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

CFX solver manager quits with error code 255

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

Like Tree1Likes
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   November 1, 2012, 10:23
Default CFX solver manager quits with error code 255
  #1
Member
 
Shuvayan Brahmachary
Join Date: Oct 2012
Posts: 34
Rep Power: 4
b.shuvayan is on a distinguished road
hi everyone!

I encountered a problem while solving it in ANSYS solver manager. The geometry is a cube and inside of which at the centre is a Hole (sphere slice section). After creating successfully the geo. and mesh and also specifying the boundary condition in the domain...THE SOLVER MANAGER QUITS WITH RETURN CODE 255 ( and no error file is generated to read the details from).

I am hoping for any suggestions. any help would really be appreciated.
Thanks in advance
b.shuvayan is offline   Reply With Quote

Old   November 1, 2012, 12:37
Default
  #2
Member
 
Shuvayan Brahmachary
Join Date: Oct 2012
Posts: 34
Rep Power: 4
b.shuvayan is on a distinguished road
Might as well have a look at the boundary conditions:

Mach NO. 8 so velocity (for Ideal gas) comes around 1272.8 m/s

Inlet conditions- Super sonic

Relative Static Pressure- 59 Pa

But I later changed it to very low value

5m/s
Subsonic
1 Pa

Still I'm having the same problem. Is it due to the geometry or mesh??

Geometry consisting of a cube and a hollow sphere.jpg

Mesh by milti zone.jpg
b.shuvayan is offline   Reply With Quote

Old   November 1, 2012, 16:40
Default
  #3
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
Can you post your CCL file?
ghorrocks is offline   Reply With Quote

Old   November 2, 2012, 02:59
Default
  #4
Member
 
Shuvayan Brahmachary
Join Date: Oct 2012
Posts: 34
Rep Power: 4
b.shuvayan is on a distinguished road
I have a RAR file for the .wbpz project file. How do I upload here because the size is too big to attact here and its an invalid file extension for cfd-online.

can u suggest something?
b.shuvayan is offline   Reply With Quote

Old   November 2, 2012, 04:04
Default
  #5
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 536
Rep Power: 11
Lance is on a distinguished road
In CFX-pre: file/export ccl
Upload the .ccl file here as it is only text.
Lance is online now   Reply With Quote

Old   November 3, 2012, 14:55
Default
  #6
Member
 
Shuvayan Brahmachary
Join Date: Oct 2012
Posts: 34
Rep Power: 4
b.shuvayan is on a distinguished road
Okay I have the CCL file but its just I have some issues with zip to i have converted it to a text file in notepad.

If you can help I would really be glad.

Thanks in advance.

notepad version of CCL.txt
b.shuvayan is offline   Reply With Quote

Old   November 3, 2012, 15:04
Default
  #7
Member
 
Shuvayan Brahmachary
Join Date: Oct 2012
Posts: 34
Rep Power: 4
b.shuvayan is on a distinguished road
the solver manager solves for about 6 iterations and shows the error. Meanwhile it shows in the solver screen.

****** Notice ****** |
| A wall has been placed at portion(s) of an OUTLET |
| boundary condition (at 11.8% of the faces, 11.8% of the area) |
| to prevent fluid from flowing into the domain. |
| The boundary condition name is: outlet. |
| The fluid name is: Fluid 1. |
| If this situation persists, consider switching |
| to an Opening type boundary condition instead. |
+------------------------------------------------


Does this has anything to do with the problem of return code 255??
Would you like to see the pictures of the geometry and mesh??
b.shuvayan is offline   Reply With Quote

Old   November 3, 2012, 15:05
Default
  #8
Member
 
Shuvayan Brahmachary
Join Date: Oct 2012
Posts: 34
Rep Power: 4
b.shuvayan is on a distinguished road
Geometry consisting of a cube and a hollow sphere.jpg

Mesh by milti zone.jpg
b.shuvayan is offline   Reply With Quote

Old   November 3, 2012, 17:43
Default
  #9
Senior Member
 
Chris DeGroot
Join Date: Nov 2011
Location: Canada
Posts: 387
Rep Power: 6
cdegroot is on a distinguished road
You haven't added a turbulence model. Based on the flow speed it looks like you need one.

