
  #11
New Member
 
Roland Su
Join Date: May 2013
Posts: 5
Rep Power: 4
Rolandy is on a distinguished road
Your FLOW REGIME:
Option = Supersonic
and your MATERIAL: Air Ideal Gas
The Air Ideal Gas is an incompressible fluid, for supersonic flow, you must choose the "Air at 25C".
please try this....
Rolandy is offline   Reply With Quote

Old   May 21, 2013, 19:18
Default
  #12
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Sorry Roland, you got them the wrong way round. "Air at 25C" is an incompressible fluid. You need to select "Air ideal gas" to active the compressible flow model.
ghorrocks is offline   Reply With Quote

Old   May 21, 2013, 23:14
Default
  #13
New Member
 
Roland Su
Join Date: May 2013
Posts: 5
Rep Power: 4
Rolandy is on a distinguished road
Thanks ghorrocks, I have a wrong theory for ideal gas. Thank you!
But why dose the dlugi91's simulation have a non-linear P-Mass? Should he change the symmetrical bounderies to openning?
Rolandy is offline   Reply With Quote

Old   May 22, 2013, 05:57
Default
  #14
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Where does it say a non-linear P-Mass?
ghorrocks is offline   Reply With Quote

Old   May 23, 2013, 00:13
Default
  #15
New Member
 
Roland Su
Join Date: May 2013
Posts: 5
Rep Power: 4
Rolandy is on a distinguished road
OUTER LOOP ITERATION = 44 CPU SECONDS = 4.967E+01
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom | 0.28 | 1.6E-04 | 8.3E-03 | 2.8E-02 OK|
| V-Mom | 0.23 | 6.2E-04 | 2.5E-02 | 5.8E-02 OK|
| W-Mom | 0.23 | 5.0E-03 | 8.3E-02 | 4.3E-02 OK|
| P-Mass | 0.01 | 2.9E-05 | 2.5E-03 | 8.6 4.9E+02 F |
Rolandy is offline   Reply With Quote

Old   May 23, 2013, 06:31
Default
  #16
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
This is just non-cenvergence of the P-Mass equation. It means smaller time steps and/or better mesh quality is required.
ghorrocks is offline   Reply With Quote

Old   May 23, 2013, 08:58
Default
  #17
New Member
 
Roland Su
Join Date: May 2013
Posts: 5
Rep Power: 4
Rolandy is on a distinguished road
Even more about the case. I met a situation, the time steps and mesh were correct, but the W-Mom or p-mass was non-linear. When I reseted the inlet boundary, the problem was resolved.
Rolandy is offline   Reply With Quote

Old   May 24, 2013, 06:16
Default
  #18
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Have you read the section in the CFX documentation about setting up boundary conditions and obtaining convergence? This discusses all these issues.
ghorrocks is offline   Reply With Quote

Old   May 30, 2013, 09:13
Default
  #19
New Member
 
Join Date: May 2013
Posts: 10
Rep Power: 4
dlugi91 is on a distinguished road
I finish my simulation with using Fluent and 2D model. Thanks all for help
dlugi91 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
Creating New Solver: For particle-laden compressible jets sankarv OpenFOAM Running, Solving & CFD 17 December 3, 2014 20:41
OpenCL linear solver for OpenFoam 1.7 (alpha) will come out very soon qinmaple OpenFOAM Announcements from Other Sources 4 August 10, 2012 11:00
Working directory via command line Luiz CFX 4 March 6, 2011 21:02
How to compile an unsteady solver based on solver of MRFSimpleFoam? renyun0511 OpenFOAM Running, Solving & CFD 0 April 27, 2010 11:16
Creating New Solver: For particle-laden compressible jets sankarv OpenFOAM 0 April 4, 2010 18:06


All times are GMT -4. The time now is 06:21.