Hi

I have a two cylinders model connect between them using a small hole (as a domain interface). The objective is using a tangential velocity create a small tornado through the hole. The simulation with the k-epsilon model works well, but the model is not able to reproduce good enough the highly turbulence zone inside the vortex. Hence, I switch to the Reynolds stress model with the k-epsilon model as initial conditions, but until now no matter what I do, the simulation crash in a fatal overflow in linear solver.

What could I do?

Hi,

After how many iterations does the case crash? When you use higher order turbulence models, you would need to use a smaller time step (steady/trans). Just check if you are using auto-tiestepping in steady solution.

Regards, test

Hi

I have used a physical timestep of 1x10^-5 s.

The simulation crash on the 12th iteration.

I made a backup on the 11, I checked in the CFX-post, and I found high velocities, around 20,000 m/s (a singularity) in some points. Another thing to mention is that I can't run the simulation using RSM from the beginning because it doesn't start. I need to use a turbulence control with transient factor of 5, which helps the code to run the first iteration as laminar model, the next one as zero eq., and so on, until it gets to the RSM. Finally, I have tried both modes, steady-state and transient, same results.

Thank you

P.S. Using lower timesteps just make the simulation crash later, for example at the 25.

Hi,

Difficult to point out the issue without looking at your problem setup, geom and mesh. I can suggest the following though:

# Since the problem is crashing very early it can be the issue with the boundary condition.

# Try using local timescale factor of about 2 for steady runs.

# Test the case with a coarse mesh which will make the solution diffusive.

Just need to find out where the error comes from..

Regards, Ananth

I found the problem, it was the domain interface. Hence, I managed to make a big assembly, and the RSM worked. Thank you for your help guys.

[zobekenobe]

What did you exactly manage to do

[ghorrocks]

There is an FAQ about linear solver overflow now: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

[juliom]

Dear friend, read thoroughly because, K-E has some limitations!! and one of them is that is based on eddy viscocity assumption.. and this yield that it can not handle "well" the anysotropy of the field!!
Take a look on the books!!

[Badi]

Hi, I didnt want to make a new thread on this since I have a similar problem.
I attached a picture of the geometry.

What I try to do:
- The longer cylinder is moving in an oscillating way
- the complete room is filled with water
- I expect cavitation because of the motion

My problem:
- fatal overflow in linear solution at around 8-12 coefficient loop of the very first iteration step
- the motion itself works but as soon as I put in a second fluid (water vapour) and enable cavitation I get this problem in the very first timestep.
=> I tryed to go down with timescale (from 1e-6 to 1e-12) but it didnt work.
The Mesh is refined in the area where the cavitation is expected


edit: I try to simplify the problem as much as possible, so I have no turbulence modell and adiabatic walls. (heat transfer: total energy)

[ghorrocks]

Combining a FSI and cavitation simulation is always going to be difficult. You should expect convergence difficulties in a simulation like this.

Why are you modelling heat transfer? Most people most cavitation as isothermal. The cavitation model in CFX assumes isothermal behaviour. Have a look at the cavitation example in the CFX, cavitating flow over a hydrofoil.

And: Removing the turbulence model does NOT simplify the problem! It causes problems and makes it harder to converge - this itself might explain your convergence difficulties! If the flow is turbulent you need a turbulence model to get sufficient dissipation for the model to converge.

[Lava kishan]

hi
while simulating with ssg turbulence im getting fatal over flow code error
but while im trying with RNG, K-omega it is running simulation but results which im getting is different plz anyone can help me

[Gert-Jan]

Why picking up such an old thread for this question.
Better start a new one.

Nevertheless, reduce the timestep bij 75%. Generally helps a lot.

[ghorrocks]

And consult the FAQ on this: https://www.cfd-online.com/Wiki/Ansy...do_about_it.3F