Fatal overflow in linear solver in mesh deformation
 

Hello guys,
I am a student,
and unfortunately I can not solve a convergence error of my simple problem of fluid dynamics .. laminar flow
I am trying to simulate a breathing movement, in CFX 15 using mesh deformation.

breathing movement = amplitude * sin (2 * pig * t / (2 * period)) * sin (2 * pig * x / (2 * L)) + y0

I tried to change a few parameters, thicken the timestep, improve the mesh, and change the exponent of the stiffness according to the report 1 / wall. But nothing, I always get:
"ERROR # 004100018 has occurred in FINMES subroutine. | | Message: | | Fatal overflow in linear solver."

all boundaries are stationary except the selected wall in green, it is set in the periodic displacement



Is my definition of breathing movement correct?
Tips?

Thanks to everyone in advance

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

As this is a moving mesh simulation this FAQ will be of assistance as well: http://www.cfd-online.com/Wiki/Ansys..._went_wrong.3F (the tip on sending the mesh motion to the results file for debugging is HIGHLY recommended)

After you have looked at these FAQs please post your CCL.

thanks a lot for the FAQ ghorrocks! :)
I read the FAQ before writing this post

- Is the physics of the simulation set up correctly? yes! no error in CFX pre

- Is the mesh of high enough quality? I have used different types of mesh from the more dense to more simple.

- Is a better initial condition required? the problem, without breathing, gives solution!

- Using a coarse mesh and interpolating as an initial condition onto the final mesh? The simulation does not start

- Is double precision required? Yes

- Does the model require small time steps to start? yes

- a better fluid mesh? yes

- meshsiffness 1/wall distance? yes

- smaller timesteps? yes

- If the mesh motion is prescribed (ie not FSI or 6DOF) then you can turn the fluid, turbulence, energy and any other solvers off using an expert parameter. This means the only work the solver is doing is calculating the mesh motion. Obviously this will speed the simulation up immensely? No turbulence, no energy, no scalar. Easy laminar flow.

there are online guided tutorials for using the mesh deformation?
thank you again

Do a google search and you should find some tutorials. There are also tutorials on the ANSYS customer page.

Can you post your CCL?

here is my CCL in .txt

I will try in customer service ansys, I hope to find something to make my case. :)

good day

You appear to be using mesh motion option of periodic displacement. You probably want to use the specified displacement option as you are defining the motion with your displacement function.

Your specification of the displacement function on the top face but stationary on the side walls is going to lead to highly distorted meshes and is probably not what you intend.

For debugging mesh motion I strongly recommend you do as the FAQ suggests and turn off all the solvers, make it output a results file every time step and run the solver to give a results file containing just the mesh motion. Then you can check the motion is what you intended. In my experience you rarely get the motion right first time so this step is essential in getting mesh motion simulations to work.

Dear Glenn,
would you be able to mention which one of the expert parameters should be on in order to debug the mesh motion, I`m trying to simulate the movement of a train with its exhaust taken into account.
I have the train as the rigid body, with a subdomain surrounding it and the main domain which is the route of my study. I cannot get it to work though.
Please let me know if you have any suggestions for me.

Cheers,
Amin

The "solve fluids", "solve turbulence" and related expert parameters are use to turn the solvers off and just resolve the mesh motion.

As a side issue - why are you modelling something like that with rigid bodies? It might be more easily modelled with moving mesh, and depending on the situation you are modelling it might be modelled with a stationary mesh.

Thanks for the reply, I`m trying to simulate a moving train at constant speed, while taking into account the wind and the exhaust which is coming out of the train.
I also tried to consider the train as moving wall, but I wasn`t able to get any results.

Can you post an image of what you are modelling?

Here are two images from my geometryAttachment 52229

Attachment 52230

I thought so :)

This can be modelled with a stationary mesh. There is no need for rigid bodies, mesh motion or anything difficult. Make the upstream inlet have the velocity of the train, and an outlet with zero pressure at the exit. Make the ground a wall with a tangential velocity equal to the velocity of the train. This means you are modelling the train in a constant velocity frame of reference fixed on the train.

Thank you so much for the help, just to make sure though, how should I define the train itself then ?! as wall? not rigid body ?!

Yes, as a wall. Have a look at the CFX tutorials which model flow past a moving object - for instance the flow around a blunt body, flow over a wing, the hydrofoil and a few others.