[AS_Aero]

Hi
I am trying to do a turbine simulation and my simulation runs for 5 timesteps and then it crashes giving me the following error

#####
****** Notice ****** |
| A wall has been placed at portion(s) of an OUTLET |
| boundary condition (at 13.5% of the faces, 5.2% 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. |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #004100018 has occurred in subroutine FINMES. |
| Message: |
| Fatal overflow in linear solver. |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX solver could not be started, or exited with return |
| code 255. No results file has been created. |
+--------------------------------------------------------------------+
#######

What could be the reason for this ? Will it be due to mesh or my time step ?
I have given adaptive timestepping with in the basic setting with time step update frequency 10
Initial timestep of 1e-5
Timestep adaption MAX Courant Numbe
Max TIemstep 1e-3
Minimumtimestep 1e-5
Courant Number 50

These are my values I have given, so what could be the reason ?

[Gert-Jan]

FINMES means FINal MESsage. And that is not a joke.


This can be anything. But it mostly is related to an unphysical setup. I happens to me when:
- I plan to do a calculation with water massflow, and then use air instead.
- Or when the scale is wrong (mm instead of m)

- I forgot to specify the outlet


Just make a backup at iteration 1,2,3 & 4. And see how everything (P, v, tke, ted, etc.) develops. Then mostly you can pinpoint the mistake.

[AS_Aero]

Regarding the scale , I did the mesh in ICEM (RotorPart) Stator Part in Ansys mesh and I gave the values in mm for meshing in ansys mesh but in ICEM it was in meters. But when I linked them to cfx it was in meter (both) but it also says it will neglect if it is different one or something. How can I know if my scales where wrong ?
This is always confusing !!

[ghorrocks]

The overflow error is an FAQ: https://cfd-online.com/Wiki/Ansys_FA...do_about_it.3F

[AS_Aero]

And I checked the backup file and the first backup file dint have anything. And second backup file is having some values but not huge enough.

[AS_Aero]

Ok I will check for all possibilities !!

[AS_Aero]

So now I changed the timestep from 1e-5 to 1e-8 and now it ran for 14 timestep and then gave me the same error.

My timestep is adaptive to the CFL limited to 50
But during the timestepping information RMS CFL is 600 nad MAX CFL is 999.99
And having this wall at outlet issue
##
A wall has been placed at portion(s) of an OUTLET |
| boundary condition (at 72.5% of the faces, 94.1% 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.
##

Will these be a reason for the crashing of the simulation ?

[ghorrocks]

The wall at the outlet sure could be the cause of the problems. That is an FAQ as well: https://cfd-online.com/Wiki/Ansys_FA...f_an_OUTLET.22

Did you check the FAQ I quoted previously?

[Christophe]

Post a screen shot of the geometry. Try extending inlet and outlet artificially far.
Look at Mesh Statistics and aspect ratio. See if any elements are above 100,000:1.
Try Upwind and First Order
Once solving, stop it before it crashes and look for ridiculously high velocity with an iso volume.

[AS_Aero]

Yes I went through the link you send, And I am still not convinced what could be wrong. And now i spoke with a guy in Support and they said for Turbomachine problems you have to use Structured grid and my mesh quality might be the problem. and also they said I have to change my interface location, as my interface might have parallel flows (which I dint understand though) When they say about mesh quality, what are the things I should see and what are the values ? I have attached some images from my geometry and some mesh image as well. Kindly have a look and let me know what could be wrong.
Thanks in advance.

https://wetransfer.com/downloads/d28...5093434/d10143

[ghorrocks]

Have to use structured grids? Rubbish. A good quality unstructured mesh will work fine.

Mesh quality might be the problem? After looking at your mesh I can confidently say it is definitely the problem.

Need to move interface to avoid parallel flows? I am unconvinced about this one. I have done it many times. But I can see how it can lead to a loss in accuracy. But as long as you have enough accuracy that is fine.

After looking at your mesh I see that you are inexperienced at CFD. It is not possible to write a how-to guide for CFD on the forum for you, you are going to have to do some work on the fundamental of CFD before attempting this simulation.

I strongly recommend you attempt some benchmark simulations and work out what is required to get them accurate before attempting this more complex one. Start on flows like "flow over a back facing step" and the "Ahmed body". Also I would recommend finding an airfoil which you can find reliable results for (either experimental or numerical) and model that too. Once you can accurately model these benchmark flows you will know what you need to do to accurately model your model.

