How to fix / solve local instability
 

Hi,

I would like to know how a local instability can be fixed. Is there any strategy when choosing the parameters for the solver?

I am attaching an image of a local instability I am experiencing when simulating a flow past a circular cilinder. The flow is from left to right.

Best regards,
Hector.

but running this solution for long time you get a numerical blow-up of the solution? Apparently it seems that something in the BC.c can be wrong...

However, check for the CFL and viscous stability parameters in that local region

Hi Filippo,

The instability appears after the flow has been stablished and had reached the end of the domain (right).
The boundary conditions I have using at the end of the domain are: du/dx = dv/dx = 0.

The CFL is far below the critical CFL (by a factor of 2 or more).

Best regards,
hector.

thus, this is not a numerical instability but a wiggle in the steady solution... check in which variables (those resolved in the code) you see such oscillations

Could you check if you have reversed flow at this point of problem.

This information is important before any judgement be made because i know one way it could arise in case of reversed flow.

Hi Arjun,

After the instability appears, the flow reverses and start growing and growing until it becomes very large.

The flow is supposed to be incompressible.

There are two parameters that control the time marching scheme (relaxation factors) that can be varied.
Theta1 for velocity which I set to 1.0 (It can be changed from 0.0 to 1.0)
Theta2 for pressure which I set to 1.0 (It can be changed from 0.0 to 1.0)

Best regards,
Hector.

Which is the difference between wiggle and instability?

Maybe I have misunderstood you in my reply.
When the instability appears, there is not any steady state solution that can be reached.

Numerical instability is a process that during the time integration drive the solution to blow-up, wiggle is a finite numerical (and unphysical) oscillation in the solution eve in the steady state.

Since your case is incompressible, I suggest to check the Div v = 0 constraint near the outflow

I think what he means is that wiggle appears but solver is able to recover from it.
Instability is some disturbance that keep growing until solver blows up the residuals.

The issue is that usually solvers add dynamic head at the pressure boundary to avoid reversed flow.

So if you specify pressure Pbnd at boundary, in case of reversed flow
it will be changed to

Pbnd - 1/2 density velocity sqr

It is done to remove reversed flow and it generally helps.

But sometimes what happens is that due to sudden change of boundary pressure from Pbnd to Pbnd - dynamic head, the pressure gradient at that cell sees sudden change.

What it means is that sudden change in fluxes and other things in that cell. Sometimes solver becomes instable or produces wiggles due to this.

I suspect what you see is this thing.

For incompressible flow pressure urf of 1 is too high, I would hesitate to try above 0.3 usually.

Only in pressure based coupled solver that i have i use p urf around 0.9

Thanks for the explanation.
Then I think that I am facing up an instability, since the solution blows up.
I have double check the boundary condition (at the outflow), and it appears to be well posed: du/dx = 0 and dv/dx=0, which I understand this is the normal way of specifying the constraints at exit flow.

On the other hand, I have been playing around with the time step (delta t), and after incresing the value of the delta t (from 0.001s to 0.005s) it seems it is working now. Why is this happening?
I have always believed that reducing the time step means incresing the accuracy of the solution.
This is someting that is puzzling me now. ???

are you solving a Poisson pressure equation? check if the continuity constraint is satisfied by using your discretized BC.s. It is just sufficient check in a single time step what happen at the outflow

I can try to use 0.3 as indicated, which I undestand is an semi-implicit strategy for the pressure. I will give it a try. I will inform you with the outcome.

By the way (only so as to frame the discussiion, in case it helps), the algorithm I am using is the Characteristics Based Split Algorithm which is a projection scheme for the Finite Element Method.

What solver are you using btw.

Decreasing time step may introduce decoupling of pressure and velocity as it weakens the Rhie and Chow dissipation.

For solving the poisson equation I am using a bi-conjugated gradient stabilizated solver.
I do not use any kind of Rhie and Chow dissipation.
Where can I find information about the Rhie and Chow dissipation. Do you know of any paper I can take a look at?

your problem is in the outflow BC.s, the dissipation term is used in cell-centred colocation to avoid pressure decoupling...

Check the BC for the pressure problem

Hi Filippo,

I have checked the BC for the pressure and the velocity at the exit of the domain, and they appear to have been defined correctly.

I have also checked the gradient of the velocity at the exit, according to your previous suggestion, and you can see in the attached images that they are well defined.
I am attaching images for both gradients du/dx and dv/dx. At the exit it can be seen that they are both zero.

By the way, I have increased a bit more the delta t of the resolution and it appears is working as well.
Even the frequency of the vortex shedding approaches the value obtained by other references.