CFX solver manager quits with error code 255
 

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). :confused:

I am hoping for any suggestions. any help would really be appreciated.
Thanks in advance
:)

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??

Attachment 16567

Attachment 16568

Can you post your CCL file?

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?

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

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.

Attachment 16627

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??

Attachment 16629

Attachment 16630

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.

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.

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. :eek:
Any suggestions??

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.

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.

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??

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.

Okay Thanks a lot :)

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