[AS_Aero]

Dear Glenn

Yes I totally agree my mesh is not at all good !! It was just my first try to get a mesh and try to run a case and see. Ofcourse I am not experienced enough, but I have done the basic simulations and normally I do some grid study during the simulations. This simulation I was not initially checking for some accuracy in results instead to get a simulation run as a first attempt. The problem is with the ansys meshing I couldnt generate a better one than this.
But could you tell me what kind of mistakes I have done in the meshing ? Like the inflation along the rotor blades ? (Its too much I guess, I gave 10 layers although 5 is enough , the number of points along the blade length is less and also the blade profile is not well adapted due to this), on the stator side the inflation layer given is not good and its ugly. but I must tell you this was just the basic first mesh I created for this case using ansys mesh so only. But kindly let me know what all other mistakes I have done or what all should I have considered while generating the mesh for this particular geometry.

[ghorrocks]

The key problem is your mesh is way too coarse. The key areas will be in areas of separations, and your model has lots of them. The basic structure is OK, everything will improve as the mesh size approaches what will be required.

My previous post did not recommend you simply model a few basic setups, it recommended you to model them and compare your results to quality benchmark results, then work on your model until you get accuracy good enough you are happy to use.

[AS_Aero]

Dear Glenn

Thanks for your suggestions.
The main problem with this geometry I am facing is
When it comes to Rotor :
I am able to generate a sweep mesh, but with the Proximity and Curvature: ON its crashing. Only Curvature option I am able to keep it open.
Secondly Inflation layer : When I wanted to give inflation layer by right clicking mesh, it asked for the boundary or the face etc, only way I am able to give inflation layer is by selecting named selection option. All these issues I am saying is for Ansys meshing.

Stator I am not able to create a Sweepable body, although I split the geometry into many bodies, but the main body which is where the rotor is placed its creating problem.

And for some reason in both when I give Proximity option ON the computer is going out of memory and it is using all the 16GB RAM. So I am really helpless with this geometry.

Now I am thinking for this huge Stator Part, can I split the entire Stator Part into different geometries and mesh it seperately like I do for Rotor and Stator Instead of one Stator Geometry, I split it into many Cubes and then mesh it and load in CFX as multiple Meshes and give the interfaces between the two surfaces where they touches ?

[ghorrocks]

ANSYS Meshing is a frustrating piece of software at times. It has moments of brilliance when complex things mesh quickly and easily, but it also has very frustrating times when this which should mesh easily just refuse to work.

Personally I move to ICEM when ANSYS Meshing frustrates me. It is much lower level, so you have to do much more manual intervention, but you really can mesh just about anything in it. Be warned, it is very different from other ANSYS software and will require some effort to learn. But I think it is worth it as you have much more control over the meshing process and you can build up meshes one step at a time far more easily.

Yes, meshing one sector of the rotor and then rotating it around to create the full geometry is a recommended process. Try to make the two periodic faces on the sector you model have a matching mesh so when you rotate it around they can be merged into a single body and do not require GGI interfaces. CFX-Pre can do this merging, as long as the mesh faces match perfectly.

[AS_Aero]

Dear Glenn

Thanks a lot for your reply. Yes I know sometimes Ansys meshing is crazy and sometimes its really easy. Anyways I will try with ANSYS ICEM as well although am not that expert in it.
Regarding the rotation of the mesh in CFX Pre, Yes I tried it and I am able to do it.
But with respect to the stator part, I cant do any mesh transformation. So only way is to split the geometry into to different geometry and load each mesh in CFX Pre. In this case will I need some interface between the meshes or ? As you have seen how the stator domain looks (I cant mirror or rotate it ) So only I had this idea in my mind, although I havent tried it.

Then regarding the inflation layer on the rotor blade surface, in Ansys mesh when I need to insert an inflation method, it asks for the body and the boundary and i am not able to understand that method. Can you tell me how to achieve that ?
In the main menu of Mesh I am keeping inflation as None because if I give there program controlled, it will create at some corners and not on the blade walls.

[ghorrocks]

Your stator part is quite simple and should mesh fine as a single body. I would not split it up. If you are running out of memory on a body like that it suggests something more fundamental is wrong.

Inflation in ANSYS meshing is, also, a bit weird. It has several methods of defining it and a few control parameters so all I can suggest is to read the documentation and try some of the options and controls.

[AS_Aero]

The problem with the Stator I guess is its a huge geometry of 10m and my RAM is 16GB and it is crashing due to lack of memory. Also inside this huge rectangle domain I have some thin (comparitively thin) gaps which was my solid casing and maybe due to this. I am not sure.

The rotor I am trying to create a sweep Hex mesh and hence the inflation option is not working or active so I am not able to generate prism layers on the blade surface

[ghorrocks]

The physical size of the domain is irrelevant. I have meshed domains 100km x 100km x 10km (see https://computationalfluiddynamics.c...ation-mystery/)

What is important is the mesh size required to resolve the features required for an accurate enough model. This is why mesh sensitivity studies are so important - they determine the size mesh you require, and this defines how big a compute system you need to solve it (if it is possible at all).