[alinik]

Hi,

I am simulating air flow around a turbine blade. I can obtain the solution when turbulence model is set to K-epsilon and K-Omega. When I want to run the case with SST, I receive the following error message. The solver crashes in the very first iteration.
The simulation is steady state. I have reduced the timescale factor to 1e-6 and moved the boundaries away from the blade and also increased the memory allocation factor.

p, li { white-space: pre-wrap; } +--------------------------------------------------------------------+
| ERROR #004100018 has occurred in subroutine FINMES. |
| Message: |
| Fatal overflow in linear solver. |
+--------------------------------------------------------------------+


Any suggestions?


Thanks

[MUMMED]

if your mesh is quite fine ,try changing relaxation factors.
I've got this problem,different case ,after changing relaxation factors in expert parameter it started to run

[oj.bulmer]

Did you try with local timescales?

[ghorrocks]

This is an FAQ: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

[alinik]

Thanks,

I fixed that issue for steady state case. Now that I want to solve the case for transient case I receive the exact same error again. Now what I can do?
I have tried decreasing time step size and used the steady case solution for initializing the domain.
Generally what should one do when encountered by this error in transient simulations? We do not have physical timescales any more to play with to overcome this error and obtain solution.

[alinik]

Originally Posted by MUMMED

if your mesh is quite fine ,try changing relaxation factors.
I've got this problem,different case ,after changing relaxation factors in expert parameter it started to run

Thanks. I solved this issue for steady case but still have problem in unsteady case. Where in expert parameters I can set underrelaxation factor? I cannot find it.

Btw what is the difference between underrelaxation factor and physical timescale for steady simulation?

Thanks

[ghorrocks]

Generally what should one do when encountered by this error in transient simulations?

Ummm - did you read the FAQ link I posted? The only difference for a transient simulation is you decrease the actual timestep size rather than the pseudo timestep size. Other than that it is all the same.

Generally what should one do when encountered by this error in transient simulations?

That is because CFX is not a SIMPLE based solver where the first thing you do when you have convergence difficulties is reduce the under relaxation factors. You do not adjust under relaxation with CFX, rather you adjust the time step size.

[dengemunzur]

Hi,

I am trying to simulate an axial flow turbine rotor in CFX. I used Meshing tool to generate mesh. A fully hexagonal mesh has been generated. In CFX Solver, after 20-25 iterations simulation diverges giving "fatal over flow error in linear solver."

A steady state analysis, and I used SST turbulence model. I tried different time scales, but could not overcome the the divergence problem. Also, I tried to improve mesh quality. With different mesh spesifications, I got the same error.

Any suggestions?

Thanks

[-Maxim-]

Have you tried all the other things mentioned here?

Originally Posted by ghorrocks

This is an FAQ: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

If yes, post pictures of your setup, your mesh and your out-file.

[dengemunzur]

Hi Maxim,

I have checked and tried most of them but transient simution. I will run a transient simulation in order to determine an appropriate time scale. Then I will let you know.

In my previous studies the simulations converged. When I changed the tip clearance of squealer geometry, I encoundered this divergence problem. I checked if it is related to the geometry, but I havent found anything related to the geometry.

Thanks

[dengemunzur]

Hi Maxim,

I tried different time scales and meshes for the calculations.

I thought it may be due to min value of "Orthog. Angle", therefore I tried to improve the mesh. Min "Orthog. Angle" has been increased up to 32 deg. However, it did not help to converge.

Then I used various physical time steps. I ended the analysis before it diverges to see what is wrong. Max value of the Courant number is too high. I have read that there is o requier Courant number to be small. But, I reduced the time scale considerably to reduce the Courant number. After that I noticed that run diverges later. After some runs, I had a solution without energy equation to see the results were acceptable. Generally the results are ok but some total pressure distributions are not physically acceptable. I carried on the run.

(By the way, the number of elements in my cases are quite high to keep the y plus values at acceptable levels)

Do you think it is all about Courant number for a steady state analysis?

thanks

[ghorrocks]

Do you think it is all about Courant number for a steady state analysis?

Courant number is just about irrelevant for steady state analysis. CFX is an implicit solver and does not have a Courant number requirement like explicit codes do. So you use the largest time step which gives you a time accurate simulation (for transient simulations) or which converges well (for steady state simulations).

If you have:
* Checked your simulation is valid and correctly set up
* Made the time step very small
* Got the best mesh you can
* Tried double precision
* Use the best initial conditions you can

(these are all listed in the FAQ, of course)

If you have done all those things and it is still not converging then your only real option is to do a transient simulation and march it to steady state in a time resolved model. This is much slower, but convergence is much more reliable. Use adaptive time stepping homing in on 3-5 coeff loops per iteration so the solver can find its own time step size. Don't guess a time step size, you will invariably get it wrong - and don't limit the time step size the solver can use, if it needs a very big or small time step let it.

[dengemunzur]

Hi Maxim,

I think I did the all steps. I tried to get a thinner boundary layer since very high velocity values near the suction side, at singular points.

I also tried transient simulations. With a few trials I achieved to reduce Courant number to acceptable levels which are given in CFX tutorials. But I could not get a solution. I will run some transient solutions.

Thanks

[ghorrocks]

Don't use Courant number as a guide. As I said, Courant number does not have a major effect on implicit solvers. Use convergence and accuracy considerations instead.

[-Maxim-]

It seems that I am late to the party now - Glenn already pointed out the ideas/suggestions I would have had, too.

As far I as know, the Courant Number ideally should be below 30 but since it corresponds directly to your selected timestep, it doesn't help as a criteria for convergence.
I found some training material slides from ansys in the www - I hope I'm allowed to link it here. They talk about the Courant number and suggest typical values of 2-10.

But as Glenn said, the Courant number isn't important for steady-state simulations.

Maybe you can post your ccl and out files and we could have a look. I'm sure you started with Auto Timescale for your steady-state calculation and tried different factors?

[dengemunzur]

Thanks Glenn.

I will run a transient simulation considering your suggestions.

Maxim, I started from auto time scale then tried various time scales.

I just ended a simulation. The simulation didnt diverge. A good point. But this time physical time scales is lower. Now, I will do some post process to see whether the results are acceptable or not.

thanks

[dengemunzur]

Hi,

I am sending one of the out files. Physical time scale was 0.001 in this case.

Thanks

[ghorrocks]

You have some translational periodic interfaces. What are they doing? This seems unusual in a rotating machine simulation. Can you show your domain so I know where these periodic interfaces are located?

You should probably make your reference pressure 100000 [Pa] - 3595 [Pa], and use 0 [Pa] for your outlet pressure. This might reduce round off error.

[dengemunzur]

Hi Glenn,

The outpuy file I sent belongs to a linear cascade arrangement, not annular cascade. In order to define flow direction, I used cylindrical coordinates. I got the velocity components from a rotating cascade to have an idea, not for a comparison. CFX makes the transformation of the components.

You can find the computational domain in the attachment.

I will try your suggestion.

Thanks for your consideration

[ghorrocks]

Are you sure you have that right? Why is the inlet using cylindrical coordinates to define the inlet flow when it is a linear blade cascade?

Does it converge when you run it entirely in cartesian coordinates?

This is looking like the XY problem: http://xyproblem.info/