[Stargazer]

Originally Posted by aerosayan

Can you retry this with a high Re flow? Your result will be different.

Your flow seems laminar.

The steady state solution that you're showing has converged (as seen by the drop in residuals, and then becoming flat).

Depending on how your steady state solver is configured, it could've used local timestepping to get the final result. This won't show any vortex shedding.

While the transient simulation shows vortex shedding because it solves each intermediate timestep until reaching the final steady state. Meaning ... if the initial and boundary conditions would create vortex shedding, then they will show up in the simulation, and at the end become as same as the steady simulation's result.

i.e both are correct.

However, Switching to transient after initializing with steady state does nothing, because the flow is already converged to what you'd expect for this low Re flow.

Yes, the flow is laminar. And the coupled solver is using the pseudo-time marching method, as you said. Why this method cannot give any vortex shedding in unsteady simulation? This doesn't make sense to me.

[sbaffini]

Physics/experience tells you that this flow is close to instability. Not fully unstable like in turbulence but at the edge of it.

Your numerical representation of this flow will certainly not be exact, especially with a low order code, but also because of bcs and initial conditions.

Finally, as the equations are non linear and the solver math is discrete, even things like how you factor terms in an equations will potentially produce differences (imagine two fully different solvers).

What happens then is that your numerical representation of the flow in the different cases falls on different sides of the stability edge. And more, one of the solvers actually introduces sufficient disturbances to let instability to kick in while the other doesn't.

In my opinion, there is nothing more natural to observe in computational physics. It probably happens more than users are capable to understand... just think about different RANS models giving qualitatively different results, it is just the same issue.

[Stargazer]

Originally Posted by andy_

OK we seem to be struggling with the details and having just checked the STAR manual doesn't seem to be openly available for non-customers. Perhaps it doesn't matter too much and we can likely guess that the differencing of the convection terms is diffusive, pressure smoothing is present and the boundary layer likely hasn't been fully resolved all of which will tend to hinder the formation of instabilities at a Reynolds number that is only just large enough for vortices to start shedding.

The scheme is likely to be consistent and so if it isn't initiating shedding (which we haven't yet fully checked) then increasing the grid resolution will lead to it eventually starting. Alternatively changing to a numerical scheme developed for LES will likely enable shedding to initiate on coarser grids.



You need to check where instabilities are likely to start forming which will be a waviness in the boundary layer over the cylinder. I would check all solution variables in a few places and get the values printed out by the solver and not the plotting software which may be averaging and dropping precision.

Hi Andy, thank you for your suggestions.
BTW, just curious, when we are talking about unsteadiness, what exactly are we referring to? In numerics wise, is the unsteadiness due to the small nonconservation in the cells, because of the for example separation or small vortices?

[Stargazer]

Originally Posted by sbaffini

Physics/experience tells you that this flow is close to instability. Not fully unstable like in turbulence but at the edge of it.

Your numerical representation of this flow will certainly not be exact, especially with a low order code, but also because of bcs and initial conditions.

Finally, as the equations are non linear and the solver math is discrete, even things like how you factor terms in an equations will potentially produce differences (imagine two fully different solvers).

What happens then is that your numerical representation of the flow in the different cases falls on different sides of the stability edge. And more, one of the solvers actually introduces sufficient disturbances to let instability to kick in while the other doesn't.

In my opinion, there is nothing more natural to observe in computational physics. It probably happens more than users are capable to understand... just think about different RANS models giving qualitatively different results, it is just the same issue.

Thank you sbaffini. I have read the instability of the non-linear equations from the fluid mechanics textbook before. Though physically it is quite reasonable due to the chaos, it's my first time to see this in CFD (maybe I have never delved into this deep before).
I am also curious about the instability from CFD side. Aside from the "errors", is the instability in CFD brought by the small non-conservations in the cells, due to like vortices or separation?