The error about the wall placed at the outlet is not directly related, it just means the solution isn't progressing very well. Eventually you want this message to go away when the simulation converges. It is just putting a wall to prevent backflow. I think the solver is quitting because the solution diverges.

You can try lowering your timescale factor to improve the convergence behaviour.
cdegroot is offline   Reply With Quote

Old   November 4, 2012, 05:09
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
If this object is in cross flow the inlet and exit boundaries are WAY too close. The recirculation will definitely hit the boundayr and cause the warning message you report. You need to move the inlet and outlet boundaries further away from the action.
ghorrocks is offline   Reply With Quote

Old   November 4, 2012, 05:56
Default
  #11
Member
 
Shuvayan Brahmachary
Join Date: Oct 2012
Posts: 34
Rep Power: 4
b.shuvayan is on a distinguished road
Thanks for the Help

I have done the following changes:
Turbulence model - k-epsilon from laminar
Timescale factor to 0.5 from 1

As far as the dimensions are concerned, I have kept them same because we are using the same model in our practical model so thats a constraint.

But the error still persists.
Any suggestions??
b.shuvayan is offline   Reply With Quote

Old   November 4, 2012, 11:53
Default
  #12
Senior Member
 
Chris DeGroot
Join Date: Nov 2011
Location: Canada
Posts: 387
Rep Power: 6
cdegroot is on a distinguished road
Looking at your images, you should consider what Glenn said. You can't put an outlet boundary that close to an object in cross flow (if I am understanding your images correctly). The outlet should be located far enough from the object that the recirculating region is contained within the domain.
cdegroot is offline   Reply With Quote

Old   November 4, 2012, 16:55
Default
  #13
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
The boundary conditions being too close is what is causing your problem. You need to extend your domain up and down stream or you will have no chance of getting this too work.

Your "practical model" has to have some system to deliver and recieve the fluid - so that is what you need to include.
ghorrocks is offline   Reply With Quote

Old   November 6, 2012, 01:45
Default
  #14
Member
 
Shuvayan Brahmachary
Join Date: Oct 2012
Posts: 34
Rep Power: 4
b.shuvayan is on a distinguished road
Thanks for the reply

I have made the following change. Time scale factor to 0.00001 and I am able to carry out iterations till 500.

But is there any disadvantage of lowering the value of time scale factor to such value which was previous 1 and showed the error 255??
b.shuvayan is offline   Reply With Quote

Old   November 6, 2012, 06:39
Default
  #15
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
The residuals and probably the imbalances are what you should judge convergence by. Once the convergence is progressing nice (monotonically converging reliably) then you can increase the time step size to accelerate convergence. Use edit run in progress to do this so you do not have to restart each time you do a change.
b.shuvayan likes this.
ghorrocks is offline   Reply With Quote

Old   November 7, 2012, 01:06
Default
  #16
Member
 
Shuvayan Brahmachary
Join Date: Oct 2012
Posts: 34
Rep Power: 4
b.shuvayan is on a distinguished road
Okay Thanks a lot
b.shuvayan is offline   Reply With Quote

Old   November 7, 2012, 01:48
Default
  #17
Member
 
Shuvayan Brahmachary
Join Date: Oct 2012
Posts: 34
Rep Power: 4
b.shuvayan is on a distinguished road
Glenn...thanks a lot. I didn't know that option existed. It was of great help. Thanks a lot
b.shuvayan is offline   Reply With Quote

Reply

Tags
ansys 14, cfx solver manager

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
CFX Solver Reynolds Number haider760 CFX 2 March 4, 2012 23:05
error message cfx solver sherlock303 CFX 5 February 14, 2012 17:35
CFX 11, solver Debabrata CFX 1 June 16, 2008 21:52
why the solver reject it? Anyone with experience? bearcat CFX 6 April 28, 2008 14:08
CFX 5.5 Roued CFX 1 October 2, 2001 16:49


All times are GMT -4. The time now is 07:15.