CFX solver manager quits with error code 255

b.shuvayan · November 1, 2012, 10:23

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 · November 1, 2012, 12:37

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

ghorrocks · November 1, 2012, 16:40

Can you post your CCL file?

b.shuvayan · November 2, 2012, 02:59

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?

Lance · November 2, 2012, 04:04

In CFX-pre: file/export ccl
Upload the .ccl file here as it is only text.

b.shuvayan · November 3, 2012, 14:55

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 · November 3, 2012, 15:04

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 · November 3, 2012, 15:05

Geometry consisting of a cube and a hollow sphere.jpg

Mesh by milti zone.jpg

cdegroot · November 3, 2012, 17:43

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.

ghorrocks · November 4, 2012, 05:09

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.

b.shuvayan · November 4, 2012, 05:56

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??

cdegroot · November 4, 2012, 11:53

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.

ghorrocks · November 4, 2012, 16:55

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.

b.shuvayan · November 6, 2012, 01:45

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??

ghorrocks · November 6, 2012, 06:39

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 · November 7, 2012, 01:06

Okay Thanks a lot

b.shuvayan · November 7, 2012, 01:48

Glenn...thanks a lot. I didn't know that option existed. It was of great help. Thanks a lot

November 1, 2012, 10:23	CFX solver manager quits with error code 255	#1
b.shuvayan Member Shuvayan Brahmachary Join Date: Oct 2012 Posts: 36 Rep Power: 14	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

November 6, 2012, 06:39		#15
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,854 Rep Power: 144	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.

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 22:52
why the solver reject it? Anyone with experience?	bearcat	CFX	6	April 28, 2008 15:08
CFX 5.5	Roued	CFX	1	October 2, 2001 17:49

November 1, 2012, 12:37		#2
b.shuvayan Member Shuvayan Brahmachary Join Date: Oct 2012 Posts: 36 Rep Power: 14	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

November 1, 2012, 16:40		#3
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,854 Rep Power: 144	Can you post your CCL file?

November 2, 2012, 02:59		#4
b.shuvayan Member Shuvayan Brahmachary Join Date: Oct 2012 Posts: 36 Rep Power: 14	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?

November 2, 2012, 04:04		#5
Lance Senior Member Lance Join Date: Mar 2009 Posts: 669 Rep Power: 22	In CFX-pre: file/export ccl Upload the .ccl file here as it is only text.

November 3, 2012, 14:55		#6
b.shuvayan Member Shuvayan Brahmachary Join Date: Oct 2012 Posts: 36 Rep Power: 14	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

November 3, 2012, 15:04		#7
b.shuvayan Member Shuvayan Brahmachary Join Date: Oct 2012 Posts: 36 Rep Power: 14	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??

November 3, 2012, 15:05		#8
b.shuvayan Member Shuvayan Brahmachary Join Date: Oct 2012 Posts: 36 Rep Power: 14	Geometry consisting of a cube and a hollow sphere.jpg Mesh by milti zone.jpg

November 3, 2012, 17:43		#9
cdegroot Senior Member Chris DeGroot Join Date: Nov 2011 Location: Canada Posts: 414 Rep Power: 18	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.

November 4, 2012, 05:09		#10
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,854 Rep Power: 144	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.

November 4, 2012, 05:56		#11
b.shuvayan Member Shuvayan Brahmachary Join Date: Oct 2012 Posts: 36 Rep Power: 14	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??

November 4, 2012, 11:53		#12
cdegroot Senior Member Chris DeGroot Join Date: Nov 2011 Location: Canada Posts: 414 Rep Power: 18	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.

November 4, 2012, 16:55		#13
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,854 Rep Power: 144	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.

November 6, 2012, 01:45		#14
b.shuvayan Member Shuvayan Brahmachary Join Date: Oct 2012 Posts: 36 Rep Power: 14	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??

November 7, 2012, 01:06		#16
b.shuvayan Member Shuvayan Brahmachary Join Date: Oct 2012 Posts: 36 Rep Power: 14	Okay Thanks a lot

November 7, 2012, 01:48		#17
b.shuvayan Member Shuvayan Brahmachary Join Date: Oct 2012 Posts: 36 Rep Power: 14	Glenn...thanks a lot. I didn't know that option existed. It was of great help. Thanks a lot