[FMDenaro]

What do you mean for lack in conservation?? That makes no sense …

[Stargazer]

Originally Posted by FMDenaro

What do you mean for lack in conservation?? That makes no sense …

Hi FMDenaro, I just want to know what instabilities are hidden in the simulation. Lack of conservation is just my naive guess

[sbaffini]

Originally Posted by Stargazer

Thank you sbaffini. I have read the instability of the non-linear equations from the fluid mechanics textbook before. Though physically it is quite reasonable due to the chaos, it's my first time to see this in CFD (maybe I have never delved into this deep before).
I am also curious about the instability from CFD side. Aside from the "errors", is the instability in CFD brought by the small non-conservations in the cells, due to like vortices or separation?

Let's first consider unsteady simulations. Your numerical representation of a flow is like a different flow, a distorted representation of the original, but still pretty much a flow. As such, it still has a certain number of the physical mechanisms which are in the original physical flow. Which ones, and how much distorted is dependent from the numerics.

Now, for non conservative methods like finite differences, non conservation is just a numerical error (altough, in a sense, more disruptive). For conservative methods, the only non conservation allowed is the one arising from the non perfect convergence of the equations but, again, this is purely numerical.

Also, do not confuse instability in CFD as in unstable numerical methods (say, too high CFL for explicit methods) with the dynamical instability I've been mentioning. The physical and numerical flow are two dynamical systems which, under certain conditions, become unstable. The closer is the numerical dynamical system to the physical one, the more the two will behave consistently. This is what I've been talking about. Unfortunately I can't explain here anything about dynamical systems or fluid dynamics in general, but you need to understand that before even try to perform unsteady CFD. In very rough terms, by instability we mean the sphere on the top of the hill kind of situation, but applied to the particles of a flow and the forces acting on them (the reference frame in fluid dynamics already makes the matter much more complex)

If we now turn our attention to steady simulations, matter is slightly more complex, because the system evolution is not anymore along the paths allowed by the (numerical representation of the) physics, but otherwise everything we said kind of applies in a certain way.

[FMDenaro]

Originally Posted by Stargazer

Hi FMDenaro, I just want to know what instabilities are hidden in the simulation. Lack of conservation is just my naive guess

FVM ensures discrere conservation even for unsteady flow. A physical flow is u steady when the sum of the fluxes is not zero and that must be balanced by the variation in time of the mean variable. But that could be true even for a transient period of time until a steady state is reached.
The correct answer depend on the specific flow problem.

[Stargazer]

Originally Posted by sbaffini

Let's first consider unsteady simulations. Your numerical representation of a flow is like a different flow, a distorted representation of the original, but still pretty much a flow. As such, it still has a certain number of the physical mechanisms which are in the original physical flow. Which ones, and how much distorted is dependent from the numerics.

Now, for non conservative methods like finite differences, non conservation is just a numerical error (altough, in a sense, more disruptive). For conservative methods, the only non conservation allowed is the one arising from the non perfect convergence of the equations but, again, this is purely numerical.

Also, do not confuse instability in CFD as in unstable numerical methods (say, too high CFL for explicit methods) with the dynamical instability I've been mentioning. The physical and numerical flow are two dynamical systems which, under certain conditions, become unstable. The closer is the numerical dynamical system to the physical one, the more the two will behave consistently. This is what I've been talking about. Unfortunately I can't explain here anything about dynamical systems or fluid dynamics in general, but you need to understand that before even try to perform unsteady CFD. In very rough terms, by instability we mean the sphere on the top of the hill kind of situation, but applied to the particles of a flow and the forces acting on them (the reference frame in fluid dynamics already makes the matter much more complex)

If we now turn our attention to steady simulations, matter is slightly more complex, because the system evolution is not anymore along the paths allowed by the (numerical representation of the) physics, but otherwise everything we said kind of applies in a certain way.

