[dyon]

I am trying to simulate a rubber ring that pulsates in water and the solution does not converge at all.
The ring is modelled in Transient Structural and expands/shrinks once in every 4s (so very low frequency).
Any idea what might I be doing wrongly ? I can provide you with any detail/screenshot/animation you may need to figure out how to help me.
Many Thanks !

[aero_head]

Hello,

You could go over this FAQ and see if you can implement some of the things they suggest:
https://www.cfd-online.com/Wiki/Ansy...gence_criteria

If nothing there works, you can report what you tried and we can try to help after.

[andy_]

Originally Posted by dyon

I am trying to simulate a rubber ring that pulsates in water and the solution does not converge at all.

Is this a time varying simulation, simple harmonic, or what?

What do you mean by not converge at all? The errors in the solved equations remain high, the flow doesn't settle down to a harmonically repeating one, or something else?

[dyon]

Originally Posted by andy_

Is this a time varying simulation, simple harmonic, or what?

What do you mean by not converge at all? The errors in the solved equations remain high, the flow doesn't settle down to a harmonically repeating one, or something else?

It is a time varying simulation, the ring pulsates (expands/contracts see Screenshots) due to time varying pressure inside. The ring is modelled and setup in Transient Structural (see PressureSetup screenshot attached).

The ring pulsates in water. The water is modelled as a cube in Transient Structural. The Geometry is shared with Fluent, where it is meshed and setup (see mesh in Fluent FluidMesh screenshot attached).

Fluent setup: Transient / Inviscid / Pressure-outlet (for all the 6 faces of the cube / System coupling in Dynamic mesh at the common face water-ring / Smoothing (Diffusion) + Remeshing / Timestep size 0.1 s for 40 timesteps.

Maximum iterations set at 10 in the System coupling (time step again 0.1 s)

On running this, the first timestep (0.1 s) never converges (I have done even 50 iterations on it). Timesteps 0.2 s to 0.5 s converge (Y), time step 0.6 s does not converge (N), 0.7 s to 1.3 s (Y), 1.4 s to 2.2 s (N), 2.3 s to 2.5 s (Y), 2.6 s (N), 2.7 s to 3.5 s (Y), 3.6 s (N), 3.7 s to 4.0 s (Y).

I have observed that continuity does not converge, more than velocities.

I would appreciate your advice. I can provide more details if needed.

Thank you vey much !

[andy_]

Originally Posted by dyon

It is a time varying simulation, the ring pulsates (expands/contracts see Screenshots) due to time varying pressure inside. The ring is modelled and setup in Transient Structural (see PressureSetup screenshot attached).

The ring pulsates in water. The water is modelled as a cube in Transient Structural. The Geometry is shared with Fluent, where it is meshed and setup (see mesh in Fluent FluidMesh screenshot attached).

Fluent setup: Transient / Inviscid / Pressure-outlet (for all the 6 faces of the cube / System coupling in Dynamic mesh at the common face water-ring / Smoothing (Diffusion) + Remeshing / Timestep size 0.1 s for 40 timesteps.

Maximum iterations set at 10 in the System coupling (time step again 0.1 s)

On running this, the first timestep (0.1 s) never converges (I have done even 50 iterations on it). Timesteps 0.2 s to 0.5 s converge (Y), time step 0.6 s does not converge (N), 0.7 s to 1.3 s (Y), 1.4 s to 2.2 s (N), 2.3 s to 2.5 s (Y), 2.6 s (N), 2.7 s to 3.5 s (Y), 3.6 s (N), 3.7 s to 4.0 s (Y).

I have observed that continuity does not converge, more than velocities.

I would appreciate your advice. I can provide more details if needed.

Apologies for the delay in replying. I saw a comment about moderation but missed the update.

If the fluid is incompressible and the external box is impermeable then you have defined a problem that cannot be solved. Is this the case? For an incompressible fluid the expansion/contraction of the ring must be balanced by an equivalent small amount of incompressible fluid flowing back and forth across the external boundary somewhere. It only needs to be, say, one side and since the flow will be tiny it won't affect the flow around the ring. Alternatively you could move one of the sides slightly so that the trapped fluid was of constant volume.

Numerically what is going wrong is that the source terms in the Poisson equation are not summing to exactly zero. This is a requirement because although the determinant of the equation is zero if the sources sum to zero a pressure field can be determined to within a constant. If they don't then the equation simply has no solution.

[dyon]

Originally Posted by andy_

Apologies for the delay in replying. I saw a comment about moderation but missed the update.

If the fluid is incompressible and the external box is impermeable then you have defined a problem that cannot be solved. Is this the case?

The fluid is incompressible, but I defined the 6 faces of the box (fluid) as pressure outlets (see screenshot). The case is with pressure-outlets and recognized as such by Fluent after hybrid initialization.
In CFD post I can see velocities at the boundary pointing forwards and backwards. I think that pressure-outlets are considered permeable by the solver.

[andy_]

Originally Posted by dyon

The fluid is incompressible, but I defined the 6 faces of the box (fluid) as pressure outlets (see screenshot). The case is with pressure-outlets and recognized as such by Fluent after hybrid initialization.
In CFD post I can see velocities at the boundary pointing forwards and backwards. I think that pressure-outlets are considered permeable by the solver.

I am not familiar with Fluent's boundary condition implementation but the boundary will be changing between inflow and outflow over time. I wouldn't expect a single pressure condition (of unknown kind) over the whole boundary to work in the sense of driving the solution towards a single solution. More worryingly the pressure equation is not converging after the first time step and that almost always follows from the mass flow in not being exactly equal to the mass flow out. Any boundary condition implementation that allows the flow to wander must impose this condition before solving the pressure equation.

Every time step must converge or else the solution in time is meaningless. I am not familiar with Fluent's time stepping scheme but non-convergence on the first time step may be due to your initial conditions not satisfying continuity which they must. Is the ring moving at t=0 and the external boundary at rest at t=0? If so, this is an invalid initial condition.

If you have an intial condition that satisfies continuity, a time step that is comfortable with respect to CFL and diffusion number limits and taking a very large number of iterations on the pressure equation doesn't drive the continuity error into roundoff then your current pressure boundary condition is likely unusable.

The simplest boundary condition would be to specify a tiny constant in space normal velocity on the external boundary that changes through time to exactly balance the mass added or subtracted by the moving ring. I would expect Fluent to supply such a boundary condition because it is a simple and robust condition for testing moving grids. However, the screen dump of your pressure condition seems to show a whole bunch of options and so it may not be directly labelled as such.

[dyon]

Originally Posted by andy_

Every time step must converge or else the solution in time is meaningless. I am not familiar with Fluent's time stepping scheme but non-convergence on the first time step may be due to your initial conditions not satisfying continuity which they must. Is the ring moving at t=0 and the external boundary at rest at t=0? If so, this is an invalid initial condition.

I have shifted the beginning of ring expansion one timestep later (0.1s) to make sure that the ring is not moving at the first time step of the computation. Now the first time step converges and the second doesn't. It is clear that non-convergence is related to the fact that the ring begins to expand. The boundary conditions are key here, but from what I have read in the Ansys Fluent manual, pressure-outlet type boundary would be most appropriate in this case because it allows backflow besides outflow. Perhaps someone knows details on how to setup the pressure-outlet boundary for this case? Or is there another type of boundary that can be used ?