I think I get your point.
The instability I am concerned about is more likely connected to the physical flow phenomena induced numerically "nonconservative". Some interpretations like: residuals start oscillating at some level in steady state, indicating instable flow characteristics (See the picture attached, snapshot from "Computational Methods for Fluid Dynamics" by Ferziger). In such a case, does this mean it is because the separation or vortices that prevent the residuals from dropping and, in other words, "bring in" the nonconservation and thus instabilities?

[FMDenaro]

No, you can get a steady state even if you have separation and vortices. The issue is if this state is stable or not under perturbations.

[andy_]

Originally Posted by Stargazer

Hi Andy, thank you for your suggestions.
BTW, just curious, when we are talking about unsteadiness, what exactly are we referring to? In numerics wise, is the unsteadiness due to the small nonconservation in the cells, because of the for example separation or small vortices?

When solving a steady-state problem with a steady-state scheme such as SIMPLE the predicted flowfield has no physical meaning until it has become steady with small residuals. When solving an unsteady problem every time step must be converged if it is to be physically meaningful/correct.

You refer to using the SIMPLE scheme for an unsteady simulation which raises the question how given SIMPLE is a steady scheme not an unsteady one? If a single pressure correction step is taken with some relaxation factors then the flowfield is not going to be a valid unsteady one regardless of whether vortices are shed or not. If the time derivative term is included and several SIMPLE-like inner iterations are performed then it is likely to be a valid unsteady flowfield but such a scheme would not normally referred to as SIMPLE.

If a very fine grid is used so that the numerical errors are negligible then everything that is supposed to be conserved will be. If a normal reasonable grid is used then the numerical errors will be small and so will the conservation errors. However, numerical scheme can be arranged to strictly conserve a few physical quantities (not all obviously) when the equations are fully solved. Which physical quantities are strictly conserved varies from scheme to scheme with some opting to not strictly conserving anything. Which physical quantities are best conserved varies from problem to problem as does the best form for the numerical/discretization errors.

In your case an optimum numerical scheme for a steady state solver is going to be rather suboptimal for an unsteady solver for vortices and vice-versa. The people behind STAR will know all this but quite what has been implemented and how/if/what can be changed via parameters is a task for those with an interest and access to the manuals.

Unsteadiness is due to viscous forces being too weak to overcome inertial forces. If the numerical errors in the numerical scheme effectively strengthen the viscous forces a bit then that could be sufficient to prevent waviness growing in the boundary layer over the cylinder. It is also possible (and ought to be looked up) that the symmetrical steady solution is still stable at your Reynolds number unless significantly perturbed.

[arjun]

Originally Posted by Stargazer

I did some tests on this case (same mesh and same time-step):
1. First steady simulation with coupled solver, then unsteady simulation with coupled solver, as shown no vortex shedding, and very low residuals;
2. First steady simulation with coupled solver, then unsteady simulation with segregated solver (SIMPLE algorithm), residuals rise gradually and vortex shedding happens in the end;
3. First steady simulation with segregated solver, then unsteady simulation with segregated solver: the steady state is very difficult to reach (high residuals, bad convergence), vortex shedding is shown even in steady simulation, and of course, there is vortex shedding in the unsteady simulation.

It seems that the solver (coupled or segregated) is the main course, which is quite astonishing to me. Because from my side, these two solvers should provide close results. Coupled solver usually is more stable and needs less iteration than segregated solver, and coupled solver is widely used, even as the best practice in many industries. In my case, it looks like the "error" is the cause of the unsteadiness. SO weird...

Coupled solver adds more flux dissipation here it seems. The solution is effectively lower Re case then. This seems to be the case.

[Stargazer]

Originally Posted by FMDenaro

No, you can get a steady state even if you have separation and vortices. The issue is if this state is stable or not under perturbations.

What could be the perturbations in numerical simulation? Could you be more specific? Thank you.

[FMDenaro]

Originally Posted by Stargazer

What could be the perturbations in numerical simulation? Could you be more specific? Thank you.

What you really solve is a set of modified PDEs, the local truncation error being one of the perturbations.
Then the imperfect level of convergence in iterative solvere, approssimate BCs, etc.